MD Nastran 2010 Release Guide

MD Nastran 2010 Release Guide

Corporate

Europe

Asia Pacific

MSC.Software Corporation 2 MacArthur Place Santa Ana, CA 92707 Telephone: (800) 345-2078 FAX: (714) 784-4056

MSC.Software GmbH Am Moosfeld 13 81829 Munich GERMANY Telephone: (49) (89) 43 19 87 0 Fax: (49) (89) 43 61 71 6

MSC.Software Japan Ltd. Shinjuku First West 8F 23-7 Nishi Shinjuku 1-Chome, Shinjuku-Ku Tokyo 160-0023, JAPAN Telephone: 0120-924-832 (toll free, Japan only) Mobile phone: 03-6911-1222 Fax: (81) (3)-6911-1201

Worldwide Web www.mscsoftware.com

Disclaimer MSC.Software Corporation reserves the right to make changes in specifications and other information contained in this document without prior notice. The concepts, methods, and examples presented in this text are for illustrative and educational purposes only, and are not intended to be exhaustive or to apply to any particular engineering problem or design. MSC.Software Corporation assumes no liability or responsibility to any person or company for direct or indirect damages resulting from the use of any information contained herein. User Documentation: Copyright 2010 MSC.Software Corporation. Printed in U.S.A. All Rights Reserved. This notice shall be marked on any reproduction of this documentation, in whole or in part. Any reproduction or distribution of this document, in whole or in part, without the prior written consent of MSC.Software Corporation is prohibited. This software may contain certain third-party software that is protected by copyright and licensed from MSC.Software suppliers. MSC, MD, Dytran, Marc, MSC Nastran, MD Nastran, Patran, MD Patran, the MSC.Software corporate logo, OpenFSI and Simulating Reality are trademarks or registered trademarks of the MSC.Software Corporation in the United States and/or other countries. NASTRAN is a registered trademark of NASA. PAMCRASH is a trademark or registered trademark of ESI Group. SAMCEF is a trademark or registered trademark of Samtech SA. LS-DYNA is a trademark or registered trademark of Livermore Software Technology Corporation. ANSYS is a registered trademark of SAS IP, Inc., a wholly owned subsidiary of ANSYS Inc. ABAQUS is a registered trademark of ABAQUS Inc. All other brand names, product names or trademarks belong to their respective owners. PCGLSS 6.0, Copyright © 1992-2005, Computational Applications and System Integration Inc. All rights reserved. PCGLSS 6.0 is licensed from Computational Applications and System Integration Inc. METIS is copyrighted by the regents of the University of Minnesota. A copy of the METIS product documentation is included with this installation. Please see "A Fast and High Quality Multilevel Scheme for Partitioning Irregular Graphs". George Karypis and Vipin Kumar. SIAM Journal on Scientific Computing, Vol. 20, No. 1, pp. 359-392, 1999. Revision 0. July 15, 2010 MDNA:2010:Z:Z:Z:DC-REL

Main Index

Contents MD Nastran 2010 Release Guide MD Nastran 2010 Release Guide

Table of Contents Preface to the MD Nastran 2010 Release Guide A Word About Prerelease Features List of Books

xiii

Internet Resources

xiv

Overview of MD Nastran 2010 Overview

2

xi

xii

Technical Support

1

2

Multi-Physics in SOL 400 Coupled Thermal-Mechanical Overview Thermal Contact

8

11

Coupled Thermal-Mechanical Implementation Uncoupled Thermal-Mechanical Analysis

3

x

20

27

Linear Perturbation Analysis in SOL 400 Linear Perturbation and Multidisciplinary Linear Analyses in SOL 400 44

4

Thermal Analysis Extensions in SOL 400 Outline of New SOL 400 RC Network Solver Capabilities RC Network Solvers

61

Advanced Radiation Features

Main Index

67

60

iv MD Nastran 2010 Release Guide

Radiation Collections (Radiation Super Elements) and Primitives Convection Correlations

80

Coating and MLI Materials

84

RC Network Thermal Contact User-Defined Routines

5

92

Fluid Structure Interaction in SOL 400 OpenFSI

6

89

100

Advanced Nonlinear (SOL 400) Offsets for Beams and Shells

136

Segment-to-Segment Contact

145

Automated Bolt Modeling

151

Load Stepping Robustness

163

Additional Output Control with NLOPRM SOL 400 Nonlinear Solution Statistics (STS) File

166

168

Large Displacement Grid Point Weight Generation (GPWG) User Subroutines

170

User Defined Module Service UDMSRV

7

171

Explicit Nonlinear (SOL 700) Introduction

174

New Capabilities in Explicit Nonlinear (SOL 700)

174

DMP for FSI Applications with Multi-Material Euler Guidelines in Using SOL 700 FSI DMP Limitations

183

184

Advanced Composites based on AlphaStar – GENOA New Material Models

Main Index

175

194

186

169

74

Contents v

Restart Option to Import an Euler Archive from Previous Run Additional Features

197

Occupant Dummies

198

New Examples in MD Demonstration Problems New SOL 700 Parameters and Bulk Data Entries

8

199 200

Implicit Nonlinear (SOL 600) SOL 600 Enhancements

9

196

204

Numerical Methods and High Performance Computing Serial Performance: Linear and Nonlinear Contact Analysis of Solid Models 210 Distributed Memory Parallel Solutions for Linear and Nonlinear Contact Analysis 213 MPI Selection

216

New Solver Available for Complex Eigenvalue Analysis

10

217

Dynamics (Noise and Vibration) Equivalent Radiated Power (ERP)

222

Frequency Dependent Rigid Absorber Properties

232

Dynamics - Monitor Points in Dynamic Solution Sequences Nonlinear Harmonic Response

238

246

Enhancements to the Frequency Response Function (FRF) and FRF Based Assembly (FBA) Capability 258 EFEA/EBEA (Pre-Release)

11

Loads Management Loads Management

Main Index

266

263

vi MD Nastran 2010 Release Guide

12

Optimization MultiOpt (Multiple Model Optimization)

272

Part Superelement Optimization Enhancements Optimization - Invariant DRESP3 Gradients Design of Monitor Points Parallel Sensitivities

280

289

293

300

DTABLE Enhancement for Dynamic Analysis Constants with DTABLE2 New Optimizer - IPOPT

303

306 310

Topology and Topometry Enhancements

318

Optimization of Nonlinear Structural Responses Phase 2 (Pre-release) 327 Build External Servers Using the SCons Tool

345

Deactivation of Original Design Sensitivity (DSA)

13

348

Aeroelasticity Input of Pressures on an Aerodynamic Mesh Aeroelasticity - Output of Trimmed Loads CSV Output of Trim Results

350 354

359

CSV Output of Stability Derivatives

362

SUBCOM/SUBSEQ with Static Aeroelasticity

365

Upper Hessenberg Complex Eigenanalysis No Longer Supported for Flutter Analysis 367

14

Elements Enhancements to Connector Elements

370

Element Enhancements - Heat Shell Element with Linear/Quadratic Temperature Distribution Across the Element Thickness 380

Main Index

Contents vii

Concentric half cylinder with view factor calculations with imposing heat flux with thermal thick shell 388 Axisymmetrical Mechanical and Heat Transfer Shell Elements Axisymmetrical Shell Elements

406

Multi-Dof Heat Shell Elements Herrmann Elements

15

408

411

Miscellaneous Enhanced MONSUM

414

PARAM,NONCUP Usage Extended to SOL 111 Application Regions

417

New Input File Reader - IFPSTAR Contact Rigid Body Growth Brake Squeal Analysis

421

422

Results and Output Changes MSC.Nastran Error List

A

423

425

Connectors Connectors Output

B

418

428

Thermo-Mechanical Theory Coupled Thermo-Mechanical Theory

C

Thermal Contact Theory Thermal Contact Theory

Main Index

452

434

416

404

viii MD Nastran 2010 Release Guide

Main Index

MD Nastran Release Guide Preface

Preface

Main Index



Preface to the MD Nastran 2010 Release Guide



A Word About Prerelease Features



List of Books



Technical Support



Internet Resources

x MD Nastran 2010 Release Guide Preface to the MD Nastran 2010 Release Guide

Preface to the MD Nastran 2010 Release Guide This Release Guide contains descriptions for the MD Nastran 2010 version, and supersedes the MD Nastran R3 and R2.1 Release Guides.

Main Index

Preface xi

A Word About Prerelease Features MD Nastran 2010 contains a number of features that have been labeled as “prerelease.” A prerelease feature or enhancement is defined as a feature or enhancement that has not yet completed MSC’s exhaustive verification and validation (V and V) testing and qualification process. Therefore, prerelease features are to be used at the client’s own risk.

Main Index

xii MD Nastran 2010 Release Guide List of Books

List of Books Below is a list of some of the Nastran documents. You may find any of these documents from MSC.Software at www.simcompanion.mscsoftware.com. Installation and Release Guides • Installation and Operations Guide • Release Guide

Guides Reference Books • Quick Reference Guide • DMAP Programmer’s Guide • Reference Manual

User’s Guides • Getting Started • Linear Static Analysis • Dynamic Analysis • MD Demonstration Problems • Thermal Analysis • Superelements • Design Sensitivity and Optimization • Implicit Nonlinear (SOL 600) • Explicit Nonlinear (SOL 700) • Aeroelastic Analysis • User Defined Services • EFEA User’s Guide • EFEA Tutorial • EBEA User’s Guide

Main Index

Preface xiii

Technical Support For technical support phone numbers and contact information, please visit: http://www.mscsoftware.com/Contents/Services/Technical-Support/Contact-Technical-Support.aspx Support Center (http://simcompanion.mscsoftware.com) Support Online. The Support Center provides technical articles, frequently asked questions and documentation from a single location.

Main Index

xiv MD Nastran 2010 Release Guide Internet Resources

Internet Resources MSC.Software (www.mscsoftware.com) MSC.Software corporate site with information on the latest events, products and services for the CAD/CAE/CAM marketplace.

Main Index

Chapter 1: Overview of MD Nastran 2010

1

Overview of MD Nastran 2010



Main Index

MD Nastran Release Guide

Overview

2 MD Nastran 2010 Release Guide Overview

Overview MSC.Software is pleased to introduce you to the exciting new technologies in MD Nastran 2010, the premier and trusted CAE solution for aerospace, automotive, defense, and manufacturing industries worldwide. This release includes a wide range of new features and enhancements to our advanced implicit nonlinear capabilities including fluid structural interaction via OpenFSI , thermal analysis, thermal-mechanical coupling, contact, robust convergence algorithms, advanced elements, and advanced materials modeling. MD Nastran 2010 also offers many enhancements to our linear solutions in the areas of durability and NVH, Optimization, and Aeroelasticity. Finally, our explicit analysis capabilities have been enhanced to include advanced composites, new material models, damage models, and distributed memory parallel processing for complex fluid structural interaction applications.

MD Extensions • Coupled Thermal-Mechanical with Contact • Linear Perturbation • RC Network Method for Thermal Analysis • OpenFSI

More information can be found in Multi-Physics in SOL 400 (Ch. 2).

Advanced Nonlinear (SOL 400) • Nonlinear Elements Offsets • Automated Bolt Modeling • Load Stepping Robustness • Additional output controls • User Subroutines

More detailed information on these enhancements to SOL 400 can be found in Advanced Nonlinear (SOL 400) (Ch. 6).

Explicit Nonlinear (SOL 700) • DMP support of Multi-Material Euler for FSI applications • Advanced Composites based on AlphaStar Genoa technology for shells, solids, and honeycombs • New shrink tight fit contact feature • New material models • Variable plasticity damage model • Support of LSTC new generation occupant dummy models

Main Index

CHAPTER 1 3 Overview of MD Nastran 2010

More detailed information on these enhancements to SOL 700 can be found in Explicit Nonlinear (SOL 700) (Ch. 7).

Implicit Nonlinear (SOL 600) • Improved Computational Efficiency Using New Parallel Solvers • Improved friction definition and rigid surface behavior • Improved super element - DMIG support • Improved dynamic integration scheme • Automatic conversion of CHEXA, CPENTA to Solid Shell • Support for RSSCON and RSPLINE • User subroutines for contact and materials • Continuous-stress contact enhancement • Arbitrary cross section and numerically integrated beams

More information on Implicit Nonlinear (SOL 600) can be found in Implicit Nonlinear (SOL 600) (Ch. 8).

Numerical Methods and High Performance Computing (Performance) • Serial Performance: Linear and Nonlinear Contact Analysis of Solid Models (Ch. 9) • Distributed Memory Parallel Solutions for Linear and Nonlinear Contact Analysis (Ch. 9)

More information can be found in Numerical Methods and High Performance Computing (Ch. 9).

Noise, Vibration and Dynamics • Equivalent Radiated Power (ERP) • Dynamics - Monitor Points in Dynamic Solution Sequences

More information can be found in Dynamics (Noise and Vibration) (Ch. 10).

Optimization • PART Superelement Optimization • Integer Input for DTABLE • Optimization - Invariant DRESP3 Gradients • Design of Monitor Points • Miscellaneous - Enhanced MONSUM • Parallel Sensitivities

Main Index


• Optimization of Nonlinear Structure Responses (Pre-release)

More information on these optimization enhancements can be found in Optimization (Ch. 12).

Aeroelastic Enhancements • Aeroelasticity - Output of Trimmed Loads • CSV Output of Trim Results

Loads Management • Loads Management

More information can be found in Loads Management (Ch. 11).

Parts and Assemblies (PAA) (Demonstration Version) The PAA functionality is for demonstration purposes only and is not supported for production work. MSC.Software makes no guarantees that any work done with PAA will be compatible with future versions of MD/MSC Nastran. PAA is a new functionality in MD Nastran and is based on the concept of “computationally reusable Parts”. A Part can be thought of as the finite element model (or matrices of that model that result after processing it) of a single component Part or of an Assembly of Parts. Using this definition everything is a Part, from the smallest component (for example, a bolt) to the complete assembled model (for example, an airplane or a car). All Parts are reusable. That is, a bolt Part may be used in several different models, without the requirement to reprocess the bolt for each model. PAA processing is manual in the current system. There are no automatic restarts. The intent is to have an external program (a Model Manager) handle the logic involved in keeping the current database “correct”. The concept of PAA is very similar to the process used in many NASA (and other) programs. That is, there is a single “system integrator” (person or company), who is in charge of the complete model and putting all of the finite element models together into a complete system model, and a series of component suppliers, each of whom is responsible for a single component or Assembly. In this paradigm, each of the suppliers is responsible for their own model and the only one who “sees” the complete system model is the system integrator. However, when the system model is solved, the system integrator then passes results (either data recovery or boundary solutions) back to the suppliers and they are able to work independently with their models. One advantage of PAA over traditional superelement analysis is the concept of Rapid Simulation-based Prototyping (RSP). The RSP method will allow the owner of each part to work independently to assess changes to their part without having to recompute and assemble the other parts of the system. In the schematic below, the RSP concept will compute results for PART 1 based on model changes to PART 1 without having to reprocess any of the intermediate assemblies.

Main Index

CHAPTER 1 5 Overview of MD Nastran 2010

More information can be found in the Overview of PAA Functionality (p. 2) in the MD Nastran 2010 PAA User’s Guide.

Elements • Connector for Durability • Element Enhancements - Heat Shell Element with Linear/Quadratic Temperature Distribution Across the Element Thickness (Ch. 14). • Axisymmetrical Mechanical and Heat Transfer Shell Elements (Ch. 14)

More information can be found in Elements (Ch. 14).

Future Platform Support MD Nastran will no longer be delivered on the SGI IRIX platform; MD Nastran R3 is available on SGI IRIX. The Linux 32 bit platform will be discontinued starting in the year 2012.

Main Index


Main Index

Chapter 2: Multi-Physics in SOL 400MD Nastran R3 Release Guide

2

Main Index

Multi-Physics in SOL 400 

Coupled Thermal-Mechanical Overview



Coupled Thermo-Mechanical Theory



Thermal Contact



Coupled Thermal-Mechanical Implementation



Uncoupled Thermal-Mechanical Analysis

8 MD Nastran 2010 Release Guide Coupled Thermal-Mechanical Overview

Coupled Thermal-Mechanical Overview Introduction Traditionally, structural simulations and thermal simulations have been performed independently of one another in separate analysis codes specialized in solving each physical discipline. In large companies there are different structural and thermal specialists and departments. These groups interact with each other as the thermal analysts provide the structural analysts with temperature data for thermal distortion and thermal stress analysis. For sophisticated systems, the thermal analysis is dependent on the structural deflection, so an iterative loop is set up to capture all the effects properly. MD Nastran has had nonlinear structural and heat transfer capabilities since its inception. Initially, these were decoupled solutions, but in MD Nastran R3 there was thermal structural chaining. This allowed the analyst to perform a thermal analysis and use the results on a subsequent structural analysis. While this is a significant improvement over manual mappings, it still did not provide a truly integrated ThermalMechanical capability. MD Nastran 2010 Solution 400 introduces true Thermal-Mechanical simulation capability. The MD Nastran implementation of multi-physics simulation employs an algorithm to ensure that both structural and thermal analyses time steps are synchronized and converged to provide a true multi-physics simulation. One of the keys to multi-physics simulations is to capture the structural and thermal load path changes caused by contact. MD Nastran has had structural contact capabilities since its inception. General structural contact allows mechanical meshes to come in to contact and change the load path. Glued structural contact will “weld” mechanical meshes together. Thermal contact is a similar concept but for thermal analysis rather than structural analysis. Thermal contact is implemented in MD Nastran 2010 Solution 400. In addition, the multi-physics aspect of MD Nastran allows for coupling thermal and mechanical contact in the same run. In thermal analysis, thermal contact is available for both steady state and transient. For coupled thermal-mechanical analysis the mechanical analysis can be static or dynamic and the thermal analysis can be steady state or transient. This allows four combinations of coupled thermomechanical analysis: HSTAT-NLSTAT, HSTAT-NLTRAN, HTRAN-NLSTAT, HTRAN-NLTRAN, where HSTAT, HTRAN, NLSTAT, and NLTRAN stand for steady state heat transfer, transient heat transfer, structural nonlinear statics, and structural nonlinear transient respectively. The coupled analysis can account for plasticity and frictional heat coupling and proper updating of interface conditions when there is relative motion between bodies. The bi-directional coupling is a weakly coupled approach between thermal and mechanical passes. The available bi-directional coupling schemes are identified in the figure below and they allow simulation of thermo-mechanical effects associated with large deformation problems and frictional contact.

Main Index

CHAPTER 2 9 Multi-Physics in SOL 400

1. Thermal Strains 2. Structural properties are a function of temperature

Thermal

Structural

3. Thermal problem to be solved on updated geometry 4. Thermal loads due to plastic work 5. Thermal loads due to friction

Benefits Coupled Thermal-Mechanical analysis benefits users who have systems where the thermal and structural solutions must be tightly coupled to capture the true behavior. In addition there are benefits from improved time stepping and convergence algorithms, from new thermal contact capabilities and from new temperature mapping capabilities between dissimilar meshes.

Coupled Thermo-Mechanical Theory Depending on the degree of coupling that needs to be included in the analysis a distinction can be made between uncoupled, weakly coupled and strongly coupled thermo-mechanical analysis. A short summary of each of these analysis types is given below. To read more about the theory behind Coupled Thermo-Mechanical Analysis, please see Coupled Thermo-Mechanical Theory (App. B) for more information. Uncoupled This is a one-way coupling from a thermal analysis to a structural analysis and is also called ‘Analysis Chaining’ in MD Nastran. Thermal effects like thermal expansion and temperature dependent structural material properties can be included in this way, but the effects of structural changes and the effects of heating due to irreversible work to heat conversions can not be icluded. In MDR3, temperature mapping from the end of a previous steady-state heat transfer analysis to a static mechanical analysis was introduced. In MD Nastran 2010, this has been expanded to allow different analysis types, different time steps and dissimilar meshes. More details on this is provided in the section Uncoupled ThermalMechanical Analysis. Weakly Coupled Within each load increment a thermal pass is followed by a structural pass. Each pass iterates until convergence is reached for that particular pass and it incorporates the changes that occured in foregoing pass. In this way it is possible to include the structural effects like changes in geometry due to large deformations, changes in contact conditions and irreversible work to heat conversions due to plasticity and friction in addition to the thermal effects of the uncoupled case. In equation form, for the steady-state case, this can be schematically shown as follows:

Main Index

10 MD Nastran 2010 Release Guide Coupled Thermal-Mechanical Overview

K TT  T

n–1

U

n–1

n

K UU  T  U

 n n–1 n–1   n–1 n n–1  U   +  QM U   T  = Q T    

n–1

n

n

n

 U  = P T  U

n–1

 n n    +  PT  T    

Here n represents the increment number, T the temperature, U the displacement, K the stiffness, Q the thermal flux , QM the additional heat flux due to plasticity and/or friction, P the mechanical load and PT the mechanical load due to thermal strains. The typical approach is to solve the thermal equations first followed by the structural equations. More details on this is provided in the section Coupled ThermoMechanical Theory (App. B). Strongly Coupled In each load increment the thermal and the coupled problem are solved simultaneously and the effects of all thermal and structural changes can be incorporated in each iteration. In equation form, for the steadystate case, this can be schematically shown as follows: K TT  T

n–1

U

n–1

 KT U  T

K UT  T

n–1

n–1

U

n–1

 K UU  T

U

n–1

n–1

U

n

n

n–1

n

n–1

 T  = Q T

n–1

n

 U  = P T

U

n–1

U



n–1



The strongly coupled approach requires special elements that have both temperature and displacement degrees of freedom. It is computationally expensive, in most cases leads to unsymmetric system matrices and is not the preferred approach in MD. The weakly coupled approach is sufficient for most practical applications and is the approach followed in MD. For more information about the assumptions made to arrive at the weakly coupled formulation from its strongly coupled form the reader is once more referred to appendix B, Coupled Thermo-Mechanical Theory.

Main Index


Thermal Contact Introduction As described in the multi-physics introduction, one of the keys to multi-physics simulations is to capture the structural and thermal load path changes caused by contact. MD Nastran has had structural contact capabilities since its inception. General structural contact allows mechanical meshes to come in to contact and change the load path. Glued structural contact will “weld” mechanical meshes together. Thermal contact is a similar concept but for thermal analysis rather than structural analysis. Thermal contact is implemented in MD Nastran 2010 Solution 400 in pure thermal analysis and coupled thermo-mechanical analysis. The user will be able to analyze thermal interactions between different contact bodies for the body areas that are in contact and thermal interactions between contact bodies and the environment for the body areas that are not in contact. In addition to “contact” and “no contact” from the pure mechanical case, there is “near contact” which allows thermal interactions between bodies that are getting near to each other, but not yet in real (mechanical) contact. Thermal contact is available for both steady state and transient analysis.

Benefits This functionality provides a user-friendly interface to defining thermal contact conditions. The user defines contact bodies with their thermal properties and contact tables defining the possible contact pairings with the thermal properties for each pairing. The program automatically identifies the body areas involved in contact and the body areas exposed to the environment and for each situation, it sets up the appropriate interface conditions for the thermal interactions. In a coupled thermal-mechanical analysis, bodies may have relative motions, causing the contact conditions to change over time. Due to friction forces in the contact interface, heat may be generated adding an extra heat flux load in the thermal phase of the analysis. All changes in the interface conditions and resulting loads are updated automatically.

Theory For information on the theory behind Thermal Contact, please see Thermal Contact Theory (App. C).

Input Analysis Types The analysis types supported for thermal contact are steady state heat transfer and transient heat transfer; these are specified in the appropriate SUBCASE / STEP / SUBSTEP with ANALYSIS=HSTAT and ANALYSIS=HTRAN, respectively. For additional details on the case control setup, please refer to the remarks for the Case Control command ANALYSIS (p. 231) in the MD Nastran Quick Reference Guide.

Main Index

12 MD Nastran 2010 Release Guide Thermal Contact

Contact Body Definition Individual contact bodies are defined on the BCBODY entry and its behavior is defined by setting the BEHAV field to “HEAT”, “DEFORM”, or “RIGID”. In a thermal analysis the behavior field can be “HEAT” (ITYPE=4) for a meshed body that can conduct heat or “RIGID” (ITYPE=1) for a rigid body defined by geometric entities that behaves as a heat sink. In a coupled thermal-mechanical analysis the behavior field can be “DEFORM” (ITYPE=2) for a meshed body that can conduct heat in the thermal phase of the analysis and that can deform in the mechanical phase of the analysis or “RIGID” (ITYPE=1) for a rigid body defined by geometric entities that behaves as a heat sink in the thermal phase of the anlysis and is completely rigid in the mechanical phase of the analysis. A contact body that will be available for heat transfer requires additional information on the HEAT keyword line. Specifically, the following body properties can be specified: BCBODY Entry (Heat Transfer related items only) 1

2

3

4

5

6

7

8

9

BCBODY

BID

DIM

BEHAV

BSID

ISTYP

FRIC

IDSPL

CONTROL

“HEAT”

CFILM

TSINK

CHEAT

TBODY

HCV

HNC

ITYPE

BNC

EMISS

HBL

HNL

BNL

HNLE

BNLE

HNCE

BNCE

CMB

CMS

10

• BEHAV - use HEAT, DEFORM, or RIGID to define the behavior type of the contact body • CFILM - Heat transfer coefficient (film) to environment; constant or function of temperature • TSINK - Environmental sink temperature; constant or function of time. • CHEAT - Contact heat transfer coefficient; constant or function of temperature • TBODY - Body temperature; constant or function of time • HCV - Convection coefficient for near field behavior; constant or function of temperature • HNC - Natural convection coefficient for near field behavior; constant or function of

temperature • ITYPE - Heat sink or heat conduction, or deformable body • BNC - Exponent associated with the natural convection coefficient for near field behavior;

constant or function of temperature • EMISS - Emissivity for radiation to the environment or near thermal radiation; constant or

function of temperature. • HBL - Separation distance dependent on thermal convection coefficient; constant or function of

temperature. • HNL -Heat transfer coefficient for nonlinear convective heat flow for near field behavior;

constant, function of temperature. • BNL - Exponent associated with the nonlinear convective heat flow for near field behavior;

constant or function of temperature

Main Index


• HNLE -Heat transfer coefficient for nonlinear convective heat flow to the environment;

constant, function of temperature. • BNLE - Exponent associated with the nonlinear convective heat flow to the environment;

constant, function of temperature. • HNCE - Natural convection coefficient for heat flow to the environment.; constant, function of

temperature. • BNCE - Exponent associated with natural convection heat flow to the environment.; constant,

function of temperature. • CMB - Heat capacity of the rigid body, when entered as a geometric entity with an associated

scalar point; constant. • CMS - Heat capacity of the environment, when associated with a scalar point; constant.

Note that heat exchange to the environment only applies to deformable or heat conducting bodies, i.e. meshed regions. Conversely a body temperature TBODY only applies to a rigid body. A heat capcity for an environment or a rigid body is only used when there exists an associated scalar point. It is recommend to enter the contact and near contact heat transfer coefficients in a contact table (BCTABLE), since in general these are not a property of a single body, but apply to one or more body pairs. Additional rules are defined in BCBODY - MD Only (p. 1153) in the entry. Contact Table Definition Each contact body potentially contacts any other contact body. The BCTABLE entry gives additional control over which bodies will be allowed to contact each other, the geometric tolerances to use, and additional heat transfer parameters. The DQNEAR field on the BCTABLE entry is used to define the distance for near thermal contact behavior. Near contact detection is not activated if this field is zero or undefined. The near contact distance is meant to model relatively small gaps that allow for heat exchange between contact bodies before real (mechanical) contact takes place. It is not intended for arbitrarily large gaps between contact bodies. For instance, the radiation law does not evaluate view factors for contact body areas that “see” each other in near contact. Contact body areas that are not in hard or near contact with other bodies may exchange heat with an environment if corresponding heat flow laws have been activated for the contact body. BCTABLE Entry (Heat Transfer related items only) 1

2

3

BCTABLE

ID

IDSLAVE

“SLAVE” IDSLA1

Main Index

4

5

6

IDMAST NGROUP COPTS ERROR

FNTOL

FRIC

ISEARCH

ICOORD

JGLUE

“HHHB”

HTC

HCV

HNC

HNL

BNL

HGLUE

7

8

9

COPTM CINTERF

IGLUE

DQNEAR

BNC

EMISS

HBL

10


1

2

3

4

5

6

7

8

9

“MASTERS”

IDMA1

IDMA2

IDMA3

IDMA4

IDMA5

IDMA6

IDMA7

IDMA8

IDMA9

...

10

• DQNEAR - Distance below which near thermal contact behavior occurs; constant. • HGLUE - Flag to activate the thermal glue option. • 0 or blank = thermal glue is off, i.e. convective heat transfer • 1 = thermal glue is on, i.e. temperature fields of bodies are tied; no convective heat transfer • HTC - Heat transfer coefficient; constant or function of temperature • HCV - Convection coefficient for near field behavior; constant or function of temperature • HNC - Natural convection coefficient for near field behavior; constant or function of

temperature • BNC - Exponent associated with the natural convection coefficient for near field behavior;

constant or function of temperature. • EMISS - Emissivity in near thermal radiation; constant or function of temperature. • HBL - Thermal convection coefficient dependant on separation distance; constant or function of

separation distance. • HNL - Heat transfer coefficient for nonlinear convective heat flow for near field behavior;

constant or function of temperature. • BNL -Exponent associated with the nonlinear convective heat flow for near field behavior;

constant or function of temperature. Additional rules and heat flow equations are defined in BCTABLE - MD Only (p. 1214) in the entry. Heat flow laws for contact, near contact and environment When two bodies are in contact with each other and thermal glue is off for the body pair then the following convective heat flow law describes the heat exchange per unit area between the body areas that are in contact: q = HCT   T A – T B  When two bodies are in contact and thermal glue is on for the body pair then the local contact condition simply becomes: TA = TB When two bodies are in near contact then the following convective heat flow law describes the heat exchange per unit area between the body areas that are in near contact:

Main Index


q = HCV   T A – T B  + HNC   T A – T B  BNL

HNL   T A

BNC BN L

– TB 4

+ +

4

  EMISS   T A – T B  + dist dist HCT   1 – ------------------------- + HBL  -------------------------   T A – T B   DQNEAR DQNEAR For body areas that are not in contact and not in near contact with other bodies the following convective heat flow law describes the heat exchange per unit area between these body areas and the environment: q = CFILM   T A – T S I N K  + HNCE   T A – T S I N K  BN LE

HNLE   T A

4

BNCE

+

B N LE

– TS I N K  + 4

  EMISS   T A – T S I N K  + Here TA is the temperature in the contact points of the touching body or the surface temperature of the points exposed to the environment and TB is the temperature in the contact point of the touched body. If the touched body is a rigid body TB is the temperature of this rigid body and should be replaced by TBODY. For heat trtansfer to the environment TSINK is the ambient temperature of this environment. The heat contribution term involving “dist” is only evaluated for nonzero HBL, where “dist” is the distance bewteen the bodies. For radiation contributions it is necessary to define s, the Stefan-Bolzmann constant, which can be entered as a parameter thru PARAM,SIGMA,value. In addition PARAM,TABS,value can be used to define an offset from the user temperature scale to the absolute temperature scale. No view factors are considered for this type of radiation. Supported Features Thermal contact is supported in static and transient thermal analysis as well as coupled thermalmechanical analysis. Mesh-to-rigid and mesh-to-mesh contact are supported for pure thermal analysis. Chained analysis and fully coupled thermal-mechanical analysis support deformable to deformable contact as well as deformable to rigid contact. Deformable and heat conducting contact bodies can be modelled by a 2D plane stress, 2D plane strain, 2D axisymmetric or a 3D mesh (solids, shells, etc.) There are two types of thermal interface conditions: 1) Convective thermal contact and 2) Glued thermal contact. Convective thermal contact distiguishes between hardcontact and near contact, where near contact allows heat exchange between bodies before hard (mechanical) contact takes place. Glued thermal contact is only possible in the hard contact sense. Glued contact can be seen as a form of convective contact with a very high contact heat transfer coefficient and is e.g. useful to connect dissimilar meshes thermally.

Main Index


Thermal-mechanical coupling contact bodies will automatically update their geometry to the current deformed state. Heat generated by plasticity and friction are accounted for in a fully coupled thermalmechanical simulation. Heat generated by friction is evenly distributed between the two bodies, i.e. half of the frictional flux is applied to the touching body and half is applied to the touched body. Refer to the NLSTEP section for more details on this coupling. Here two factors are specified that control the fractions of plastic work and frictional work that get converted into heat (HGENPLAS and HGENFRIC). For thermal properties that can be expressed as a function of temperature or time, the following tables are supported: • TABLEM1 and TABLEM2 for temperature dependencies • TABLED1 and TABLED2 for time dependencies • TABL3D (0,1,2) for time and temperature dependencies and multi-dimensional tables

A rigid geometry can have a scalar point associated with it. In this case, a lumped heat capacity can be defined for the body. If no scalar point is associated with it, its temperature can be directly prescribed, but it can not have a heat capacity. The environment can have a scalar point associated with it. In this case, a lumped heat capacity can be defined for the environment. If no scalar point is associated with it, its temperature can be directly prescribed, but it can not have a heat capacity. The BCONTACT - MD Only Case Control logic of thermal contact definitions over different subcases of an analysis is thee same as that of a stress analysis with contact.

Limitations 1. In a coupled thermal-mechanical analysis, the body of type HEAT (i.e., ITYPE = 4), i.e., a body that does heat conduction in the thermal pass, but behaves as a rigid in the mechanical, is not supported. 2. Beam-to-beam and beam-to edge thermal contact is not supported. 3. Shell edge-to-edge thermal contact is not supported 4. Glued thermal contact to a rigid body with an associated scalar point is not supported yet. 5. Frictional heat coupling to a rigid body with an associated scalar point is not supported yet. 6. Friction heat coupling to bottom faces of shell elements is not supported yet. 7. The formula option in TABL3D tables is not supported.

Test Cases Test problem shell_edge_thermal_glue1.dat This example problem demonstrates static heat transfer analysis including thermal contact with a glued contact (HGLUE=1). The thermal conductivity is 4 W/in/degreeC, Heat flux is defined as 20W/in^2 on

Main Index


the curved edge (QBDY3). Temp(INIT)=20degreeC on edge opposite the body with TEMP(INIT)=0 elsewhere.

Figure 2-1

Glued Edge Thermal Contact Example Geometry

Listing 2-1

Partial listing of TPL problem shell_edge_thermal_glue1.dat

TEMPERATURE(INITIAL) = 1 SUBCASE 1 STEP 1 ANALYSIS = HSTAT NLPARM = 1 BCONTACT = 7 SPC = 1 LOAD = 2 THERMAL(SORT1,PRINT)=all FLUX(SORT1,PRINT)=ALL $ Direct Text Input for this Subcase BEGIN BULK NLPARM 1 10 FNT BCTABLE 7 1 SLAVE 2 1 1 0 FBSH HHHB 0.

1 MASTERS 1 plplane,3,1, pshln2,3,1,,0.1,ih, $ Deform Body Contact LBC set: coarse_mesh BCBODY 1 2D HEAT 3 0 ,heat, BCPROP 3 3

Main Index

YES

1061

1061


Figure 2-2

Edge Glue Thermal Results

GUI Support Patran Patran currently supports post-processing of the thermal results. Patran does not currently support the creation of the input file. SimXpert SimXpert can be used to setup the thermal contact table and post-process the thermal results. Below are a few figures on how to access the contact table. Note that the thermal contact table in SimXpert is still undergoing enhancements and design review, so the version of SimXpert you use may appear slightly different.

Main Index


Figure 2-3

Main Index

SimXpert Contact Table Setup Forms

20 MD Nastran 2010 Release Guide Coupled Thermal-Mechanical Implementation

Coupled Thermal-Mechanical Implementation Introduction For bi-directional coupled thermal-mechanical analysis, an increment-level staggered approach has been implemented with sub-increments specified through the SUBSTEP entry for heat-transfer and mechanical analyses. Note that this staggered coupling is solved for the same time steps and on the same FE mesh. Time stepping and convergence parameters for the coupled analysis are specified through the NLSTEP entry. While the implemented framework is general, only coupling of heat and mechanical is supported in MD Nastran 2010. Both static and transient thermal types (HSTAT and HTRAN) and corresponding mechanical types (NLSTATIC and NLTRAN) are allowed. This allows 4 combinations: HSTATNLSTAT, HTRAN-NLSTAT, HTRAN-NLTRAN, HSTAT-NLTRAN. The implemented multi-physics framework is a staggered scheme and works as follows: • When the solution procedure moves on to a new sub-increment, relevant information from other

sub-increments (temperatures, displacements, generated heat, etc.) is passed in. Regular (full) Newton-Raphson iterations are conducted within each sub-increment until convergence is achieved. This procedure is followed until all sub-increments converge. • If a particular sub-increment does not converge, the time step is bisected. The increment is then

repeated starting at the first sub-increment with the smaller time step. • Time step sizes are synchronized across thermal and mechanical sub-increments. Either fixed

time stepping scheme or adaptive time stepping scheme can be used. When adaptive time scheme is used, each individual physics (thermal pass and mechanical pass) is allowed to predict the time step for the next increment independently. The actual time step used for the next increment is synchronized by choosing the smaller of the predicted step sizes. • The above steps are repeated for each increment until the load step is completed.

The thermo-mechanical coupled implementation is schematically depicted by the following figure:

Main Index


• Input plastic/friction heat flux from previous increment. • Transfer displacements from pervious increment and

form thermal matrices/loading on updated geometry

Heat transfer sub-increment

Iterate until converged

Transfer nodal temperatures from heat to mechanical sub-increment downstream

Mechanical sub-increment

One Increment

Iterate until converged

With SimXpert, the user can view the results of the coupled analysis. For each load step, there are two sets of result data available. One is the thermal analysis result and the other is mechanical analysis results. Only OP2 and MASTER files are supported. With MD Patran, limited post-processing capability for coupled analysis is supported at this time.

Benefits Bidirectional coupling allows a realistic modeling of both thermal and mechanical physics for a structure. It allows simultaneous solution of HSTAT-NLSTAT, HSTAT-NLTRAN, HTRAN-NLSTAT, HTRAN-NLTRAN problems. It also allows chaining of multi-physics steps with linear perturbations/single physics steps.

Input The MD Nastran Case Control consists of SUBCASE and STEP to control the SOL 400 nonlinear solutions. With the incorporation of the multi-physics capability, Case Control command SUBSTEP is introduced to define the physics discipline to be used within a STEP. Case Control command NLSTEP is used to refer to the NLSTEP Bulk Data entry which defines solution convergence criteria for each analysis type. For more information on the NLSTEP Bulk Data entry, see Load Stepping Robustness (Ch. 6). The usage of NLSTEP and SUBSTEP is best demonstrated with a sample Case Control: Listing 2-2

Example Case Control for NLSTEP and SUBSTEP

SUBCASE 100 TEMPERATURE(INIT)=3 STEP 10 SET 1456 = LIST NLSTEP = 84

Main Index


SUBSTEP 1 ANALYSIS=HTRAN IC=3 SPC=35 DLOAD=11 THERMAL=ALL FLUX=ALL ENTHALPY=ALL SUBSTEP 2 ANALYSIS=NLSTAT SPC=2 LOAD=110 DISP(PLOT)=1456 STRESS=ALL NLSTRESS=ALL

The following features should be noted in the above example. The thermo-mechanical coupling is between HTRAN and NLSTAT. The initial temperatures are specified through TEMP(INIT) = 3 for the mechanical substep (NLSTAT) and IC = 3 (same ID) for the thermal substep. This specification allows both the thermal and mechanical substeps to begin at the same temperature. Output requests, loading, SPC specifications for each substep are separate. NLSTEP applies to both substeps.

Output The .f06 output is similar to output for standard structural and heat transfer solutions. Note that all of the heat transfer output is printed followed by all of the structural output. In addition to .f06 and .pch output, both OUTPUT2 and MASTER/DBALL output formats are supported. Listing 2-3

1

TWO BODY CONTACT

SUBCASE 1 TIME =

... ... ... 1

JULY

STEP 1 1.250000E-01

POINT ID. 1 7 13

TYPE S S S

POINT ID. 1 2 3 4

T E M P E R A T U R E ID VALUE 1.999978E+01 2.000000E+01 2.000000E+01

ID+1 VALUE ID+2 VALUE 1.999946E+01 2.007018E+01 2.000000E+01 2.000000E+01 2.000614E+01 {etc.}

MD NASTRAN

7/13/09

PAGE

65

PAGE

391

V E C T O R ID+3 VALUE 2.000163E+01 2.000000E+01

JULY

STEP 1 1.25000E-01 TYPE G G G G

17, 2009

SUBSTEP 1

TWO BODY CONTACT

0 SUBCASE 1 LOAD STEP =

Main Index

Example Output for SUBSTEP

ID+4 VALUE 2.000020E+01 2.000000E+01

17, 2009

ID+5 VALUE 2.000000E+01 2.000000E+01

MD NASTRAN

7/13/09

SUBSTEP 2 D I S P L A C E M E N T T1

0.0 0.0 6.415519E-04 2.385733E-04

T2

0.0 0.0 -7.616700E-04 2.329112E-04

T3

V E C T O R

0.0 0.0 0.0 0.0 2.270600E-05 0.0 5.125663E-05 {etc.}

R1

0.0 0.0 0.0

R2

0.0 0.0 0.0

R3


Guidelines and Limitations The following guidelines for thermo-mechanical coupled analysis should be noted: 1. Initial Temperatures • The initial temperatures of the system should be physically valid starting temperatures (not

guess temperatures as is sometimes done in HSTAT analysis). • Care should be taken to ensure that both the heat transfer substep and the mechanical substep

start at the same initial temperatures. For static heat HSTAT combined with mechanical substeps (NLSTAT or NLTRAN), TEMP(INIT) is sufficient to specify starting temperatures for both the heat and mechanical runs. For transient heat HTRAN combined with mechanical substeps, use TEMP(INIT) for the mechanical substeps (NLSTAT or NLTRAN) and IC with the same ID for the transient heat substep. 2. TEMP(LOAD/MATERIAL/BOTH) is not necessary for coupled analysis. Any given temperature loading data for the mechanical substep is ignored. Temperatures obtained from the heat transfer pass are automatically transferred to the mechanical pass. 3. Coupled analysis can be used in conjunction with analysis chaining. All the multi-physics steps should be defined first. For a particular physics, transient substeps should follow the static substeps. For example, Step 1: HTRAN-NLSTAT followed by Step 2: HTRAN-NLTRAN is allowed. Linear perturbation steps and single physics steps can follow the multi-physics steps in any particular order. Supported linear perturbation steps include MODES, BUCK, DFREQ, MFREQ, MTRAN, DCEIG, MCEIG. 4. Use PARAM,LGDISP judiciously for large displacement analysis. PARAM,LGDISP,1/2 implies that the thermal problem is still solved on the original geometry while the mechanical problem is solved on the current geometry. PARAM,LGDISP,11 or 12 implies that both the thermal and mechanical problems are solved on the current geometry. The following limitations should be noted. 1. CLOAD, LOADSET and DEFORM commands are not supported for SUBSTEP. 2. XDB output is not supported. 3. NLIC restart is not allowed for elements using property extensions like PSHLN1, PSLDN1. They only support restarts from the last converged increment. Note that this is a general limitation for single physics too. 4. Radiation view factors are not supported on updated geometry. They are only computed on the original geometry. 5. Temperature mapping from heat to structural only works for nonlinear elements. For a linear analysis or for an analysis with linear elements (e.g., CQUAD8, CTRIA6, CHEX20), automatic mapping is done in the code using property extensions (e.g., PSHLN1, PSLDN1) to allow mapping of temperatures in all cases. The Case Control command SUBSTEP must obey the following rules: 1. The SUBSTEP command can only be used in nonlinear solution sequence SOL 400 (NONLIN).

Main Index


2. The SUBSTEP command can only be used within in a STEP command. 3. When used in a STEP command two SUBSTEP commands must occur. 4. Each SUBSTEP must contain a unique ANALYSIS=type statement. Currently there is a limitation of only two SUBSTEPs per STEP with the following options: • ANALYSIS=HSTAT for the first SUBSTEP and ANALYSIS=NLSTAT for the second

SUBSTEP. • ANALYSIS=HTRAN for the first SUBSTEP and ANALYSIS=NLTRAN for the second

SUBSTEP • ANALYSIS=HTRAN for the first SUBSTEP and ANALYSIS=NLSTAT for the second

SUBSTEP • ANALYSIS=HSTAT for the first SUBSTEP and ANALYSIS=NLTRAN for the second

SUBSTEP 5. Within a STEP the SUBSTEP identification number n must be in increasing order and not greater then 9999999.

Test Cases The following test cases are available in the TPL in directory /tpl/subdir: TPL problem cpl_fric_heat.dat TPL problem cpl_fric_heat.dat demonstrates large displacement coupled thermal / mechanical with the heat being generated by friction. The case control, contact commands, and NLSTEP Bulk Data entry should be evident: Listing 2-4

Example Output for SUBSTEP

subcase 1 bcontact = 0 set 1 = 46,49,85,93,99,212,227 step 1 nlstep = 211 temp(init)=100 substep 1 analysis = htran bcontact = 999 ic = 100 thermal(sort1) = all substep 2 analysis = nlstatics bcontact = 999 spc = 3 load = 20 disp(sort1) = all BEGIN BULK param,lgdisp,1 NLSTEP,211,1.0 ,FIXED,200,1 ,MECH,UPV,.01,.01,,PFNT,-1,

Main Index


,HEAT,UPV,.01,.01,,PFNT,-1, ,COUP,,0.9 tempd,100,20.0 BCPARA, ,FTYPE,6,FKIND,1 $ BCBODY bcbody,1,3d,deform,1,1,0.02 ,heat, 2.0e2,2.0e1, 0.0, 0.0, ,, 0.0, 0.0, 0.0, bsurf,1,81 thru 107 bcbody,2,3d,deform,2,1,0.02 ,heat, 2.0e2,2.0e1, 0.0, 0.0, ,, 0.0, 0.0, 0.0, bsurf,2,1 thru 80 $ BCTABLE bctable,0,,,1 ,slave ,1,0.01,,0.1,, 0, ,,,,,0,0.0,0 ,,hhhb, 0.0e+0, 0.0, 0.0, ,masters,2 bctable,999,,,1 ,slave ,1,0.01,,0.1,, 0, ,,,,,0,0.0,0 ,,hhhb, 0.0e+0, 0.0, 0.0, ,masters,2, $

Figure 2-4

Main Index

0.0, 0.0,

0.0, 0.0,

0.0,

0.0,

0.0

0.0,

0.0,

0.0

SimXpert Multi Physics Post Processing


GUI Support Patran None. SimXpert SimXpert supports both SUBSTEP and NLSTEP setup as well as post processing. The SimXpert contact setup is shown in Thermal Contact, 11.

Figure 2-5

SimXpert SUBSTEP support

Post processing support is demonstrated in the example section.

Main Index


Uncoupled Thermal-Mechanical Analysis Introduction It is very common for a thermal finite element mesh and a structural finite element mesh to have different mesh densities because the fidelity required to capture accurate results for each physics discipline is different. The structural analyst who needs the thermal data can use interactive tools such as Patran to perform the coupling. The uncoupled thermal-mechanical analysis process introduced in MD Nastran 2010 supports dissimilar mesh and different time steps for related thermal and structural jobs. The user will be able to access thermal results directly from an MD Nastran thermal database in structural runs.

Benefits This functionality provides a user-friendly interface to retrieve temperature results directly from thermal database. The user need not save the thermal results to a punch file and then include it in structural runs. It also offers the power of performing real time temperature interpolations for nonlinear transient structural analysis. It also offers the flexibility of allowing different mesh sizes and time steps between thermal and structural models, i.e. run a heat transfer job and transfer the nodal temperatures to another group in a different location to perform a separate structural analysis with temperature-dependent material properties. The latter will use a different mesh and a different time stepping. This is particularly important to analysts performing engine block thermal stress analysis, and airplane fuselage and wing analysis.

Input The user will run a thermal analysis job in MD Nastran SOL 400. The database is saved (submit with SCR=NO). A subsequent structural analysis is performed in MD Nastran SOL 400 with a TEMP(LOAD) Case Control command with the new options HSUBCASE, HSTEP, and HTIME described here. Format:  INITIAL    t TEMPERATURE  MATERIAL   HSUBCASE = i  HSTEP = j  HTIME =   LOAD ALL     BOTH

Main Index

= n

28 MD Nastran 2010 Release Guide Uncoupled Thermal-Mechanical Analysis

HSUBCASE

Specifies a SUBCASE executed in the selected thermal job. See Remark 14.

i

Identification number of a SUBCASE executed in the selected thermal job. (Integer > 0, Default = 0 is the first SUBCASE) See Remark 14.

HSTEP

Specifies a STEP executed in the selected thermal job. See Remark 14.

j

Identification number of a STEP executed in the selected thermal job. (Integer > 0, Default = 0 is the first STEP) See Remark 14.

HTIME

Specifies the time of a time step executed in the selected nonlinear transient thermal job. See Remark 14.

t

Time of a time step executed in the selected nonlinear transient thermal job. (Real > 0.0, Default is the last time of the specified SUBCASE and/or STEP) See Remark 14.

ALL

Selects all time steps executed in the selected nonlinear transient thermal job. See Remark 14.

Remark 14 For TEMPERATURE(LOAD) requests in SOL 400, HSUBCASE, HSTEP, and HTIME are used to retrieve the temperature results from an existing thermal database. This feature allows user to select either steady state or transient thermal results for nonlinear structural analysis, with the flexibility of different time steps and dissimilar mesh sizes between thermal and structural runs. The following rules apply for using this capability: • HSUBCASE, HSTEP, and HTIME keywords must follow a LOAD keyword. • Although all three keywords have default values, at lease one keyword must exist to apply this

uncoupled multi-physics feature in analysis. • HTIME=ALL is used in nonlinear transient structural analysis to perform real time

temperature interpolations. In this case, the nodal temperatures of nonlinear elements are updated at each time step. These temperatures are equal to the temperature results of the selected thermal database at current time. • The set IDs of TEMP(LOAD) must be different from the set IDs of TEMP(INIT). • To save temperature results of thermal analysis in MASTER Nastran database, use the

following command. nastran thermal_job_name scratch=no In addition, the user must specify the following Bulk Data entry PARAM,NLPACK,-1 for transient thermal models with number of time steps greater then the default NLPACK output time steps. • The following File Management Statements are required in the current structural model to

select the thermal database.

Main Index


ASSIGN hrun='thermal_job_name.MASTER' DBLOC DATABLK=(HEATDB) LOGI=hrun

Guidelines and Limitations Remark 14, 28 of the updated TEMPERATURE Case Control command provides the rules associated with uncoupled thermal-mechanical mapping.

The following guidelines should be noted: • The default value of HSUB is the first subcase. The default value of HSTEP is the first step. • The default value of HTIME is the last time step of a particular step. HTIME = t is supported for

mapping from HSTAT --> NLSTAT, HTRAN --> NLSTAT or HTRAN --> NLTRAN. A linear ramp is used from initial temperatures specified by TEMP(INIT) to reach the temperatures read from the thermal database for HTIME = t. • When HTIME = ALL is used, all elements should be nonlinear and the structural analysis type

should be NLTRAN. If linear elements are used in such analyses, they are automatically mapped to nonlinear counterparts using property extensions like PSHLN1, PSLDN1. • Nodal temperatures can be post-processed for a thermal run. Normally, the mapped temperatures

are unavailable for verification in a mechanical run. For enhanced elements using property extensions, the NLOUT Bulk Data entry with TOTTEMP post code in conjunction with the NLSTRESS Case Control command allows one to verify the temperatures in a mechanical analysis at the integration points of the mesh. • For the analysis with incongruent finite element mesh sizes between thermal and structural

models, the user may adjust the mesh mapping tolerance by specifying NLMOPTS, MAPTOL option in the Bulk Data Section. The default value of MAPTOL is 0.2, i.e., the mapping scheme accepts a structural grid that is located within 20% of the dimension of the closest thermal element even though the grid lies outside the associated thermal element. Note:

In MD Nastran 2010, contact body integrity is not maintained while doing the thermal mapping. While this would not be a restriction for bodies that are not physically in contact or in glued thermal contact, it could lead to undesirable temperature mapping for bodies that are in regular thermal contact with temperature gradients across the contact interface.

Test Cases The following test cases are available in the TPL in directory /tpl/uncoupl400: nluch##.dat - nlucs##.dat. These are ‘paired’ examples of the heat transfer analysis (nluch##) and the structural analysis (nlucs##). The heat transfer is run first, followed by a structural analysis restart.

Main Index


TPL Problems nluch14.dat and nlucs14.dat Example nluch14/nlucs14 demonstrates the modeling of uncoupled analysis using a pair of thermal and structural models with composite elements. Note that the GRIDs from each model do not align.

Figure 2-6

/tpl/uncoupl400/nluch14.dat and nlucs14.dat geometry

The thermal model nluch14 is run first by the following command to save temperature results. mdnastran nluch14.dat scr=no

The temperature results are retrieved from the subsequent nonlinear transient structural run by the File Management Statements ASSIGN and DBLOCATE. The temperatures are applied by specifying the appropriate TEMPERATURE Case Control command. Listing 2-5

FMS and Case Control for job nlucs14.dat

assign hrun='nluch14.MASTER' dbloc datablk=(heatdb) logi=hrun $ id msc, nlucs14.dat $ sjf 16-Mar-2009 mdr4 SOL 400 TIME 60 CEND SEALL = ALL SUPER = ALL TITLE = Uncoupled thermal & structural analysis prob 14 - structural part SUBTITLE = HTIME=ALL and quad4 TEMPERATURE(INITIAL) = 1 SUBCASE 1 analysis=NLTRAN step 1 TSTEPNL= 1 SPC = 2 TEMPERATURE(LOAD,hsubc=3) = 3 DISPLACEMENT(SORT1,REAL)=ALL nlstress = all stress = all step 2 TSTEPNL= 2 SPC = 2 TEMPERATURE(LOAD,hsubc=10,htime=0.80) = 4 DISPLACEMENT(SORT1,REAL)=ALL nlstress = all stress = all SUBCASE 2 analysis=NLTRAN step 3 TSTEPNL= 3 SPC = 2 TEMPERATURE(LOAD,hsubc=10,htime=all) = 5 DISPLACEMENT(SORT1,REAL)=ALL nlstress = all

Main Index


stress = all

Turbine blade coarse thermal mesh using Restart into fined structure mesh for thermal stress analysis using SOL 400 Turbine Blade Example The Thermal job is submitted with SCR=NO. The FMS, EXEC, and CASE control sections define the job setup for the thermal run: SOL 400 CEND $ Direct Text Input for Global Case Control Data TITLE = MD Nastran job created on 29-May-09 at 11:19:39 ECHO = NONE TEMPERATURE(INITIAL) = 1 SUBCASE 1 STEP 1 TITLE=This is a default subcase. ANALYSIS = HSTAT NLPARM = 1 SPC = 1 THERMAL(SORT1,PRINT)=ALL FLUX(SORT1,PRINT=ALL BEGIN BULK The FMS, EXEC, and CASE control for the structural restart job: assign hrun='map_heat1.MASTER' dbloc datablk=(heatdb) logi=hrun SOL 400 CEND $ Direct Text Input for Global Case Control Data TITLE = MD Nastran job created on 02-Apr-10 at 13:30:31 ECHO = NONE SUBCASE 2 ANALYSIS=NLSTAT TITLE=This is a default subcase. temp(load,hsub=1)=9 NLPARM = 1 SPC = 2 DISPLACEMENT(plot,SORT1,REAL)=ALL SPCFORCES(plot,SORT1,REAL)=ALL STRESS(plot,SORT1,REAL,VONMISES,BILIN)=ALL $ Direct Text Input for this Subcase BEGIN BULK The resulting temperature profile from the thermal run is automatically mapped onto the structural mesh for the structural analysis. The results are shown below:

Main Index


Figure 2-7

Main Index

Thermal mapping of a turbine blade analysis onto a structural analysis.


Figure 2-8

Thermal model

NASTRAN test deck: tpl/m_physics/map_heat1_m.dat Thermal Boundary conditions: 1. Convection exposed to hot gas at 800 F with h equals to 0.2 Btu/sec-in2*F along the edge of the turbine blade 2. Fix the bottom of base temperature at 70 F

Main Index


Figure 2-9

Main Index

Temperature contour


Figure 2-10

Main Index

Temperature of the blade


Figure 2-11

Thermal mesh

Since the blade exhibits many temperature gradients across the surface, and in order to capture the thermal stress, we will refine the mesh in this region.

Main Index


Here is the refined structure mesh:

Figure 2-12

Refine the mesh for structure analysis

Structure Boundary conditions: 1. Fix at the top surface of the blade 2. Fix the bottom surface of the base The following is the structure material property: MAT1 1 1.2+6 .33 $ Material Record : blade_st $ Description of Material : Date: 02-Apr-10 MAT1 2 2.+6 .33

1.0-6 1.2-6

Time: 13:47:02

Please note that for mesh mapping, there is a parameter for which you can control the interpolation between the coarse and fine mesh. In this case, the default for NLMOPTS, MAPTOL is 0.2. This means that the boxes for the thermal mesh and structure mesh are within 20 percent. In this case, the MAPTOL tolerance is adjusted to 0.5. Then, the interpolating from the coarse thermalmesh temperature is able to map to the fined structure mesh.

Main Index


NLMOPTS,MAPTOL,0.5

Figure 2-13

Main Index

Refined map temperatures


Figure 2-14

Main Index

Map temperature on refined mesh


Figure 2-15

Main Index

Refine mesh (Thermal displacement)


Figure 2-16

Thermal displacement

NASTRAN test deck: tpl/m_physics/map_structure1b_m.dat assign hrun='map_heat1_m.MASTER' dbloc datablk=(heatdb) logi=hrun

NASTRAN system(316)=7 SOL 400 CEND

TITLE = MD Nastran job created on 02-Apr-10 at 13:30:31 ECHO = NONE SUBCASE 2 ANALYSIS=NLSTAT TITLE=This is a default subcase. temp(load,hsub=1)=9 NLPARM = 1 SPC = 2 DISPLACEMENT(SORT1,REAL)=ALL SPCFORCES(SORT1,REAL)=ALL STRESS(SORT1,REAL,VONMISES,BILIN)=ALL nlstress(nlout=12)=all BEGIN BULK nlout,12,tottemp nlmopts,maptol,0.5

Main Index


Please note that using the advance nonlinear elements along with nlstress output that request the tottemp allows the interpolated temperatures to be shown with refined mesh. You can use the param,post,-1 (OP2) file or use NASTRAN SYSTEM(316)=7 (MASTER) file to see the results with SimXpert.

Main Index

Chapter 3: Linear Perturbation Analysis in SOL 400 MD Nastran 2010 Release Guide

3

Linear Perturbation Analysis in SOL 400 

Main Index

Linear Perturbation and Multidisciplinary Linear Analyses in SOL 400

44 MD Nastran 2010 Release Guide Linear Perturbation and Multidisciplinary Linear Analyses in SOL 400

Linear Perturbation and Multidisciplinary Linear Analyses in SOL 400 Introduction Linear perturbation analysis provides the analyst with the ability to perform an analysis based on the nonlinear equilibrium state of a structure. This allows the user to take into account the stress stiffening (or stress softening), large displacement, material nonlinear, and contact effects when performing an analysis. A common example is to perform a normal modes analysis of a structure that changes load path because of contact. Linear perturbation analysis was introduced to MD Nastran R3 but was limited to normal modes, direct and modal complex Eigenvalues, and brake squeal analysis. MD Nastran 2010 extends the linear perturbation capability to include direct frequency response, modal frequency response, and modal transient response. Note that performing a static nonlinear solution followed by a nonlinear transient response has been available since MD Nastran R2 and is referred to as analysis chaining. Therefore, direct transient response is not available for linear perturbation analysis. Multidisciplinary linear analysis will allow multiple linear analysis types to be executed within the same analysis job. For instance, the user might want to run linear static, normal modes, buckling, and modal frequency response in the same run and have a complete set of results for all the disciplines. The multidisciplinary linear analysis is new in MD Nastran 2010 and includes linear static, normal modes, buckling, direct frequency response, modal frequency response, modal transient response, direct complex eigenvalues, modal complex eigenvalues, static aeroelasticity, and flutter analysis types. It is noted that both linear perturbation analysis and multidisciplinary linear analyses can be combined in a single solution. And since these capabilities share similar Case Control, these topics are covered together in this section. Users familiar with the multidisciplinary features of design optimization (SOL 200) will recognize the similarities in the case control for SOL 400. With the same rule as the MD Nastran R3 release on the linear perturbation analyses, a nonlinear static analysis is required to precede a linear perturbation analysis. Linear perturbation analyses are performed in a way as what is called Analysis Chaining.

Benefits The linear perturbation analysis and multidisciplinary linear analysis features are another step in completing MD Nastran, which will ultimately bring together multi-physics, multidisciplinary analyses and design optimizations in a single software platform. Linear perturbations, with response analyses in either frequency or time domain, will further enable the users to perform comprehensive analyses beyond Nastran existing capabilities offered by SOL 1xx sequences, such as SOLs 108, 111, 112, and 106. It allows the finite element analysts to conduct more sophisticate nonlinear analyses with geometric, material and contact nonlinearities prior to the linear perturbation analyses.

Main Index

CHAPTER 3 45 Linear Perturbation Analysis in SOL 400

Linear analyses by SOL 400 will offer the users more flexibility in terms of both modeling and analyses. It also opens the door for the future enhancement in both analysis capabilities and design optimizations in MD Nastran.

Method and Theory of Linear Perturbation Analyses Linear perturbation analyses, in its definition, are performed at an instant of nonlinearly deformed equilibrium state, by linearizing the nonlinear equation of motion. The linearized perturbation equation of motion, is formulated as P P M  u u·· + B  u  u· + K  u P  u = f  t 

where M, B and K are system mass, damping and tangent stiffness matrices, respectively, at a nonlinear static solution state, represented by total nonlinear displacement and applied load vectors, u and P, and a set of history-dependent internal variables,  P , such as plastic strains. Both u and f  t  are perturbed displacement vector and applied perturbation load, respectively. Parameter, t, is either the real time or a time-like variable, starting from t = 0 for the perturbation solutions. Both u· and u·· are the first and second-order derivatives of u , respectively, with respect to time, t. It should be emphasized that load vectors, P and f  t  , are completely independent of each other. In general, the system matrices, M, B and K are nonlinear in nature. In other words, they are dependent on the deformation history and the loading path. The tangent stiffness matrix, K, can be asymmetric. One example is when a friction or follower force is applied on the structure. Their contribution to the structural stiffness is one of the sources that cause its asymmetry. The unsymmetrical stiffness is essential in the study of dynamic instability of structures, such as brake squealing. Standard linear solution procedures can be applied to solve the linear perturbation equation. In the previous MD Nastran release, we implemented the eigenvalue solutions, such as Normal Modes, both Direct and Modal Complex Eigenvalues, with special applications to brake squeal analyses. In MD Nastran 2010, the solutions are further sought in either frequency or real-time domain. For the linearly-perturbed responses in the frequency domain, we have both direct and modal approaches. For the responses in the time domain, the modal approach has been implemented. For all the solutions of linear perturbation analyses, either eigenvalues or responses, the contact constraints are applied at the specified nonlinear loading step or increment, where the linear perturbation analysis is performed. The contact constraints, in the form of MPC equations and handled by the Augmented Lagrange Multiplier Method, are kept unchanged for the linear solutions. In other words, we actually apply the permanent glued contact in the linear perturbation analyses, even though a general contact is involved in the preceding nonlinear solution process. For the linear perturbation with modal transient responses, this is the only sensible approach in case the contact is included in the solutions. For the users who are more interested in the direct transient responses with the general contact, they must resort to the nonlinear transient analysis, offered by SOL 400. The incremental, or perturbed, displacement vector, u , from solving the linear perturbation equation, is measured from the nonlinearly deformed structural configuration. The total displacement vector is

Main Index


u T = u + u where u is the nonlinear displacement vector at specified nonlinear loading step or increment. The element perturbation strains are computed from u based on the linear theory. Element stresses are calculated from the strains on the ground that the constitutive relation is linear. For most of Nastran elements, the material constants can be found in material Bulk Data entries, such as MAT1, MAT2 and so on. The total element stresses are the sum of nonlinear stresses,  NL , and the linear perturbation stresses,  L .  T =  NL +  L Other solution results, such as element forces, SPC and MPC forces, are computed accordingly.

Input Input of Linear Perturbation Analyses A linear perturbation analysis is invoked by the Case Control command ANALYSIS=analysis_type. A nonlinear static analysis is required before performing the linear perturbations. For complicated loading conditions the user must specify which nonlinear initial conditions should be used by the perturbation analysis. In this case the Case Control command NLIC can be used to reference the nonlinear solution at a specific loading step or increment in a preceding STEP with ANALYSIS=NLSTATIC. In MD Nastran R3, the analysis types that were supported for linear perturbation analysis were: • Normal modes analysis (ANALYSIS=MODES) • Direct and Modal Complex Eigenvalues (ANALYSIS=DCEIG, MCEIG) • Brake Squeal Analysis (BSQUEAL)

In MD Nastran 2010, the newly added analysis types for linear perturbation are: • Direct frequency analysis (ANALYSIS=DFREQ)

This is for the linear perturbation Direct Frequency Response Analysis. The normal Case Control commands and Bulk Data entries required by running SOL 108 (SEDFREQ) must be present. • Modal frequency analysis (ANALYSIS=MFREQ)

This is for the linear perturbation Modal Frequency Response Analysis. A Case Control command, METHOD, needs to be specified for the modal approach. Other Case Control commands and Bulk Data entries, required by running SOL 111 or SEMFREQ, must be present. • Modal Transient Analysis (ANALYSIS=MTRAN)

This is for the linear perturbation Modal Transient Response Analysis. A Case Control command, METHOD, needs to be specified for the modal approach. Other Case Control commands and Bulk Data entries, required by running SOL 112 or SEMTRAN, must be present.

Main Index


Input of Regular Linear Analyses A regular linear analysis is introduced by Case Control command, ANALYSIS=analysis_type, in a SUBCASE. Neither STEP - MD Only nor SUBSTEP - MD Only are supported in linear analyses. Each analysis is an independent solution discipline. For linear buckling analysis the Case Control command STATSUB(BUCKLING)=subcaseid must be specified to select the appropriate stress-stiffening SUBCASE. The following ANALYSIS types, supported by SOL 400, are also shared by SOL 200. • ANALYSIS=STATICS, linear statics • ANALYSIS=MODES, normal modes • ANALYSIS=BUCK, buckling analysis • ANALYSIS=DFREQ, direct frequency response • ANALYSIS=MFREQ, modal frequency response • ANALYSIS=MTRAN, modal transient response • ANALYSIS=DCEIG, direct complex Eigenvalues • ANALYSIS=MCEIG, modal complex Eigenvalues • ANALYSIS=SAERO, static aeroelastic response • ANALYSIS=FLUTTER, aerodynamic flutter

Output 1. The output of both linear perturbation and regular linear analyses share the same data formats and data-blocks as their corresponding individual solution sequences, such as SOL 101, 103, 105, 108, 112, and so on. 2. The linear perturbation solutions, such as displacements, stresses, strains, element forces, SPC and MPC forces, are not superposed on their corresponding nonlinear static solutions. 3. Data recovery of a linear perturbation analysis is performed in its current SUBCASE-STEP, while the solutions of a nonlinear analysis are output after all iterations are completed, except for the nonlinear solution PHASE II output. 4. If there are linear, nonlinear and perturbation subcases, the linear subcases will be solved first. The linear subcases are reordered for processing and the output will be in the following order regardless of original subcase number: STATICS, MODES, BUCKLING, DFREQ or MFREQ, MTRAN, DCEIG or MCEIG, SAERO, FLUTTER.

Guidelines and Limitations With more and more capabilities of both multi-physics and multidisciplinary analyses brought into SOL 400, it has recently evolved enormously well beyond its original analysis capacity of nonlinear static and transient analyses. The solution environment, which is set up for nonlinear analyses, may not be suitable for a regular linear analysis. This is particularly obvious when it comes to the default settings of Case Control commands and Nastran system cells. One example is Case Control command,

Main Index


RIGID=elimination_method. In SOL 400, its default is RIGID=LAGRAN, for the Augmented Lagrange

Multiplier method when there are some rigid elements in the model, while in the rest of SOL 1xx sequences, the default is RIGID=LINEAR. Although RIGID=LAGRAN is also supported by some of SOL 1xx sequences, users are less motivated to use it in a linear analysis. Another example is AUTOSPC. In nonlinear analyses, AUTOSPC=YES could be detrimental to the solution procedure, while it is almost universally used in linear analyses. The default setting, AUTOSPC=YES, which is universal for both nonlinear and linear analyses, is the uncharted water that needs more exploration to identify the issues in order to make it more robust and user-friendly in the future. In this MD Nastran 2010 release, it is advised that the user explicitly specify the solution-critical Case Control commands rather than the defaults. This is particularly important when running a job that combines all linear, nonlinear and linear perturbation analyses together. It is also helpful that similar and related analyses are run together in a single job submittal. For example, nonlinear and related linear perturbation analyses are executed in a separate job from other regular linear analyses. The aeroelastic analyses, such as static-aero and flutter, are better put in a job separated from other unrelated analyses, such as a nonlinear transient analysis or a linear perturbation. In doing so, it will cause less confusion in case something goes wrong. The following items have been identified and need special attention: 1. Lagrange rigid elements (Case Control command RIGID=LAGRAN) do not work with residual vectors (Case Control command RESVEC=YES) when either a modal analysis or an modal approach is performed in either a linear perturbation or a regular linear analysis. a. For a linear analysis SUBCASE it is recommended to specify RIGID=LINEAR and RESVEC=YES b. For a linear perturbation STEP with a modal approach (ANALYSIS=MODES, MFREQ, MTRAN, or MCEIG), it is recommended to set RIGID=LAGRAN and RESVEC=NO 2. Lagrange rigid elements (Case Control command RIGID=LAGRAN) do not work well with aeroelastic analyses, such as SAERO and FLUTTER. For linear analysis it is recommended that RIGID=LINEAR be used for SUBCASES with ANALYIS=SAERO or ANALYSIS=FLUTTER. 3. In linear perturbation analyses, all element stresses, strains and forces are not computed for advanced nonlinear elements (PBARN1, PBEMN1, PCOMPLS, PRODN1, PSHEARN, PSHLN1, PSHLN2, and PSLDN1) and MD Nastran nonlinear-only elements, such as hyperelastic elements. 4. In linear analyses, ANALYSIS=DFREQ and ANALYSIS=MFREQ cannot be executed in the same job, even though they are in different SUBCASE. Linear perturbation analyses have no such restriction. 5. Case Control command STATSUB(BUCKLING)=subcaseid is recommended for linear subcases with ANALYSIS=BUCKLE. 6. STATSUB(PRELOAD) is not supported in a linear analysis subcase. 7. Enforced motion (SPCD method) is not supported in either linear or linear perturbation transient, frequency response, or flutter analyses. The large mass method is supported.

Main Index


8. When a superelement analysis is performed the Case Control command ANALYSIS=analyis_type must be defined in each SUBCASE assigned to a specific superelement. 9. The linear perturbation analysis uses the nonlinear deformation as the initial geometry. Therefore, the linear perturbation deflections are relative to the nonlinear deformation associated with the nonlinear initial condition (NLIC). It should be noted that the linear perturbation solutions are not superimposed upon the nonlinear solutions. It should also be noted that PARAM,ADSTAT has no effect in linear perturbation analysis. 10. Inertia relief is supported in linear analysis only (PARAM,INREL).

Examples The following examples are available in the TPL in the following directories • /tpl/perturb400: nlfreq01.dat, nlfreq03.dat, nlfreq05.dat, nlmtra02.dat, nlmultib.dat,

nlmultsa.dat, nlfreq02.dat, nlfreq04a.dat, nlmtra01.dat, nlmultia.dat, nlmultic.dat • /tpl/aero_400: nlcfreqs.dat, nlflut01.dat, nlflut02.dat, nlha200a.dat, nlsaer01.dat

TPL Example nlcfreqs.dat: Linear Perturbation Analysis with both DFREQ and MFREQ Here is an example that shows how non linearities, such as large displacements and contact, work with linear perturbation analyses of frequency responses, in both direct and modal approaches. The structure consists of two cantilever beams of plate elements. Under pressure load on the upper beam, the structure deflects in finite or large displacements with contact, as shown in Figure 3-1. At the end of nonlinear static loading, both direct and modal frequency response analyses are performed as linear perturbations with contact constraints applied in the form of permanent glued contact. The perturbed displacement responses at different excitation frequencies are plotted in Figure 3-2 and Figure 3-3. The excitation forces are applied at the free end of the upper beam. It should be mentioned that the perturbed deflections are plotted on the undeformed structure configuration. It can be seen that the contact constraints are reflected in responses. Both direct and modal solutions match with each other. Input File ID MSC, NLCFREQS $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ STEP 1: NLSTATIC with contact, LGDISP is on $ Two plates contact with sliding. $ STEP 2: Linear perturbation with DFREQ $ STEP 3: Linear perturbation with MFREQ; NLIC at STEP 1 $ Load factor=1.0% $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ SOL 400 $ CEND TITLE=MD Nastran SOL 400, Linear Perturbation Analysis SUBTI=3D General Contact with Large Displacement Turned on $ SUBCASE 1 STEP 1 LABEL=Nonlinear Static Analysis with Contact ANALYSIS = NLSTATIC

Main Index


NLPARM = 1 BCONTACT = 1 BOUTPUT=ALL SPC = 2 LOAD = 3 DISPLACEMENT(SORT1,REAL)=ALL STEP 2 LABEL=Linear Perturbation, DFREQ ANALYSIS = DFREQ DLOAD=200 FREQ =10 AUTOSPC=YES SPC = 2 DISPLACEMENT = ALL STEP 3 LABEL=Linear Perturbation, MFREQ ANALYSIS = MFREQ NLIC STEP 1 LOADFAC 1.0 METHOD = 30 DLOAD=200 FREQ =10 AUTOSPC=YES RESVEC =NO SPC = 2 DISPLACEMENT = ALL $ BEGIN BULK PARAM LGDISP 1 PARAM PRTMAXIM YES NLPARM 1 2 FNT BCTABLE 0 3 SLAVE 3 0. 0. 0. 0. 0 1 0 0 MASTERS 3 SLAVE 3 0. 0. 0. 0. 0 1 0 0 MASTERS 4 SLAVE 4 0. 0. 0. 0. 0 1 0 0 MASTERS 1 BCTABLE 1 3 SLAVE 3 0. 0. 0. 0. 0 1 0 0 MASTERS 3 SLAVE 3 0. 0. 0. 0. 0 1 0 0 MASTERS 4 SLAVE 4 0. 0. 0. 0. 0 1 0 0 MASTERS 4 $ FREQ 10 600.0 1200.0 RLOAD1 200 100 3 TABLED1 3 0. 1. 100. 1. ENDT FORCE 100 101 10.0 FORCE 100 122 20.0 FORCE 100 143 10.0 $ EIGRL 30 200 $ $ Elements and Element Properties for region : left PSHELL 1 1 .1 1 1 $ Pset: "left" will be imported as: "pshell.1" CQUAD4 1 1 1 2 23 22 CQUAD4 2 1 2 3 24 23 . . . $ Elements and Element Properties for region : right PSHELL 2 2 .1 2 2 $ Pset: "right" will be imported as: "pshell.2" CQUAD4 101 2 101 102 123 122 CQUAD4 102 2 102 103 124 123 . . . MAT1 1 6.+7 .3 2.59-4

Main Index

P

-1. -1. -1.

YES


MAT1 2 6.+7 .3 2.59-4 $ Nodes of the Entire Model GRID 1 0. -0.1 0. GRID 2 .5 -0.1 0. GRID 3 1. -0.1 0. GRID 4 1.5 -0.1 0. GRID 5 2. -0.1 0. . . . SPCADD 2 1 3 LOAD 3 1. 1. 2 $ Displacement Constraints of Load Set : fixed-ends SPC1 1 123456 1 22 43 $ Displacement Constraints of Load Set : fixed-ends.1 SPC1 3 123456 121 142 163 $ Deform Body Contact LBC set: left BCBODY 3 3D DEFORM 3 0 BSURF 3 1 2 3 4 5 8 9 10 11 12 13 16 17 18 19 20 21 24 25 26 27 28 29 32 33 34 35 36 37 40 $ Deform Body Contact LBC set: right BCBODY 4 3D DEFORM 4 0 BSURF 4 101 102 103 104 105 108 109 110 111 112 113 116 117 118 119 120 121 124 125 126 127 128 129 132 133 134 135 136 137 140 $ Pressure Loads of Load Set : p-right PLOAD4 2 101 -5. $ Referenced Coordinate Frames CORD2R 1 0. 0. .05 0. 1. 0. .05 ENDDATA $

Figure 3-1

Main Index

6 14 22 30 38

7 15 23 31 39

106 114 122 130 138

107 115 123 131 139

THRU

140

0.

Nonlinear Static Deflection with Contact

1.05


Figure 3-2

Main Index

Displacement Response at Frequency, 0.6KHz


Figure 3-3

Displacement Response at Frequency, 1.2KHz

TPL example nlmultic.dat: Combined Nonlinear Static, Linear Perturbation and Regular Linear Analyses This example shows how we can combine nonlinear, linear perturbation and regular linear analyses together in a single run of job. The model is simple and solutions are trivial. The main purpose is to show the Case Control structure. The linear analyses are executed first. They are followed by the nonlinear static analyses. Linear perturbation analysis is the last. Input File ID MSC, NLMULTIC $ SOL 400 CEND $ TITLE =SOL 400: Multi-discipline Analyses SUBCASE 101 DISP = 10 STRESS = ALL STEP 11 LABEL=Nonlinear Statics, Load 1001 ANALYSIS = NLSTATIC NLPARM = 11 LOAD = 1001 STEP 12 LABEL=Nonlinear Statics, Load 1005 ANALYSIS = NLSTATIC NLPARM = 11 LOAD = 1005

Main Index


STEP 13 LABEL=Linear Perturbation, Modes ANALYSIS = MODES METHOD = 1003 RESVEC = NO AUTOSPC(NOPRINT) = YES DISPL = ALL SUBCASE 1001 LABEL=Linear Static ANALYSIS = STATIC LOAD = 1001 DISP = 10 STRESS = ALL SUBCASE 1002 LABEL=Direct Frequency Response ANALYSIS = DFREQ DISPL(PHASE) = 10 DLOAD = 1002 FREQ = 1002 SUBCASE 1003 LABEL=Modal Transient Response ANALYSIS = MTRAN DISPL = 10 DLOAD = 1003 METHOD = 1003 TSTEP = 1003 OLOAD = ALL SUBCASE 1004 LABEL=Normal Modes ANALYSIS = MODES SVECTOR = ALL METHOD = 1004 SUBCASE 1005 LABEL=Linear Static; 2nd Static Subcase ANALYSIS = STATIC LOAD = 1005 SPC = 1005 DISP = 10 STRESS = ALL SUBCASE 1006 LABEL=Direct Frequency Response; 2nd Direct Subcase ANALYSIS = DFREQ SPC = 1005 AUTOSPC(NOPRINT) = YES DLOAD = 1006 FREQ = 1006 DISPL(PHASE) = 10 STRESS = ALL SUBCASE 1007 LABEL=STATIC for BUCK ANALYSIS = STATIC LOAD = 1007 DISPL = 10 STRESS = ALL SUBCASE 1008 LABEL=Buckling with STATSUB=1007 ANALYSIS = BUCKLING STATSUB = 1007 DISPL = ALL METHOD = 1008 BEGIN BULK $ PARAM, WTMASS, .002588 PARAM, LGDISP, 1 NLPARM 11 FNT 1.0-4 1.0-4 1.0-4 GRID 100 0. 0. 0. GRID 101 2. 0. 0. GRID 102 4. 0. 0. . . . ENDDATA $

Main Index

PWU

YES


TPL example nlha200a.dat: Aeroelastic Analyses in SOL 400 This example is converted from a SOL 200 file. It runs analyses of both SAERO and FLUTTER. Case Control command, RIGID=LINEAR, is put above all SUBCASE's to override the default in SOL 400. The solution results are verified with the ones from SOL 200. Input File ID MSC, NLHA200A $ $$$$$$$$ HANDBOOK FOR AEROELASTIC ANALYSIS EXAMPLE HA200A $$$$$$$$ $ $ $ MODEL DESCRIPTION FULL SPAN 30 DEG FWD SWEPT WING $ $ WITH AILERON, CANARD AND AFT SWEPT $ $ VERTICAL FIN AND RUDDER. $ $ BAR MODEL WITH DUMBBELL MASSES. $ $ $ $ SOLUTION QUASI-STEADY AEROELASTIC ANALYSIS $ $ AND UNSTEADY FLUTTER ANALYSIS USING $ $ DOUBLET-LATTICE METHOD $ $ AERODYNAMICS AT MACH NO. 0.9. $ $ $ $ OUTPUT STANDARD AEROELASTIC OUTPUT PLUS $ $ A TABLE IDENTIFYING RESPONSES $ $ FOR WHICH SENSITIVITY RESULTS ARE $ $ AVAILABLE FOLLOWED BY A MATRIX OF $ $ SENSITIVITY VALUES. $ $ $ $ $ $$$$$$$$ $$$$$$$$

TIME 30 $ CPU TIME IN MINUTES SOL 400 $ MD SOL 400 with AEROELASTICITY CEND TITLE = EXAMPLE HA200A: 30 DEG FWD SWEPT WING WITH CANARD AND SUBTI = DEMONSTRATION OF AEROELASTICITY IN MD(SOL 400) RIGID = LINEAR $ sol 400 default: RIGID=LAGRAN SPC = 1 DISP = ALL $ STRESS = ALL $ FORCE = ALL $ AEROF = ALL $ APRES = ALL $ SUBCASE 1 LABEL = SUBSONIC SYMMETRIC PULLOUT ANALYSIS = SAERO TRIM = 1 $ SUBCASE 2 LABEL = SUPERSONIC SYMMETRIC PULLOUT ANALYSIS = SAERO TRIM = 2 $ SUBCASE 3 LABEL = HIGH SPEED ROLLING PULLOUT ANALYSIS = SAERO TRIM = 3 $ SUBCASE 4 LABEL = HIGH SPEED PULLUP WITH ABRUPT ROLL ANALYSIS = SAERO TRIM = 4 $ SUBCASE 5 LABEL = SUBSONIC ENTRY INTO SNAP ROLL ANALYSIS = SAERO TRIM = 5 $ SUBCASE 6 LABEL = SUBSONIC FLUTTER ANALYSIS ANALYSIS = FLUTTER SET 10 = 1,THRU,100000 PARAM OPPHIPA,1 DISP = 10 STRESS = NONE $ FORCE = NONE $

Main Index

HA200A


AEROF = NONE $ APRES = NONE $ METHOD = 20 FMETHOD = 30 SUBCASE 7 LABEL = SUPERSONIC FLUTTER ANALYSIS ANALYSIS = FLUTTER DISP = NONE $ STRESS = NONE $ FORCE = NONE $ AEROF = NONE $ APRES = NONE $ METHOD = 20 FMETHOD = 40 $ BEGIN BULK $ INCLUDE 'TPLDIR:fswtwo.dat' $ $ * RIGHT WING STRUCTURE * $ $ THE CBAR ENTRY DEFINES A SIMPLE BEAM ELEMENT. LISTED ARE $ ITS PROPERTY ENTRY ID, THE TWO GRID POINTS JOINED BY THE $ BEAM AND COMPONENTS OF A VECTOR FROM THE FIRST POINT. $ THIS VECTOR DEFINES THE DIRECTION OF THE STRUCTURAL DE$ FLECTION OF THE POINT AND ITS POSITIVE SENSE. $ $ EID PID GA GB X1,GO X2 X3 CBAR 110 101 100 110 0. 0. 1. CBAR 120 102 110 120 0. 0. 1. $ $ THE RBAR ENTRY DEFINES A RIGID BAR. LISTED ARE THE GRID $ POINTS AT EACH END AND THE DEPENDENT AND INDEPENDENT DOFS $ AT EACH END. THE NUMBER OF INDEPENDENT DOFS AT THE TWO $ ENDS MUST EQUAL SIX. BY DEFAULT THOSE NOT DECLARED INDE$ PENDENT ARE MADE DEPENDENT. $ $ EID GA GB CNA CNB CMA CMB RBAR 111 110 111 123456 RBAR 112 110 112 123456 RBAR 121 120 121 123456 RBAR 122 120 122 123456 $ $ THE PBAR ENTRY DEFINES GEOMETRIC PROPERTIES OF THE BEAM. $ LISTED ARE ITS ASSOCIATED MATERIAL ENTRY ID, ITS CROSS SEC$ TIONAL AREA, AREA MOMENTS OF INERTIA, TORSIONAL MOMENT $ OF INERTIA AND NON-STRUCTURAL MASS PER UNIT AREA. THE $ OPTIONAL CONTINUATION ENTRY CONTAINS STRESS RECOVERY $ COEFFICIENTS, I.E., Y,Z COORDINATES WHERE STRESSES ARE $ TO BE COMPUTED. K1 AND K2 ARE AREA FACTORS FOR SHEAR $ STIFFNESS (DEFAULT IS BLANK; THEN SHEAR STIFFNESS IS $ INFINITE, I.E., SHEAR FLEXIBILITY IS ZERO. I12 IS THE $ AREA PRODUCT OF INERTIA. $ $ INBOARD WING $ $ PID MID A I1 I2 J NSM PBAR 101 2 1.5 0.173611+2.0 0.462963 $ C1 C2 D1 D2 E1 E2 F1 F2 +PB1W 0.5 3.0 0.5 -3.0 -0.5 3.0 -0.5 -3.0 $ K1 K2 I12 +PB2W 0.0 $ $ OUTBOARD WING $ $ PID MID A I1 I2 J NSM PBAR 102 2 1.5 0.173611+2.0 0.462963 $ C1 C2 D1 D2 E1 E2 F1 F2 +PB3W 0.5 3.0 0.5 -3.0 -0.5 3.0 -0.5 -3.0 $ K1 K2 I12 +PB4W 0.0 $ $ * LEFT WING STRUCTURE * $ $ EID PID GA GB X1,GO X2 X3 CBAR 210 101 100 210 0. 0. 1. CBAR 220 102 210 220 0. 0. 1. $

Main Index

$ $ $ $ $ $ $ $

$ $ $ $ $ $ $

$ $ $ $ $ $ $ $ $ $ $

+PB1W +PB2W

+PB3W +PB4W $ $ $


$ RBAR RBAR RBAR RBAR $ $ $ $ CBAR $ $ PBAR $ +PB1V $ +PB2V $ $ RBAR RBAR . . . ENDDATA

EID 211 212 221 222

GA 210 210 220 220

GB 211 212 221 222

CNA 123456 123456 123456 123456

CNB

CMA

CMB

$ $ $

* FIN STRUCTURE * EID 310

PID 103

GA 100

GB 310

X1,GO 0.

PID 103 C1 0.5 K1

MID 3 C2 3.0 K2

A 1.5 D1 0.5 I12 0.0

I1 I2 0.173611+2.0 D2 E1 -3.0 -0.5

J NSM 0.462963 E2 F1 3.0 -0.5

EID 311 312

GA 310 310

GB 311 312

CNA 123456 123456

CMA

CNB

X2 0.

X3 1.

$ F2 -3.0

+PB1V +PB2V

CMB

TPL Example nlmultsa.dat: Linear Analyses with Superelements This example shows how both STATICS and MFREQ are run with a super-element FE model. It is required that the different analysis types be assigned to the same super-element to complete the analyses. Input File ID MSC, NLMULTSA $ SOL 400 CEND $ TITLE= Super-Elements with Multiple boundary conditions SUBTI= MFREQ and STATICS SET 101 = 99 SET 102 = 1,6,101,301 SET 103 = 111,202,206 DISP = ALL SPCFORCE = 101 STRESS = 102 STRAIN = 102 METHOD = 99 FREQ = 33 $ SUBCASE 1 SUBTI= SUBCASE 1; ANALYSIS=MFREQ LABEL= SUPERELEMENT 1 ANALYSIS = MFREQ SUPER = 1 MPC = 88 MPCFORCE = ALL SUBCASE 2 SUBTI= SUBCASE 2; ANALYSIS=STATICS LABEL= SUPERELEMENT 1 ANALYSIS = STATICS SUPER = 1 MPC = 88 MPCFORCE = ALL DISP = ALL SUBCASE 11 SUBTI= SUBCASE 11; ANALYSIS=MFREQ LABEL= SPC 11; Residual ANALYSIS = MFREQ SPC = 11 DLOAD = 101 SDAMP = 11 SUBCASE 22 SUBTI= SUBCASE 22; ANALYSIS=MFREQ LABEL= SPC 22; Residual

Main Index


ANALYSIS = MFREQ SPC = 22 DLOAD = 202 SDAMP = 22 SUBCASE 33 SUBTI= SUBCASE 33; ANALYSIS=MFREQ LABEL= SPC 11; Residual ANALYSIS = MFREQ SPC = 11 DLOAD = 101 SDAMP = 22 SUBCASE 44 SUBTI= SUBCASE 44; ANALYSIS=STATICS LABEL= SPC 11; Residual ANALYSIS = STATICS SPC = 11 DISP = ALL LOAD = 44 BEGIN BULK PARAM,WTMASS,.00259 PARAM,AUTOSPC,YES FORCE 2 104 100.0 FORCE 2 204 100.0 FORCE 44 111 100.0 FORCE 44 211 100.0 SESET 1 104 204 RLOAD1 101 701 RLOAD1 202 702 DAREA 701 111 3 2000. DAREA 701 211 3 2000. DAREA 702 111 3 4000. DAREA 702 211 3 4000. . . . ENDDATA

0. 0. 0. 0. 31 32

GUI Support SimXpert supports multistep case control.

Main Index

0. 0. 0. 0.

-1. -1. -1. -1.

Chapter 4: Thermal Analysis Extensions in SOL 400 MD Nastran 2010 Release Guide

4

Main Index

Thermal Analysis Extensions in SOL 400 

Outline of New SOL 400 RC Network Solver Capabilities



RC Network Solvers



Advanced Radiation Features



Radiation Collections (Radiation Super Elements) and Primitives



Convection Correlations



Coating and MLI Materials



RC Network Thermal Contact



User-Defined Routines

60 MD Nastran 2010 Release Guide Outline of New SOL 400 RC Network Solver Capabilities

Outline of New SOL 400 RC Network Solver Capabilities The SOL 400 RC Network Solver is a part of MD Nastran 2010. It combines the advanced features of MSC SINDA and some of MSC Patran/Thermal. It has the following unique advanced thermal features: • Advanced Radiation Features

Links to 5 spacecraft thermal REF/orbital heating analysis codes: THERMICA, NEVADA, TSS, TRASYS and SINDARad. The radiation exchange factors (REF’s) and orbital heating will be calculated in these commercial codes and brought back to the RC Network Solver. SINDARad also supports geometry and exchange view factor visualization. • RC Network Solvers

Add 4 steady state solvers and 14 transient solvers for thermal analysis. User can pick adequate thermal solvers for different kinds of models, and compare the results from different solvers. • Radiation Collections (Radiation Super Elements) and Primitives

Support some advanced radiation features, such as “radiation collections” and “Primitives” which are geometric primitives utilizing “true geometric shapes”. The radiation mesh does not have to be congruent with the conduction mesh. • Convection Correlations

Supports the convection correlation library (Materials and Properties/Correlation), allowing users to pick one of 44 industry-standard convection correlations, model internal/ external forced convection and natural convection, and then attach these to a convection load. • Coating and MLI Materials

Supports Coating and MLI materials which can be referenced directly from the loads. These are often used in space thermal analysis. • Advanced Thermal Contact and its Visualization

Supports thermal contact loads based on the projection algorithm, including edge-to-edge, edge- to-surface, and surface-to-surface contact, coupled advection, and gap radiation. The contact pair does not need to have congruent meshing. • User-Defined Routines

Supports user defined routines and C/Fortran logic.

Main Index

CHAPTER 4 61 Thermal Analysis Extensions in SOL 400

RC Network Solvers Introduction Choosing an appropriate steady state or transient solver and good control constant values can be essential for obtaining an accurate RC Network solver thermal solution. FE-based models can become quite large and the solver/control constant selection can have an even more dramatic effect on accuracy and/or runtime. MD Nastran 2010 adds the capability to use 4 steady state solvers and 14 transient solvers for thermal analysis. The user can pick adequate thermal solvers for different kinds of models, and compare the results from different solvers. When running FE-based models, default solvers and control constants are pre-selected, but can always be overridden by the user. Typically, SNSOR is the default steady state solver, and ATSDUF the default for transient. Although these defaults usually suffice, the need to make different choices is not uncommon, most often caused by radiation or some other nonlinearity in the model. The user should never trust the first apparently successful RC Network solver solution for any real-work model. Whether the method was steady state or transient, the solution needs to be verified before the model can be trusted. Several methods are available for verifying the solution. • Obtain nearly identical results with a different numerical method • Obtain nearly identical results with tighter convergence (steady state or transient) • Obtain nearly identical results with a smaller time step (transient) • Obtain nearly identical results with more rays or different random seeds (external radiation

solvers)

Benefits MD Nastran 2010 allows the user to select from 4 steady state and 14 transient RC network solvers so that the most appropriate solver can be used for the specific analysis task.

Input Additional fields have been added to NLSTEP to run the RC Network thermal solvers. In general, iterative solvers are good choices for highly nonlinear models, very large models, and models with 3-dimensional heat conduction. Direct matrix solvers are good choices for linear or mildly nonlinear problems, especially for sparse problems or numerically stiff problems. 1 NLSTEP

Main Index

2

3

ID

TOTTIME

“GENERAL”

MAXITER

4

5

6

MINITER

MAXBIS

CREEP

7

8

9

10

62 MD Nastran 2010 Release Guide RC Network Solvers

“FIXED”

NINC

NO

“ADAPT”

DTINITF

DTMINF

DTMAXF

NDESIR

SFACT

INTOUT

NSMAX

LIMTAR

RSMALL

RBIG

NSMAXA

IDAMP

DAMP

CRITTID

IPHYS

ADJUST

MSTEP

RB

UTOL

“ARCLN”

TYPE

DTINITFA

MINALR

MAXALR

SCALEA

NDESIR

“HEAT”

CONVH

EPSUH

EPSPH

EPSWH

KMETHODH

KSTEPH

MAXQNH

MAXLSH

LSTOLH

CONV

EPSU

EPSP

EPSW

KMETHOD

KSTEP

MRCONV

MAXQN

MAXLS

LSTOL

FSTRESS

BALENG

DAMPC

GRVCON

CSGFAC

“MECH”

“COUP” “RCHEAT”

NLSTEP

HGENPLAS HGENFRIC SOLVER

DRLXCA

ARLXCA

NRLOOP

OUTINV

DTIME1

SNSOR

0.001

0.001

0.0

0.0

9.81

0.0

9.81

1 RCHEAT

5000

Example: NLSTEP

Main Index

1

1000

RCHEAT

SNDUFR

0.001

0.001

0.0

5000

100

10

5

1.0

20

Field

Contents

ID

Identification number. (Integer > 0)

TOTTIM

Total time for the load case. (Real; Default = 1.0)

KSTEP

Number of iterations before the stiffness update for the ITER method. (Integer; Default = 10).

“RCHEAT”

Keyword to indicate that RC Heat Transfer Analysis is to be performed. See Remark 10.

SOLVER

The Relaxation scheme to be used. See Remark 12. (Character; Default = “SNSOR”)

DRLXCA

Diffusion node convergence criterion. See Remark 11. (Real > 0; Default = 1.e-3)

ARLXCA

Arithmetic node convergence criterion. See Remark 11. (Real > 0.0; Default = 1.0e3 degrees)

BALENG

Allowable system energy imbalance. See Remark 11. (Real > 0.0; Default 0.0 energy/time)

DAMPC

Damping constant. (Real > 0.0; Default 0.0 non dimensional)


2

GRVCON

Gravitation constant. (Real > 0.0; Default 9.81 length/time )

CSGFAC

Time step control factor. See Remark 13. (Real > 0.0; Default 1.0 nondimensional)

NRLOOP

Number of relaxation loops allowed. (Integer > 0; Default 5 loop)

OUTINV

Output interval. See Remark 13. (Real > 0.0; Default 60.0 time)

DTIME1

Time step. See Remark 13. (Real > 0.0; Default 0.0 time)

Remarks: 1-9 current QRG description 10. This entry is used for a non-finite element, Resistance-Capacitor network method of analysis for heat transfer. 11. Convergence is determined by the combination of DRLXCA, ARLXCA, and BALENG. DRLXCA and ARLXCA determine if relaxation is met on a node by node basis, rather then a residual vector length. 12. If in Case Control the ANALYSIS=RCNS, then valid values are: SNSOR (Default)

Successive over-relaxation method

SSQMR*

Steady state Quasi Minimal Residual method

SSSPM†

Steady state sparse matrix solver method

STDSTL

An iterative solver aimed at the fourth root of a quartic for the network equations (good for strong radiation dependence).

*These routines (SSQMR, ATSQMR, TRQMR )are based on the QMR (quasi-minimal residual) algorithm developed by Roland Freund and Noel Nachtigal ( © 1992). †These sparse matrix solvers (SSSPM, TRSPM and ATSPM) are based on the Y12M algorithm as described in the following papers Z. Zlatev, J. Wasniewski and K. Schaumburg: "Y12M - solution of large and sparse systems of linear algebraic equations". Springer-Verlag, Berlin-Heidelberg-New York, 1981. O. Østerby and Z. Zlatev: "Direct methods for sparse matrices". Springer-Verlag, BerlinHeidelberg-New York, 1983. Z. Zlatev: "On some pivotal strategies in Gaussian elimination by sparse technique". SIAM Journal on Numerical Analysis, Vol. 17 (1980), 18-30. Z. Zlatev: "Use of iterative refinement in the solution of large and sparse systems". SIAM Journal on Numerical Analysis, Vol. 19 (1982), 381-399. Z. Zlatev: "Computational methods for general sparse matrices". KLUWER Academic Publishers, Dordrecht-Boston-London, 1991.

Main Index


If in Case Control the ANALYSIS=RCNT, then valid values are SNDUFR (Recommended)

An unconditionally stable, explicit method based on a modified DufortFrankel scheme

SNFRDL

Fast, accurate explicit forward differencing transient method

FWDBKL

Implicit forward/backward differencing Crank Nicolson method

SNADE

Alternating direction explicit method

ATSDUF

SNFUFR with automatic time step based on ERRMIN/ERRMAX

ATSFBK

FWDBKL with automatic time step based on ERRMIN/ERRMAX

SNTSM

Weighted implicit forward/backward differencing method

SNTSM3


SNTSM1


SNTSM4


TRSPM

Transient sparse matrix solver method

ATSSPM

TRSPM with automatic time step based on ERRMIN/ERRMAX

TRQMR

Transient Quasi Minimal Residual

ATSQMR

TRQMR with automatic time step based on ERRMIN/ERRMAX

If SOLVER is left blank or set to SNSOR and ANALYSIS=RCNT then internally the RC code will select SNDUFR. 13. About the time step: a. The default computed time step (DTIMEU) = CSGMIN*CSGFAC. CSGMIN is based on the conductance in the model and can be checked in the .sot file. If CSGFAC is not specified, it is internally set to 1.0. b. In a normal sized model, CSGMIN is usually small enough for the time step which will assure a convergent transient run. c. CSGFAC is used to adjust the time step. It is recommended to determine the best CSGFAC to the model while maintaining acceptable temperature errors. d. If OUTPUT < CSGFAC*CSGMIN or OUTPUT < DTIMEI, then OUTPUT becomes the time step. All the OUTPUT points are automatically required to be calculated. e. DTIMEI is the forced time step which will ignore any other factors. Sometimes it may lead to inaccurate answers if it is too large. DTIMEI does not affect the automatic time step solvers. f. If the model size is very small, CSGMIN may be too big for the time step. A small CSGFAC or DTIMEI should be used to adjust the time step. g. CSGFAC*CSGMIN or DTIMEI should be small enough to “catch” any details in time fields, temperature fields or flux arrays.

Main Index


Maintained for legacy, but not shown in GUI: SNSOR1, SNSORA, SNSOR1A, SNHOSD, SNSOSS, SNHOSS, SCROUT, SNDSNR, TRSPMA About non-default solvers: For non-spacecraft, non-radiation problems • Solid type model – SNSOR, SNTSM1 • Very large solid type model – SSQMR, ATSQMR • Very large plate type model – SSSPM, ATSSPM

For spacecraft/radiation models • SNSOR (with user-specified DAMPD if necessary) • FWDBKL if thermo-stats are present • ATSDUF, SNTSM1 for most other cases

Output Output is in the form of temperatures in the f06 file and optionally, temperatures in the XDB or OP2 files.

Test Cases The following test cases are available in the TPL in directory tpl/thermal400. Test Case: QT3_start_a.dat -------- Steady State QT12_start_b.dat -------- Transient Steady state Key cards:

Transient Key cards:

Main Index


Additional Information and References • MSC SINDA User’s Guide • MSC SINDA Tutorial Guide • Sinda for Patran Workshop 1 – Getting Started

Main Index


Advanced Radiation Features Introduction Links to 5 spacecraft thermal REF/orbital heating analysis codes: THERMICA, NEVADA, TSS, TRASYS, and SINDARad. The radiation exchange factors (REF’s) and orbital heating will be calculated in these commercial codes and brought back to the RC Network Solver. SINDARad also supports geometry and exchange view factor visualization. The enclosure radiation loads (small facet, super element, and primitive loads) are transferred into the radiation codes to generate the radiation model. The RC Network translator will create the radiation model which can be displayed in the GUI of the radiation codes. The orbital, pointing, kinematics and mission parameters are defined in the radiation GUI. The radiation codes calculate the view factors and orbital fluxes. The view factors and orbital fluxes can be time dependent. These results are transferred back and mapped with the conduction mesh to create the input file of the RC Network solver.

Benefits Supports space thermal analysis with orbital view factors and orbital heating calculation. User can define different orbit parameters, pointing constraints, and missions. The radiation model built in SimXpert or PATRAN is not dependent on a particular radiation code. If you currently use NEVADA and decide to switch to TSS, or TRASYS, the models will run automatically and not become obsolete. You may also switch to THERMICA which is an add on package that may be purchased from MSC.

Input The VIEWEX Bulk Data entry defines the radiation solver and correlating solver parameters for radiation calculations in RC heat transfer. Note that you must have a copy of the external radiation code to use it. Each entry type is designed for one specific radiation solver, except the very last two types, which are for SINDARad’s two options. Note: SINDARad is not included with the MD Nastran license but can be purchased as an add on package from MSC. Format: (NEVADA)

Main Index

1

2

3

4

5

6

VIEWEX

ICAVITY

Run Interactively

RADK Distro Method

Orbital

Re-use existing results

“NEVADA”

RENO Reflection

Restart

Reno Ray count

Vegas Ray count

GRID iterations

Time Scale

RADK cutoff

7

8

9

Energy Cutoff

Confidence

GRID closure

10

68 MD Nastran 2010 Release Guide Advanced Radiation Features

Example: VIEWEX

2

T

FULL

T

F

NEVADA

T

T

5000

5000

-3

99.

0.001

300

1.0

1.0-8

7

8

9

10

7

8

9

10

Suppress VF Articulation

Radiation ray count

Orbital flux ray count

Format: (TSS) 1

2

3

4

5

6

VIEWEX

ICAVITY

Run Interactively

RADK Distro Method

Orbital


T

FULL

T

F

“TSS”

Example: VIEWEX

3 TSS

Format: (THERMICA) 1

2

3

4

5

6

VIEWEX

ICAVITY

Run Interactively

RADK Distro Method

Orbital


“THERMICA”

Solar Flux

Planet Albedo

Planet BlackBody

Restart

Confidence

Time scale

RADK cutoff

4

T

FULL

T

F

THERMICA

1380.0

0.3

-19.0

T

F

5000

5000

99.0

1.0

1.0-8

7

8

9

Example: VIEWEX

Format: (TRASYS) 1

2

3

4

5

6

VIEWEX

ICAVITY

Run Interactively

RADK Distro Method

Orbital


“TRASYS”

Axi Radial mesh

Axi Axial mesh

Axi Angular mesh

Time scale

5

T

FULL

T

F

TRASYS

1

1

4

1.0

RADK cutoff

Example: VIEWEX

Main Index

1.0-8

10


Format: (SRR) 1

2

3

4

5

6

VIEWEX

ICAVITY

Run Interactively

RADK Distro Method

Orbital


“SRR”

Gebhart Solver

Convergence Tol

Max Iter

Fij smoothing method

Bij smoothing method

Bij Filter cutoff

Bij Smoothing Tol

Bij Max Iter

T

FULL

T

F

7

8

9

Fij Filter cutoff

Fij Smothing Tol

Fij Smooth Iter

1.0-8

1.0-4

50

7

8

9

Filter cutoff

Fij Smoothing Tol

Fij Smooth Iter

.0-8

1.0-4

50

10

Example: VIEWEX

6 SRR

GS

1.0-5

50

CROP

CROP

1.0-8

1.0-4

50

Format: (SRQ) 1

2

3

4

5

6

VIEWEX

ICAVITY

Run Interactively

RADK Distro Method

Orbital


Max Iter

Fij smoothing method

“SRQ”

Flux solver Convergence Tol

10

Example: VIEWEX

7

T

FULL

T

F

SRQ

GS

1.0-5

50

CROP

Field

Contents

ICAVITY

Cavity identification number (Integer > 0; Required)

Run Interactively

Run the radiation code interactively (Character; “T” or “F”, Default “F”) Do not currently have batch mode for Thermica or TSS Do not have interactive mode for TRASYS

RADK Distro Method How to redistribute RADK onto elements. (Character; “FULL”, “AREA”, or “DIRECT”; Default “FULL”)

Main Index

Orbital

Use orbital analysis for radiation (Character,;“T” or “F”; Default “F”) Not supported in SindaRad


Reuse previous radiation results (Character; “T” or “F”; Default “F”)

“NEVADA”

Identification that NEVADA will be used (Character)


Field

Contents

RENO Reflection

Use reflection method of ray tracing for RADK (Character; “T” or “F”; Default “T”)

Restart

Use Restart (Character; “T” or “F”; Default “F”)

Reno Ray count

Number or rays cast for Reno module (Integer > 0; Default 5000)

Vegas Ray count

Number or rays cast for Vegas module (Integer > 0; Default 5000)

Energy Cutoff

Energy cutoff level (Integer; Default -3)

Confidence

Confidence Level % (Real > 0.0; Default 99.0)

GRID closure

GRID closure tolerance (Real > 0.0; Default 0.001)

GRID iterations

Maximum GRID iterations (Integer > 0; Default 300)

Time Scale

Orbital time scale factor, number of time units in an hour. Ex. If using seconds, value would be 3600.0. (Real > 0.0; Default 1.0)

RADK cutoff

RADK filter smallest element (Real > 0.0; Default 1.0e-8)

“TSS”

Identification that TSS will be used (Character)

“THERMICA”

Identification that THERMICA will be used (Character)

Solar Flux

Quantity of solar flux (Real > 0.0; Default 1380.0 W/m2)

Planet Albedo

Planetary Albedo (Real; Default 0.3; assumes Earth orbit)

Planet BlackBody

Planet Blackbody (Real; Default -19.0; assumes Earth orbit)

Restart

Use Restart option (Character, “T” or “F”; Default “F”)

Suppress VF Articulation

Suppress view factor articulation (Character; “T” or “F”; Default “T”)

Radiation ray count

Number or rays cast for radiation calculation (Integer > 0; Default 5000)

Orbital flux ray count Number or rays cast for orbital flux (Integer > 0; Default 5000)

Main Index

Confidence

Confidence Level % (Real > 0.0; Default 99.0)

Time Scale


RADK cutoff


“TRASYS”

Identification that TRASYS will be used (Character)

Axi Radial mesh

Axisymmetric element mesh in radial direction (Integer > 0; Default 1)

Axi Axial mesh

Axisymmetric element mesh in axial direction (Integer > 0; Default 1)

Axi Angular mesh

Axisymmetric element mesh in angular direction (Integer > 0; Default 4)

Time Scale


RADK cutoff


“SRR”

Identification that the SindaRad RADK method will be used (Character)


Field

Contents

Gebhart Solver

Which RADK solver to use (Character; “GS” or “FGS”; Default “GS”)

Convergence Tol

Tolerance for convergence of RADK calculation (Real > 0.0; Default 1.0e-5)

Max Iter

Maximum allowable iterations to converge (Integer > 0; Default 50)

Fij smoothing method How to filter view factors (Character; “CROP” or “HIGH”; Default “CROP”) Fij Filter cutoff

Parameter for filter (Real > 0.0; Default 1.0e-8)

Fij Smoothing Tol

Tolerance for smoothing (Real; Default 1.0e-4)

Fij Smooth Iter

Maximum allowable iterations to smoothing (Integer > 0; Default 50)

Bij smoothing method How to filter conductors (Character; “CROP” or “HIGH”; Default “CROP”) Bij Filter cutoff


Bij Smoothing Tol


Bij Max Iter


“SRQ”

Identification that the SindaRad QRad method will be used (Character)

Flux Solver

Which QRad solver to use (Character, “GS” or “CG”; Default “GS”)

Convergence Tol

Tolerance for convergence of QRad calculation (Real > 0.0; Default 1.0e-5)

Max Iter

Maximum allowable iterations to converge (Integer > 0; Default 50)

Fij smoothing method How to filter view factors (Character, “CROP” or “HIGH”; Default “CROP”) Fij Filter cutoff


Fij Smoothing Tol


Fij Smooth Iter


Remarks: 1. This entry is for RC Network solver only. 2. Each entry type is designed for one specific radiation solver, except the very last two types, which are for SindaRad’s two options. NEVADA TSS THERMICA TRASYS SINDARad RADK method SINDARad Q method 3. For more details about the parameters in the entry, please reference SINDA for Patran User’s Guide and the SINDARad User’s Guide.

Main Index


Output Files containing view factors, radiation exchange factors (REFs), and fluxes from orbital heating.

Test Case The following test cases are available in the TPL in directory tpl/thermal400: Test Case: QT13_satellite_steady.bdf This is a simple satellite model. THERMICA is selected as the radiation code. The orbit can be a round orbit, or composed by a few curves. The pointing of the satellite can be adjusted. The solar panel can point to the Sun while the satellite body points to the Earth. The thermal results (temperature, view factor, and orbital flux) can be displayed along with the satellite orbit.

Product Dependencies User needs a copy of a radiation code. Currently supported are 5 radiation codes, including THERMICA, NEVADA, TSS, TRASYS and SINDARad.

GUI Support SimXpert supports both the pre- and post-processing requirements of the RC thermal network approach in MD Nastran. Patran directly supports the SINDA product or post-processing of the RC thermal network approach in MD Nastran.

Main Index


Additional Information and References • Sinda for Patran Workshop 9 – Satellite and Orbit

Main Index

74 MD Nastran 2010 Release Guide Radiation Collections (Radiation Super Elements) and Primitives

Radiation Collections (Radiation Super Elements) and Primitives Introduction Supports some advanced radiation features, such as “radiation collections”, geometric primitives utilizing “true geometric shapes”. The radiation mesh does not have to be congruent with the conduction mesh.

Benefits Many elements are grouped together and treated as one single element in the radiation code. This greatly reduces the radiation calculation time. The results from the small sized radiation model are distributed back to the real, finer model using advanced algorithms. The primitives are real curved surfaces, instead of flat facets in the radiation models. These can yield higher accuracy, especially in situations where true curved surfaces are required, such as optical mirrors, parabolic antenna, etc. The AB mesh does not have to match the conduction mesh. The speed is dependent on how fine the AB mesh is.

Input A new Bulk Data entry RADCOL is used to define a Radiation Collective Entity (Super Element).RADCOL specifies a collection of element free faces to be used as a single face in the radiation calculation. This will decrease computation time at the small cost of accuracy. Computational savings and accuracy are dependent on the coarseness of the collection versus the constituents. View factors of the collection are redistributed across the elements for calculation of the radiative energy transfer. Format: 1 RADCOL

2

3

4

5

6

7

RADCOLID

IVIEWF

IVIEWB

RADMIDF

RADMIDB

SET3ID

5

6

2

3

7

8

9

10

Example: RADCOL

101

A new Bulk Data entry PRIMx is used to define Thermal Geometric Primitives for RC Radiation (Primitive). PRIMx (where x can be from 1-8) specifies the properties of geometric primitives to be used in radiation calculations in place of elements. PRIM1: Rectangle PRIM2: Quadrilateral PRIM3: Triangle PRIM4: Disc

Main Index


PRIM5: Cylinder PRIM6: Cone PRIM7: Sphere PRIM8: Parabola Format: 1 PRIM1

2

3

4

5

6

7

PRIMID

IVIEWF

IVIEWB

RADMIDF

RADMIDB

SET3ID

P1(1)

P1(2)

P1(3)

P2(1)

P2(2)

P2(3)

P3(1)

P3(2)

P3(3)

A_mesh

B_mesh

11

101

102

3

4

2

0.

0.

0.

1.

0.

0.

0.

1.

0.

3

4

8

9

10

8

9

10

A_mesh

B_mesh

Example: PRIM1

Format: 1 PRIM2

2

3

4

5

6

7

PRIMID

IVIEWF

IVIEWB

RADMIDF

RADMIDB

SET3ID

P1(1)

P1(2)

P1(3)

P2(1)

P2(2)

P2(3)

P3(1)

P3(2)

P3(3)

P4(1)

P4(2)

P4(3)

12

102

103

3

4

2

0.

0.

0.

1.

0.

0.

0.

1.

0.

1.

1.

0.

3

4

8

9

Example: PRIM2

Format: 1 PRIM3

2

3

4

5

6

7

PRIMID

IVIEWF

IVIEWB

RADMIDF

RADMIDB

SET3ID

P1(1)

P1(2)

P1(3)

P2(1)

P2(2)

P2(3)

P3(1)

P3(2)

P3(3)

A_mesh

B_mesh

13

103

104

3

4

2

0.

0.

0.

1.

0.

0.

0.

1.

0.

3

4

Example: PRIM3

Main Index

10


Format: 1 PRIM4

2

3

4

5

6

7

PRIMID

IVIEWF

IVIEWB

RADMIDF

RADMIDB

SET3ID

8

9

10

P1(1)

P1(2)

P1(3)

P2(1)

P2(2)

P2(3)

P3(1)

P3(2)

P3(3)

Diam1

Diam2

Angle1

A_mesh

B_mesh

14

104

105

3

4

2

0.

0.

0.

0.

1.

0.

0.

0.

1.

1.

0.

60.

180.

3

4

2

3

4

5

6

7

8

9

10

PRIMID

IVIEWF

IVIEWB

RADMIDF

RADMIDB

SET3ID

P1(1)

P1(2)

P1(3)

P2(1)

P2(2)

P2(3)

P3(1)

P3(2)

P3(3)

Diam1

Angle1

A_mesh

15

105

106

3

4

2

0.

0.

0.

0.

1.

0.

0.

0.

1.

1.

60.

180.

3

4

8

9

Angle2

Example: PRIM4

Format: 1 PRIM5

B_mesh

Example: PRIM5

Format: 1 PRIM6

2

3

4

5

6

7

PRIMID

IVIEWF

IVIEWB

RADMIDF

RADMIDB

SET3ID

P1(1)

P1(2)

P1(3)

P2(1)

P2(2)

P2(3)

P3(1)

P3(2)

P3(3)

Diam1

Diam2

Angle1

A_mesh

B_mesh

16

106

107

3

4

2

0.

0.

0.

0.

1.

0.

0.

0.

1.

1.

0.

60.

3

4

Angle2

Example: PRIM6

Main Index

80.

10


Format: 1 PRIM7

2

3

4

5

6

7

PRIMID

IVIEWF

IVIEWB

RADMIDF

RADMIDB

SET3ID

8

9

P1(1)

P1(2)

P1(3)

P2(1)

P2(2)

P2(3)

P3(1)

P3(2)

P3(3)

Diam1

Angle1

Angle2

Trunc1

Trunc2

A_mesh

B_mesh

17

107

108

3

4

2

0.

0.

0.

0.

1.

0.

0.

0.

1.

1.

60.

180.

-0.5

0.5

3

4

8

9

Trunc1

Trunc2

1.

0.5

10

Example: PRIM7

Format: 1 PRIM8

2

3

4

5

6

7

PRIMID

IVIEWF

IVIEWB

RADMIDF

RADMIDB

SET3ID

P1(1)

P1(2)

P1(3)

P2(1)

P2(2)

P2(3)

P3(3)

Diam1

Angle1

Angle2

P3(1)

P3(2)

A_mesh

B_mesh

18

108

109

3

4

2

0.

0.

0.

0.

1.

0.

0.

0.

1.

1.

60.

180.

3

4

10

Example: PRIM8

Output The output is in the form of temperatures in the .f06 file. Additionally, Radiation Exchange Factors (REFs) are created from the external radiation program.

Test Cases The following test cases are available in the TPL in directory tpl/thermal400

Main Index


Test Case: QT16_hemi_sph_sf.dat QT33_hemi_sph_se.dat QT32_hemi_sph_pr.dat The example model has a hemisphere and a plate. They are all primitives. The hemisphere and plate radiate to each other, the other sides are radiation insulated. A heat flux 1000 W/ m is applied to the inner side of the hemisphere. A black coating is applied on the surface of both hemisphere and plate.

Radiation Executing Time (s)

Temperature Result (C)

Small facet method

43

-79.7 – 104.8

Super element method

1

-79.7 – 104.6

Primitive method

1

-79.6 – 104.3

$! Primitive Shape $!----------------------------------------------------------------------------!$ PRIM7 3 4 2 2 0.0 0.0 0.0 0.0 0.0 1. 1. 0.0 0.0 1. 0.0 360. -0.5 0.0 1 1

Main Index


GUI Support SimXpert supports Radiation Collections

Known Issues PRIM8 (parabola) is not yet available in SimXpert.

Additional Information and References • MSC SINDA for PATRAN training workshops • MSC SINDA for PATRAN User’s Guide • Sinda for Patran Workshop 7 – Super Element and Primitive

Main Index

80 MD Nastran 2010 Release Guide Convection Correlations

Convection Correlations Introduction Supports convection correlation library (advanced fluid materials), which allows users to pick one of 44 industry-standard convection correlations, model internal/ external forced convection and natural convection, and easily attach this to a convection load.

Benefits • Allows the user to model airflow through avionic packages or electronic equipment, without

using complex and time consuming CFD codes • Allows the user to easily incorporate industry standard convection correlations in a thermal

model. • Allows the user to easily change or modify the fluid material for any convection correlation.

The convection correlation library provides simple forms with graphic depictions of various flows and adds these convection correlations automatically to the Nastran model.

Feature Description The PCONV1 Bulk Data entry is added to define Thermal Convection Calculation Properties. PCONV1 defines the properties required to calculate convective heat transfer. It can exist in a simple mode with the convection coefficient defined in the MID or in advanced mode where the H-value is calculated using the geometric parameters and referenced material. Format: 1 PCONV1

2

3

PID

4

5

6

7

8

9

CorrID

MID

Mdot

Velocity

Length or Diameter

Flow Cross Section

Mdot f

Velocity f

Length or Diameter f

Flow Cross Sec f

Length Flow Cross function type Sec type C1

C2

C3

C4

C5

C6

C7

C8

C9

C10

C11

C12

C13

C14

C15

C16

C17

C18

C19

C20

C21

C22

C23

C24

701

2

10

Example: PCONV1

2

Output Output is in the form of temperatures in the .f06 file and optionally, temperatures in the XDB or OP2 files.

Main Index


Test Cases The following test cases are available in the TPL in directory tpl/subdir. Test Case: QT25_pcb_forced.bdf A convection correlation (507) is used to simulate the forced convection of PCB and chips. The forced convection is applied to both sides of the PCB and outer side of the chips. The inlet air temperature is 20 C°.

Main Index

82 MD Nastran 2010 Release Guide Convection Correlations

PRJCON and SET3 key card

Main Index


GUI Support Patran and SimXpert both support Convection Correlations. Pre-processing is also supported by SimXpert.

Additional Information and References • MSC SINDA for PATRAN User’s Guide • MSC SINDA for PATRAN training workshops • MSC SINDA User’s Guide • Sinda for Patran Workshop 6—Convection and Contact

Main Index

84 MD Nastran 2010 Release Guide Coating and MLI Materials

Coating and MLI Materials Introduction Supports Coating and Multilayered Composite Insulation (MLI) materials that can be referenced directly from the loads. These are often used in space thermal analysis.

Benefits Coating and MLI material options are used for radiation loads only, i.e., they do not influence the thermal conductivity or the specific heat of the material. They cannot be referenced by any properties. Users have the choice to input emissivity or absorptivity directly into the load input form, or they can input coating or MLI materials instead. The advanced coating has parameters for IR, UV specularity, transparency, translucence, and refraction index.

Input New Bulk Data entries COAT, MLI, and RADCT are introduced to define Thermal Radiative Coating Properties and Multi-layer Insulation Properties. COAT defines the radiative properties of advanced materials such as coatings and multilayer insulation, commonly used in the aerospace market. Format: (COAT) 1 RADC

2

3

4

5

6

RADMID

Emis

Absorptivity

IR Spec

UV Spec

7

8

“COAT”

IR Traspa

IR Transluc

IR Refrac Ind

UV Refrac Ind

0.

1.

1.

7

8

UV Transpa UV Transluc

9

10

9

10

Example: RADC

101

1.

1.

0.

COAT

0.

0.

0.

Format: (MLI) 1 RADC

Main Index

2

3

4

5

6

RADMID

Emis

Absorptivity

IR Spec

UV Spec

“MLI”

Estar


Example: RADC

102

1.

MLI

0.02

1.

0.

4

5

RADCT Format: 1 RADCT

2

3

6

7

8

9

10

RADMID Emis f(T) Abs f(T)

Example: RADCT

11

101

102

Output The output is in the form of temperatures in the .f06 file. Additionally Radiation Exchange Factors (REFs) are created from the external radiation program.

Test Cases The following test cases are available in the TPL in directory tpl/subdir. Test Case: QT31_MLI_Coating_orbit.bdf The good example will be a plate with a MLI (or coating) material in the orbital space.

Main Index


α/ε = 0.25 / 0.81

ε* = 0.02

White coating

Reference line: Gamma point Earth Oriented

C Conductors due to element conduction 1, 1, 2, 2, 1, 3, 3, 1, 4, 4, 2, 3, 5, 2, 4, 6, 3, 4,

0.2783333E-01 0.5566667E-01 0.2783333E-01 0.2783333E-01 0.5566667E-01 0.2783333E-01

C Conductors due to MLI node to surface links -7, 1, 6, 0.5000000E-02 -8, 2, 7, 0.5000000E-02 -9, 3, 8, 0.5000000E-02 -10, 4, 9, 0.5000000E-02 C Conductors due to solved radiation loads (THERMICA) -11, 1, 5, -12, 2, 5, -13, 3, 5, -14, 4, 5, -15, 6, 5, -16, 7, 5, -17, 8, 5, -18, 9, 5, END

Main Index

0.2025000 0.2025000 0.2025000 0.2025000 0.2125000 0.2125000 0.2125000 0.2125000

General Ellip. Orbit: (round orbit) Apogee km: 334 Perigee km: 334 Inclination deg: 42.8 Rht.asc.nde deg: 338.9 Sun decl. deg: -9.422


The red curve shows the temperature vs time on the plate. The temperature on the plate is mainly affected by the solar flux. The average temperature of the plate is low because we applied the white coating on the plate which absorbs far fewer solar fluxes. The MLI on the side toward the Earth shields the heat flux from the Earth. We can not use SimXpert Results/Chat to generate the temperature curves for the MLI nodes, because the MLI nodes are added by the translator. These MLI nodes do not really exist in SimXpert. To draw the temperature curves for the MLI nodes, we have to use Thermal Studio, or add some Fortran logic to output a text file, and then draw the curve in Excel, but they are not available within SimXpert. RADC key cards:

GUI Support Patran SimXpert

Main Index


Additional Information and References • MSC SINDA for PATRAN User’s Guide • MSC SINDA for PATRAN training workshops • Sinda for Patran workshop 3 Radiation and Orbital Heating • Sinda for Patran workshop 8 MLI and Honeycomb Panel

Main Index


RC Network Thermal Contact Introduction Supports thermal contact loads based on the projection algorithm, including edge-to edge, edge-tosurface, and surface-to-surface contact, coupled advection, and gap radiation. The contact pair does not have to have congruent meshing.

Benefits Contacts can be created between any two regions. This includes element groups and nodal groups. Advanced materials are used to specify the properties of energy transfer between these groups. The projection method is used instead of the “nearest neighbor method”. The projection method provides higher accuracy.

Input The Thermal RC Element Contact specifies a thermal connection between two regions of elements. The connection is automatically determined geometrically as a projection of the slave region onto the master, and the strength of the connection is calculated based on the properties given. Format: (HEAT1) 1 PRJCON

2

3

4

5

SET3 MASTER

SET3 SLAVE

h

1

2

1.2

3

4

5

SET3 MASTER

SET3 SLAVE

MAT6 ID

1

2

1001

6

7

8

9

10

6

7

8

9

10

BID “HEAT1”

Example: PRJCON

1 HEAT1

Format: (HEAT2) 1 PRJCON

2 BID “HEAT2”

Example: PRJCON

1 HEAT2

Main Index

90 MD Nastran 2010 Release Guide RC Network Thermal Contact

Format: (HEAT3) 1

2

PRJCON

3

4

5

6

7

SET3 MASTER

SET3 SLAVE

F

Emis Master

Emis Slave

1

2

1.

0.85

0.5

3

4

5

6

7

SET3 MASTER

SET3 SLAVE

F

RADC ID Master

RADC ID Slave

1

2

1.

1001

1002

8

9

10

8

9

10

BID “HEAT3”

Example: PRJCON

1 HEAT3

Format: (HEAT4) 1

2

PRJCON

BID “HEAT4”

Example: PRJCON

1 HEAT4

Thermal Contacts Edge-to-edge Edge-to-surface Surface-to-surface

Output Output is in the form of temperatures in the f06 file and optionally, temperatures in the XDB or OP2 files.

Test Cases The following test cases are available in the TPL in directory tpl/subdir. Test Cases: QT10_e2e_contact.bdf QT18_contact.bdf

Main Index


There are many contact examples.

PRJCON key card:


Additional Information and References

Main Index

•

MSC SINDA for PATRAN User’s Guide

•

MSC SINDA for PATRAN training workshops

92 MD Nastran 2010 Release Guide User-Defined Routines

User-Defined Routines Introduction Supports user-defined FORTRAN logics and routines. The EntUDS is a generalized entry point for the solution sequence but has no specific function. Users may construct their own interface through the standard input parameters, then adjust model data accordingly through the interface back to the Solver interface.

Benefits Adds greater flexibility to the RC Network solver, especially for some specific engineering projects.

Input The User Defined Logic at Entry Point calls user-defined logic within a SCA service at the point specified within the solution sequence. Format: 1

2

ENTUDS

3

4

5

6

7

8

9

IDATA6

IDATA7

ENTID

ENTPNT GROUP

“INT”

IDATA1

IDATA2

IDATA3

IDATA4

IDATA5

IDATA8

IDATA9

...

...

IDATAn

“REAL” RDATA1 RDATA2 RDATA3 RDATA4 RDATA5 RDATA6 RDATA7 RDATA8 RDATA9

...

...

RDATAn

“CHAR” CDATA1 CDATA2

...

...

CDATAn

Example: ELEMUDS

1

RCENT1 MY_FUNC

INT

2

17

REAL

.5

.25

Output The output varies according to what function was carried out by the user routine.

Test Cases The following test case files are available in the TPL in directory tpl/subdir.

Main Index

10


Test Case files needed: tut4.bdf; PrintServer.idl; RCEnt.idl; RCSolv.idl; SConopts; SConscript; SConstruct; Tut4Ent.cdl; Tut4Ent.cpp; Tut4Ent.h; Tut4Ent.sdl This model consists of a copper bar with natural convection. The convection is computed by a user defined routine. 2

Circular cross sectional area of 1.0 in 2 2.5fin 5.0 0.5f 1.0 in Boundary Node 1 200°F

Node 2 R1

Node 3 R2

R3

R7

Node 5

Node 4

R8

R4

R9

R10

Boundary Node 7 200°F

Node 6 R5

R6

R11 Convection Conductors

Air Boundary Node 8 75°F

Custom Convection Calculator SCAResult Tut4Ent::RCEnt1(const SCAInt32Sequence& Idata, const SCAReal32Sequence& Rdata, const SCAStringSequence$ Cdata) { // Idata[0] – First ID of conductors to update // Idata[1] – First ID of nodes to get temps for (correlates to conductor) // Idata[2] – # of conductors/nodes from 0 and 1 // Idata[3] – Ambient node ID // Rdata[0] – Cross sectional area of bar // Rdata[1] – Length per bar chunk // Get model data from solver service. DynReal64 T(NULL,0,0); DynReal64 C(NULL,0,0); DynReal64 Q(NULL,0,0); DynReal64 G(NULL,0,0); DynReal64 A(NULL,0,0); DynReal64 K(NULL,0,0); DynReal64 X(NULL,0,0); Solv->Arrays64( T,C,Q,G,A,K,X);

Main Index


// And Calculate…. SCAInt32 idr,ambr; double temp, diam; diam = sqrt( Rdata[0] / 3.14159 ) * 2.0; // Get ambient relative index ambr = Solv-.ActRel( “NR”, Idata[3] ); for( int i=0; iActRel( ”NR”, Idata[1] +i) ); // Find temperature difference to ambient temp = fabs( T[idr] – T[ambr] ) / diam; // Get relative conductor index idr = Solv->ActRel( “NGR”, (IData[0] +1) ); // Calculate the new conductor value G = hA= (0.27*(dT/diam)^0.25)*(pi*diam*len) G[idr] = pow( temp, 0.25) * 0.84823 * diam *RData[1]; } Return SCASuccess; } Nastran Model CONNECT SERVICE MYGN1 'SCA.MDSolver.Obj.Uds.Tut4Ent' SOL400 CEND ANALY= RCNS ECHO= NONE TEMP(INIT)=1 SUBCASE 1 NLSTEP = 77 SPC = 1 THERM = ALL FLUX = ALL BEGIN BULK $-----------------------------------$ Solver parameters $-----------------------------------$234567812345678123456781234567812345678123456781234567812345678 NLSTEP 77 RCHEAT SNSOR PARAM SIGMA 5.67-8 PARAM POST 0 PARAM TABS 0.0 $-----------------------------------$ Nodes $-----------------------------------$234567812345678123456781234567812345678123456781234567812345678 GRID 1 0. 0. 0. GRID 2 .25 0. 0. GRID 3 .75 0. 0. GRID 4 1.25 0. 0. GRID 5 1.75 0. 0. GRID 6 2.25 0. 0. GRID 7 2.5 0. 0. $------------------------------------

Main Index


$ Bar elements $-----------------------------------$234567812345678123456781234567812345678123456781234567812345678 CBAR 1 20 1 2 0. 1. 0. CBAR 2 20 2 3 0. 1. 0. CBAR 3 20 3 4 0. 1. 0. CBAR 4 20 4 5 0. 1. 0. CBAR 5 20 5 6 0. 1. 0. CBAR 6 20 6 7 0. 1. 0. $-----------------------------------$ Bar element Property $-----------------------------------$234567812345678123456781234567812345678123456781234567812345678 PBAR 20 101 6.944-3 $-----------------------------------$ Material $-----------------------------------$234567812345678123456781234567812345678123456781234567812345678 MAT4 101 223. 552.96 0.092 MAT4 102 1.65 $-----------------------------------$ Boundary Elements $-----------------------------------$234567812345678123456781234567812345678123456781234567812345678 CHBDYP 501 30 TUBE 1 2 CHBDYP 502 30 TUBE 2 3 CHBDYP 503 30 TUBE 3 4 CHBDYP 504 30 TUBE 4 5 CHBDYP 505 30 TUBE 5 6 CHBDYP 506 30 TUBE 6 7 $-----------------------------------$ Boundary Element Properties $-----------------------------------$234567812345678123456781234567812345678123456781234567812345678 PHBDY 30 .1477 0.09403 0.09403 $-----------------------------------$ Scalar Points $-----------------------------------$234567812345678123456781234567812345678123456781234567812345678 SPOINT 8 $-----------------------------------$ Temperature loads $-----------------------------------$234567812345678123456781234567812345678123456781234567812345678 SPC 1 1 1 200. SPC 1 7 1 200. SPC 1 8 1 75. TEMPD 1 0. $-----------------------------------$ Convection loads $-----------------------------------$234567812345678123456781234567812345678123456781234567812345678 CONV 501 40 8 CONV 502 40 8 CONV 503 40 8 CONV 504 40 8 CONV 505 40 8 CONV 506 40 8 $-----------------------------------$ Convection properties

Main Index


$-----------------------------------$234567812345678123456781234567812345678123456781234567812345678 PCONV 40 102 $-----------------------------------$ Our super UDS convection solver $-----------------------------------$234567812345678123456781234567812345678123456781234567812345678 ENTUDS 1 RCENT1 MYGN1 $ As created and described in our service: INT 7 2 5 8 $ 1. First ID of conductors to update (This is $ unfortunately a magic number because I already know $ which conductor the convection will end up as $ after RC translation. A better way is $ to use tables because table ID's become equal array $ ID's in Sinda. $ 2. First ID of nodes to get temps for $ 3. # of conductors/nodes from 0 and 1 $ 4. Ambient node ID REAL 6.944-3 .5 $ 1. Cross sectional area of bar $ 2. Length per bar chunk $ $ Service takes temperature difference between bar nodes and ambient $ to calculate conductance of convection conductors $-----------------------------------ENDDATA T E M P E R A T U R E POINT ID. 1 7

Main Index

TYPE S S

V E C T O R ID VALUE 2.000000E+02 2.000000E+02

ID+1 VALUE 1.899454E+02 7.500000E+01

ID+2 VALUE 1.785880E+02

ID+3 VALUE 1.749153E+02

ID+4 VALUE 1.785881E+02

ID+5 VALUE 1.899454E+02


Additional Information and References • MSC P/Thermal User’s Guide • EntUDS.ppt

Main Index


Main Index

Chapter 5: Fluid Structure Interaction in SOL 400 MD Nastran 2010 Release Guide

5

Fluid Structure Interaction in SOL 400 

Main Index

OpenFSI

100 MD Nastran 2010 Release Guide OpenFSI

OpenFSI Introduction The MD OpenFSI interface provides the ability to solve coupled fluid structure interaction (FSI) problems as well as to generally access forces calculated by an external service. MSC Software has partnered with select CFD vendors to provide an interface for fluid structure interaction problems. Users can similarly utilize the published APIs and build environment to create a custom OpenFSI interface. A custom OpenFSI interface can be as simple as a lookup table for forces or as extensive as an interface to an in-house CFD code. This document describes how to utilize an available OpenFSI interface, as well as how users can create their own OpenFSI interface.

Benefits OpenFSI is intended for problems where the boundary conditions cannot be specified simply by a table or field. Instead, OpenFSI boundary conditions must be solved by coupling to an external code or application. A common OpenFSI multidisciplinary application is where the fluid flow affects the structural response and the structural response in turn affects the fluid flow. In such applications the structural model must be coupled to a flow field solution in an external CFD code or user-defined application. This release supports structural applications where MD Nastran provides displacements and velocities on the OpenFSI boundary while the service returns the calculated forces on the wetted surface nodes. Some sample applications in MD Nastran 2010 include:

Main Index

CHAPTER 5 101 Fluid Structure Interaction in SOL 400

• Automotive – Door seal

aspiration, shock absorbers, hydraulic engine mounts, convertible top

• Aerospace – Flexible wings,

Time Domain Flutter, Latch loads

• Energy & Biomed - Wind

Turbines, Flows in blood vessels

For CFD services, the partner has implemented the Open FSI APIs and the service is delivered as part of the CFD software installation. The CFD code should support a model with boundary conditions that can be tagged by the OpenFSI service. A list of current commercially available OpenFSI services from CFD partners can be found on the MSC website: http://www.mscsoftware.com/partners/technology.cfm?Q=434&Z=436. In the case of look-up table services, the user creates a SCA service that complies with the APIs (OpenFSI IDL). The tools for building these custom SCA services are delivered in the MD Nastran solver SDK. An OpenFSI lookup table use case is described in OpenFSI Look-up Table Service for Forces - Example 2, 127.

Feature Description OpenFSI is based on the Simulation Component Architecture (SCA) framework. It allows the MD nonlinear solver to communicate with a CFD code or other external code to access forces computed by the CFD code and send structural displacements and velocities computed by MD Nastran during dynamic simulations. MSC has partnered with several CFD vendors who have agreed to implement the published OpenFSI APIs. These interfaces are delivered in the form of a library and SCA catalog entry that enables the communication. To use a commercial CFD OpenFSI service, you simply point to the location of these SCA services files on the network. You can similarly create OpenFSI interfaces for in-house CFD codes or other application

Main Index


by implementing the OpenFSI APIs with the SCA build environment included in MD Nastran. The SCA service has to be built on the same platform as MD Nastran. However, the implementation can accommodate the flexibility to run MD Nastran and the CFD solutions on a different platform; e.g., one on Windows the other on Linux. This allows OpenFSI simulations where the CFD code may reside on a platform not supported by MD Nastran. For coupling with CFD codes, the OpenFSI approach assumes a pre-existing CFD model with wall boundaries corresponding to the wetted surface of the structural model. The CFD model should be ready to run except for displacement information to be passed by OpenFSI. MD Nastran only needs to be aware of results on the wetted surface nodes. The CFD wall surfaces and the MD Nastran wetted surfaces participating in the FSI solution should have similar geometric form, although their respective meshes will likely be different. In MD Nastran 2010, data interpolation of coupling regions will be performed by the CFD code. MD Nastran obtains the required coupling definition from SimXpert and the CFD solver accesses the structural wetted surface via the API. The CFD coupling region should be collocated and in the same units as the MD Nastran structural model. MD Nastran and the CFD code exchange data on the on the wetted surfaces to account for the viscous and pressure loads, and corresponding displacements during the simulation. The Open FSI process is illustrated in Figure 5-1.

Main Index


Figure 5-1

Schematic of OpenFSI Interface APIs

The OpenFSI service is called from the MD nonlinear solution (SOL 400) at each solution time step or at a user specified iterative frequency. The basic dataflow is illustrated in Figure 5-2.

Main Index


Figure 5-2

Basic Data Flow in OpenFSI Service

The OpenFSI interface communicates the data on so called wetted surfaces, see Figure 5-3, which are the surfaces where the fluid is in contact with the structures. The wetted surfaces are defined in MD Nastran as meshes consisting of triangular and quadrilateral elements. The MD Nastran wetted surface mesh coordinates and elements are sent to the CFD code (or external code) in an OpenFSI initialize call. The matching surfaces in the CFD code can take any form chosen by the CFD vendor, and the mapping between the possibly discrepant wetted surface representations is performed by the CFD code. Note that in this implementation, the mesh topology is constant during the simulation, which means that no mesh adaptivity is supported.

Figure 5-3

Main Index

Example of CFD and MD Nastran wetted surface meshes


Nastran User Interface For a user to run a simulation using the OpenFSI interface, a SCA service must be defined in the file management section in the Nastran input file, which is associated with one ore more wetted surfaces defined in the bulk data section in the input file. The connection between the SCA service and a wetted surface is done by defining a load on the wetted surface, which is tagged with the SCA service name. The load on the wetted surface is specified as a dynamic load in the case control section in the Nastran file, but it must be done using a TLOAD1 Bulk Data entry. To this end, the DLOAD entry in the case control section references a TLOAD1 entry in the Bulk Data Section, which in turn references the load on the wetted surface, defined by the new WETLOAD entry. The entries in the Nastran input file related to the OpenFSI interface are given in Table 5-1, which indicates that five new bulk data entries need to be defined. The structure of the Nastran input file is shown in Table 5-2.

Main Index

Table 5-1

Nastran input file entries

Table 5-2

Nastran input file structure for single wetted load WL1, and a single wetted surface WS1.


The dependency between the entries used for OpenFSI using a single load (with input file structure as Table 5-3) is illustrated in the diagram. Table 5-3 Case Control DLOAD

File Management TLOAD1

WETLOAD

OpenFSI SCA service

FSICTRL

WETSURF

WETELMG

WETELME

If a linear combination of TLOAD1 entries are specified in the DLOAD Bulk Data entry (as in Table 5-3), we have the dependency between the entries used for OpenFSI as follows:

Main Index


Case Control DLOAD

File Management DLOAD

TLOAD1

WETLOAD

OpenFSI SCA service

FSICTRL

WETSURF

WETELMG

WETELME

The definitions of the OpenFSI Bulk Data entries are explained below. The FSICTRL and WETLOAD entries reference SERV ID, an OpenFSI SCA service. If more than one FSICTRL and WETLOAD entries are used, they may reference different OpenFSI SCA interfaces, which is useful if different external codes are used for different sets of wetted surfaces. Two different approaches may be used to define the wetted surface elements: • Using the WETELMG entry, the grid points making up a wetted element are specified; • Using the WETELME entry, a wetted element is defined by referencing a face (or a side) of a

parent structural element. If a shell has wetted surfaces on both faces, separate WETELMG or WETELME are provided on each face. OpenFSI support an implicit or explicit type coupling with the external service. Explicit coupling is the simplest type of service, as the nodal forces from the external code are only read at the beginning of the time step, and the nodal results, the displacement and velocity, are only sent at the end of the time step. The data flow for an explicit service is illustrated in Figure 5-4,

Main Index


.

Figure 5-4

Data Flow for Explicit Coupling

In the implicit service coupling, the data is communicated inside the Newton-Raphson loop at a frequency specified by the FSICTRL entry in the Bulk Data Section. Note that the nodal forces are also read at the beginning of the time step before entering the Newton-Raphson loop (not shown here), in which case the FSI forces do not have to be read at the first iteration. The data flow for an implicit method service coupling is illustrated in Figure 5-5.

Main Index


Figure 5-5

Data Flow for Implicit Coupling

The formats of the Bulk Data entries FSICTRL - MD Only, 1876, WETLOAD, WETSURF, WETELME, and WETELMG to support OpenFSI are described here: FSICTRL 1 FSICTRL

2

3

4

SERV_ID

TYPE

FREQ

EXPLICIT

1

Examples: FSICTRL

Main Index

scafsi

5

6

7

8

9

10


Field

Contents

Type

Default

SERV_ID

OpenFSI SCA service name associated with the wetted surface loads. The OpenFSI SCA service is defined using the CONNECT SERVICE File Management Section statement

Character

None

TYPE

Type of solution strategy coupling between the external Character code and MD Nastran. TYPE can be either EXPLICIT or IMPLICIT.

EXPLICIT

FREQ

External force and displacement update frequency per time step, for the exchange with the external code using the IMPLICIT solution strategy TYPE.

1

Integer > 0

WETLOAD 1

2

3

4

WETLOAD

WLID

WSID

SERV_ID

1

1001

scafsi

5

6

7

8

9

10

Example: WETLOAD

Main Index

Field

Contents

WLID

Load set ID, referenced by the EXCITEID field in the TLOAD entry. (Integer > 0; no Default)

WSID

Wetted surface identification number. The wetted surface must be defined in the WETSURF Bulk Data entry. (Integer > 0; no Default)

SERV_ID

OpenFSI SCA service name associated with the wetted surface loads. The OpenFSI SCA service is defined using the CONNECT SERVICE FMS entry. (Character; no Default)


WETSURF 1 WETSURF

2

3

WSID

WTAG

4

5

6

7

8

9

WEID4

WEID5

WEID6

WEID7

WEID8

WEID2

“BY”

INC

BY

4

82

86

79

WEID1

WEID2

WEID3

WEID9

WEID10

-etc.-

10

Alternate Format: WETSURF

WSID

WTAG

WEID1

“THRU”

Example: WETSURF

10001

wall1

5

THRU

21

27

30

33

35

THRU

44

67

68

70

72

77

89

THRU

110

BY

3

Field

Contents

WSID

Wetted surface identification number. (Integer > 0; no Default)

WTAG

Wetted surface tag name exported to an external code using the OpenFSI SCA interface. (Character; no Default)

WEID1, WEID2, ...

Wetted element identification numbers defined using the WETELMG or WETELME Bulk Data entries. (Integer > 0; no Default)

THRU, BY

Keywords to specify a range of wetted elements. (Character; no Default)

INC

Increment to use with the “THRU” and “BY” keywords. (Integer; Default = 1)

WETELME 1

2

3

4

WETELME

WEID

EID

SIDE

10001

34

3

Example: WETELME

Main Index

5

6

7

8

9

10


Field

Contents

WEID

Wetted element identification number. (Integer > 0; no Default)

EID

Structural element identification number, which corresponds to a surface element CQUAD4, CQUAD8, CQUADR, CQUAD, CTRIA3, CTRIA6, CTRIAR; or a solid element CTETRA, CPENTA, or CHEXA. (Integer > 0; no Default)

SIDE

Side identification number of element EID. (1 < Integer < 6; no Default)

WETELMG 1

2

3

WETELMG

WEID

TYPE

G1

G2

10001

QUAD4

23

35

4

5

6

7

8

9

G3

G4

G5

G6

G7

G8

124

28

10

Example: WETELMG

Field

Contents

WEID

Wetted element identification number. (Integer > 0; no Default)

TYPE

Wetted element type, which can be any of TRIA3, TRAI6, QUAD4, QUAD8, LINE2 or LINE3. (Character; no Default)

G1, ..., G8

Grid point identification numbers for the wetted surface element WEID. (Integer > 0; no Default)

Limitations The following limitations should be noted for MD Nastran 2010: 1. OpenFSI is limited to structural applications, where MD Nastran solves for displacements and velocities on the wetted surface and the service calculates the forces on the wetted surface nodes. The plan is to extend OpenFSI to heat transfer applications in a future release. 2. The wetted surface is limited to triangular or quadrilateral faces of 3D elements or 2D faces. A line surface element is supported but without accounting for moments. 3. Interpolation of dissimilar meshes are performed by the CFD code. A mapping component is planned in a future release. 4. The CFD coupling region should be collocated and in the same units as the MD Nastran structural model. This restriction may be relaxed in a future release.

Main Index


Example Two OpenFSI examples are presented in this section. The first example utilizes a predefined OpenFSI CFD service (AcuSolve from Acusim). MD Nastran and the CFD code are coupled for the transient FSI simulation. The second example involves building a user defined OpenFSI service that calculates nodal forces on the wetted surface nodes based on an expression that is a function of time and node number. Deformable Baffle in a Duct using OpenFSI CFD Partner Service - Example 1

This example illustrates setting up a transient FSI simulation using one of the available OpenFSI CFD partner interface. MD Nastran calculates the baffle deformation and nodal velocities while the CFD code calculates the flow induced loads on the baffle wetted surfaces. The initial condition is a converged CFD solution on the undeformed baffle. The SOL 400 nonlinear transient solution references the connected OpenFSI service. This is transient FSI problem as indicated by the XY-plot. The steps in this analysis follow a typical scenario in industry. The CFD group has created the CFD model ignoring the baffle deformation. The structural analyst has an existing model of the baffle that may have been solved based on the undeformed pressure distribution. The baffle geometry and spatial location are the same in both models. The objective is to get the true baffle behavior based on the fluid structure interaction. This example illustrates the OpenFSI-AcuSolve service from Acusim (the steps should be similar for other CFD partners). The basic steps are: 1. The CFD partner will deliver the OpenFSI service in the form of a library (.dll or .so) and a SCAServiceCatalog (.xml). Make sure that the partner CFD code has been installed and the SCA service environment variables are set to locate the OpenFSI CFD service (SCA_LIBRARY_PATH, SCA_RESOURCE_DIR, SCA_SERVICE_CATALOG). See the User Defined Services guide for more detail on user services. 2. Obtain the ready to run CFD model. The input file may need to be edited to enable FSI coupling. 3. The structural file for this example is included in the vendor example (tentatively named plate_baffle_cfd.dat) 4. The SCA OpenFSI library and service catalog need to be moved under the Nastran installation directory or included in the environmental variables for finding SCA interfaces.

Main Index


5. The user creates a model in SimXpert that references the OpenFSI service for loads on wetted surfaces. 6. The model is submitted to MD Nastran. MD Nastran will use the SCA environment path to locate and load the service. 7. Displacement results appear in the standard MD Nastran output files and are post-processed by SimXpert. The CFD model should be ready to run except for a few input file changes involving the coupling to the structural code. The task for the structural engineer is to determine the deformation and stresses in the baffle. The fluid loads on the wetted surfaces of the baffle are obtained by the CFD solver. The user should obtain the CFD model for the baffle in a duct. A link for the AcuSolve CFD model illustrated below can be found in the MD Demonstration Problems, Chapter 60. The geometry in the CFD model is illustrated in Figure 5-6.

Figure 5-6

CFD Geometry

The CFD model consists of approximately 800K tets. Note the baffle surface in the CFD model is made up of triangular faces while in the structural model the baffle wetted surfaces are quadrilateral. The mapping will be handled by AcuSolve. Flow enters the channel on the left face of the volume. The flow conditions should create sufficient pressure to deform the baffle (~2000 N/m2). The coupling feature has to be enabled in the CFD input file. The following illustrates this step in AcuSolve: EXTERNAL_CODE { communication socket_initiate socket_host socket_port }

= = = =

socket off "name_of_nastran_host" 10000

The specified host is where the MD Nastran model will be running on the network. It can be a different platform than where the CFD code is running (e.g., MD Nastran on Linux, AcuSolve on Windows). The socket host name must include the quotes. The port number (10000) has been set in the AcuSolve service but could be changed if there conflicts through the environment variable “"ACUSIM_NASTRAN_PORT".

Main Index


The set of CFD surface elements corresponding to the baffle structural wetted surface are also identified in the input file. EXTERNAL_CODE_SURFACE( "baffle" ) { surfaces = Read( "baffle.srf.tri" ) shape = three_node_triangle element_seT = "interior" mesh_displacement_type = tied velocity_type = wall gap = 0.0 gap_factor = 0.0 }

Once the CFD part has been prepared, the rest of the OpenFSI problem can be set up through SimXpert. The OpenFSI service is delivered by the CFD vendor and the location of the service should be set as described earlier. Launch SimXpert and Import the Structural Model

Main Index


Define the Service for the Coupled Solution

Note:

Main Index

The form above shows a generic name (myService.openFSI) for the OpenFSI Service name. This will be translated to the Connect Service entry in the MD Nastran input file along with the alias Name (8 characters or less). Check for the actual service in the SCAServiceCatalog.xml as defined by the vendor, for example, 'acuSolveService.openFSI'


Define the OpenFSI LBCs (Wettted Surfaces)

Main Index


Main Index


Define a Nonlinear Simulation

Main Index


Main Index


Main Index


Main Index


Launch MD Nastran OpenFSI-AcuSolve Simulation

Main Index


Main Index


Launch MD Nastran OpenFSI-MpCCI Simulation (for Fluent & StarCD)

Examine the Results Using SimXpert

Main Index


Main Index


OpenFSI Look-up Table Service for Forces - Example 2 In this example, the user wants to reference an external service that provides a time-dependent force over various wetted surface application regions. The left end of the cantilever beam is constrained. The OpenFSI boundaries are applied over the remaining 5 free faces of the beam. The forces returned by the service on the wetted surface nodes are a function of time based on the following formula: force_x = 0.00 force_y = 0.01*sin( 2.0*PI * fsiTime / 2.0 ) force_z = -10.0*cos( 2.0*PI * fsiTime / 2.0 ) where “fsitime” is the transient time in the nonlinear solution. The nonlinear simulation is to determine the transient deformations resulting from the external service load.

Figure 5-7

Cantilever beam with loads referencing an OpenFSI service

The steps in this example are as follows: 1. Make sure that you have installed the MSC_ SDK version consistent with the MD Nastran delivery. The OpenFSI IDL file appears under MD Nastran Installation \sdk\idl\SCA\MDSolver\Util\OpenFSI while the service example for external forces appears under \nast\services\Implementations\OpenFSI subdirectory. The input file that references the service is included under the OpenFSI/model directory. 2. The user defines an external function that complies with the OpenFSI IDL. 3. The service is built using the SCA service tools. 4. The SCA OpenFSI library and service catalog are moved under the Nastran installation directory or included in the environmental variables for finding SCA interfaces.

Main Index


5. The user creates a model in SimXpert that references the OpenFSI service for loads on wetted surfaces. 6. The model is submitted to MD Nastran. MD Nastran will use the SCA environment path to locate and load the service. 7. Displacement results appear in the standard MD Nastran output files and are post-processed by SimXpert. In many situations, the service creation in steps 1 and 2 above will have been done by a commercial vendor (e.g., CFD code) or a methods group in the company. In these cases the user would start with Step 3. The example below will first illustrate the case where the service exists. The second part will illustrate how to create the service. SimXpert Graphical User Interface for this Example SimXpert provides the user interface to create all the required bulk data entries for OpenFSI. A new button has been added in the “Loads” toolbox as shown in Figure 5-8.

Figure 5-8

SimXpert Main Menu OpenFSI load

This brings up the OpenFSI LBC form shown in Figure 5-9.

Main Index


Figure 5-9

SimXpert Open FSI LBC form

SCA Service allows selection from a list of OpenFSI interfaces that have been defined under the User Services menu. Wetted Surface defines the surfaces where loads are to be applied from the OpenFSI external service. The user can select either surface(s) or element face(s) as wetted surface. If the user selects a surface, then all the elements faces lying on the surface will be exported as WETELMG*. Coupling Region Tag Name is passed to the OpenFSI service and usually represent the BC name in the CFD code corresponding to the OpenFSI wetted surface. In the case of a lookup table, this tagname can be used to define an entry point in the service. The default name of the companion region will be given as WS_. Load Scale Factor can be used to scale the loads coming from the OpenFSI service (default is 1.0). This Open FSI object will create the TLOAD1 along with the WETLOAD.

Open FSI Control Parameters The OpenFSI control parameters are defined under User Services. The user service should be selected and control parameters set before applying the OpenFSI load. Open FSI allows two coupling methods. An implicit coincident OpenFSI MD Nastran simulation makes the “get force” and “put displacements and velocities” calls multiple times within the nonlinear (Newton) loop. For implicit coupling, the user can defined a frequency (default is 1). The Explicit coupling method simply couples the solution at each timestep. The Open FSI control parameter UI is shown in Figure 5-10.

Main Index


Figure 5-10

SimXpert OpenFSI Control form

OpenFSI allows pointing to different interfaces for each OpenFSI LBC. Only one FSICTRL entry per service will be exported in the bulk data entry, irrespective of the number of WETLOAD entries. The input file generated by SimXpert for this example is as follows:

Input File: plate.bdf (full file provided separately) connect service CFDFSI 'myopenFSI' $======================================================================= $ Executive Control Section $======================================================================= ID Example OpenFSI SOL NONLIN $ CEND $======================================================================= $ Case Control Section $======================================================================= TITLE = FSI plate SUBTITLE = OpenFSI example $ECHO = NONE $ DISPLACEMENT=ALL GPFORCE=ALL $ PARAM,POST,0 $ SUBCASE 1 STEP 1 ANALYSIS = NLTRAN DLOAD = 100 $ NLPARM = 1 TSTEPNL = 1 $ BEGIN BULK $ $---------------------------------------------------------------------$ Parameter for newton raphson (static) $NLPARM ID NINC DT KMETHOD KSTEP MAXITER CONV INTOUT $ 1 10 AUTO 25 UPW YES $ EPSU EPSP EPSW MAXDIV MAXQN MAXLS FSTRESS LSTOL

Main Index


$ 0.01 0.01 0.01 3 0 4 0.2 0.5 $ MAXBIS MAXR RTOLB MINITER $ 5 20.0 20.0 1 $-------$-------$-------$-------$-------$-------$-------$-------$------NLPARM 1 3 .1 FNT U .1 0 $---------------------------------------------------------------------$ Parameter for newton raphson (transient) $TSTEPNL ID NDT DT NO METHOD KSTEP MAXITER CONV $ $ EPSU EPSP EPSW MAXDIV MAXQN MAXLS FSTRESS ------$ $ MAXBIS ADJUST MSTEP RB MAXR UTOL RTOLB MINITER $ TSTEPNL 1 20 0.10 1 FNT 25 U $---------------------------------------------------------------------$ Material $-------$-------$-------$-------$-------$-------$-------$-------$------MAT1 1 2.1+11 .33 7.0 PSOLID 1 1 $-------$-------$-------$-------$-------$-------$-------$-------$------GRID 1 0.00000 0.00000-0.01000 12345 GRID 2 0.01000 0.00000-0.01000 <<<< deleted for clarity >>> GRID CHEXA CHEXA

3333 1 1214 2 1215

1 1213 1 1214

1.00000 0.10000 0.01000 1 2 103

102

1112

1113

2

3

104

103

1113

1114

2120

2121

2222

2221

3231

3232

103

102

104

103

<<<< deleted for clarity >>> CHEXA WETELMG WETELMG

2000 3333 1 1 2 2

1 3332 QUAD4 2 QUAD4 3

<<<< deleted for clarity >>> WETELMG

2420 QUAD4 2221 2222 3333 3332 $-+-+-+-$-+-+-+-$-+-+-+-$-+-+-+-$-+-+-+-$-+-+-+-$-+-+-+-$-+-+-+-$-+-+-+-$-+-+-+WETSURF 1 wall1 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16 <<<< deleted for clarity >>> WETSURF

993 2 1001 1009

994 wall2 1002 1010

995

996

997

998

999

1000

1003 1011

1004 1012

1005 1013

1006 1014

1007 1015

1008 1016

1995

1996

1997

1998

1999

2000

2003 2011 2019

2004 2012 2020

2005 2013

2006 2014

2007 2015

2008 2016

2023 2031

2024 2032

2025 2033

2026 2034

2027 2035

2028 2036

2215

2216

2217

2218

2219

2220

2223 2231

2224 2232

2225 2233

2226 2234

2227 2235

2228 2236

<<<< deleted for clarity >>> WETSURF

WETSURF

1993 3 2001 2009 2017 4 2021 2029

1994 wall3 2002 2010 2018 wall4 2022 2030

<<<< deleted for clarity >>> WETSURF

2213 5 2221 2229

2214 wall5 2222 2230

<<<< deleted for clarity >>>

Main Index


2413 2414 2415 2416 2417 2418 2419 2420 $-+-+-+-$-+-+-+-$-+-+-+-$-+-+-+-$-+-+-+-$-+-+-+-$-+-+-+-$-+-+-+-$-+-+-+-$-+-+-+FSICTRL CFDFSI EXPLICIT 1 WETLOAD 101 1 CFDFSI WETLOAD 102 2 CFDFSI WETLOAD 103 3 CFDFSI WETLOAD 104 4 CFDFSI WETLOAD 105 5 CFDFSI $-+-+-+-$-+-+-+-$-+-+-+-$-+-+-+-$-+-+-+-$-+-+-+-$-+-+-+-$-+-+-+-$-+-+-+-$-+-+-+DLOAD 100 1.0 1.0 101 1.0 102 1.0 103 1.0 104 1.0 105 TLOAD1 101 101 10 TLOAD1 102 102 10 TLOAD1 103 103 10 TLOAD1 104 104 10 TLOAD1 105 105 10 TABLED1 10 0.0 1.0 10000.0 1.0 ENDT $-+-+-+-$-+-+-+-$-+-+-+-$-+-+-+-$-+-+-+-$-+-+-+-$-+-+-+-$-+-+-+-$-+-+-+-$-+-+-+-

User Defined OpenFSI External Service The above input file Connect Service entry references an external OpenFSI service called 'myService.openFSI' The desired service will return forces returned on the wetted surface nodes are a function of time based on the following formula: force_x = 0.00 force_y = 0.01*sin( 2.0*PI * fsiTime / 2.0 ) force_z = -10.0*cos( 2.0*PI * fsiTime / 2.0 ) This example OpenFSI service along with the source structure is included in the delivery. See the OpenFSI.idl file for the details of the interface, and openFsi.cpp for the implementation example. The following methods are implemented in an OpenFSI service: • For the initialization stage: • initialize • For the solver stage: • initializeTimeStep • getWettedNodeForces • putWettedNodeDisplacementsAndVelocities • finalizeTimeStep • For the termination stage: • terminate

The abbreviated source for this user-defined service is given below (OpenFSI.cpp file).

Main Index


To make the build, just execute • scons

in the OpenFSI root directory. This will generate an Apps directory containing the library (dll or so) and the SCA service catalog. If the service has been built in a directory not in the default path, the user will have to set the following environment variables (Windows example shown).

Main Index


• SCA_LIBRARY_PATH /Apps/WINNT/bin/ (/lib on Linux and Unix) • SCA_SERVICE_CATALOG

/Apps/res/SCAServiceCatalog.xml • SCA_RESOURCE_DIR /Apps/res/

For a detailed description of how to build a SCA service, see the MD Nastran 2010 User Supplied Subroutines and SCA Service Guide.

Product Dependencies A CFD interface requires an OpenFSI enabled CFD code. These are either commercial codes that have implemented the OpenFSI APIs or in-house codes that have created custom interfaces. In MD Nastran 2010, SimXpert provides the graphical user interface for defining the structural wetted surface application regions and selecting the OpenFSI service. For CFD OpenFSI interfaces, the CFD model and coupling boundary are defined in the CFD pre-processor. In the case of the OpenFSI-UVLM (Unsteady Vortex Lattice Method) service from Zona Technologies, the aero model is included in the Nastran input file.

Documentation Dependencies User defined OpenFSI interfaces are created using the SCA build environment delivered with MD Nastran. For more information on creating SCA interfaces see the following documents: • MD Nastran 2010 - SCA Service Guide • MD Nastran 2010 - User Defined Services

Main Index

Chapter 6: Advanced Nonlinear (SOL 400)

6

Main Index

MD Nastran R3 Release Guide

Advanced Nonlinear (SOL 400) 

Offsets for Beams and Shells



Segment-to-Segment Contact



Automated Bolt Modeling



Load Stepping Robustness



Additional Output Control with NLOPRM SOL 400



Nonlinear Solution Statistics (STS) File



Large Displacement Grid Point Weight Generation (GPWG)



User Subroutines



User Defined Module Service UDMSRV

136 MD Nastran 2010 Release Guide Offsets for Beams and Shells

Offsets for Beams and Shells Introduction The original design of the BAR, BEAM and shells included an offset feature. This feature allows you to specify a BAR/BEAM axis of shear centers offset from connected grid points; and, a shell element reference plane offset from the connected grids for triangular and quadrilateral shell elements. The axis of the elastic BAR/BEAM was assumed to extend from the two endpoints offset from the connected grid points; and, the reference surface of the shell element connected points offset from the connected grids. The elastic stiffness was then calculated in the offset element coordinate system and transformed to the connected grid points using the rigid body transformation equations.

Figure 6-1

CBAR and CBEAM Element Offset Definitions

Figure 6-2

CQUAD4 and CQUAD8 Element Coordinate System Definitions

Prior to the offset project in MD Nastran 2010, element offsets had the following limitations: • The differential stiffness is not supported. Therefore, they are not applicable in solution sequence

where differential stiffness is required, such as linear buckling analysis (SOL 105). • The effect of offsets is not included the mass matrix. • The effect of offset is not included in computation of thermal loads, pressure loads, or gravity

loads.

Main Index

CHAPTER 6 137 Advanced Nonlinear (SOL 400)

• For curved shell problems, the offset is defined in the z direction of the element and not the shell

normal direction, this results in gaps between elements when offset geometry is applied. • The transformation is linear and therefore, it cannot be used in nonlinear analysis.

This enhancement extends the use of offsets to nonlinear solutions, linear differential stiffness, load and mass generation and maintenance of geometric continuity for adjacent curved shells along the common shell normal.

Benefit The enhanced offset method has the following benefits: • DIFFERENTIAL STIFFNESS - The differential stiffness is computed for the offset so that it

is applicable to solution sequences that required differential stiffness. These include, for example, SOL 103, SOL 105, and SOL 400. • MASS - The effect of offset is included in the mass matrix generation. • LOADS - The effect of offset is included in the load generation. • GEOMETRY COMPATIBILITY - For QUAD4, TRIA3, QUADR, TRIAR, QUAD8 and

TRIA6 elements the shell normal is used as the offset direction. Thus, the new offset will enhance solution of a model in two aspects: there is no gap in the offset geometry, and the mass and stiffness matrices are computed based on the offset geometry. Figures New Offset Behavior when Angle between adjacent elements is less than SNORM and New Offset Behavior when Angle between adjacent elements is greater than SNORM demonstrate how the new offsets are considered in conjunction with SNORM. • NONLINEAR EFFECTS - The transformations are nonlinear so that it can be used in

nonlinear analysis such as SOL 400.

Feature Description Differential Stiffness The original offset method does not compute the differential stiffness for offset. Therefore, it is not applicable to solution sequences where differential stiffness is needed such as SOL 103 or SOL 105. The enhanced offset computes the differential stiffness for offset, using the same formulation as that of the Lagrange RBAR element. The Lagrange multipliers are eliminated internally. For the new offset method, the differential stiffness is computed for offsets for solution sequences that require it. These include SOL 105, SOL 400 and any linear solution that supports differential stiffness effects via the case control entry STATSUB. Mass Matrix For an element, the mass matrix is computed at the offset locations of the element. The mass matrix needs to be transformed from the offset locations to the external grid points. In performing this transformation, mass moments of inertial are created. Without this transformation, the mass matrix for model with offsets

Main Index


is only an approximation. With this transformation, the mass matrix for SOL 103, and other dynamic solution sequences are correctly computed. The additional terms in the mass matrix may adversely affect the solution time for dynamic solutions. Therefore, a provision to disable the mass offset calculation while retaining other offset effects is available. Load Effects Element loads, such as thermal, pressure, and gravity load, are computed at the offset locations of the element. These loads are then transformed from the offset locations to the external grid points. For thermal load, there are two types of effect due to offset: • The location of thermal load is changed due to offset, i.e. the thermal load is first computed at the

element offset locations and then transformed to the external grid points. This effect is computed for both linear solution sequences and nonlinear solution sequence SOL 400. • The temperature load will change the length of the offset. This effect is computed for the

nonlinear solution sequence SOL 400 only. If you don’t want these effects to be calculated, a provision to disable the offset load effects is available. Offset Direction For beam elements, the direction of offset is given by the WiA and WiB on the connection Bulk Data entries. For shell elements, the old offset direction is in z-direction of the element coordinate system. For curved shell model, such as cylindrical shell, this approach has two deficiencies: • The offset geometry has gap or overlap in the structure model. • The computations of stiffness matrix, mass matrix, and element load are based on the original

geometry, which is not the same as the offset geometry. In order to remedy these deficiencies, the new offset method for QUAD4, TRIA3, QUADR, TRIAR, QUAD8, and TRIA6 use the shell normal as the offset direction for default. If you don’t want the geometric advantages of the new offset method, a provision to revert to the previous offset behavior for shell elements is available.

Figure 6-3

Main Index

Unique Grid Point Normal for Adjacent Shell Elements


Figure 6-4

New Offset Behavior when Angle between adjacent elements is less than SNORM

Figure 6-5

New Offset Behavior when Angle between adjacent elements is greater than SNORM

Nonlinear Analysis For nonlinear analysis, the following are implemented for the new offset method: • The offsets are formulated based upon large rotation theory. • The differential stiffness for offsets is computed. • For thermal loads, the length of the offsets may change due to thermal loads. This effect has

been implemented.

Input The new offset formulation must be invoked by specifying the MDLPRM,OFFDEF ,option in the Bulk Data Section. The format of the MDLPRM entry and options associated with OFFDEF are shown.

Main Index


MDLPRM Format: 1

2

3

4

5

6

7

8

MDLPRM

PARAM1

VAL1

PARAM2

VAL2

PARAM3

VAL3

-etc.-

QR6ROT

2

QRSHEAR

1

OFFDEFF

LROFF

9

10

Example: MDLPRM

Name OFFDEF

Main Index

Description, Type, and Default Values Element offset definition. A flag to determine how shell elements and bar and beam elements behave when the user supplies ZOFF values on the shell connection entries (CQUAD4, CQUADR, CTRIA3, CTRIAR, CQUAD8, and CTRIA6) and WiA and WiB on CBAR, CBEAM, and CBEAM3 connection entries. (Character)

ELMOFF

Standard Nastran offset method. The ZOFF rotate with the shell element. The WiA and WiB offsets for beams are fixed. MD Nastran R3 and earlier. (Character, Default)

LROFF

Large rotation offsets. The shell normal directions are used to define the offset direction at each shell grid. This method allows for thermal load effects on ZOFF for shells and WiA and WiB for beams. Thermal load effect for offset is computed based on the grid point or element temperature, and thermal coefficient of the element (see NOTHRM). The mass moment of inertia is computed for the offset due to the grid point location change introduced by offset. Differential stiffness is computed for the offset using the same method as that of the Lagrange formulation of the RBAR. (Character)

NODIF

LROFF is used but the differential stiffness effect is turned off. (Character)

NOTHRM

LROFF is used but the thermal load effects are turned off. The thermal load has two effects: 1) the location of thermal load changes due to offset and 2) the length of offset changes due to thermal load. Effect (1) is computed for all solution sequences and Effect (2) is computed for MD Nastran SOL 400 only. Both effects are turned off by NOTHRM. (Character)

NODT

LROFF is used but the differential stiffness and thermal load effect are turned off. (Character)

ELMZ

LROFF is used but the element z-direction is used for the offset direction. IF PARAM, SNORM, 0.0 or the computed value for SNORM is greater then the PARAM,SNORM,value, then the LROFF option will revert to this method for CQUAD4, CTRIA3, CQUADR, and CTRIAR. (Character)


Name

Description, Type, and Default Values NOMASS

LROFF is used but the no mass effects are included. (Character)

NDMTZ

LROFF is used but the element z-direction is used for the offset direction and the differential stiffness, the thermal load effects, and the mass effects are turned off. For CQUAD4 and CTRIA3 elements this method should get similar results to the standard ELMOFF method. (Character)

Notes:

This entry only effects ZOFF calculations for ZOFF specified on the shell connection entries. For ZOFF specified on the PCOMP or PCOMPG entries, the standard ELMOFF method will be used. For CBEAM, CBAR, CQUAD8 and CTRIA6 elements, the LROFF option will revert to the ELMZ sub option.

If the computed value for SNORM is greater then the PARAM,SNORM,value and the user wishes not to change the parameter value, the Bulk Data entry SNORM can be used to override the shell normal. Solution sequences affected: For linear - all solution sequences. For MD Nastran - SOL 400 nonlinear only. The new method is not implemented into SOL 106 and 129. Note that there is no Case Control modification or other modifications to the input file required. By default, the old offset definition is used (MDLPRM,OFFDEF,ELMOFF)

Output There is no new output associated with the new offset methodology.

Guidelines and Limitations Solution Sequences and Element Type to be Supported by Offset Solution sequences and element types supported by the new offset method are: • All linear solution sequences that use differential stiffness such as SOL 103, 105 and dynamic

solution sequences support the new offset method. • For nonlinear solution sequences, only SOL 400 is supported. SOL 106 and SOL 129 use the old

offset method. • For linear solution sequences, the new offset method supports the following elements: QUAD4,

TRIA3, QUADR, TRIAR, BEAM, BAR, BEAM3, QUAD8, and TRIA6. • For SOL 400, the new offset supports QUAD4, TRIA3, QUADR, TRIAR, and BEAM. • For advanced nonlinear elements in SOL 400, in addition to QUAD4, TRIA3, QUADR, TRIAR

and BEAM elements, QUAD8, TRIA6 and AXISYM are also supported.

Main Index


For QUAD4 and TRIA3, the stiffness for drilling DOF’s is zero. The offset is not completely constrained by the elements. For the linear solution sequences, this will not create any problem. For nonlinear analysis, this will not impede the solution of QUAD4/TRIA3 for most cases. However, for certain type of models, especially if the model is completely flat, the zero stiffness will make the solution with offset difficult to converge in SOL 400. If this happens, a large value K6ROT, in the order of 1,000.0 - 10,000.0, may be used to resolve this problem. Another work around is to use the QUADR/TRIAR elements. The new offset method has not been implemented for composites using the PCOMP or PCOMPG Bulk Data entries. For these entries, the user needs to transfer the offset definition to the connection entries in order to use the new offset method.

Test Problems The following test cases are available in the TPL in directory /tpl/offsetmeth: TPL Example ofsl014.dat This example is a simple cantilever with offsets, model by QUAD4 and TRIA3 to obtain solution in the linear buckling analysis (SOL 105). There are two types of element in the file. The first subcase is preload. The second subcase is for QUAD4 and the third subcase is for TRIA3. Both loading and geometry are exaggerated to show the differential effect of offset. Bulk data input required for new offsets: “MDLPRM, OFFDEF, LROFF” The first buckling factor for both QUAD4 and TRIA3 are 1.52 with differential stiffness of offset. However, if we ignore the differential stiffness of offset (OFFDEF=NODIFF), the first buckling factor is 6087.

Figure 6-6

TPL example problem ofsl014.dat

TPL Example ofslq416.dat This example is a cylindrical shell to demonstrate the effect of shell normal using linear static analysis SOL 101. Bulk data input required for new offsets: “MDLPRM, OFFDEF, LROFF”. In this example, both elastic element stiffness and mass matrix are computed based on the offset geometry of the model. Since the shell normal is used as the direction of the offset, there is no gap in the geometry. For this model, the weight for shell normal model (OFFSET=LROFF) is 120.8, while for the z-direction model (OFFSET=ELMZ) the weight = 109.8. Results are obtained from grid point weight table. The

Main Index


displacement at T1 of grid 1 is 0.1095. However, if we use offset in z-direction (OFFDEF=ELMZ), then the corresponding displacement is 0.0996.

Figure 6-7

TPL example problem ofslq416.dat

TPL Problem ofsnbm01.dat This example is for the nonlinear solution of SOL 400. A simple cantilever beam is modeled by BEAM with offset. Bulk data input required for new offsets: “MDLPRM, OFFDEF, LROFF”. Both geometry and loads are exaggerated to show effects of offset and geometric nonlinear. In this model, the large rotation theory and differential stiffness are computed for the offsets of beam. This model is verified by explicitly modeling the offset by RBAR element. Both offset and RBAR give the same results.

Figure 6-8

TPL example problem ofsnbm01.dat

GUI Support Patran Currently Patran does not support the definition of MDLPRM,OFFDEF,offdef. However, it is expected that this will be supported in Patran 2008r3.

Main Index


SimXpert SimXpert supports the definition of MDLPRM,OFFDEF,option. Figure 6-9 shows the GUI interface.

Figure 6-9

Main Index

SimXpert Support for MDLPRM,OFFDEF,option


Segment-to-Segment Contact Introduction The automated contact algorithm introduced in a previous version of MD Nastran is based on grid points or nodes being in contact with a segment (a curve, surface, element edge, or element face), and can thus be called a node-to-segment algorithm. This contact algorithm has matured and has been successfully applied to a large variety of contact problems. However, there are a few weaknesses of this algorithm especially for deformable contact, which call for the development of an alternative contact algorithm: • When contact has been detected, the non-penetration constraint is enforced on a grid point basis.

Because of this point-wise application of constraints, the node-to-segment algorithm does not generally maintain stress continuity across the contact interface of deformable contact bodies (this can be easily illustrated using the contact patch test, where a uniform stress distribution should be obtained in two deformable contact bodies with dissimilar meshes). • Since the non-penetration constraints are enforced using multi-point constraint equations, there

is a potential dependency of the solution on the selection of the master and the slave nodes. In other words, the solution depends on which grid points are touching and which grid points correspond to a touched contact segment. Although there are various options to optimize the multi-point constraint equations, it is not always possible to achieve the best results everywhere in the model and to completely eliminate the dependency on the contact body numbering. • If there would be contact detected at the top and the bottom face of a shell element, it is not

possible to only use the grid points of the shell element to apply both multi-point constraint equations. This implies that there are limited modeling options for so-called double sided shell contact. A similar problem occurs when the edge of a shell element is in contact with the face of another element. If this happens, then the contact constraints are based on either the shell top or the shell bottom face. Consequently, the “footprint” of the shell edge is not directly related to the shell thickness. In MD Nastran 2010, a new contact algorithm has been introduced based on a segment-to-segment algorithm, where the non-penetration constraints are enforced using augmented Lagrangians.

Benefits The easy way to define contact bodies in the node-to-segment algorithm is maintained in the segmentto-segment algorithm, while the difficulties of finding the optimal contact body numbering and getting the correct constraints in case of shell contact are avoided.

Feature Description Instead of using automatically generated multi-point constraint equations to enforce the contact constraints in a point-wise manner, the segment-to-segment contact algorithm tries to enforce the contact constraints on the common area of contacting bodies. The methodology used is that of augmented Lagrangians, which can be seen as a combination of a penalty method and a Lagrange multiplier method.

Main Index

146 MD Nastran 2010 Release Guide Segment-to-Segment Contact

In contrast to a Lagrange multiplier method, there are no extra degrees of freedom in the system of equations to be solved, but there may be extra iterations needed to improve the fulfillment of the contact constraints. An important parameter in the algorithm is the augmented Lagrange penalty factor. Typically, a too high value of this factor can cause an ill-conditioned stiffness matrix, where a too small value can cause a relatively large penetration after the first iteration in the Newton-Raphson process and many iterations to remove this penetration. The default value of the penalty factor is determined by the program, but the BCPARA and BCTABLE options allow the user to overrule the default value. The default value of the penalty factor E n depends on the body stiffness of the two contact bodies involved and a characteristic length (note that the dimension of the penalty factor is force per cubic length). The body stiffness is either defined by the average trace of the initial stress-strain law of the elements defining the two contact bodies or by the average bulk modulus for (nearly) incompressible rubber materials, whichever of the two is the largest. For continuum elements, the characteristic length is given by one half of the average length of all the edges being part of the contact boundary. For shell elements, the characteristic length is given by half of the average thickness of all the shell elements being part of a contact body. When there is contact between a solid and a shell element, then the characteristic length is defined by the shell element. If there is contact between the deformable bodies k and l , with body stiffnesses S k and S l , and the characteristic length of the model is L , then the default value of E n is given by: 0.5  S k + S l  E n = ----------------------------L In case of contact with a rigid body, the default value of E n is related to the deformable body k only and is given by: 1000S E n = -----------------k L Since the contact constraints are generally fulfilled in an iterative fashion, a threshold value of the penetration distance is needed to decide whether or not the augmentation procedure will be invoked. Like the penalty factor discussed above, this penetration distance beyond which an augmentation is applied has a default value determined by the program. but can also be user-defined via the BCPARA and BCBODY options. The default value is based on the characteristic length L according to:  a u g = 0.001L As for the augmentation procedure, the following options are available: • No augmentation. This results in a pure penalty method and is recommended for most analyses,

since it gives reasonably accurate results in a relatively small number of iterations. • Augmentation based on a constant penetration field. This is the recommended augmentation

procedure for linear finite elements. • Augmentation based on a (bi-)linear penetration field. This augmentation procedure should be

used only for quadratic finite elements.

Main Index


It is also possible to let the program decide on the use of a constant or (bi-)linear penetration field, based on the element types involved (linear or quadratic).

Guidelines and Limitations Currently, the segment-to-segment algorithm has the following limitations: • Mechanical contact only; no thermal or coupled contact; • Small sliding for deformable-deformable contact (large sliding is allowed for deformable-rigid

contact); • No friction (glued contact is allowed).

The default contact algorithm is still the node-to-segment algorithm. If one has to solve a contact problem which does not go beyond the just mentioned limitations and typical drawbacks of the node-tosegment algorithm play a role, then the segment-to-segment algorithm should be invoked with preferably default settings (no augmentation and default penalty stiffness).

GUI Support The segment-to-segment algorithm is supported by SimXpert. The menu to select this method and to eventually overwrite the default parameters is shown below.

Main Index


Test case As an example of the segment-to-segment algorithm (see TPL problem ns2sc69), a clamped cantilever beam with a tip load is analyzed. The beam is partly modeled with continuum elements and partly with shell elements (see the figure below). The material properties of both parts are given by Young’s modulus F

h2

h1 L1

L2

7

E = 1 10 and Poisson's ratio  = 0.3 . The length of the two parts is the same: L 1 = L 2 = 5 and the out of plane thickness for both parts is t = 1 . Two analyses will be performed, one where h 1 = h 2 = 1 and one where h 1 = 1 and h 2 = 0.5 . The total tip load is given by F = 1 , which is applied using point loads. The solid part is meshed using quadratic tetrahedral elements, the shell part is meshed using linear quadrilateral elements.

Main Index


According to elementary beam theory, the tip deflection for the two cases can be calculated as: –4

w ti p  h 1 = h 2 = 1  = 4 10

w ti p  h 1 = 1 ;h 2 = 0.5  = 7.75 10

–4

In the finite element analysis, two deformable contact bodies are defined, one consisting of the solid elements and one consisting of the shell elements. They will be joined together using glued contact. The segment-to-segment contact algorithm is selected on the BCPARA option: BCPARA

0

METHOD

SEGSMALLNLGLUE

1

It should be noted that, unlike the node-to-segment algorithm, there is no need to specify moment carrying glue on the BCTABLE option. Instead, when there is contact with shell elements, the segmentto-segment algorithm always generates constraints in which the rotational degrees of freedom are involved. This implies that on the BCTABLE option IGLUE = 1 is equivalent to IGLUE = 3 and, similarly, IGLUE = 2 is equivalent to IGLUE = 4. The default value of the augmented Lagrange penalty factor is used. The calculated displacement fields are shown below. It can be seen that the tip displacements are in very good agreement with the theoretical solution.

Main Index


h1 = h2 = 1

h 1 = 1 ;h 2 = 0.5

Main Index


Automated Bolt Modeling Introduction Bolt preload is a critical design consideration for detailed joint analysis in all industries. One of the critical factors for a proper joint analysis is to capture the bolt preload effects properly. The bolt spacing, preload, and general joint design will affect items like gasket pressure, o-ring seal behavior, and gapping analysis for instance. In the automotive industry, bolt modeling is important in analyses of engine assemblies. Gasket joints, which are used in such assemblies to prevent steam or gas from escaping, are often fastened by a number of bolts. In a typical loading sequence of an engine assembly, the bolts are first fastened until a certain pre-tension force is present in the bolts. This can be achieved by shortening the bolts until the desired force is reached. Next, the bolts are “locked”, that is, the amount of shortening remains fixed, while the assembly is subject to other (thermo-)mechanical loads. Finally, the bolts are loosened again, either by decreasing the shortening or by releasing the bolt forces. MD Nastran has had automatic bolt modeling available in SOL 600 with the MBOLT and MBOLTUS entries. MD Nastran 2010 improves the MBOLT and MBOLTUS formulations and offers the new BOLT formulation in SOL 400.

Benefits The new bolt formulation will benefit users who are performing detailed joint analysis that require preload and contact. Applications are many in automotive, machinery, aerospace, and other industries that have critical joints. Although existing MPCs can be used to pre-stress bolts, the required split of the structure (bolt) causes limitations when used in a contact analysis. The new BOLT option is formulated so that there are no issues with contact at the split.

Feature Description Historical Methods In MD Nastran R3, the bolt loading sequence can be simulated by splitting the finite element mesh of the bolt along element boundaries into two disjoint parts (see Figure 6-11). The grid points on the bottom side of the split are connected with user-defined multipoint constraints to the corresponding grids on the top side and a “control grid point”. The latter is shared by all multi-point constraints of the bolt. The multipoint constraints are defined via the MPC Bulk Data option in such a way that an overlap of the two mesh parts (hence a shortening of the bolt) can be created by prescribing the displacements of the control grid point via SPC(D) Bulk Data options. Moreover, the total force in the bolt can be prescribed via FORCE bulk data options on the control grid point.

Main Index

152 MD Nastran 2010 Release Guide Automated Bolt Modeling

This method works well, but is difficult to use in combination with contact for two reasons: 1. Due to the mesh split, the internally generated contact surface of the bolt is no longer continuous and also consists of two disjoint parts. Grid points which touch the bolt surface and slide across the split will first have to separate from the bottom part, say, and will then have to be found in contact again with the top part before they can continue; and 2. The slave grid points in the user-defined multipoint constraints are fully constrained by the multipoint constraints, so contact of these grids, for example with the bolt hole, has to be avoided. New Implementation In MD Nastran 2010 a new Bulk Data entry for BOLT has specially designed for bolt modeling in SOL 400. Assuming that the finite element mesh of the bolt has been split up in two disjoint parts along element boundaries across the shaft of the bolt, the new option will impose the proper multipoint constraints on these parts, such that the bolt can be prestressed, locked and loosened by applying appropriate boundary conditions to a special “control grid point” associated with the bolt. Special treatment of the constraints by the contact algorithm will ensure that the option can be used with contact and that the internally generated contact surface will be continuous across the split. Grids touching the bolt surface can then slide across the split without problems. The automated bolt modeling method is based on a mesh split principle and a control node. Figure 6-10 demonstrates how the mesh split principle is applied to a typical joint.

Figure 6-10

Main Index

Example of a Bolted Joint using BOLT using the Mesh Split Principle


The key to the new BOLT formulation is the concept of the control node.

Figure 6-11

Control Node and “Top Nodes” / “Bottom Nodes” Definition

The user defines the “Top Nodes” (GT) and the “Bottom Nodes” (GB) and the control node (GC). MD Nastran generates internal MPC equations that satisfy the equation: • u GB = u GT + u G C • u : Displacement of the nodes in the bolt direction n • GT’s: Independent nodes (N-set; Master) • GB’s: Dependent nodes (M-set; Slave) • GC: Control node (N-set; Master)

Main Index


The Mesh Split Principle Figure 6-12 will be used to derive the equations used in the mesh split principle. :

Figure 6-12

MPC equations generated by the Mesh Split Principle

1. Let: u=  u 1 bot u 2 bot u 1 top u 2 top  T and u =  u 1 top u 2 top u control  T 2. Constraint matrix:

T =

1 0 1 0 0 1 0 1 1 1 0 0

T

3. Constraint imposed by MPCs: u = Tuˆ 4. Force vectors work-conjugate to u and u : T T F=  F 1 bot F 2 bot F 1 top F 2 top  and Fˆ =  Fˆ 1 top Fˆ 2 top Fˆ control 

5. Principle of zero work for MPCs: ˆ F T u – F T uˆ

Main Index


T 6. It follows that: T F = Fˆ (3+5) or:

F 1 bot + F 1 top = Fˆ 1 top , F 2 bot + F 2 top = Fˆ 2 top , F 1 bot + F 2 bot = Fˆ 1 control . In the non-mechanical parts of a coupled analysis, the constraint will guarantee continuity of the primary field variables across the split mesh (for example: temperatures). Therefore, the control node is not required and it will be ignored. The MPC relationship for non-mechanical parts becomes:  G Bi =  GT i

BOLT

Defines the Multi-Point Constraints for a Bolt

Defines a rigid bolt by a set of MPC constraints. Format: 1

2

3

BOLT

ID

GRIDC

TOP BOTTOM

4

5

6

7

8

9

GT1

GT2

GT3

GT4

GT5

GT6

GT7

GT8

GT9

etc.

GB1

GB2

GB3

GB4

GB5

GB6

GB7

GB8

GB9

etc.

10

Example: BOLT

Main Index

100

1025

TOP

101

102

103

104

105

BOTTOM

1

2

3

4

5

Field

Contents

ID

Element ID of the bolt. (Integer; Required; no Default)

GRIDC

Control GRID ID where forces or displacements are applied. (Integer; no Default; Required)


Field

Contents

TOP

Enter the character string TOP to define the start of the entry that defines all of the grids at the “top” of the bolt intersection with the structure. (Integer; no Default)

GT1, GT2, etc.

Grid IDs of the grid points at the top of the bolt intersection. (Integer; no Default)

BOTTOM

Enter the character string BOTTOM to define the start of the entry that defines all of the grids at the “bottom” of the bolt intersection with the structure (do not enter the ID for GRIDC). (Integer; no Default)

GB1, GB2, etc.

Grid IDs of the grid points at the bottom of the bolt intersection. (Integer; no Default)

Remarks: 1. The GRIDS entries of the TOP and BOTTOM keywords are open-ended. 2. GRIDC is the control grid point and usually not connected to any element. 3. (GTi, GBi) are pairs of grid on top and bottom. 4. To each pair of (GTi, GBi) and GRIDC, MPCs are created internally to all 6 DOFs. Since the GBs always belong to dependent-DOFs, they cannot be applied to any SPC, SPC1, SPCD and SPCR. 5. Same number of grid points in TOP and BOTTOM. They should be coincident but it is not required. Users who do otherwise do so at their own risk since the current design does not consider the initial offset between them. 6. Bolt loads, including enforced motion, are usually prescribed on GRIDC to represent the pretension, overlap or loading of the bolt. BOLT relative displacements are given in the global coordinate system of the control node. 7. Global Coordinate System may have to be defined at the Control Node if the bolt direction is not a Basic Coordinate direction and the user wants to apply the loads along the shaft of the bolt. 8. Loads in directions other than the shaft of the bolt direction are possible. 9. The internally written MPC relationship is of the form: uG B = uG T + uG C 10. In 3D Contact analysis, it replaces GBi (Bottom bolt segment) by GTi (Top bolt segment) on the internally generated contact surface, which makes contact surface continuous across the mesh split between them. 11. Force output is obtained through Case Control MPCFORCE.

Test Cases The following test cases are available in the TPL in directory /tpl/solid_101:

Main Index


TPL Examples simple_solid.dat and simple_solid2.dat The following example demonstrates how to create a BOLT for a 3-D model using two different methods in SimXpert. The cross-sectional area of the BOLT is 1.0 area units, a preload force of 5000 load units. The boundary conditions are chosen such that Poisson’s effect will not add additional stresses to the model. The resulting SimXpert test case are are available as simple_solidn.dat and simple_solid2n.dat. SimXpert Automatic Method Steps for creating an “automatic” BOLT with a 5000 unit preload Force in SimXpert. 1. In the SimXpert Assemble tab, select the “Create 3D Bolt” icon to access the “3D Bolt Model” form 2. Set the Axial Preload Type to “Force” and enter a Value of 5000. 3. Set the “Method” to “Automatic”. 4. Select the Part and press OK to complete the operation. SimXpert will automatically detect the “long” direction of the Part and split the mesh at the center. A new coordinate system will be created so that the “Z” is aligned with the long direction. SimXpert automatically splits the mesh and creates duplicate nodes at the center of the part. The control node is set above the part and the BOLT is graphically displayed with lines connecting the control node to the split plane. When the model is run, the stresses are a constant 5000 as expected. The figures below demonstrate the steps in SimXpert.

Figure 6-13

Main Index

Creating BOLT in SimXpert using the automatic method - step 1


Figure 6-14

Creating BOLT in SimXpert using the automatic method - step 2-3

Figure 6-15

Creating BOLT in SimXpert using the automatic method - step 4 and results

SimXpert Assisted Method Steps for creating an “assisted” BOLT with a 5000 unit preload Force in SimXpert. Preliminaries: 1. Create a local coordinate system at the “split plane” location. Note that “Z” direction of the local coordinate system must be aligned with the axial direction of the BOLT because SimXpert will create the “split plane” in the XY plane of the local coordinate system. In this example the “Z” direction of coordinate system 1 is used as the axial direction. 2. Create a Control Node anywhere in space - it is common to create this node near the split plane

Main Index


Proceed to set up the bolt using the following steps: 1. In the SimXpert Assemble tab, select the “Create 3D Bolt” icon to access the “3D Bolt Model” form 2. Set the Axial Preload Type to “Force” and enter a Value of 5000. 3. Set the “Method” to “Assisted”. 4. Select the Control Node, Splitting Plane (coordinate system) and Part. 5. Press OK to complete the operation. SimXpert will automatically split the nodes closest to the XY plane of the splitting plane coordinate system. When the model is run, the stresses are a constant 5000 as expected. The figures below demonstrate the steps in SimXpert.

Main Index


Figure 6-16

Main Index

Creating BOLT in SimXpert using the assisted method


TPL Example Gasket Assembly Based on MDUG Problem nug_10.dat The following example is based on the MD User Guide Example problem 10. Example problem nug_10.dat is modified to use the MD Nastran 2010 BOLT entry. In this case, the control node has a local coordinate system aligned with the Y direction. The preload is defined by a bolt shortening of 0.175” which is defined using an enforced displacement on an SPCD Bulk Data entry.

Main Index

Figure 6-17

MD Demonstration Problem example nug_10.dat geometry

Figure 6-18

MD Demonstration Problem example nug_10.dat BOLT entry (file nug_10_bolt.dat with BOLT)


Figure 6-19

MD Demonstration Problem example nug_10_bolt.dat Stress from BOLT preload.

GUI Support Patran Patran supports the MBOLTUS option. The Patran interface will appear similar to the following form:

SimXpert The SimXpert GUI support is covered in detail in the Test Cases Section.

Main Index


Load Stepping Robustness Introduction In MD Nastran 2010 the load stepping procedure has been improved by introducing a new NLSTEP option which replaces the existing NLPARM, TSTEPNL, NLPCI, and NLADAPT options. The new time stepping scheme has the following features: 1. Unified format of bulk data for step control: NLSTEP bulk data card is introduced to define the time step control for both single and multi-physics jobs. 2. NLSTEP is the only supported time stepping scheme for multi-physics. The time step is synchronized between the substeps. Generated output for each substep also corresponds to this synchronized time. 3. All results are provided in terms of “TIME” with NLSTEP rather than “LOAD FACTOR”.

Benefits Nonlinear statics jobs are more apt to run better while also being more robust. More options will also be available to control the adaptive load stepping, i.e., user specified criteria. Having a single option for the load case settings will make it easier both for people writing pre-processors and for susers that edit the input file.

Feature Description The development on the time stepping schemes is applicable to both single physics and coupled analysis: • The new bulk data option NLSTEP is provided as a unified load stepping scheme that replaces

existing options like NLPARM, TSTEPNL, NLPCI, and NLADAPT. This option can be used for statics and dynamics, fixed and adaptive load stepping, definition of convergence criteria and other options for mechanical and thermal and the definition of creep. Apart from the improved load stepping for statics, the options in NLSTEP are mapping to the same data as previously obtained from NLPARM and TSTEPNL. This is only a change in input format with the program performance being the same. The improved load stepping basically implements the algorithms already used in MSC Marc. The basic algorithm works with a user input “desired number of recycles”. The time step is increased for the upcoming increment if the current increment uses fewer recycles than desired. If the number of recycles during an increment exceeds the desired number a time step cutback (bisection) is performed and the time step is reduced. If the increment is converging the time step decrease is postponed until the next increment. Special care is taken for contact when changes in contact occurs, like new contact, sliding or separation. A distinction is made between Newton-Raphson iterations and Contact-Induced iterations - only the former is used for controlling the time step changes. Without this the time step would often be reduced excessively.

Main Index

164 MD Nastran 2010 Release Guide Load Stepping Robustness

In addition to this algorithm there is also a scheme based upon artificial damping in a static analysis. Estimations of strain energy changes are used for applying artificial damping for unstable situations (with sudden reductions of strain energy). These estimates are also used for modifying the time step. This algorithm may be restricted to the advanced elements in the first release. For adaptive stepping, user-defined criteria for controlling the time step are also available. The user criteria ID is specified through the CRITTID field on the “ADAPT” keyword of the NLSTEP entry and this in turn refers to a TABSCTL Bulk Data entry where the actual criteria is specified. The user can set a limit on the incremental displacements, rotations, stresses, temperature, etc. If a criterion would be violated, a bisection and time step reduction is done. The user criteria thus work as limits. There is also an option to treat the criteria as targets, in which case the time step for the next increment will be increased in order to reach the specific displacement increment for instance. The time step is never increased during an increment. • The restriction of using virtual time of 1.0 for static analysis has been removed. Earlier, real-time

was only supported for transient analysis. The real-time feature is supported by simply specifying the total time for the step TOTTIME on the NLSTEP entry.

Guidelines and Limitations The following guidelines for the new load stepping scheme should be noted: 1. The default tolerance for mechanical is 10% relative testing on the residual force vector components (CONV = PV). For some applications, it may be beneficial to have more iterations in the solution by checking on the incremental displacement vector also (CONV = UPV). The default iteration scheme followed is Full Newton-Raphson (KMETHOD = PFNT). 2. The default tolerance for thermal is 1% relative testing on displacements, residuals and energy (CONV = UPW). The default iteration scheme followed is Modified Newton-Raphson with Automatic Stiffness Update (KMETHOD = AUTO). The following limitations for the new load stepping scheme should be noted: 1. NLSTEP is not supported for the CREEP material option. It is only supported for elements using MATVP. CREEP should still be specified through NLPARM with DT > 0.0. 2. NLSTEP with ARCLN does not support contact. This is also an existing limitation of the arclength scheme specified through NLPCI. 3. Quasi-static damping (IDAMP) specified on the ADAPT keyword of NLSTEP is only available for enhanced elements that use property extensions. Automated element defaults automatically map all possible elements to the enhanced ones in conjunction with IDAMP.

Main Index


GUI Support SimXpert 2010 supports Load Stepping Robustness..

Test Cases Test cases and GUI support are described in Coupled Thermal-Mechanical Implementation (Ch. 2).

Main Index

166 MD Nastran 2010 Release Guide Additional Output Control with NLOPRM SOL 400

Additional Output Control with NLOPRM SOL 400 Introduction There are several minor enhancements which are made for MD Nastran users to better control, monitor and understand the outcome of a nonlinear analysis. A new Case Control command, NLOPRM, bundles various existing and new nonlinear solution debugging and output functionalities together in a single command.

Benefits Case Control command, NLOPRM, can be used to better control the nonlinear solution output during solution process, to provide MD Nastran users a direct access to nonlinear solutions even while the job is still running, to give the users some tools to monitor and debug the nonlinear solution process and gain some insight of nonlinear solution procedure and also to allow users to print out MPC and MPCY equations from contact constraints before and during a contact process.

Input Format NLOPRM =  OUTCTRL =  STD,SOLUTION,INTERM    NONE     N3DBAS    NLDBG =     NLBASIC,NRDBG,ADVDBG,  N3DMED       N3DADV    NONE    LTIME   NONE      DBGPOST =  LSTEP   MPCPCH =  BEGN,OTIME,STEP       LSUBC   TBEGN,YOTIME,YSTEP   ALL  Examples NLOPRM NLOPRM

Main Index

OUTCTRL=STD,SOLUTION DBGPOST=LTIME OUTCTRL=(SOLUTION,INTERM), MPCPCH=(OTIME,STEP)


Output The output from Case Control command, NLOPRM, is basically controlled by four keywords of OUTCTRL, NLDBG, DBGPOST and MPCPCH. Each keyword has a group of descriptors that are assigned to either by one at a time or more in juxtaposition. The output is destined to almost all Nastran output media, such as F06, PCH, OP2 and DBALL, depending on which keyword is used.

Guidelines 1. Case Control command, NLOPRM, may only appear above all SUBCASE, STEP and SUBSTEP delimiters. 2. For OUTCTRL=SOLUTION, only nonlinear solutions, such as nonlinear stresses, strains, contact status and so on, are output at the user-specified output intervals. Any solution results in super-elements are not computed and recovered in what we called Phase 3 data recovery. The job is terminated as soon as all nonlinear iterations are completed. The nonlinear solution results are also saved in DBALL when a job is launched with scratch=post. They are ready for post-processing when the job is completed. 3. When OUTCTRL=INTERM is specified, the nonlinear solutions, such as stresses, strains, contact status and so on, are output into individual OP2 files for post-processing at the userspecified output intervals. The user is able to access these files while the job is still running. The name of a typical OP2 file is the job name followed by a suffix name of eight-digit number, for instance, my_job.00000008. In an F06 file, the relevant information of an OP2 file is indicated as corresponding to the load or time increment, STEP, SUBSTEP, and SUBCASE. 4. NLDBG is intended for those sophisticated SOL 400 users, who want to look into the details of nonlinear iterations. The data printed out in the F06 file is in its raw form and some effort is required to interpret its meanings. Among the debugging options, N3DBAS can be used to print out some basic contact information in the F06 file. It includes the contact condition of touching node on the touched patch and separation contact forces. Standard contact status output can be requested by Case Control command, BOUTPUT. 5. DBGPOST is used to select the output of nonlinear iterations for debugging purpose. When DBGPOST is activated, a Nastran data block, OFDBGDT, is created to store both residual and displacement vectors at user-specified iterations pertaining to load or time increments, STEP and SUBCASE. 6. MPCPCH allows the user to punch out multipoint constraint equations from a contact process in the format of either MPC or MPCY Bulk Data entries. This is probably the most useful tool for the user to gain some insight of how a Nastran contact job proceeds.

Main Index

168 MD Nastran 2010 Release Guide Nonlinear Solution Statistics (STS) File

Nonlinear Solution Statistics (STS) File The STS file is created for SOL 400 nonlinear analyses and a SOL 101 analysis as well with a general contact process, as one of standard MD Nastran output files. The name of an STS file consists of the root name of the job and the extension of STS, for instance, my_job.sts. It has a similar format of data output as MSC Marc, SOL 600, and ABAQUS. While an STS file provides MD users a convenient and succinct means to monitor the incremental solution process and examine the relevant information of the overall iteration procedure, a sophisticated user is encouraged to look into the F06 file for the nonlinear iteration module output, which is led by the percent sign “%” in each entry. The F06 file is a real haven of all nonlinear solution information. A typical STS file is shown as follows. Its content is well self-explained by the file itself.

information summary of job: ./nug_39a version: MD Nastran 2009.0.0, Built on Jun 01, 2009 date: Jun 01, 2009; Day Time: 16:02:19 subcase inc cycl sepa cut cycl split separ cut rmesh time step total time wall time /step # # # # # # # # # # of of 100 |--of the inc--|-----------of the analysis-----------| the inc the job 1 0 0 0 0 0 0 0 0 0 0.0000E+00 0.0000E+00 8.00 1 1 3 1 0 3 0 1 0 0 1.0000E-01 1.0000E-01 9.00 1 2 2 0 0 5 0 1 0 0 1.0000E-01 2.0000E-01 10.00 1 3 2 0 0 7 0 1 0 0 1.0000E-01 3.0000E-01 10.00 1 4 2 0 0 9 0 1 0 0 1.0000E-01 4.0000E-01 11.00 1 5 2 0 0 11 0 1 0 0 1.0000E-01 5.0000E-01 12.00 1 6 2 0 0 13 0 1 0 0 1.0000E-01 6.0000E-01 12.00 1 7 2 0 0 15 0 1 0 0 1.0000E-01 7.0000E-01 13.00 1 8 2 0 0 17 0 1 0 0 1.0000E-01 8.0000E-01 14.00 1 9 2 0 0 19 0 1 0 0 1.0000E-01 9.0000E-01 14.00 1 10 2 0 0 21 0 1 0 0 1.0000E-01 1.0000E+00 15.00 Job ends with exit number : 0 total wall time: 19.00 total cpu time: 10.91

Main Index

cpu time 0.87 1.85 2.53 3.19 3.87 4.55 5.22 5.89 6.57 7.25 7.92

max displ. 0.0000E+00 5.4988E-02 1.1103E-01 1.6795E-01 2.2570E-01 2.8430E-01 3.4390E-01 -4.3202E-01 -6.5000E-01 5.2527E-01 5.8834E-01


Large Displacement Grid Point Weight Generation (GPWG) The Grid Point Weight Generator (GPWG) provides the user information on the mass matrix, including center of gravity information and principal moments of inertia. The GPWG calculations are triggered by PARAM,GRDPNT,gridid. Where gridid > -1; if gridid = 0, then the Basic Origin is used. In MD Nastran 2010 SOL 400, when a geometrically nonlinear or large displacement analysis is performed, all the weight and balance information is obtained based on the deformed structural geometry and printed out at user-specified nonlinear output intervals. Prior versions of MD Nastran used the original geometry only in the GPWG calculations and printout. The printed GPWG information, such as the reference point, rigid body mass matrix, and others, follows the standard GPWG format. Detailed information about the GPWG calculations and printout can be found in Appendix B of the Linear Static Analysis User’s Guide.

Main Index

170 MD Nastran 2010 Release Guide User Subroutines

User Subroutines Introduction MD Nastran 2010 introduces a set of user definable objects in SOL 400 in the following areas: • User defined elements • User defined materials • User defined contact

The objects are implemented and built as SCA services external to the Nastran application. A set of tools are provided to facilitate implementation and build of the services. User defined services can then be loaded and called upon at run time through special entries in the Nastran BDF file.

Building Services To facilitate the implementation and build of services, a set of files that define the service shell and its APIs along with a script to build the service is delivered for each user defined object in MD Nastran 2010. Using the service shell provided, the user can implement the service either in C++ or FORTRAN. The user can then build the service using the script provided for that user service.

Using Services There are two steps involved in using a user defined service in MD Nastran: • Specify the name and location of the service. This is done through the FMS statement CONNECT (p. 48) in the MD Nastran Quick Reference Guide. • Identify the name of user-defined objects and tie the object to a service name. This is done

through the following entries: • ELEMUDS for user defined elements • MATUDS for user defined materials • BCONUDS for user defined contact

Additional Information and Resources For details on how to build and use user-defined services, please refer to the Introduction (Ch. 1) in the User Defined Services User’s Guide. Additional information can be located in the Introduction (Ch. 1) in the SCA Framework User’s Guide.

Main Index


User Defined Module Service UDMSRV Introduction MD Nastran 2010 introduces a User Defined Module Service, UDMSRV which provides a mechanism for Nastran users to develop their own user defined modules and integrate them into Nastran’s solution sequence through DMAP solution sequences. The module services are callable from DMAP programming language.

Benefits The User defineUsers who want to create their own DMAP modules to calculate new quantities, or augment the existing Nastran solutions with their own proprietary methods. This provides a more modern and integrated method of modifying the solution sequences than the ISHELL method.

Additional Information and Resources For more information please see, User Defined Module Service UDMSRV (Ch. 2) in the User Defined Services User’s Guide.

Main Index

172 MD Nastran 2010 Release Guide User Defined Module Service UDMSRV

Main Index

Chapter 7: Explicit Nonlinear (SOL 700)

7

Main Index

MD Nastran R3 Nastran Release Guide

Explicit Nonlinear (SOL 700) 

Introduction



New Capabilities in Explicit Nonlinear (SOL 700)



DMP for FSI Applications with Multi-Material Euler



Guidelines in Using SOL 700 FSI DMP



Limitations



Advanced Composites based on AlphaStar – GENOA



Impact of a Rigid On Composite Laminate Using GENOA PFA Material



Rigid Impact on Composite Foam Laminate using Genoa Material



New Material Models



Restart Option to Import an Euler Archive from Previous Run



Additional Features



Occupant Dummies



New Examples in MD Demonstration Problems

174 MD Nastran 2010 Release Guide Introduction

Introduction Several new capabilities have been added to the Explicit Nonlinear Solution - SOL 700 in MD Nastran 2010 to dramatically improve the performance of Fluid Structure Interaction (FSI) applications, extend the material models, and enhance the capabilities and robustness.

New Capabilities in Explicit Nonlinear (SOL 700) The following new capabilities are added in this release:

1. Parallel support for FSI applications with multi-material Euler based on Distributed Memory Parallel (DMP) Technology. In addition, the following capabilities are also supported for a DMP simulation: • ROE solver • Graded mesh • Failed elements in coupling surface • Biased meshing • Coupling surface output and markers • Geometric boundary conditions • Viscosity

2. Advanced Composites based on AlphaStar – GENOA technology for shells, solids, and honeycombs 3. New shrink tight fit contact feature 4. New material models 5. Support for new LSTC occupant dummy models 6. Restart option to import a Euler Archive from a previous run 7. Additional features and capabilities In addition, several software defects have been corrected.

Main Index

CHAPTER 7 175 Explicit Nonlinear (SOL 700)

DMP for FSI Applications with Multi-Material Euler With the release of MD Nastran 2010 and completion of the second phase of the project, the DMP support for FSI applications is extended to include the multi-material euler. The capability allows many CPU intensive FSI applications that require multi-material interactions to dramatically reduce the simulation time. Below are some typical applications: • Sloshing with air and fuel (contrary to fuel and void in the type 9 solver) • Underwater explosions with air and water (contrary to void and water in the type 9 solver) • Birdstrike where the bird is made up of a fluid volume with strength (a stress-tensor) • Shaped charge, bullet impact with Euler only or with a coupling to a Lagrangian mesh. • Hydroplaning • All other applications with the MMHYDRO and MMSTREN solver

In the previous release, MD Nastran R3 Parallel FSI capability was limited to single material hydrodynamics and general coupling using the MESH box. Several benchmarks were run to study the performance improvements and investigate the scaling sensitivities to the model size, number of cube partitions, platforms, etc. The benchmarks are selected from different applications that require multi-material interactions. Please see below for some typical performance results.

Summary of Typical Benchmarks and Performance Results 1. Landmine blast on armored plate • The number of Euler elements: 1,000,000 • The number of Lagrangian elements: 32 • Multi-Material Strength example • Total Simulation Time: 5E-1 seconds

Main Index

176 MD Nastran 2010 Release Guide DMP for FSI Applications with Multi-Material Euler

Main Index


2. Fluid Filled Bottle Drop Test • The number of Euler elements: 410,435 • The number of Lagrangian elements:

10,000 • Multi-Material Hydro example • Total Simulation Time: 1E-2 seconds

Main Index


3. Rigid bullet penetrates Skull • The number of Euler elements: 1,162,851 • The number of Lagrangian elements: 0 • Multi-Material Strength example • Total Simulation Time: 1.0e-3 seconds

Main Index


4. Submerged Tunnel • The number of Euler elements: 108,000 • The number of Lagrangian elements: 10,374 • Multi-Material Hydro example

Main Index


• Total Simulation Time: 1.0E-2 seconds

Main Index


5. Projectile Impact • The number of Euler elements:

360,000 • The number of Lagrangian elements:

312 • Multi-Material Strength example • Total Simulation Time: 3.7E-5 seconds

Main Index


Main Index


Guidelines in Using SOL 700 FSI DMP • Performance is enhanced using larger-size models. • Performance can be influenced by no. of “cubes” and its configurations but variance is not

significant. • Performance varies across platforms and sensitive to machine configurations. • Scalability is much better on an “even” number of processors than “odd” number of processors

due to nature of dual-core and quad-core processors. • Avoid using prime number of CPUs as the partitioning of the Euler mesh will be in one direction

only and this will reduce the performance of FSI DMP. • The optimum partitioning heavily depends on the shape of the Euler mesh. The ultimate shape

of each partition should be as square as possible (i.e. have as many Euler mesh on the boundary in each direction). • Linux X8664 has shown better scaling than Windows Platforms even though Windows runs

faster on single processor for the applications we tested. • FSI Applications without Coupling scale better. • DMP FSI Performance in MD Nastran 2010 will be improved in future releases with further

optimization in the following areas: • Load Balancing • Adaptive Coupling • Volume Fraction computation in Coupling • Additional updates in the DMP schema of Dytran DMP • Additional updates in the DMP interface of LS-Dyna coupling with Dytran • Improve editing for DMP

Main Index

184 MD Nastran 2010 Release Guide Limitations

Limitations The following limitations exist in MD Nastran 2010 DMP FSI: • Adaptive Euler • Resize option for Euler mesh • Complete Load Balancing and Optimization • Arbitrary Euler mesh (Only “MESH” command used for Euler region ) • General coupling with fast coupling deactivated. • Output request (ARC, THS) for Specific Euler Elements • PEULER property • FLOW between COUPLE and GBAG • Import OF EULER ARCHIVES • PARAM EUSUBMAX not supported • Single Material Euler with Strength solver. • TICREG using ELEM.

How to Run DMP FSI The following example demonstrates how to run a typical DMP application. For more details please refer to “System Information and Parallel Processing” chapter in the MD Nastran SOL 700 Users Guide. It is important to make sure that the sol700.pth file that resides in your directory includes the following additional line: fsidmp=yes nproc=4 (no. of processors used, 4 processors as in this example)

In addition, use the following DYPARAM entries to define options for Fast Coupling and number of euler cubes for partitioning: DYPARAM, FASTCOUP DYPARAM,EULERCB Please refer to the MD Nastran Quick Reference Guide for more details.

Main Index


Delivery Platforms The MD Nastran SOL 700 and DMP capability are supported on the following modern platforms and operating systems: Platform

Operating System

Windows 32 Windows 64

Windows XP-SP2

SGI Altix

Propack 4

HP-UX – PA RISC 2.0 **

HPUX B.11.11

HP-UX Itanium2

HPUX B.11.23

Sun Sparc Solaris **

Solaris 10 ( = SunOS 5.10 )

Solaris X64

Solaris 10

IBM RS/6000

AIX 5.3

Linux Itanium2 IA64 *

RedHat 4 update 5

Linux x86_64

RedHat 4 update 5

Intel Linux **

Red Hat 4 update 5

*For correct operation of the Intel Fortran compiler, MS Visual Studio .NET must be installed prior to installing the Intel 8.1 compiler. For SOL 700, these installs are not mandatory. **The SOL 700 does not support the following configurations: SGI: R4k and R5k; HP: HP-UX 10.20; SUN: Solaris 7; Linux: Redhat 7.3, Windows NT

Main Index

186 MD Nastran 2010 Release Guide Advanced Composites based on AlphaStar – GENOA

Advanced Composites based on AlphaStar – GENOA In MD Nastran R3 we introduced two major advanced composite capabilities to support the Progressive Failure Analysis (PFA) and honeycomb material behavior. The first capability was based on prediction of delamination and failure of composite shell structures CQUAD4, CTRIA3, and PCOMP. MD Nastran 2010 extends these capabilities to include the support of solids (thick shell element) CHEXA, CTQUAD, CTTRIA, PCOMPLS for honeycomb material. In addition MATM has been extended to support the material nonlinearity by defining stress-strain relationship. There are up to six different material models with up to 24 different failure criteria (see below). • Up to 6 different materials • Fiber Matrix • Ply • Isotropic • Orthotropic Foam • Isotropic Foam • Honeycomb • Up to 24 different Failure Criteria • Maximum Stress/Strain • Failure theory • Honeycomb

Impact of a Rigid On Composite Laminate Using GENOA PFA Material Summary Ref. No.

MD User Guide

Title

Impact of a rigid body on Composite Laminate using GENOA PFA material

Features

Main Index

• Using Genoa composite shell material for impact simulation


Geometry

Material properties

• Impactor (Rigid)

Mass = 0.138 lbf-s2/inch = 53.2 lbm Diameter = 1 inch • Plate (Deformable, GENOA 2D material)

G30-500/45 R6367: /-45/0/90/0/90/0/90/0/90/-45/45 Density = 1.962E-3 lbf-s2/inch4 12 layers (Details will be explained) Analysis characteristics Boundary conditions Applied loads

Transient explicit dynamic analysis (SOL 700) • Fixed boundary at sides of the plate

Initial velocity of a rigid body

Element type

• 4 node shell element CQUAD4

FE results

1. Displacement and contact force time histories 2. Stress Distribution plot at the end

Introduction MD Nastran predicts complex, large deformation composite behavior with extensive material degradation. GENOA PFA (Progressive Failure Analysis) material model available in MD Nastran SOL 700 allows prediction of complex composite material behavior and degradation of the plies and laminates at micro-mechanical level. In the following example which includes two parts, the simulation results are compared and correlated closely to those of test results during a high velocity impact event. In part 1, the plate material is a composite laminate using shell elements while in part 2, the plate material is a combination of laminate composites and solid foam material.

Requested Solution The displacement and contact force time histories are computed and compared with the test results.

Main Index


Model Details of Part 1 - Composite Shells The 10-inch width by 11-inch length composite panel is sandwiched by two supporting plates during impact (Test and Simulation Setup). The one-inch diameter impactor has a mass of 53.75 lbs with an impact velocity of 3.01 ft/sec resulting in a impact energy of 7.58 ft-lbs. The panel was made with six layers of G30-500/R3676 fabric (in which the fiber volume was 60 percent) with the ply lay-up of (45,45), 4x(0,90),(45,-45). Each fabric ply is 0.014 inches thick and the total thickness of the panel is 0.084 inches. For details of the test results, please refer to the paper, “Impact, and Tension After Impact of Composite Launch Space Structure” (Frank Abdi, at al, Conference Paper 2001.)

Impacted panel

Figure 7-1

Test and Simulation Setup

The composite shell panel is modeled using PCOMP entry. The panel has 12 layers and the thickness of each layer is 0.007 inch. The panel is made with the ply lay-up of (45,-45), 4x(0,90),(45,-45) which is the same as the test model. PCOMP + + + + + +

1 1 1 1 1 1 1

.007 .007 .007 .007 .007 .007

45.00000 0.0 0.0 90.00000 90.00000 -45.

1 1 1 1 1 1

.007 .007 .007 .007 .007 .007

-45. 90.00000 90.00000 0.0 0.0 45.00000

The composite material is modeled using MAT1, MAT8, and MATM entries. MAT1 and MAT8 represent general isotropic and orthotropic material properties, respectively. Both materials are referred by MATM material where the fiber/ply and matrix properties of composite materials can be assigned. In addition, the failure criteria can also be defined in the MATM material model. MAT1 MATM + + + + + + + MAT8

Main Index

333 1 PLY

560000.0 0.33 1.962E-3 1 1 0 .6 0.0 1 33 333000.0266000.0333000.0266000.0333000.0 266000.03846.0003846.0003846.000

MATRIX 333 11000. 55000. CRITICALS11T NONCRIT S11C S22C S33T MDE RROT CRSH 33 3.400E+72500000.0.2

21000.

2.00E-02 .05

4.00E-02

S33C S12S S23S S13S DELM FMBK S22T 2500000.2500000.1000000.1.962E-3


Results The results of the simulation were compared with those of the test. MD Nastran SOL 700 generates Lagrangian time history results into the binout binary and d3plot file while the Eulerian time history results are output in the THS file. The following displacement time history is generated using SimXpert reading the results from d3plot. Displacement time history at node 1 shows the displacement time history result at node 1 which is located in the center of the panel and shows the maximum displacement of 0.22 inches which correlates very closely to the maximum displacement from the test of 0.20 inches.

Figure 7-2

Displacement time history at node 1

To generate the contact force time histories, an ASCII file is generated. This is because XY plots generation from binout binary file is not currently supported in SimXpert or Patran at this time. Alternatively, LS-Post can be used to generate the XY plot by reading the binout file directly. To generate the ASCII file from binout file, a convertor tool called “I2a” is used. “l2a” is an executable that resides in the MD Nastran SOL 700 installation directories and reads in the binout binary file and generates an equivalent ASCII file. The command is: “l2a filename.dytr.binout0000” After running this command, several ASCII files are generated that include nodal forces (ncforc), contact forces (rcforc), element forces (elout) etc. In the “rcforc” file the slave and master time history contact forces are recorded. The magnitude of contact forces on slave and master bodies are the same but with opposite signs. Using a contact force time history of the master contact body, the Figure 7-3 is generated by sorting the data first and then using MS xl for actual plot. The maximum z-contact force is 878.6 lbf compared to 897 lbf from the test results.

Main Index


Figure 7-3

Summary Test

Simulation

Maximum displacement (in)

0.20

0.22

Maximum contact force (lbf)

897

878.6

Rigid Impact on Composite Foam Laminate using Genoa Material Model Details – Composite Shells and Solid Foam Material The 10-inch wide by 11-inch high panel was fully fixed at each side. The one-inch diameter impactor had mass of 53.75 lbs and impact velocity of 62.04 inch/sec. The panel was made with a composite foam, adhesive, and skin composite fabric (Skin: G30-500/R3676, adhesive; FM-300, foam core: Rohacel 200WF.) The panel was laid up by skin, adhesive, foam core, adhesive and skin from the bottom surface. Each skin fabric ply is 0.014 inch thick and the total thickness of the skin ply is 0.056 inches (Upper skin ply lay-up angle: -45, 45, 90, 0 and Lower skin ply lay-up angle: 0, 90, 45, -45). The thickness of the FM300 adhesive layer is 0.01 inch and the thickness of the core foam is 0.37 inch. To get the test results, please refer the report, (Dade Huang, Frank Abdi, Mohsen Khatiblou “Progressive Failure Analysis (PFA) and Verification of Composite Test Panel Under Impact and Compression After Impact (CAI) Loading Using GENOA”. Alpha STAR Technical Report to Boeing 12/14/1999. Filename: 299_Report-impact_compression.) The composite shell is modeled using PCOMP entry and the solid composite foam is modeled using PCOMPLS entry.

Main Index


PCOMP + + PCOMPLS + + + + + +

8 1 1 6 1 2 3 4 5 6

1.4E-02 0.00 1.4E-02 45.0 2 3 3 3 3 3

1.0E-02 2.4E-02 2.4E-02 2.4E-02 2.4E-02 2.4E-02

1 1

1.4E-02 90.0 1.4E-02 -45.

0.00 0.00 0.00 0.00 0.00 0.00

To predict the progressive fracture, the material is modeled using MAT1, MAT8 and MATM entries. MAT1 and MAT8 represent general isotropic and orthotropic material properties, respectively. Both materials are referred by MATM material. The fiber/ply and matrix properties of composite materials and their failure criteria can be assigned by using the MATM entry shown below: MAT1 MATM + + + + + + + + MAT8

333 1 PLY

560000.01 0.33 1.308-4 1 0 .6 0.01 1 33 333000. 266000. 333000. 266000. 333000. 266000.03846.0003846.0003846.0001.00E-021.00E-021.00E-02 1.00E-021.00E-021.00E-021.00E-021.00E-021.00E-02 0.03 0.03 MATRIX 333 11000. 55000. 21000. 1.00E-02 .01 1.00E-02 CRITICALS11T NONCRIT S11C S22C S33T S33C S12S S23S S13S MDE RROT CRSH DELM FMBK S22T 33 3.400E+72500000.0.2 2500000.2500000.1000000. 1.632-4

Results of Part 2: The results of the simulation were compared with those of the test. To plot the results, same methodology as part 1 was followed.

Main Index


Figure 7-4

Contact force time history

The maximum z-contact force is 1510 lbf compared to 1514 lbf from the test results.

Summary

Maximum contact force (lbf)

Main Index

Test

Simulation

1510

1514


.New

Contact Feature

The contact features in BCTABLE are extended to support the shrink tight fit capability by introducing two new variables ITTID1 and ITTID2 referring to table IDs. The purpose of this contact feature is to model those parts that are shrink-fitted together and are therefore, prestressed in the initial configuration. The prestressing can be defined by using two tables, whereby the first table is used to gradually increase the interference stiffness from zero to its final value and the second table is used to define the interference stiffness during transient analysis.

Main Index

194 MD Nastran 2010 Release Guide New Material Models

New Material Models The following material models are added: • MATD130: Special Orthotropic material • Based on a resultant stress formulation • In-plane behavior is treated separately from bending behavior. • MATD147: FHWA (Federal Highway Administration) soil material • Isotropic material with damage • Available for solid elements • Modified Mohr-Coulomb surface is applied • Developed for applications involving road-based soils. • MATD170: Resultant Anisotropic material • Based on a resultant stress formulation • In-plane behavior is treated separately from bending behavior. • It is similar to MATD130 except anisotropic characteristics • MATD193: Drucker Prager Material Model • Suitable for Soil Modeling • Definition of the yield surface and popular geotechnical parameters • Modified Drucker-Prager yield surface is used for a more realistic definition of soils. • MATD025: Geological Cap Material Model • Suitable for modeling geomechanical problems such as concrete • Two invariant cap theory is extended to include nonlinear kinematic hardening as suggested

by Isenberg, Vaughan, and Sandler [1978]. • One of the major advantages of the cap model over other classical pressure-dependent

plasticity models is the ability to control the amount of dilatancy produced under shear loading. • Another advantage of the cap model over other models such as the Drucker-Prager and Mohr-

Coulomb is the ability to model plastic compaction. • MATD159: Continuous, smooth Cap Model • Includes Brittle and ductile damage • Suitable for concrete and rock modeling • Includes softening behavior • Includes viscoplastic rate effects, depending on tension and compression • MATDMG: State Variable Plasticity-Damage Model (based on research work from

Mississippi State University

Main Index


• ISV plasticity formulation of Bammann [1990] with the addition of porosity [Bammann et al.,

1993] and the void nucleation, growth, and coalescence rate equations For more details, see the MD Nastran Quick Reference Guide.

Main Index

196 MD Nastran 2010 Release Guide Restart Option to Import an Euler Archive from Previous Run

Restart Option to Import an Euler Archive from Previous Run This capability will allow the user to do an initial run with very fine mesh and then use the results in a subsequent run by importing the results. This capability is especially useful in blast simulation where the distance between the structure and the blast is often large, resulting in excessive CPU time for the blast wave to reach the structure. In addition, the simulation may have to be repeated several times for different structures or for different positions. To reduce the simulation time, the simulation is split up in two parts. In the first simulation, the structure is omitted. In subsequent runs, the result can be imported into a simulation which includes the structure. The blast wave will almost immediately hit the structure at the start of the run without using a lot of CPU time. In addition, importing the Euler archive also allows mapping the fine mesh to a coarser mesh resulting in significant performance improvement. Figure 7-5 shows an Eulerian fine mesh where a blast wave is propagated. The blast results are then passed on to a coarser Eulerian mesh with structure Figure 7-5b. To use the restart capability, use the following command in the SOL 700 .pth file to read in the results from the previous run.

eid-filename.ARC

a Figure 7-5

Main Index

b

Blast wave formulation with fine mesh and restart with structure.


Additional Features The following features are also added in MD Nastran 2010: • EULFOR: Body force on Euler elements • CROSSEC: Cross-Section Output Control • New Time History Variables: • BNDOUT option added (Boundary x, y, and z forces) • SECFORC option added • New BJOIN capability: connect several nodes automatically using tolerance • New Initial Condition Entries • ISTRNSH: Initialize strain tensor of shell elements • ISTRNSO: Initialize strain tensor of solid elements • ISTRSSS: Initialize the stress in solid elements that are part of a section definition to create

a preload • TABISTR: Table control for stress initialization • Output request for a subset of the model and select elements by using $S700 flag in Case

Control Section • New Parameters • DYPARAM,LSDYNA,ENERGY: Control for energy dissipation • DYPARAM,LSDYNA,IMPLICIT: Control implicit analysis for Prestress and Springback

simulation • New Bias mesh control of Euler elements • BIAS: MESH Bias Definition • Bias options are also added in MESH entry • New options in RBJSTIF entry • DYFSISW: Control of activation of Euler elements and Coupling • Shell offset: SOL 700 supports Shell offset using CQUAD4 • Creation of Dynamic Relaxation database for post processing

Main Index

198 MD Nastran 2010 Release Guide Occupant Dummies

Occupant Dummies MD Nastran 2010 SOL 700 supports the following new occupant dummies developed by LSTC: • Hybrid III - 50% Full FE Dummy • Hybrid III - Rigid-FE (5%, 50% and 95%) • Side Impact Dummy (SID)

The new Hybrid III 50% male dummy

Main Index


New Examples in MD Demonstration Problems Several new examples are created and are made available in MD Demonstration Problems Manual1 and the SOL 700 User’s Guide. Many of the examples include step-by-step tutorials with SimXpert to demonstrate how to set up the model, run the analysis, and post-process the results.

Hydroplaning Simulation

1

Formerly called the MD User’s Guide - Application Examples

Main Index

200 MD Nastran 2010 Release Guide New SOL 700 Parameters and Bulk Data Entries

New SOL 700 Parameters and Bulk Data Entries Table 7-1 contains new Parameters and Table 7-2 lists the new Bulk Data entries for SOL 700 in MD

Nastran 2010. More details can be found in the MD Nastran Quick Reference Guide. Table 7-1

New Parameters for SOL 700

New for MD Nastran 2010 (SOL 700) Parameters

Description

EUSUBCYC

Controls the maximum growth of the subcycling interval in Euler computations.

COSUBCYC

Controls the growth of the subcycling interval in the coupling surface.

COSUBMAX

Defines the maximum number of subcycles that can occur in Euler/Lagrange coupling.

Table 7-2

New Bulk Data Entries for SOL 700

New for MD Nastran 2010 (SOL 700) Bulk Data Entries

Main Index

Description

BIAS

Specifies a variation of the mesh-size in one direction for use in the MESH entry.

CROSSEC

Defines a cross section for resultant forces written to SECFORC in MD Nastran SOL 700.

DYFSISW

Allows activating or deactivating Fluid Structure Interaction and Eulerian solver.

DYPARAM,COHESION

Print initial time step sizes for elements in the first cycle in MD Nastran SOL 700.

DYPARAM,EULERCB

Divides a Euler domain into several cubes.

DYPARAM,EUSUBMAX

Defines the maximum number of subcycles that can occur in the Euler solver.

DYPARAM,LSDYNA, ENERGY

Provide controls for energy dissipation options.

DYPARAM,LSDYNA, IMPLICIT

Options to modify convergence tolerances and initial/geometric stiffness of prestress (PRESTRS) or springback (SPRBCK) simulations.

EULFOR

Defines a body force loading (acceleration) on Euler elements per unit mass.

ISTRNSH

Initialize stresses and plastic strains in the Hughes-Liu beam elements.

MATD025

This is an inviscid two invariant geologic cap model.


Table 7-2

New Bulk Data Entries for SOL 700

New for MD Nastran 2010 (SOL 700) Bulk Data Entries

Main Index

Description

MATD77H

This material model provides a general hyperelastic rubber model combined optionally with linear viscoelasticity as outlined by Christensen [1980].

MATD77O

This material model provides the Ogden [1984] rubber model combined optionally with linear viscoelasticity as outlined by Christensen [1980].

MATD130

Special Orthotropic material

MATD147

FHWA (Federal Highway Administration) soil material

MATD159

Continuous, smooth Cap Model

MATD170

Resultant Anisotropic material

MATD193

Drucker Prager Material Model

MATDMG

Mississippi State U State Variable Plasticity-Damage Model

TABISTR

Defines the usage of table for the stress initialization

202 MD Nastran 2010 Release Guide New SOL 700 Parameters and Bulk Data Entries

Main Index

Chapter 8: Implicit Nonlinear (SOL 600)

8

Implicit Nonlinear (SOL 600)



Main Index

MD Nastran R3 Release Guide

SOL 600 Enhancements

204 MD Nastran 2010 Release Guide SOL 600 Enhancements

SOL 600 Enhancements Introduction MD Nastran SOL 600 is a Solution Sequence that allows MSC.Nastran users to use the familiar MD Nastran input file format to execute complex nonlinear problems via a translation to MSC.Marc. A series of enhancements have been made to increase the functionality of the product based upon customer input since the MD Nastran R3 release.

Benefits This allows a broader set of Nonlinear Problems to be solved within the Nastran framework. These enhancements are outlined below: • Added Pardiso and MUMPS solvers for parallel and multi-threaded processing for Linux and

Windows machines using Intel or AMD processors. These solvers allow features in the Marc input file that are not allowed for DDM parallel processing, such as coordinate transformations using the "COORD SYS" option. Please see the following sections in the QRG for more details: NLSTRAT, PARAM,MRTHREAD, MARAM,MARCSOLV, PARAM,MUMPSOLV. • Added plane stress to add Marc’s capabilities – use the MRALIAS PARAM or the ALIASM

Bulk Data option • Implemented PARAM,TSTATIC for dynamic analyses • Added friction vs other variable described by tables capability – see BCBODY and /or

BCTABLE • Better control of 2-D Rigid bodies Rx, Ry for 2D rigid contact orientation • Provide support for contact user subroutines ufric, ufricbbc, uhtcon, digeom, sepstr, spfor – see

BCBODY and BCONUDS • Added rigid contact rigid surface temperature and sink temperature for heat transfer simulations

– see BCBODY and BCTABLE • Added new options for BCBOX, such that the user can specify if the complete element needs to

be in the box to be put in body, or only a single node • Allow contact variables such as velocity to be defined using tables • Added conversion of CHEXA and CPENTA to solid shell (customer request) • Add delamination capabilities – see MDELAM Bulk Data entry • Improved VCCT crack propagation so the path along the crack tip in 3-d can be easier to

describe - see VCCT Bulk Data Option – Not supported by GUI • Add material mixtures capability – see MIXTURE Bulk Data entry • SOL 600 now supports RSSCON. • SOL 600 now supports RSPLINE.

Main Index

CHAPTER 8 205 Implicit Nonlinear (SOL 600)

• Added new type of RBE3 to uniformly distribute applied loads – see the RBE3U Bulk Data

entry. Note that this does not distribute stiffness. • Added generalized alpha method for dynamics, this includes support for the Hilbert-Hughes-

Taylor (HHT) procedure. Use the HMOUBOLT Param and set dynamic operator to 7. • Added PARAM,MARALPHA to choose between secant and instantaneous CTE’s vs

temperature with options to obtain high accuracy • Added general capability for user subroutines. – See the MATUDS and BCONUDS Bulk Data

entries. This will only be available in Beta 2. • Added stiffness matrices in output4 and Boeing Hartwell formats. This is controlled using the

MSTIFOT option. • Added improved superelement capability (S6SUPER). This will only be available in the Beta 2

release. • Exposed simplified nonlinear elasticity models available in Marc NLELAST option. See

MATNLE Bulk Data options. • Exposed user defined hypoelastic material model. See MATHYP • Allow user subroutines to be used with rate dependent creep material models. See the MATVP

Bulk Data entry. • Allow nonlinear material behavior over a solid section beam of arbitrary cross section. This

beam will be numerically integrated. The definition of the beam section and the integration procedure is entered through the PBMARB6 Bulk Data entry. • Added options to improve complex loading • Added option to keep or remove mpi services on Windows systems for a run using parallel

processing with DDM • Added an option to convert MAT1 entries with bad Poisson ratio’s to MATORT

New SOL 600 Parameters and Bulk Data Entries Table 8-1 contains new Parameters and Bulk Data entries for SOL 600 in MD Nastran 2010. More details

can be found in the MD Nastran Quick Reference Guide.

Main Index


Table 8-1

New Parameters and Bulk Data Entries for SOL 600 New for MD Nastran 2010 (SOL 600) Description Parameters

Main Index

MARAUTO

Determines whether NLAUTO entries for SOL 600,129 will override the default or not.

MARCTOTD

Determines whether for SOL 600 dynamic analyses will use full table association.

MARCTOTL

Determines whether total or incremental loads are used in a SOL 600 static nonlinear analysis.

MARCTOTT

Determines whether total loads, including pressures, gravity, spcd, etc., with associated tables are used in a SOL 600 static or dynamic analysis.

MARCL001

Determines whether Marc’s POINT LOAD (without tables) 2nd datablock, 3rd field will be honored or not. If this value is set to 1, multiple loads at the same dof in the same subcase will usually be summed.

MARFATAL

Determines whether nonexistent grid id’s for BCBODY entries will cause fatal errors or not.

MARTET10

Controls how to treat badly shaped 10-node tetra elements in SOL 600 if renumbering the element does not correct problems.

MARTETIN

Controls whether additional information messages are output to the .f06 file or not when param,martet10 is set to a positive value.

MCORDUPD

Determines the coordinates will be updated if one of the CONTINUE options is specified on the SOL 600 Executive Control statement.

MINSOUTT

Determines that elements that deform so much that they go inside-out in an analysis will be deactivated.

MMBOLTUS

Controls how the top and bottom nodes are placed in the Marc “tying 69” input when MBOLTUS is used in a SOL 600 model.

MQUATERN

Controls whether quaternions will be used for SOL 600 models with large rotation.

MREVPLST

Determines whether 2D plain stress triangular element node numbers will be reversed or not.

MRDYNOLD

Determines whether dynamic loads created by SOL 600 are the same as in MD Nastran R3 (and MSC Nastran 2008) and prior releases or if they use a new calculation method.

MRCONTAB

Determines whether CONTACT and CONTACT TABLE for SOL 600 use avtable-driven form or not.

MRPLOD4R

Determines how PLOAD4 pressures are treated in Marc when PARAM,MRPLOAD4,2 is set.

CHAPTER 8 207 Implicit Nonlinear (SOL 600)

Table 8-1

New Parameters and Bulk Data Entries for SOL 600 New for MD Nastran 2010 (SOL 600) Description

MRPOISCK

Controls whether to check if a “bad” Poisson ratio has been entered in SOL 600 for MAT1 entries.

MRSPRVER

Controls how CELAS and all other items map to the Marc input data.

MNASTLDS

Option to determine complex force and/or moments using OLOAD’s as calculated from SOL 101.

MSPLINC0

This parameter controls whether to enforce C0 continuity for all spline options if any are requested by setting IDSPL=1 on any BCBODY entry.

MSTTDYNE

Controls whether SOL 600 may have static and dynamic load cases in the same analysis.

MTABIGNR

Determines whether tables for VCCT analyses will be ignored or used.

MTEMPCHK

Controls how temperature-dependent properties are checked in the Marc portion of SOL 600.

MTEMPDWN

Option to automatically choose the FeFp multiplicative decomposition plasticity model (PARAM,MARCPLAS,5) for plasticity problems with thermal loading when the temperature decreases (see PARAM,MARCPLAS).

MTET4HYP

Controls settings for TET4 elements with hyperelasticity.

MUALLUDS

Controls how material, contact and element-related user subroutines are specified in SOL 600.

MVERMOON

Controls whether 5-term Mooney series or 5-constant Mooney will be used in the Marc portion of SOL 600. Bulk Data Entries

Main Index

CSSHLH

Defines conversion of CHEXA elements to Solid Shell elements in SOL 600 only.

CSSHLM

Defines conversion of CHEXA or CPENTA elements described by material ID to Solid Shell elements in SOL 600 only.

CSSHLP

Defines conversion of CPENTA elements to Solid Shell elements in SOL 600 only.

DMIGROT

Defines large rotation and other characteristics of a matrix entered using DMIG in SOL 600.

ISTRESS

Defines initial stress values. This is the MSC Marc’s initial stress option used in SOL 600 only.

MATNLE

The MATNLEx entries specify advanced forms of nonlinear elastic materials.

MATTUSR

Specifies table variation of user defined generic materials in SOL 600 and MD Nastran SOL 400 only.


Table 8-1

New Parameters and Bulk Data Entries for SOL 600 New for MD Nastran 2010 (SOL 600) Description

MATUDS

Allows the user to provide material routines for use with enhanced material models in SOL 600.

MATUSR

Specifies user-defined, generic material properties for hypoelastic material models in SOL 600 and user defined material models in MD Nastran SOL 400 only.

MAUXCMD

Defines auxiliary command to spawn on a Nastran process from another Nastran process in SOL 600.

MDELAM

Defines materials for which delamination may occur in SOL 600 only.

MDMIAUX

Specifies the DOMAINSOLVER command to be used in conjunction with secondary spawned jobs when MDMIOUT is used. SOL 600 only.

MISLAND

Defines an island of connected elements that will be completely removed if the number of elements within the island becomes smaller than a specified value in SOL 600 only.

MIXTURE

Defines constituents of “composite” material on original and potentiality damaged state.

PBMARB6

Defines arbitrary beam/bar cross section for use in SOL 600.

PBMNUM6

Defines four specific numerically integrated BEAM/BAR cross section for use in SOL 600.

RBE3U

Defines Method to Distribute Applied Loads to a Surface in SOL 600

TABD1MD

Defines how TABLED1 entries are internally modified in SOL 600.

Additional Documentation In addition to the MD Nastran Quick Reference Guide, the user should refer to Marc Volume A for a theoretical discussion of material models, fracture mechanics, and dynamics. For additional information on the nonlinear solid section beams, the user should refer to Marc Volume B.

Main Index

Chapter 9: Numerical Methods and High Performance Computing

9

Main Index


Numerical Methods and High Performance Computing 

Serial Performance: Linear and Nonlinear Contact Analysis of Solid Models



Distributed Memory Parallel Solutions for Linear and Nonlinear Contact Analysis



MPI Selection



New Solver Available for Complex Eigenvalue Analysis

210 MD Nastran 2010 Release Guide Serial Performance: Linear and Nonlinear Contact Analysis of Solid Models

Serial Performance: Linear and Nonlinear Contact Analysis of Solid Models Introduction Linear and nonlinear contact analysis is available in MD Nastran SOL 101 and SOL 400. The CASI element based iterative solver was integrated into contact analysis for the MD Nastran R2.1 release. This enhancement enabled efficient computation for the solution of equations  A   x  =  b  for contact with solid models. Contact between two or more solid bodies, over a varying contact area, involves a significant computational cost. The original implementation of contact in MD Nastran utilized previously existing functional and computational tools. For MD Nastran 2010, a more streamlined solution was developed by eliminating unnecessary and extraneous operations. New computational tools and procedures have been implemented to support these changes, resulting in improved performance.

Benefits Users should observe improved computational efficiency and performance for both linear and nonlinear contact analysis, especially for solid models of modest size, using the CASI element based iterative solver.

Inputs There are no changes to the basic user interface for contact analysis. To select the CASI iterative solver, specify the SMETHOD command in the Case Control Section. SMETHOD = ELEMENT To modify parameters for the CASI solver, specify the ID of an ITER Bulk Data entry: SMETHOD = 10 For example, to specify a convergence tolerance of 1.0e-4 for the CASI solver: ITER, 10

PRECOND=CASI, ITSEPS=1.0E-4

The user interface for the CASI iterative solver for contact analysis is the same as it is for linear static analysis in SOL 101. Refer to the SMETHOD, 488 Case Control command and the ITER (p. 1982) in the MD Nastran Quick Reference Guide, for more information.

Main Index

CHAPTER 9 211 Numerical Methods and High Performance Computing

Outputs There are no new engineering outputs associated with this feature other than informational and diagnostic messages. In addition, a “PCS” output text file contains additional diagnostic output.

Guidelines and Limitations The CASI solver is not designed to handle indefinite coefficient matrices. Differential stiffness effects and follower stiffness can produce an indefinite and possibly unsymmetrical coefficient matrix that may result in a FATAL error in the NLSOLV module and termination of the run. Due to the unsymmetrical nature of the follower stiffness matrix, use caution when follower stiffness is present and the SMETHOD is ELEMENT or selects the CASI solver. By default, the presence of any of the MOMENTi, FORCEi, PLOADi, and RFORCE Bulk Data entries causes automatic generation of follower stiffness. If CASI is specified and follower-stiffness is present, it is automatically symmetrized. In cases where this is not acceptable, PARAM,FOLLOWK,NO must be specified in the Bulk Data Section. However, this will alter the analysis results by not including follower stiffness. Currently, follower stiffness resulting from RFORCE, PLOADX and GRAV loadings cannot be handled by the CASI solver interface. Therefore, the presence of these Bulk Data entries will generate User Fatal Message 9192 unless PARAM,FOLLOWK,NO is also specified.

Demonstration Example Examples are taken from actual models from industry. The model below is proprietary, so it may not be displayed. However, the basic model characteristics are shown along with the performance comparison.

Example

Main Index

Analysis type:

Nonlinear contact of an engine block

Number of grid points:

697,896

Number of solid elements:

568,264

Number of iterations:

35

Compute platform used:

Intel Linux 8664 2.9GHz

212 MD Nastran 2010 Release Guide Serial Performance: Linear and Nonlinear Contact Analysis of Solid Models

Main Index


Distributed Memory Parallel Solutions for Linear and Nonlinear Contact Analysis Introduction Nonlinear analysis is available in MD Nastran SOL 400 and SOL 101. At each nonlinear iteration, a solution of the equations  A   x  =  b  is executed. For large models, the bulk of the solution time is spent computing  x  . For MD Nastran R3, support was limited to serial execution and shared memory parallel. For MD Nastran 2010, distributed memory parallel (DMP) solvers are introduced into MD Nastran nonlinear solutions. These solvers perform a matrix based domain decomposition of the global matrix into N partitions, where “N” is specified on the command line via the “dmp=” keyword.

Benefits For large models, especially large solid models, users should experience significant performance increases by enabling multiple processors in a distributed environment. DMP solvers available are: • DMP matrix based iterative solver • DMP direct solver

DMP processing may be combined with shared memory parallel (SMP) for the DMP direct solver.

Inputs There are no changes required to activate Distributed Memory Parallel processing for nonlinear analysis. Users activate DMP processing by specifying “dmp=” on the MD Nastran job submittal command. For more information on DMP job submittal options, see the MD Nastran 2010 Installation and Operations Guide.

Outputs There are no new outputs associated with this feature.

Guidelines and Limitations Distributed Memory Parallel processing for nonlinear analysis is generally recommend for large models where a high percentage of runtime is spent performing the solution of equations required at each nonlinear iteration. This consideration results in certain limitations. In addition, there are database definition and restart limitations for DMP processing in general.

Main Index

214 MD Nastran 2010 Release Guide Distributed Memory Parallel Solutions for Linear and Nonlinear Contact Analysis

Stiffness Update Strategy Distributed Memory Parallel processing is targeted at large models where a full solution of equations is required at every iteration. There may be no performance gain if one specifies DMP solvers for a direct solution (DECOMP/FBS) in situations where many FBS operations are performed using the factor matrix from a single decomposition. These processing paths are controlled by the KMETHOD field of Bulk Data entries NLPARM and NLSTEP. The KMETHOD field controls the stiffness matrix update strategy for nonlinear analysis. In general, only the full Newton iteration method is recommended for DMP processing. Accordingly, DMP execution is limited to analyses where KMETHOD is set to “FNT” or “PFNT”. For linear contact in SOL 101, DMP is allowed for the “AUTO” method. For other KMETHOD values, a User Fatal Message is issued and the job terminates.

Restarts DMP processing is not supported for database restarts. This is a general limitation of DMP database specification and not a specific limitation of nonlinear analysis.

Demonstration Example Examples are taken from actual models from industry. The model below is proprietary, so it may not be displayed. However, the basic model characteristics are shown along with the performance comparison.

Example

Main Index

Analysis type:

Nonlinear contact


146,979

Number of solid elements:

97,927

Number of iterations:

60




Main Index

216 MD Nastran 2010 Release Guide MPI Selection

MPI Selection A single analysis executable is now provided for serial execution as well as DMP execution with all supported MPI implementations. In previous versions: • A separate analysis executable was delivered for DMP execution. • If more than one MPI (Message Passing Interface) implementation was supported on a given

platform, a separate analysis executable had to be delivered for each supported MPI implementation. • An unsupported MPI implementation could not be used without creating a new, separate analysis

executable Starting with MD Nastran 2010, a single analysis executable will be delivered which can be used for both DMP and serial jobs, and which can be used with any supported MPI implementation on a given platform. Moreover, it is possible to use an unsupported MPI implementation with the same executable.

New Keyword: mpiimplementation On platforms which support more than one MPI implementation, a supported MPI implementation may be selected using the mpiimplementation keyword. This keyword may be abbreviated as mpiimp. The table below lists the platforms which support more than one MPI implementation, and the available MPI implementations: Platform : linux32 : linux64 : linuxipf : windows64:

mpi implementations openmpi (default), hpmpi openmpi (default), hpmpi, intelmpi openmpi (default), hpmpi, intelmpi msmpi (default) , hpmpi, intelmpi

For example, to select hpmpi on linux64, mpiimp=hpmpi should be set on the command line or in an rc file. The environment variable MPIIMP may also be used to select the MPI implementation. In the case where both the MPIIMP environment variable and the mpiimplementation keyword are set, the keyword value will be used.

New Keyword: mpilibrary An alternate MPI library may be specified using the mpilibrary keyword. This keyword may be abbreviated to mpilib. The specified MPI library must be in the user’s library path on all nodes used during the computation.The environment variable MPILIB may also be used to select the MPI library. In the case where both the MPILIB environment variable and the mpilibrary keyword are set, the keyword value will be used.

Main Index


New Solver Available for Complex Eigenvalue Analysis Introduction The UMFPACK linear equation solver was first incorporated into Nastran in 2004. It was embedded in the Auto-Mset capability, as well as integrated into the frequency response module (FRRD1) where it is available for complex unsymmetric solutions. In MD Nastran 2010, UMFPACK is available in the complex Lanczos eigenvalue extraction method of the CEAD module. More information about UMFPACK is available at the following URL: http://www.cise.ufl.edu/research/sparse/umfpack/.

Benefits The UMFPACK linear equation solver is more efficient than the default Nastran sparse unsymmetric solver. This is accomplished by employing contemporary matrix reordering techniques and computational kernels.

Inputs To invoke the UMFPACK solver for complex eigenvalue analysis, the UMFLU keyword must be specified as the factorization method, which must be present on the SPARSESOLVER Executive Command: SPARSESOLVER

CEAD

(FACTMETH=UMFLU)

Outputs Use of UMPACK will cause User Information Message 4216 is appear in the F04 file: 11:04:19 0:25 5969.0 948.0 15.6 1.2 UMFD BGN *** USER INFORMATION MESSAGE 4216 (FACDRVI) PARAMETERS FOR IN-CORE SPARSE UNSYM. DECOMP ( MATRIX TYPE=RDP) FOLLOW MATRIX SIZE =185931 ROWS NUMBER OF NONZEROES =12587614 T NUMBER OF ZERO COLUMNS =0 NUMBER OF ZERO DIAGONAL TERMS =0 MEMORY REQUIREMENT = 147711 K WORDS MEMORY AVAILABLE = 496541 KWO MAX FRONT SIZE = 2964 NONZERO TERMS = 67880689 11:04:44 0:50 7013.0 1044.0 40.7 25.2 UMFD END

The “UMFD” time stamp indicates use of UMFPACK.

Main Index

218 MD Nastran 2010 Release Guide New Solver Available for Complex Eigenvalue Analysis

Guidelines and Limitations UMFPACK is a memory resident solution algorithm. It does not feature “spill” logic. This means that the solution is limited by available memory. If insufficient memory is available for UMFPACK, the CEAD module will produce System Warning Message 6136, an example of which is shown here: *** SYSTEM WARNING MESSAGE 6136 (CLASSD) INSUFFICIENT CORE FOR IN-CORE SPARSE DECOMPOSITION. USER ACTION: INCREASE CORE BY AN ESTIMATED 86618 K WORDS. WARNING: THE ABOVE NUMBER IS ONLY AN ESTIMATE, THE ACTUAL CORE SIZE NEEDED MAY BE HIG USER INFORMATION: AN ALTERNATVE SPARSE DECOMPOSITION METHOD WILL BE ATTEMPTED.

Demonstration Example An example models is shown here.

Main Index


Example Analysis type:

Main Index

SOL 107 complex eigenvalue analysis


63,007

Number of elements:

42.137

Number of complex eigenvalues:

100



220 MD Nastran 2010 Release Guide New Solver Available for Complex Eigenvalue Analysis

Main Index

Chapter 10: Dynamics (Noise and Vibration) MD Nastran R3 Release Guide

10

Main Index

Dynamics (Noise and Vibration)



Equivalent Radiated Power (ERP)



Frequency Dependent Rigid Absorber Properties



Dynamics - Monitor Points in Dynamic Solution Sequences



Nonlinear Harmonic Response



Enhancements to the Frequency Response Function (FRF) and FRF Based Assembly (FBA) Capability



EFEA/EBEA (Pre-Release)

222 MD Nastran 2010 Release Guide Equivalent Radiated Power (ERP)

Equivalent Radiated Power (ERP) Introduction In automotive applications, the noise inside the passenger compartment can be caused by many sources including vehicle drive train, vibrating body panels, tire noise, etc. The Equivalent Radiated Power (ERP) calculation focuses on the vibration of body panels, which radiate acoustic power to the passenger cabin. Understanding which panels are responsible for the radiated power is important in understanding the structural behavior and acoustic consequences. The radiated power is a function of skin normal velocity, fluid density, and speed of sound through the fluid. Note:

ERP was introduced in MD Nastran R3.1, but is included in the MD Nastran 2010 release Guide for those who are not aware of the MD Nastran R3.1 release.

Benefit The ERP calculation can be used to compare laser measurements to calculated values in a quantitative way to validate calculations. ERP can also be used during the design phase to understand the effect of individual panels on the overall acoustic response. Previously, the calculations were performed by inhouse tools. In MD Nastran 2010 the ERP calculation is made directly by the solver and provides convenient output in the form of a CSV file.

Theory In a mathematical sense, ERP squares the normal velocity and multiplies it with the element area. The sum over this product, multiplied with a constant yields the ERP over a panel. ERP values can be calculated for both structure and structure-fluid models. panel

ERP = C



2

V n S

surf

where C =   ERPRLF  ERPRHO  ERPC and  for Frequency Response, 1.0 for Transient Response ERPRLF= Radiation Loss Factor ERPRHO= Fluid density ERPC= Speed of sound in fluid In MD Nastran 2010 only direct frequency response and modal frequency response are supported. In addition to the ERP calculation, an ERPDB calculation is also performed to calculate an equivalent radiated power sound pressure level.

Main Index

CHAPTER 10 223 Dynamics (Noise and Vibration)

RHOCP ERPdB = 10LOG  ---------------------------------  ERP v a lu e  ERPREFDB 

Input The ERP calculation is typically requested for a group of elements defined on a SET3 Bulk Data entry. The parameters ERPRHO, ERPC, ERPRLF, ERPREFDB, and RHOCP can be defined on either the ERP Case Control command, or as PARAM entries in the Bulk Data Section. The RHOCP parameter can only be specified on the ERP Case Control command. The ERP Case Control also references an ERPPNL Bulk Data entry. The new Bulk Data entry for ERPPNL is:

ERPPNL

Equivalent Radiated Power Definition

Defines one or more panels by referencing sets of elements or properties. Format: 1

2

3

4

5

6

7

8

9

ERPPNL

NAME1

SETID1

NAME2

SETID2

NAME3

SETID3

NAME4

SETID4

NAME5

SETID5

ROOF

1

DOORLF

16

10

Example: ERPPNL

Field

Contents

NAMEi

Panel label. (CHAR)

SETIDi

Identification number of a SET3 Bulk Data entry that lists the panel property entries or the panel elements. (Integer > 0)

Remarks: 1. The SET3 entries can only refer to CQUAD4, CQUADR, CTRIA3, or CTRIAR structural elements or PSHELL or PCOMP property entries. CQUAD8 and CTRIA6 entries are ignored. 2. NAMEi are used in a Case Control SET definition defining setp to select the panels in the Case Control command ERP.

Main Index


The new ERP Case Control command is:

ERP

Equivalent Radiated Power Panel Participation Factor Output Request

Requests the form and type of ERP panel participation factor output. Format: SORT2 PRINT, PUNCH ERP    SORT1 PLOT

SOLUTION =

ALL setf

,

0.01  frequency    KEY =    FILTER =   , fraction real _value     1.0 1.0     ERPRHO =    ERPC =   real _value real _value     1.0 1.0     RHOCP =    ERPRLF =    real _value   real _value  1.0   ERPREFDB =     CSV = unit   real _value 

 ALL    =  setp     NONE 

Examples: SET 17 = 10.,20.,30.,40.,80.,100. $ A list of frequencies SET 25 = ROOF, DOORLF $ A list of ERP Panel names $ from a ERPPNL Bulk Entry ERP ( PRINT,PUNCH,SOLUTION=17,KEY=frac ) = 25

Main Index

Describer

Meaning

SORT1

Output is presented as a tabular listing of ERP panels for each frequency

SORT2

Output is presented as a tabular listing of frequency for each ERP panel

PRINT

Output is written to the .f06 file

PUNCH

Output is written to the .pch file

PLOT

Results are computed and placed on the ERP table but not output.

SOLUTION

Keyword to select frequencies

setf

Identifier of Case Control SET command defining frequencies


Describer

Meaning

ALL

If associated with SOLUTION, all frequencies are selected. If associated with setp, all ERPPNL entries are selected.

KEY

Keyword selecting the output item used to sort the printed output. The default produces output sorted on either frequency (SORT2) or ERP panel name (SORT1). KEY=fraction produces output sorted in descending order of the fractional ERP value of total ERP.

FILTER

Keyword specifying the value of a filter to be applied to the printed output only. ERP values are printed only if the fractional ERP value of total ERP exceeds the filter value.

ERPRHO

Fluid density for Equivalent Radiated Power (ERP) analysis. This item is actually an MD Nastran parameter.

ERPC

Phase speed of the fluid for Equivalent Radiated Power (ERP) analysis. This item is actually a Nastran parameter.

ERPRLF

Radiation loss factor. In frequency the scale factor, C = ERPRLF * (½ERPRHO * ERPC). In transient the scale factor, C = ERPRLF * (ERPRHO * ERPC).

RHOCP

Scale factor used in dB computation. This item is actually an MD Nastran parameter.

ERPREFDB

Scale factor used in dB computation. This item is actually an MD Nastran parameter. ERP - . The dB calculation is ERPdB = 10 log  RHOCP  ---------------------------- ERPREFDB

CSV

Results will be written to a .csv file.

unit

Unit of the .csv file as used on the required ASSIGN statement

setp

Identifier of Case Control SET command defining NAMEi entries from an ERPPNL Bulk Data entry defining panels.

NONE

No ERP output is produced.

Remarks: 1. ERP is required to produce any ERP output. 2. Output is generated in SORT2 by default. Unlike other Case Control requesting SORT2 format, the ERP command does not force all other output into SORT2 format. 3. FILTER has no effect on PUNCHed, CSV or OP2 output. 4. In addition to individual panel output, a summary named ALLPANEL is produced. If there are multiple subcases, the panel name is formed from the serial subcase number (1-nsubc) and the characters ‘ALLP’ as in ALLP0002 unless the ERP command request output for ALL panels across the Subcases. In this case, the summary panel name ALLPANEL is retained. 5. Selectable frequencies are dependent on the presence of an OFREQ Case Control command. 6. ERPRHO, ERPC, ERPRLF, RHOCP, and ERPREFDB are actually PARAM,name,value entries.

Main Index


7. The filter process avoids printing ERP for cases where ERP/ERPMAX is less than the FILTER value. ERPMAX is the maximum ERP value across all frequencies for a panel. 8. If output to a .csv file is requested, the file must be assigned with logical key USERFILE and FORM=FORMATTED, e.g., ASSIGN USERFILE = myfile.csv UNIT=50 FORM=FORMATTED STATUS=NEW The SET3 Bulk Data entry is also necessary to define: Set 3 Examples: • Set3,id,prop,pshellid1,pshellid2,etc. • Set3,id,elem,elemid1,elemid2,etc. • Set3 prop, can be exchanged between acoustic and ERP panels.

See Bulk Data entry SET3 (p. 3116) in the MD Nastran Quick Reference Guide. Also, see the Bulk Data entry ERPPNL (p. 1815) in the MD Nastran Quick Reference Guide.

Example Input The following input is typical for ERP calculation including CSV output. File Management ASSIGN USERFILE=’myerp.csv’ UNIT=30 FORMATTED NEW DELETE Case Control ERP(PUNCH,Filter=0.0,rhocp=2.0E9,ERPRHO=1.189E-12,ERPC=3.43E5,CSV=30)=ALL

Example ERP Panel Definition Bulk Data ERPPNL,ROOF1,103,ROOF2,203,ROOF3,303 set3,103,prop,100 set3,203,prop,200 set3,303,element,114,124,134,214,224,234, ,314,324,334

Output The results are available in the OP2, MASTER, Print, Punch, and CSV formats. The output includes ERP, Fraction, and ERP(dB). Note that the fraction is not based on the entire ERP of the model, just the ERP that is calculated and there is no check for overlapping or missing elements. There is also a summation of total ERP. Both SORT1 and SORT2 options are available.

Main Index


Figure 10-1

Representative ERP results for a complicated system.

Guidelines and Limitations 1. ERP is calculated currently for linear elements 3 and 4 node shells only. If desired the user can generate a layer of linear shells on top of quadratic solids. 2. PSHELL and PCOMP are supported 3. ERP is supported in direct and modal frequency response only. 4. There is no Direct Results Access (DRA) support. 5. ERP is not supported in Optimization. 6. No limits on coordinate systems

Test Cases The following test cases are available in the TPL in directory /tpl/erp_mdr4: erp_1000.dat, erp_base1_frac.dat, erp_base2_frac.dat, erp_c_param.dat, erp_erpx3.dat, erp_fs.dat, erp_rhocp.dat, erp_soln.dat, erp_base1.dat, erp_base2.dat, erp_c.dat, erp_def.dat, erp_frac_c.dat, erp_ofreq.dat, erp_rho.dat TPL Example Problem erp_base1.dat Test problem erp_base1.dat is a simple fluid bound by two panels. The excitation is on one panel and the ERP is measured.

Main Index


Figure 10-2

Example erp_base1.dat geometry.

The input for erp_base1.dat is a standard modal frequency response with a pressure loading and including fluid-structure interaction. The case control and bulk data entries required for ERP calculation are as follows: Case Control ERP(PRINT,PUNCH,FILTER=0.0)=ALL

Example ERP Panel Definition Bulk Data ERPPNL,ERPX0,103,ERPX3,203,erpeid3,303 set3,103,prop,100 set3,203,prop,200 set3,303,element,114,124,134,214,224,234, ,314,324,334

Listing 10-1

FREQUENCY = PANEL ERPX0 ERPX3 ERPEID3 ALLPANEL

Main Index

TPL example erp_base1.dat Output in SORT1 format.

8.000000E+00 E Q U I V A L E N T ERP 2.702487E-02 4.871353E-03 4.871353E-03 3.189623E-02

R A D I A T E D

FRACTION 7.543413E-04 3.356652E-04 3.356652E-04 6.336370E-04

P O W E R

ERP(dB) -1.568236E+01 -2.312350E+01 -2.312350E+01 -1.496261E+01

AREA 1.000000E+01 9.000000E+00 9.000000E+00 1.900000E+01


Listing 10-2

PANEL = ERPX3

TPL example erp_base1.dat Output in SORT2 format.

(AREA = 9.000000E+00) E Q U I V A L E N T R A D I A T E D

FREQUENCY 2.000000E+00 4.000000E+00 6.000000E+00 8.000000E+00 1.000000E+01 1.200000E+01 1.400000E+01 1.600000E+01 **ERP MAX**

ERP 4.220276E-03 1.497942E-03 1.099377E-01 4.871353E-03 2.019563E+00 1.467790E-01 1.451253E+01 2.543595E-02 1.451253E+01

FRACTION 2.908022E-04 1.032172E-04 7.575362E-03 3.356652E-04 1.391599E-01 1.011395E-02 1.000000E+00 1.752689E-03

P O W E R ERP(dB) -2.374659E+01 -2.824505E+01 -9.588533E+00 -2.312350E+01 3.052574E+00 -8.333361E+00 1.161743E+01 -1.594552E+01

To obtain CSV output, an ASSIGN statement is added and the ERP case control is modified as follows: ASSIGN USERFILE='MYERP.CSV' UNIT=30 FORMATTED NEW DELETE ERP(PRINT,PUNCH,SORT1,FILTER=0.0,CSV=30) = ALL The resulting CSV file is easily manipulated into a graph using Microsoft Excel, or other programs that understand CSV format. Note that the graph shown in Figure 10-3 is based on a modified erp_base1.dat file that has a FREQ1 entry with more output frequencies. Note, the most signficant panel contributiosn switch at 31 and 33Hz. Listing 10-3

Subcase, 1000 " EQUIVALENT RADIATED POWER " " ALL IN 1 SUBCASE " " FIRST SUBCASE (1000) Equivalent Radiated Power , ERP , Area , 1.00000E+01, Frequency , ERPX0 , 2.00000E+00, 3.60158E-03, 4.00000E+00, 3.66840E-04, 6.00000E+00, 9.09168E-02, 8.00000E+00, 2.70249E-02, 1.00000E+01, 5.50420E+00, 1.20000E+01, 2.83194E-01, 1.40000E+01, 3.58258E+01, 1.60000E+01, 2.49801E-02,

Main Index

TPL example erp_base1.dat Output in CSV format (partial listing)

IN PANELS OF QUAD4S

SUBCASE 1000 ERP , 1.90000E+01, ALLPANEL , 7.82186E-03, 1.86478E-03, 2.00855E-01, 3.18962E-02, 7.52376E+00, 4.29973E-01, 5.03383E+01, 5.04161E-02,

Fraction , 1.00000E+01, ERPX0 , 1.00530E-04, 1.02395E-05, 2.53775E-03, 7.54341E-04, 1.53638E-01, 7.90474E-03, 1.00000E+00, 6.97266E-04,

Fraction , ERP(dB) , ERP(dB) 1.90000E+01, 1.00000E+01, 1.90000E+01 ALLPANEL , ERPX0 , ALLPANEL 1.55386E-04,-2.44351E+01,-2.10669E+01 3.70450E-05,-3.43552E+01,-2.72937E+01 3.99009E-03,-1.04136E+01,-6.97118E+00 6.33637E-04,-1.56824E+01,-1.49626E+01 1.49464E-01, 7.40694E+00, 8.76435E+00 8.54165E-03,-5.47917E+00,-3.66559E+00 1.00000E+00, 1.55420E+01, 1.70190E+01 1.00154E-03,-1.60241E+01,-1.29743E+01

"


Figure 10-3

TPL example erp_base1.dat plot in Microsoft Excel.

ERP for a Complicated Automotive Assembly The example shown in Figure 10-4 is used to demonstrate a more complicated system level automotive example. The loading is based on an engine event and the Equivalent Radiated Power is calculated for various panels that connect directly to the passenger compartment. Note that this example does not perform an acoustic response, but the ERP calculations provide insight into which panels would contribute to an acoustic response at various frequency levels.

Figure 10-4

Main Index

System Level ERP Example


GUI Support Neither SimXpert nor Patran currently support pre- or post-processing of ERP. However, the CSV output provides a convenient interface for users who want to generate plots using Microsoft Excel.

Main Index

232 MD Nastran 2010 Release Guide Frequency Dependent Rigid Absorber Properties

Frequency Dependent Rigid Absorber Properties Introduction The capability to model basic rigid porous absorber properties in acoustic response analysis was introduced in MD Nastran R2. It allows modeling for some types of absorbent material such as vehicle seat structures or lining materials with stiff carcasses. The absorber material is described, taking into account an equivalent fluid analogy, and is modeled as standard fluid elements using: • Standard fluid solid elements (CHEXA, CPENTA or CTETRA) • Connecting grid points with CD field defined as -1 • Referenced PSOLID entry with option PFLUID defined in field 8 • Referencing MAT10 entry where the ‘normalized admittance coefficient’ is defined in field 7

and equivalent values are used for density and bulk modulus The limitation for MD Nastran R2 implementation is that the normalized admittance coefficient cannot be defined to be frequency dependent. In MD Nastran 2010 the frequency dependency for this coefficient has been implemented. The new option FFLUID has been added for field 8 of PSOLID entry. Furthermore, the user must take care to define the normalized admittance coefficient in the MAT10 entry properly calculated at  = 1.0 .

Benefits The new capability introduced in MD Nastran 2010 allows defining an automatic calculation of a different value for the normalized admittance, depending on the value of the excitation frequency. The major benefit for the user is the possibility to describe, in a very simple way, the right absorbing behaviors of the rigid porous material at the different excitation frequencies. Note the user interface chosen to define the frequency dependency of the porous absorber allows: • Maintaining the backward compatibility (frequency independent porous absorbers can still be

modeled) • Defining one set of fluid elements to have a frequency-dependent normalized admittance

coefficient and another set to be frequency-independent

Theory The porous absorber properties are described by complex parameters (density and bulk modulus). The general implementation allows for the introduction of complex material properties for elements in the

Main Index


fluid which represent a region where sound energy is absorbed. It implies that if the complex density and bulk modulus are constant: Mass density  2

 =  r + i i

2



r + i  e = -----------------r



Br + Bi B e = ------------------Br

Bulk Modulus B 2

B = B r + iB i

2

Damping coefficient GE  GE = -----i r The normalized admittance coefficient is a function of the frequency: Bi Bi  =  ----- = 2f ----Br Br

Input As already mentioned, the equivalent fluid analogy allows using the same entries used to describe a standard fluid region. PSOLID and MAT10 entries are affected by this implementation.

PSOLID Entry A new option for field 8 (FCNT) of the PSOLID entry has been introduced. 1 PSOLID

2

3

4

5

6

7

8

9

PID

MID

CORDM

IN

STRESS

ISOP

FCTN

COROT

10

FAC FCTN

Main Index

Fluid element flag. (Character: “FFLUID” indicates a fluid element with frequency dependent rigid absorber properties, “PFLUID” indicates a fluid element, “SMECH” indicates a structural element; Default = “SMECH.”)


All the elements which refer to a PSOLID entry where the option FFLUID has been selected will be considered as rigid porous absorber with frequency dependent normalized admittance coefficient. MAT10 Entry No modification has been done in the format of this entry and no new options have been added. The only remark that has to be done is relative to the meaning of field 7 in case of frequency-dependent rigid porous absorber. 1 MAT10

2

3

4

5

6

7

MID

BULK

RHO

C

GE

ALPHA

8

9

10

In fact: • If the MAT10 entry is referenced in a PSOLID entry where FFLUID option is selected, the value

in the 7th field (ALPHA) is considered as the normalized admittance coefficient calculated at unit circular excitation frequency  = 1.0 ; • If the MAT10 entry is referenced in a PSOLID entry where PFLUID option is selected, the value

defined in field 7 (ALPHA) has no special meaning but it is only the normalized admittance coefficient calculated at the most appropriate excitation frequency (defined in order to have good results in the range of interest). The use of a nonzero value in field 7 of the MAT10 entry causes the generation of a damping matrix, because the normalized admittance coefficient is multiplied by the imaginary operator i. Consequently, the use of modal methods on the fluid are not appropriate and frequency response analysis must be carried out using the direct method, at least for the fluid.

Output There is no additional output that are generated for the elements used to describe the frequency dependent rigid absorber region.

Guidelines and Limitations No special modelling technique is required for the mesh representing the rigid porous absorber; the fluid mesh should be a continuum from air to rigid porous absorber where the elements of the rigid porous absorber simply discretize the form of the absorbing structure. Unlike the other absorber types in MD Nastran, the rigid porous absorber does not have to be on the wetted surface between fluid and structure, although it may be if desired. When using modal methods, for certain configurations where the bulk modulus becomes negative, the eigensolution may fail due to negative terms in the mass matrix. This has been reported in CR 1241950251 and will be fixed in the next release. For the moment the avoidance is to use the direct method of frequency response.

Main Index


Test Cases There are many test cases available in the TPL in subdirectory /tpl/fdr_absorb TPL problem fh8pr10.dat Consider the following unbounded fluid (air) and porous absorber medium domains as in Figure 10-5. An acoustic source is placed at the location indicated and the acoustic response (pressure) at the center of the fluid is monitored.

Figure 10-5 Using experimental methods the following properties have been determined. Density

Speed of Sound

Bulk Modulus

Air

1.225 + 0.0i *

340.0 + 3.4i

141595.8 + 2832.2i

Porous Absorber

3.8663 + 14.2204i

92.7076 + 70.2854i

– 171190.0 + 102356.3i

*Where i =

–1

The equations illustrated above have been used to calculate the equivalent properties to be used in the MAT10 entries. Two different calculations have been executed to check the effect of the new frequency dependent porous absorber properties implementation. 1. Frequency-independent materials have been considered and frequency of 250 Hz was selected to calculate the values of alpha for air and the porous absorber. Air Material

MAT10

Main Index

MID

BULK

RHO

1

141652.5

1.225

C

GE

ALPHA

0.0

31.41907


PSOLID

PID

MID

CORDM

1

1

0

MID

BULK

RHO

2

-232389.

56.16948

PID

MID

CORDM

2

2

0

IN

STRESS

ISOP

FCNT PFLUID

Porous Absorber Material

MAT10

PSOLID

C

IN

GE

ALPHA

-3.67804

-939.196

STRESS

ISOP

FCNT PFLUID

2. Frequency-dependent materials have been considered. The normalized admittance coefficients for air and porous absorbers have been calculated for  = 1.0 . AirMaterial

MAT10

PSOLID

MID

BULK

RHO

1

141652.5

1.225

PID

MID

CORDM

1

1

0

MID

BULK

RHO

2

-232389.

56.16948

PID

MID

CORDM

2

2

0

C

IN

GE

ALPHA

0.0

0.020002

STRESS

ISOP

FCNT FFLUID

Porous AbsorberMaterial

MAT10

PSOLID

C

IN

GE

ALPHA

-3.67804

-0.59791

STRESS

ISOP

FCNT FFLUID

Both the analyses have been executed using 2 different models in which 8 HEXA and 20 HEXA elements have been used. Notice that the values of bulk modulus, GE damping coefficient and alpha are all negative; this is a normal characteristic of the implementation. The response at the center of the air domain is calculated and the results compared with the same model run in the reference solution. Both HEXA-20 and HEXA elements are compared.

Main Index


The results using frequency-dependent rigid absorber properties fit completely with those from the reference solution. In fact, the increasing differences obtained using the original implementation for porous material properties departing from the reference excitation frequency (250 Hz in the example) disappear.

GUI Support Currently, neither Patran or SimXpert support the pre-processing definition of the FFLUID option in field 8 of the PSOLID entry. The post-processing capability of Patran and SimXpert is not affected by this implementation.

Additional Information and References Additional documentation regarding the implementation of rigid porous absorbers can be found in the following references: 1. M.E. Delany and E.N. Bazley, Acoustical Characteristics of Fibrous Absorbent Materials, National Physics Laboratory, Aerodynamics Division, NPL Aero Report Ac 37, March 1969. 2. J. Wandinger, Possible Implementations of Porous Absorbers in Nastran, MSC internal memo, April 2006. 3. M. Etchessahar, Caracterérisation mécanique en basses fréquences des matériaux acoustiques, Thèse de Doctorat, Université du Maine, 2002. 4. MD Nastran Quick Reference Guide 5. MD Nastran R2/R2.1 Release Guide

Main Index

238 MD Nastran 2010 Release Guide Dynamics - Monitor Points in Dynamic Solution Sequences

Dynamics - Monitor Points in Dynamic Solution Sequences Introduction Monitor points is a generic name for four types of user capabilities. The MD Nastran R1 Release Guide provided the most comprehensive discussion of these inputs. Briefly, 1. MONPNT1 – The MONPNT1 provides integrated loads at a user defined point in a user defined coordinate system. 2. MONPNT2 – The MONPNT2 provides element results (e.g., Stress, Strain, Force). 3. MONPNT3 – The MONPNT3 provides a summation of grid point forces at a user-specified monitor point. 4. MONDSP1 – The MONDSP1 allows for the sampling of a displacement vector to create a blended displacement response at a user-specified point and coordinate system. Prior to MD Nastran 2010, monitor points were only available in SOLs 101, 103, 144 and 146. Design of Monitor Points, 293 discusses the MD Nastran 2010 implementation in SOL 200. These sections discuss their application in the linear dynamic response solution sequences; i.e., SOLs 108, 109, 111, and 112.

Benefits MONPNT1 was first introduced in MSC.Nastran 2001 and provides the user with a way to extract the applied loading for a specified set of structural nodes (or aerodynamic elements for static or dynamic aeroelasticity). This enables the batch calculation of VMT (shear, moment, and torque) data for userspecified regions and locations. MONPNT2 provides a way of pinpointing a particular response for output, as opposed to finding it in a large OFP listing. MONPNT3 provides a summation of the internal loads and therefore, is useful in calculating resultant forces at a cut in the structure. The MONDSP1’s ability to provide an averaged displacement is seen as providing a qualitative assessment of the deflection of a structure.

Input There is no change to the input required to define the monitor points, only the solution sequences which are supported. The MD Nastran Quick Reference Guide provides guidance on specifying the MONPNT1, MONPNT2, MONPNT3, and MONDSP1 Bulk Data entries. The MONITOR Case Control command must be used to obtain output results in the dynamic solution sequences. The command provides options for frequency response results in terms of either the Real/Imag or MAG/Phase form.

Main Index


Output The output is limited to the .f06 file in all solution sequences except SOL 146 which also has op2 support.

Guidelines and Limitations 1. Dynamic monitor points are not available as design responses in SOL 200. 2. Inertia results are available for the MONPNT1 but have not been implemented for the MONPNT3. 3. The MONSUM feature can be used but is of limited utility when the MONSUM spans monitor types as described in Connectors (Ch. A) of this guide. 4. In Frequency Response analysis, the monitor point output is in SORT2 format.

Test Cases The following test cases are available in the TPL in directory /tpl/ue6_09a. There are four TPL files with the name sXXXm13d and four with sXXXm2 where the XXX is one of 108,109,111 or 112. The m13d files contain MONPNT1, MONPNT3 and MONDSP1 entries while m2 files contain MONPNT2 entries.

TPL example problem s111m13d.dat Example problem s111m13.dat is a modal frequency response model that contains MONPNT1, MONPNT3, and MONDSP1 entries. There are two subcases for a central load. The 1st subcase is shown in Figure REF.

Figure 10-6

Main Index

TPL example s111m13d.dat


A set of MONDSP1s are generated to define virtual point displacement results using an RBE3 derived from the GRIDs defined on the SET1 lists referenced on the AECOMP entry: MONDSP1 DISP2 123456 AECOMP PLATE3 SET1 3 SET1 4

THIS IS PLATE3 SET1 110901 110801

A DISPLACEMENT MONITOR POINT 52 1. 2. 3. 3 4 110902 110903 110904 110905 110802 110803

MONDSP1 DISPREF 123456 AECOMP POINT1 SET1 110902

THIS SHOULD MATCH GRID 110902 POINT1 4. 18. SET1 110902 110902

0.

123456

A set of MONPNT1s are generated to define integration load monitor points; the integration occurs over the GRIDs associated with the SET1 entries defined on the AECOMP entry: MONPNT1 MPT11 123456 AECOMP PLATE1 SET1 1 SET1 2

THIS IS PLATE1 SET1 110000 110505

THE FIRST MONPNT1 52 1. 2. 1 2 110010 111010 111000

MONPNT1 MPT12 123456 AECOMP PLATE2 SET1 1

THIS IS THE SECOND MONPNT1 PLATE2 20. 20. SET1 1 110000 110010 111010 111000

3.0

0.0

Finally, a set of MONPNT3s are generated to sum Grid Point Forces defined on the GRIDSET and ELEMSET. MONPNT3 MPT31 123456 SET1 5 SET1 6

THIS IS 5 110901 1100081

THE FIRST MONPT3 6 1. 119992 110903 110904 9999980

2. 110905

3.

MONPNT3 MPT41 123456 SET1 3 SET1 4

THIS IS 3 110901 110801

THE SECOND MONPT3 4 1. 110902 110903 110904 110802 110803

2. 110905

3.

Typical output for each output is shown below:

STATIC LOAD

SUBCASE 1 S T R U C T U R A L

M O N I T O R P O I N T (REAL/IMAGINARY)

D I S P L A C E M E N T S

MONITOR POINT NAME = DISP2 COMPONENT = 123456 GENERAL LABEL = THIS IS A DISPLACEMENT MONITOR POINT CP = 52 X = 1.000000E+00 Y = 2.000000E+00 FREQUENCY -----------1.000000E+02 2.000000E+02 3.000000E+02 4.000000E+02

Main Index

T1 -----------9.331630E-06 -5.560066E-08 9.721770E-06 -1.203002E-07 1.044643E-05 -2.072620E-07 1.165478E-05 -3.416177E-07

T2 -----------7.714264E-06 -4.663981E-08 8.044613E-06 -1.010250E-07 8.658742E-06 -1.743763E-07 9.684080E-06 -2.881529E-07

T3 -----------1.142239E-06 -6.488654E-09 1.186316E-06 -1.398631E-08 1.267942E-06 -2.394549E-08 1.403449E-06 -3.912291E-08

R1 -----------3.345541E-07 -1.900483E-09 3.474638E-07 -4.096495E-09 3.713716E-07 -7.013472E-09 4.110607E-07 -1.145883E-08

SUBCASE NO. Z = 3.000000E+00 R2 ------------4.731310E-07 2.687689E-09 -4.913880E-07 5.793319E-09 -5.251988E-07 9.918547E-09 -5.813276E-07 1.620524E-08

1 CD =

R3 -----------4.621815E-07 -3.033787E-09 4.847471E-07 -6.610803E-09 5.268791E-07 -1.152342E-08 5.976722E-07 -1.929935E-08

52


STATIC LOAD

SUBCASE 1 S T R U C T U R A L

M O N I T O R P O I N T (REAL/IMAGINARY)

I N T E G R A T E D

MONITOR POINT NAME = MPT11 COMPONENT = CX GENERAL LABEL = THIS IS THE FIRST MONPNT1 CP = 52 X = 1.000000E+00 Y = 2.000000E+00 FREQUENCY

INERTIAL

-----------1.000000E+02 2.000000E+02 3.000000E+02 4.000000E+02 STATIC LOAD S T R U C T U R A L

------------4.455447E-05 2.311694E-07 -1.835128E-04 1.957264E-06 -4.345861E-04 7.308116E-06 -8.349048E-04 2.028260E-05

EXTERNAL -----------1.306395E+01 0.000000E+00 1.306395E+01 0.000000E+00 1.306395E+01 0.000000E+00 1.306395E+01 0.000000E+00

I N T E G R A T E D

F R E E

FLEXIBLE INCREMENT ------------

GUST ------------

B O D Y M O N I T O R (REAL/IMAGINARY)

MONITOR POINT NAME = MPT31 COMPONENT = CMY LABEL = THIS IS THE FIRST MONPT3 CP = 0 X = 1.000000E+00 Y = 2.000000E+00 FREQUENCY -----------1.000000E+02 2.000000E+02 3.000000E+02 4.000000E+02

L O A D S (MONPNT1)

SUBCASE NO. Z = 3.000000E+00 TOTAL AERO -----------0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00 0.000000E+00

P O I N T

3 CD =

52

TOTAL -----------1.306390E+01 2.311694E-07 1.306376E+01 1.957264E-06 1.306351E+01 7.308116E-06 1.306311E+01 2.028260E-05

SUBCASE 1 L O A D S (MONPNT3) SUBCASE NO.

1

Z = 3.000000E+00

RESULTANT ------------3.689061E-01 -3.930317E-05 -3.910366E-01 4.639984E-04 -4.319148E-01 2.253416E-03 -4.992898E-01 6.649540E-03

GUI Support Patran Patran supports Monitor Point creation via the Flight Loads application. To access Flight Loads, it needs to be installed during the Patran installation, and the current analysis type must be Aeroelasticity. The figures in this section provide a general description of how to create the various Monitor Points described in this chapter. After the Monitor Points are created, the user can export them to a .bdf file for subsequent inclusion in a non-aeroelasticity solution. Finally, the user will have to change the Analysis Type back to Structures. Currently Patran does not support the post-processing of Monitor Point results.

Main Index


Main Index

Figure 10-7

Setting Analysis Type to Aeroelasticity for Monitor Point Access via Flight Loads

Figure 10-8

Flight Loads icon enables the flight loads menus

Figure 10-9

Monitor Point Action-Object-Type menu


Figure 10-10

Main Index

Example of Creating a MONPNT1


Main Index

Figure 10-11


Figure 10-12



Figure 10-13

Example of Creating a MONDSP1

Figure 10-14

Exporting Monitor Points from Flight Loads

SimXpert SimXpert does not currently support Monitor Point Creation.

Main Index

246 MD Nastran 2010 Release Guide Nonlinear Harmonic Response

Nonlinear Harmonic Response Note: Nonlinear Harmonic Response has been delivered with MD Nastran since MFD R1. However, it was undocumented until now.

Introduction There is a class of dynamic response analyses where a structure exhibiting nonlinearities is subjected to a harmonic excitation in which the response is essentially periodic. That is to say that the degree of nonlinearity in the system is light enough that the response may be described as sufficiently accurate by a combination of harmonic responses, i.e. periodic; this is achieved using a Fourier series. Some examples of this class of dynamic response problems are rotor/stator contact under abnormal running conditions, or an overload condition in an oscillating mechanism causing periodic contact. The response of such systems may exhibit multiple solutions in a steady-state vibration response scenario, possibly with amplitude jumps as the system moves from one frequency to another, such as might occur in a rotor that is increasing or decreasing in speed. These jumps reveal different behavior of the dynamic system with increasing or decreasing excitation frequency. The nonlinear harmonic response solution sequence uses the harmonic balance method to calculate the periodic response of a non-linear system under harmonic excitation. This requires the definition of a frequency domain problem in the presence of nonlinearities. The harmonic balance method assumes the steady-state response consists of a sum of sinusoidal responses finding the coefficients of the sinusoids to satisfy the equations of motion. Harmonic balance is only efficient if a small number of sinusoids are necessary to approximate the solution to a desired accuracy. This is why the nonlinearities in the system must be mild. As with any nonlinearity, it must only be present in the residual structure. However, this does not preclude the use of superelements or ASET degrees of freedom to perform dynamic reduction using CMS. In fact, this is a recommended technique in order to keep the number of degrees-of-freedom for harmonic balance to a minimum. Nonlinear harmonic response is available in the presence or absence of rotors, but there must be at least one degree-of-freedom defined on nonlinear force type entries such as the NLRGAP, NLRSFD, and NOLINi entries. Other types of nonlinearity that may be defined include the CBUSH2D element or indeed any elements having frequency dependent properties. MD Nastran R3, which incorporated SCA technology, added the possibility of creating a user-defined service whereby the NLRSFD entry is able to call external user-defined behavior to replace the standard NLRSFD behavior.

Main Index


Benefit Input The FMS Section If a user-defined nonlinear transient radial squeeze film damper is required, then the FMS CONNECT entry is required in conjunction with the NLRSFD and MATUDS. When a user-defined service (UDS) is to be utilized to describe the behavior of the NLRSFD type nonlinearity in nonlinear harmonic response, the FMS CONNECT entry is used with the SERVICE qualifier to make the connection between the GROUP name on the NLRSFD Bulk Data entry and the name of the external service. Refer to References [1.], [2.], and [3.] for more details. Executive Control Nonlinear harmonic response is available as SOL 128 or SOL SENLHARM. This is a complete solution sequence, based around linear direct frequency response (SOL 108) in which nonlinearities may be taken into account. Case Control The Case Control command NLHARM has been added for nonlinear harmonic response to reference the NLHARM Bulk Data entry. The existing NONLINEAR Case Control command may now also be used in nonlinear harmonic response to reference nonlinear force Bulk Data entries (NOLINi, NLRGAP, NLRSFD,…). Refer to Reference [1.] for a description of the NLHARM Case Control command. Bulk Data There are three new Bulk Data entries (NLHARM, NLFREQ, and NLFREQ1) relating specifically to a nonlinear harmonic response, one general new Bulk Data entry (TABLED5) and modifications to two existing Bulk Data entries (NLRGAP and NLRSFD). The NOLINi Bulk Data entries may now be used in a nonlinear harmonic response, but do not require any special remarks. NLHARM The NLHARM Bulk Data entry is used to define the parameters for nonlinear harmonic response.

Main Index

1

2

NLHARM

ID

3

4

5

SUBFAC NHARM NLFREQ

6

7

8

9

10


Field

Contents

ID

Identification number referenced by the NLHARM Case Control command. (Integer > 0)

SUBFAC

Factor for capturing sub-harmonic response. See Remark 3. (Integer > 1, Default = 1)

NHARM

The number of harmonics to include in the solution. See Remark 2. (Integer > 0)

NLFREQ

Identification number of the NLFREQ or NLFREQ1 entry specifying the forcing frequency list. (Integer > 0)

NLFREQ The NLFREQ entry is used to define the forcing frequencies for a nonlinear harmonic response. 1 NLFREQ

2

3

4

5

6

7

ID

F1

F2

F3

...

Fn

8

9

10

Field

Contents

ID

Identification number referenced by the NLFREQ field (field 5) of an NLHARM Bulk Data entry. (Integer > 0)

F1...Fn

Forcing frequency values in cycles per unit time. (Real > 0.0)

NLFREQ1 The NLFREQ1 entry is used to define the forcing frequencies for a nonlinear harmonic response by using a start frequency, a frequency interval and a number of intervals.

Main Index

1

2

3

4

5

NLFREQ1

ID

F1

DF

NDF

6

7

8

9

10

Field

Contents

ID

Identification number referenced by the NLFREQ field (field 5) of an NLHARM Bulk Data entry. (Integer > 0).

F1

First forcing frequency in the set. (Real > 0.0)

DF

Frequency increment. See Remark 1. (Real < > 0.0; Required)

NDF

Number of frequency increments/decrements. (Integer > 0, Default = 1)


TABLED5 The TABLED5 entry is used generally to define a value as a function of two variables for use in generating frequency-dependent and time-dependent dynamic loads. In nonlinear harmonic response it is used to define an NLRGAP whose force-penetration characteristics vary with frequency. 1 TABLED5

2

3

4

5

6

7

8

9

X(1)

TID(1)

X(2)

TID(2)

X(3)

TID(3)

X(4)

TID(4)

...

...

ENDT

10

TID

Field

Contents

TID

Table identification number. (Integer > 0)

X(i)

X value for the function specified by TID(i) (Real; no Default).

TID(i)

ID of a TABLED1, TABLED2, TABLED3 or TABLED4 defining the function Y for the given value of X. (Integer > 0; no Default).

Modifications have also been made to the existing NLRGAP and NLRSFD entries in support of nonlinear harmonic response. Refer to the MD Nastran Quick Reference Guide for further remarks on these entries.

Using Nonlinear Harmonic Response The nonlinear harmonic response solution uses a combination of sinusoids to form the steady-state response. Its limitation therefore is that it can only capture harmonic components, so any frequencies which are not pure sub- or super-harmonics of the excitation will be lost. It is also possible that either no solution exists (an unstable dynamic system), or that more than one solution is possible. The nonlinear system being studied may exhibit bifurcation or turning points; points for which a small incremental change in frequency results in more than one solution. In addition, the system may exhibit a step change in the response from one frequency to the next in what is referred to in the literature as “jump phenomena”. In its present form, the presence of bifurcation or turning points cannot be determined in nonlinear harmonic response analysis, and the resulting solution is just one of the possible states. Jump phenomena are revealed by examining the response curves. In a system with bearing clearance, like hydrodynamic or magnetic bearings, the stiffness of the system changes depending on whether the bearing forces overcome the clearance in the bearing, resulting in contact or no-contact conditions. Each of the contact/no-contact states may have essentially linear behavior, but the overall behavior is nonlinear if the system changes from one state to another. The simplest example of such a system is the Duffing oscillator. The Duffing equation is: 3 ax·· + bx· + cx + dx = f cos t

Main Index


and is defined in any text book on nonlinear dynamics. This equation exhibits jump phenomena for certain frequency values where the solution “jumps” from one significantly different value to another for a small change in frequency. To complicate matters, the jump differs depending on whether the change in frequency is positive or negative. When the system is nonlinear, there is also the possibility of sub- and super-harmonic responses. The response frequencies in linear harmonic analysis are the same as the forcing frequency. Permanent oscillations whose frequencies are a fraction of the forcing frequency (½, ¼, ...) may occur in a nonlinear system. These oscillations are known as subharmonic responses. Subharmonic responses require special conditions (e.g. particular damping characteristics and a non-symmetric stiffness) whereas superharmonic responses, i.e. permanent oscillations whose frequencies are a multiple of the forcing frequency (2, 3, …), are always present. Whether or not they show significant response levels depends on the damping in the system. These are complex phenomena which may exhibit jumps, further complicating matters. Refer to [4.] for a more complete discussion of sub and super-harmonic responses. A nonlinear harmonic response uses an iterative procedure to find the coefficients for the combination of sinusoids that form the steady-state response. Newton’s method of iteration is employed to solve a system of nonlinear algebraic equations. A trial solution is attempted for displacements and the corresponding forces in any NLRGAP, NLRSFD, or NOLINi entries are calculated from the user- supplied data on the relevant tables. The residual forces in the system are calculated and a convergence error is obtained. Based on the size of the convergence error, the solution is either accepted or an updated displacement scaling is calculated and the new displacements calculated. The sequence loops until either a diverging system is detected or convergence obtained.

Controlling Nonlinear Harmonic Response The interface to nonlinear harmonic response is driven via only the few inputs defined above. The nonlinear characteristics are defined on NOLINi, NLRSFD, or NLRGAP Bulk Data entries and accompanying tables. The sequence of excitation frequencies is defined on NLFREQ or NLFREQ1 entries and harmonic response control data supplied on the NLHARM entry. This allows specification of the number of harmonics and subharmonics to consider for the nonlinear harmonic response analysis, as well as referencing the excitation frequency Bulk Data entries NLFREQ or NLFREQ1. PARAM, MXICODE0, 5 In nonlinear harmonic response analysis, if the solution fails to converge more than MXICODE0 times in succession, a new trial displacement vector is calculated. MXICODE0 allows the number of successive failed convergences to be modified before a new trial displacement vector is calculated. (Default is 5). PARAM, NHPLUS, 20 In nonlinear harmonic response analysis, in order to avoid aliasing in the calculation of the Fourier coefficients, a certain number of extra evaluation points are used. NHPLUS allows the number of extra points to be defined.

Main Index


A literature search suggests this technique comes from reference [6] where the number of time steps, S, selected should be in the range (2K-1) S 3(2K-1) and K is the number of frequencies present in the signal. PARAM, NLHTOL, 1.0E-5 During the iteration procedure of nonlinear harmonic response, the norm of the residual load vector for the current step is divided by the norm of the residual load vector for the previously converged step. This value is then compared with NLHTOL. If the value is smaller than NLHTOL, the system is assumed to have converged. (Default is 1.0E-5). PARAM, NLHTWK, 1.1 In nonlinear harmonic response analysis, if convergence is not obtained, a line search procedure is initiated to calculate a scaling factor for the displacement vector from which updated nonlinear loads are subsequently calculated. If the solution fails to converge more than 5 times in succession (modifiable by PARAM,MXICODE0), a new trial displacement vector is calculated using a push-off factor the size of which is defined by NLHTWK. (Default is 1.1).

Handling Nonconvergence in Nonlinear Harmonic Response During the ascending or descending sequence of excitation frequencies defined on the NLFRQi entries, if instability is encountered at a particular frequency, the solution may fail to converge at that frequency. Nonconvergence may be attributed to several causes, and the possibility must always be considered that there is simply no solution to the system at a particular frequency because the system has become dynamically unstable. In most cases of nonconvergence that is not attributed to dynamically unstable conditions, either the number of harmonics or the subharmonic content is insufficient, or the system has reached a bifurcation or turning point. Try increasing the number of harmonics or subharmonics (NLHARM entry) as well as adjusting the parameters described above. If none of these are successful, the system may have struck a bifurcation point. Try adjusting the excitation frequencies slightly. For example, if using the following excitation frequencies: 5.0, 10.0, 15.0, 20.0…etc., try adjusting these to 5.1, 10.1, 15.1, 20.1. In the current implementation, there is no automatic treatment for possible bifurcation points, and the subject of using a continuation strategy is under discussion for a future development. In the case of nonconvergence, the response quantities are set to zero, and the calculation continues to the next excitation frequency in the sequence retaining the initial conditions of the solution from the last converged frequency. If the solution at the next excitation frequency does not converge, the same procedure is followed until a converged solution is found. There may come a time when it is judicious to change the initial conditions, particularly when the next excitation frequency becomes distanced from the last converged frequency after a sequence of failed attempts to converge excitation frequencies. In this situation, where the initial conditions for an excitation frequency have become somewhat distanced from the previously converged excitation frequency, it may not mean very much physically to continue to use the initial conditions from that previously converged excitation frequency.

Main Index


Therefore, it may be favorable to start from zero conditions as always happens for the first frequency of an analysis starting from scratch. There is some difficulty in deciding how far away from the previously converged excitation frequency is acceptable to return to zero initial conditions. There is presently no logic for handling this situation and the only course available is to reset the initial conditions to zero by starting a completely new analysis with a starting frequency somewhere after the instability point.

Example A nonlinear harmonic response was developed to study rotor/stator contact problems, but the presence of a rotor is not obligatory. The capability may be used to study any periodic response to a harmonic excitation in the presence of light nonlinearities. The following example taken from [6.] shows a rotor bearing system in which an out-of-balance load excites a rigid overhung disk mounted on a flexible shaft turning in bearings exhibiting nonlinear stiffness.

The round solid shaft of diameter 0.1 metres is 1.0 metre long and runs in two bearings, one located at one end of the shaft while the other is positioned just inboard of the disk such that the disk is overhung. The bearings are mounted on an isolation material that exhibits nonlinear stiffness varying with a cubic law. The overhung massive rigid disk exhibits a small eccentricity in its mass distribution. Shaft Material Properties: Young’s modulus

2.07E+11 Nm-2

Density

7750 kgm-3

Disk Properties:

Main Index

Mass of disk

2000 kg

Inertia (polar)

200 kgm2

Inertia (diametral)

100 kgm2


Bearing Stiffness and Damping (Symmetrical) Linear stiffness

1.5E+7 Nm-1

Nonlinear stiffness

1E+12d3 Nm-3 (d is the value of displacement)

Damping

1.72E+4 Nsm-1

Firstly, the analysis is run in a linear direct frequency response with linear-bearing properties. The analysis is then repeated in the nonlinear harmonic solution sequence, still with linear bearing properties and the answers compared. Finally, the nonlinear bearing stiffness properties are added, and the response is compared against theory [7.] The bulk data for the model is shown. This data is common to all runs and for the subsequent files is assumed to be saved to a file called common.dat. PARAM,GRDPNT,0 PARAM,COUPMASS,1 $ $ ROTOR ROTORG,1,1,2,3,4 RGYRO,66,SYNC,1,FREQ RSPINR,1,1,4,FREQ,1. GRID,1 GRID,2,,.5 GRID,3,,1. GRID,4,,.99 CBEAM,1,1,1,2,,1. CBEAM,2,1,2,4,,1. CBEAM,3,1,4,3,,1. PBEAM* 1 1 * 4.9087390-6 + .68 .68 MAT1,1,2.07+11,,.27,7.75+3 $ $ DISK MASS & INERTIA CONM2,6,3,,2000. ,200.,,100.,,,100. $ $ STATOR GRID,5 GRID,6,,.99 $ $ ROTOR TO STATOR CONNECTION RBE2,941,5,123456,1 RBE2,953,6,123456,4 $ $ GROUND GRID,105 GRID,106,,.99 $ $ BEARING DAMPING CDAMP2,20442,1.72+4,105,2,5,2 CDAMP2,20443,1.72+4,105,3,5,3 CDAMP2,20552,1.72+4,106,2,6,2 CDAMP2,20553,1.72+4,106,3,6,3

Main Index

7.8539820-3 9.8174780-6

4.9087390-6


$ $ REMOVE SINGULAR DOFS SPC1,1,14,2,3,5,6 SPC1,1,123456,105,106 $ $ OUT OF BALANCE FOR ROTOR DLOAD,77,1.,60.,1001,60.,1002 RLOAD2,1001,1001,,,1000 RLOAD2,1002,1002,,1002,1000 DAREA,1001,2,2,9.4286-5 DAREA,1002,2,3,9.4286-5 DPHASE,1002,2,3,-90. TABLED4,1000,0.,1.,0.,1000. ,0.,0.,39.47842,ENDT

Firstly, a direct linear frequency response analysis is run to allow the results to be compared with the nonlinear harmonic response with nonlinear forces defined with linear behaviour. Below is the case control and additional bulk data required for the linear frequency response. SOL 108 CEND LINE=9999999 DISP(SORT2,PHASE)=ALL SPC=1 RGYRO=66 DLOAD=77 FREQ=88 BEGIN BULK include ‘common.dat’ $ $ BEARING STIFFNESS CELAS2,10442,1.5+7,105,2,5,2 CELAS2,10443,1.5+7,105,3,5,3 CELAS2,10552,1.5+7,106,2,6,2 CELAS2,10553,1.5+7,106,3,6,3 $ FREQ1,88,9.549296,.0530516,240 ENDDATA

Now the same problem is run in a nonlinear harmonic response which solves the problem in an iterative manner. Half the stiffness of the linear bearings is replaced with nonlinear force definition on NOLIN1 entries. The force-displacement relationship is defined as linear. Below is the case control and additional bulk data required for the linear harmonic response in SOL 128. SOL 128 CEND LINE=9999999 DISP(SORT2,PHASE)=ALL SPC=1 RGYRO=66 DLOAD=77 NONLINEAR=1000 NLHARM=2000 BEGIN BULK include ‘common.dat’ $ $ LINEAR BAERING STIFFNESS (HALVED)

Main Index


CELAS2,10442,7.5+6,105,2,5,2 CELAS2,10443,7.5+6,105,3,5,3 CELAS2,10552,7.5+6,106,2,6,2 CELAS2,10553,7.5+6,106,3,6,3 $ $ LINEAR BEARING STIFFNESS (HALF PROVIDED BY NOLIN1) NOLIN1,1000,5,2,-1.,5,2,1001 NOLIN1,1000,5,3,-1.,5,3,1001 NOLIN1,1000,6,2,-1.,6,2,1001 NOLIN1,1000,6,3,-1.,6,3,1001 TABLED1, 1001, , -1.0, -7.5+6, 1.0, 7.5+6, ENDT $ NLFREQ1,88,9.549296,.0530516,240 NLHARM,2000,1,1,88 $ ENDDATA

When these two linear analyses are run, the magnitude response of GRID point 3 in the Y direction looks like this:

The linear frequency response curve and the nonlinear harmonic response curve are superposed. This shows the linear problem can be solved using the 2 different methods (SOLs 108 and 128) and the response is the same.

Main Index


Now the bearing stiffness is replaced by a cubic stiffness defined by NOLIN3 and NOLIN4 entries. Here is the case control and additional bulk data required for the nonlinear harmonic response in SOL 128. SOL 128 CEND LINE=9999999 DISP(SORT2,PHASE)=ALL SPC=1 RGYRO=66 DLOAD=77 NONLINEAR=1000 NLHARM=2000 BEGIN BULK include ‘common.dat’ $ $ BEARING STIFFNESS CELAS2,10442,1.5+7,105,2,5,2 CELAS2,10443,1.5+7,105,3,5,3 CELAS2,10552,1.5+7,106,2,6,2 CELAS2,10553,1.5+7,106,3,6,3 $ $ CUBIC NONLINEAR STIFFNESS (TENSION) NOLIN3,1000,5,2,-1+12,5,2,3. NOLIN3,1000,5,3,-1+12,5,3,3. NOLIN3,1000,6,2,-1+12,6,2,3. NOLIN3,1000,6,3,-1+12,6,3,3. $ CUBIC NONLINEAR STIFFNESS (COMPRESSION) NOLIN4,1000,5,2,-1+12,5,2,3. NOLIN4,1000,5,3,-1+12,5,3,3. NOLIN4,1000,6,2,-1+12,6,2,3. NOLIN4,1000,6,3,-1+12,6,3,3. $ $ Spin up NLFREQ1,88,9.549296,.1591549,240 $ Spin down $NLFREQ1,88,47.74648,-.1591549,240 NLHARM,2000,1,1,88 $ ENDDATA

The analysis is run in two parts, the first starting from a cyclical frequency of 9.55 Hz (60 radians/second) with an increasing frequency up to a frequency of 47.7 Hz (300 radians/second); this simulates a spin-up event where each frequency is considered in its steady state condition. The second part of the analysis simulates a spin-down event starting from a cyclical frequency of 47.7 Hz with a decreasing frequency. The magnitude of the Y direction response of GRID point 3 is plotted against rotational frequency with the resulting two curves:

Main Index


Clearly there is a zone of bifurcation just before 23 Hz; that is to say, after 23 Hz, two possible states exist. In the spin-down case, the solution jumps from one solution to the other and then retraces the spinup response curve; an unstable condition exists between these two. The results are in good agreement with those reported in Reference [7.] References 1. MD Nastran Release Guide 2. MD Nastran R3 SCA Service Guide 3. MD User’s Guide User Defined Services 4. Shock and Vibration Handbook, Page 4-8, 3rd Edition, Cyril M. Harris, McGraw Hill, 1987. 5. Frequency-domain analysis of nonlinear circuits driven by multi-tone signals, A.Ushida and L.O.Chua, IEEE Trans. Circuits Syst., Vol. CAS-31, pp. 766-778, Sept. 1984. 6. A User Guide for Nonlinear Harmonic Response 7. Steady-State Response of Continuous Nonlinear Rotor-Bearing Systems Using Analytical Approach, J.W. Zu and Z.Y. Ji, Journal of Engineering for Gas Turbines and Power, ASME, 120, pp 751 - 758, 1998

Main Index

258 MD Nastran 2010 Release Guide Enhancements to the Frequency Response Function (FRF) and FRF Based Assembly (FBA) Capability

Enhancements to the Frequency Response Function (FRF) and FRF Based Assembly (FBA) Capability Introduction The FRF / FBA (Frequency Response Function / FRF Based Assembly) capability was first introduced in MD Nastran R2. This capability facilitates the computation of the FRFs of individual components and also the subsequent computation of the FRFs of an assembly of such components from their individual FRFs. The capability available in MD Nastran R2 had several limitations that were removed by major enhancements made in MD Nastran R3. With a view to enhance user convenience further, the following improvements have been made in MD Nastran 2010: • Support for test FRF components in the FBA process • Expanded output from FBA job giving details of the FRF components comprising the FRF-

based assembly • Allow the FBA process to handle a single FRF component without any connection data • Enhanced subcase IDs for user-specified loads in FRF generation and FBA job output • Enhancements to FRF Case Control command • Enhancements to FRFCOMP Bulk Data entry to support test FRF components

Details of these enhancements are discussed in the following sections.

Benefits The enhancements made in MD Nastran 2010 for the FRF/FBA capability greatly enhance user convenience and makes the feature an excellent tool for practical situations and a viable tool for Noise and Vibration studies.

Support for Test FRF Components in the FBA Process The FBA process in MD Nastran 2010 offers support for test FRF components. The fact that an FRF component is a test component rather than a Nastran-generated component is indicated by the FRFCOMP Bulk Data entry for that component. The FRFCOMP entry has been enhanced for this purpose, as is described later in this section. The FRF and other data for a test FRF component is expected to be resident on a Universal File (UF). The information on the UF is grouped by so-called Universal Dataset Numbers (UDNs). Details of the various UDNs and their formats can be obtained from the following website: http://www.sdrl.uc.edu/universal-file-formats-for-modal-analysis-testing-1

Main Index


As far as the FBA process is concerned, the heart of the information on the UF for a test FRF component is in UDN 58 which contains FRF data for that component. When an FBA job involves test FRF components, an ASSIGN UNVFILE specification is required in the File Management Statement (FMS) Section to identify the physical file and the Fortran unit number for the UF for each test FRF component. Details will be clear from the description of the enhanced FRFCOMP Bulk Data entry given in the MD Nastran Quick Reference Guide.

Expanded Output from FBA Job Giving Details of the FRF Components Comprising the FRF-Based Assembly The output from an FBA job has been expanded in MD Nastran 2010 to give details of the FRF components that comprise the FRF-based assembly. The information given consists of the following: • Component count • FRF component ID and name • How the FRF information for the component was generated (from a previous or current Nastran

execution or from test) • Medium on which the FRF information resides (database, OP2 file or Universal File, with unit

numbers identified for the latter two options)

Allow the FBA Process to Handle a Single FRF Component Without Any Connection Data In MD Nastran R3, the FBA process would not allow a configuration that did not involve some sort of connection data (via FRFCONN and/or FRFFLEX/FRFRELS Bulk Data entries). This is a meaningful requirement when more than one FRF component is involved. However, this is not a reasonable requirement when only one FRF component is involved, since such a component may or may not involve connection data. In MD Nastran 2010, the FBA process does allow a single FRF component without any connection data after issuing a User Warning Message about the lack of connection data. This feature is extremely helpful in performing load studies and Transfer Path Analysis (TPA) for a single FRF component.

Enhanced Subcase IDs for User Specified Loads in FRF Generation and FBA Job Output When the user specifies a dynamic load via the DLOAD Case Control request in an FRF generation or FBA job, the number of excitations for which the results are output is determined by the XITOUT keyword in the FRF Case Control command. As explained under the description of the FRF Case Control in the MD Nastran Quick Reference Guide, if XITOUT = USER is specified (or assumed by default), the FRF results are output for the following excitations: • A separate excitation for each individual DOF that has a non-zero load specified for it

Main Index


• An excitation representing the total load

Thus, if a DLOAD Case Control request involves nonzero load values on N DOFs, then XITOUT = USER gives results for (N+1) excitations, with the first N in such excitations representing individual and separate loads on the N DOFs and the (N+1)th excitation representing the total load. If XITOUT = USERTOTL is specified, then the results are given only for the (N+1)th excitation representing the total load. In MD Nastran R3, the subcase IDs for the above (N+1) excitations were identified by sequential numbers 1 through (N+1) for the XITOUT = USER case and by a subcase ID of 1 for the XITOUT = USERTOTL case. If the loading involved multiple subcases, then the above sequential numbering scheme was continued further across the subcases. This made it very difficult to associate a particular excitation subcase number in the output with the user-specified subcase associated with it, particularly when multiple subcases were involved. This led to a lot of confusion in interpreting the results. In order to avoid the above confusion, subcases in MD Nastran 2010 are numbered using a coded scheme. Under this scheme, each of the (N+1) subcases mentioned above is given a coded subcase ID of the form xxxxyyyy. Here xxxx is the user subcase ID corresponding to the DLOAD under consideration. For the first N excitations described above, yyyy has values ranging from 1 through N (with leading zeros where appropriate). For the (N+1)th excitation mentioned above, the coded subcase ID is of the form xxxx9999. This makes it very easy and convenient for the user to associate a particular excitation subcase number in the output with the user-specified subcase associated with it.

Enhancements to FRF Case Control Command Several enhancements have been made to the FRF Case Control command. These are described below and may also be found under the description of this command in the MD Nastran Quick Reference Guide. Enhancements to the ASMOUT Keyword In MD Nastran R3, the ASMOUT keyword could be specified to request output in the FBA process for either all of the FRF components comprising the FRF assembly (ASMOUT = COMP, the default), or for all of the FRF components plus the assembled FRF configuration considered as a separate entity (ASMOUT = ALL). Enhancements have been made in MD Nastran 2010 to allow for several additional output requests. A description of all of the options available for the ASMOUT keyword is given below: ASMOUT = CONNINFO • Terminate the FBA job after generating the FRF component connection information output

without performing any further FRF assembly operations ASMOUT = COMP (Default) • Generate output from the FBA process for all of the individual FRF components comprising the

assembly. ASMOUT = ALL

Main Index


• Generate output from the FBA process not only for all of the individual FRF components

comprising the assembly, but also for the assembled FRF configuration considered as a separate entity. ASMOUT = ASSEMBLY • Generate output from the FBA process only for the assembled FRF configuration considered as

a separate entity. This is equivalent to specifying ASMOUT = 0 (see later). ASMOUT = n • n is an integer with the following meanings:

n=0 Generate output from the FBA process only for the assembled FRF configuration considered as a separate entity. This is equivalent to specifying ASMOUT = ASSEMBLY (see earlier). n>0 Generate output from the FBA process only for those FRF components of the assembly whose IDs are specified by SET ID n. n<0 Generate output from the FBA process only for that single FRF component of the assembly whose ID is given by |n|. ASMOUT = cname • Generate output from the FBA process only for that single FRF component of the assembly

whose name is given by cname. Addition of New LOADLBL Keyword A new keyword called LOADLBL has been added to the FRF Case Control command. This keyword can be used to control the load labels in the output of both FRF generation and FBA jobs. Details are given below: LOADLBL = STD (Default) • The load labels in the output of the FRF generation and FBA jobs explicitly identify the grid (or

scalar) point and its component where the load is applied. LOADLBL = ALT • The load labels in the output of the FRF generation and FBA jobs identify the grid (or scalar)

point and its component where the load is applied by using the following notation: GGGGGGGG:+C where GGGGGGGG is the grid (or scalar) point ID and C indicates the component where the load is applied. C may have the following values: X Indicates grid point component 1 or scalar point

Main Index


Y Indicates grid point component 2 Z Indicates grid point component 3 RX Indicates grid point component 4 RY Indicates grid point component 5 RZ Indicates grid point component 6 LOADLBL = ALTX • Same meaning as ALT except that the load labels also identify whether the load applied is an unit

load or an user load

Enhancements to FRFCOMP Bulk Data Entry In MD Nastran R3, Field 4 of the FRFCOMP Bulk Data entry was allowed to have two values, DB or OP2, to indicate whether the FRF and other data for a Nastran-generated FRF component to be employed in an FBA process is resident on the database or on an OP2 file, respectively. In MD Nastran 2010, Field 4 may also have the value of UF to indicate that the FRF component is a test component with its FRF and other data resident on an Universal File (UF). In this case, Field 5 of the entry indicates the Fortran unit number for the UF and Fields 6 and 7 give the length and force scale factors that are to be applied to the FRF quantities on the UF. An ASSIGN UNVFILE specification is required in the File Management Statement (FMS) Section of the FBA job to identify the physical file and the Fortran unit number for the UF. Details will be clear from the description of the enhanced FRFCOMP Bulk Data entry given in the MD Nastran Quick Reference Guide.

Main Index


EFEA/EBEA (Pre-Release) The Energy Finite Element Analysis (EFEA) and Energy Boundary Element Analysis (EBEA) provide a powerful solution for high frequency acoustics. In contrast to traditional FEA solvers that use displacements as the primary variables, the EFEA methods use energy based variables which enables noise and vibration simulations at much higher frequencies than those attained by conventional FEA analysis. The EBEA solution provides airborne noise loads for use by the EFEA solution. The combination of EBEA and EFEA methods can be used to predict the interior noise levels in a vehicle due to exterior acoustic sources. These new solvers are provided through collaboration with Michigan Engineering Services and are provided as a pre-release in MD Nastran 2010. Please see the EFEA/EBEA User’s Guides included with the MD Nastran 2010 release for more information.

Main Index

264 MD Nastran 2010 Release Guide EFEA/EBEA (Pre-Release)

Main Index

Chapter 11: Loads Management

11

Loads Management



Main Index


Loads Management

266 MD Nastran 2010 Release Guide Loads Management

Loads Management Pre-Release in MD Nastran 2010.

Introduction The internal loads management process of the aircraft design which normally involves static analysis of the airframe due to various loading conditions, poses a number of challenges to the user on the analysis engine. This chapter describes challenges specific to this process and presents an extension to the Statics solution of MD Nastran that addresses these challenges. Some of the challenges involved include: Multiple FEM Models There may be a number of vehicle level FEM models that have to be analyzed and whose results have to be somehow combined. For example, there may be models with and without doors. There may also be models with and without landing gear. Analysis results related to these models will have to be combined to produce critical loads used in subsequent steps. Multiple Loading Conditions Internal loads analysis process may include more than 10,000 unique load cases due to flight maneuvers, ground load cases, cabin pressure, cargo loads, and thermal loads. Loads from these various sources will have to be combined to achieve critical loads used for design. Revisions The loads passed on to the internal loads team frequently change. Changes may be due to model changes or new maneuver loads from the external loads process. Revisions normally do not affect the entire set of loads but only a small fraction—up to 10% of the load cases. Figure 11-1 shows the internal loads management process as it relates to the FEM model analysis. The

traditional statics analysis in Nastran does cover the steps highlighted in green as part of an end-to-end solution, but it does not provide users with access to independent steps of this process. For example, in traditional statics analysis, the user cannot change few load cases and perform data recovery without having to rerun all load case. The solution presented in this section provides users with a lower level of access to individual steps in the Statics solution in MD Nastran. So changes in load cases or solution vectors do not necessarily require a complete rerun of the model. This level of control can result in significant improvements in overall process of internal loads management.

Main Index

CHAPTER 11 267 Loads Management

Model Building Generic Properties

Actual Properties

Generate External Loads

Model Check

Combine Loads

Solve

Load Case Changes

Change Management Data Recovery

Figure 11-1 Overview of Solution Functionality The key functionality that supports the internal loads process is the componentization of the statics solution in MD Nastran that allows for the close alignment of the solution steps with the engineering process steps. Figure 11-2 shows the components of the Statics solution that can now be individually called upon. It also shows the dependencies the components may have on one another.

Main Index


The internal loads solution capabilities can be categorized in the following groups: Componentized MD Solution Read FEM Model in DB Build Matrices Factorize

Read Load Cases in DB Solve Load Cases

Generate Results

Combine Load Cases

Combine Solution Vectors

Delete Load Cases

Figure 11-2

Traditional End-to-End Solutions

Loads Management Loads can now be partially modified without the need to rerun the analysis with the entire set of loads. Load cases can be incrementally added, deleted, or combined. The user can also get a report on the current contents of the database in terms of loads.These operations can be driven through a high level command language described in the next section. Solution Vector Management Similar to how loads are individually managed, users also have full control in generating individual solution vectors associated with load vectors. Individual solution vectors can be generated, combined, or deleted. The user can also get a report on the current contents of the database in terms of solution vectors. These operations can also be driven through a high level command language. Data Recovery Users can generate results on a given subset of the model and/or a subset of load cases. So when a subset of loads are modified, it is not necessary to regenerate all results. Data recovery operations can also be driven through a high level command language.

Main Index

CHAPTER 11 269 Loads Management

References The complete description of the user interface, data recovery, etc. can be found in the MD Nastran 2010 Loads Management User’s Guide.

Main Index


Main Index

Chapter 12: Optimization

12

Main Index


Optimization



MultiOpt (Multiple Model Optimization)



Part Superelement Optimization Enhancements



Optimization - Invariant DRESP3 Gradients



Design of Monitor Points



Parallel Sensitivities



DTABLE Enhancement for Dynamic Analysis



Constants with DTABLE2



New Optimizer - IPOPT



Topology and Topometry Enhancements



Optimization of Nonlinear Structural Responses Phase 2 (Prerelease)



Build External Servers Using the SCons Tool



Deactivation of Original Design Sensitivity (DSA)

272 MD Nastran 2010 Release Guide MultiOpt (Multiple Model Optimization)

MultiOpt (Multiple Model Optimization) Introduction The MultiOpt (Multiple Model Optimization) capability was created in order to combine two or more related optimization tasks into a single combined optimization task. This enables support for the ability to perform design optimization when the design conditions are produced by two or more MD Nastran design models. The MultiOpt application initiates servers that start the processing of the separate design models up to the point where the optimization is to occur. At this point, a new server is invoked to merge the design information, perform the optimization and partition the results. The servers running the individual models are then resumed in a design loop that is terminated when either convergence is achieved or the maximum design cycles are reached. A flow chart of this process with two design models is given in Figure 12-1. Initial Design

Model 1

Model 2

Structural Analysis

Structural Analysis Check Convergence

Sensitivity Analysis

Sensitivity Analysis

Merge Approximate Models

Approximate Optimization

Figure 12-1

Main Index

Improved Design

Partition Constraints/Responses

CHAPTER 12 273 Optimization

The boxes ‘Merge Approximate Models’, ‘Approximate Optimization’, and ‘Partition Constraints/Responses’ are driven by a subDMAP that is invoked by a MutiOpt created input deck (i.e, the user does not need to create or even know about this deck).

Benefits The ability to merge multiple design models allows the user to have separate models that differ in their topology or in their analyses but still perform a combined optimization. One scenario might be if different variants of an aircraft share a common wing design but have different fuselages (standard and stretch configurations). It would be difficult to design this with the previous version of SOL 200, but it is readily achievable with this capability. Another scenario is one where a detailed model of a component is available and can be used to match analysis data with test results. At the same time, a less detailed model of the same component is included in a global model that is being used to perform optimization with global constraints, such as flutter speed. MultiOpt can be used in this case to perform both optimizations simultaneously and thereby maintain a common design.

Input The process of combining the models and performing the optimization is performed by a MSC.Toolkit application referred to as MultiOpt (Multiple Optimization). The user can combine up to five separate design models using this process. Each of the models has its own data deck that is complete to the extent that it could be run “stand-alone” in MD Nastran SOL 200. The following changes need to be made in each of these separate input files for a MultiOpt submittal: 1. A DESMOD Case Control command (see below) needs to be inserted in each model of the form: DESMOD = model Where model is a unique, user specified name of up to eight characters that designates the model 2. The DOPTPRM entry in the separate models control parameters that are used by the optimizer and others that are used in the iterative process. It is recommended that an identical DOPTPRM be used in each model. The DOPTPRM in the first model controls what is used by the optimizer; e.g., OPTCOD, while convergence parameters and DESMAX are controlled by the local DOPTPRM entry. 3. If the objectives are to be combined, the first model must have its DESOBJ request point to a DRESP2 that contains the structure of the combined objective function. This is expanded upon below. Invoking MultiOpt The most basic way to invoke MultiOpt is using a command line of the following form: MultiOpt nastran n deck1.dat … deckn.dat coef c1 c2 ..cn mem m1 m2..scr=sopt [options]

Main Index


A more flexible form of the input, which supports all of the previous features, and also allows for running jobs in parallel across different machines is: Multiopt file.xml Where file.xml is of the form: where:

Option

Main Index

Description

nastran

A name to invoke the relevant Nastran executable (e.g., /nast/bin/nast2008)

N

Number of models to be merged (1 < n < 6)

Jobname=

For the xml form, indicates the subsequent data is a job name

deck1.dat

Name of the first input data model

deckn.dat

Name of the nth input data model

coef

A flag to indicate the following input is objective weighting coefficients

coef=

For the xml form, indicates the subsequent data is a coefficient for this model

c1

Coefficient that provides the objective weighting for the first model (Default = 1.0)

c2

Coefficient that provides the objective weighting for the second model (Default = 0.0)

Cn

Coefficient that provides the objective weighting for the nth model (Default = 0.0)

Mem

A flag to indicate the following input are memory requests for the individual models. If this flag is not used all models require the same amount of memory.

Mem=

For the xml form, indicates the subsequent data is a memory request for this model

m1

Memory for the first model and also for the merge operation in the basic MultiOpt invoking


Option

Description

m2

Memory for the second model

mn

Memory for the nth model

Mm

Memory for the merge operation

Node=“platform”

For the xml form, indicates the this job is to be run on the indicated computer. Default is to run on the local platform

Blocking=“bopt”

For the xml form, indicates whether that job is to be run in parallel or serially. Blocking =yes (Default) runs the job serially while blocking=no enables running the job in parallel.

Scr=“sopt”

Option for scr=yes or no. Scr=yes is recommended.

args=“value”

Any command line option of the form args=value that is a valid Nastran command line option.

Note:

The user is required to specifically identify the directory where the executable resides. This would be something like /nast/bin/nast2000t1. This limitation is due to the fact that the MultiOpt has been written using FORTRAN and the utilities required for embedding the Nastran path within the manager have not been identified.

Combining the Objectives Combining objectives from several models relies on a DRESP2 that has to be constructed with some specific rules: 1. The DRESP2 must have a “DTABLE” with nmod (the number of models) LABLi values. The value specified for the first LABL1 must be 1.0 and the subsequent LABLi values must be zero. In this way, the objective of the first model is simply the first response. 2. The DRESP2 must have either nmod DRESP1 quantities or nmod DRESP2 quantities. It is not possible to mix DRESP2 and DRESP1 responses in the combined objective. The DEQATN that corresponds to the DRESP2 performs a linear addition of the responses: COBJ =

 C i  OBJ

Any other form for specifying the combined response will produce unpredictable results. If no combining of objectives is desired, the COEF flag can be omitted from the input or, if COEF is specified, c1 must be 1.0 and c2,c3..cn must be 0.0.

Main Index


Output The separate models each provide their separate .f06 files and any other outputs that would be expected from a SOL 200 run. There is also a merge.f06 file produced from the optimization portion of the process and could provide some insight into how the optimization is progressing and highlight any problems. The toolkit application scrolls .log information to the screen while the process so that no .log files are produced. The process generates a “debug” file named multiopt.log that may be of some benefit in showing the problem when the process breaks down.

Test Case and Examples This section provides details on a test case that is both simple and exercises many of the developed features. The example is based on the tpl deck dsoug1.dat and is the classic three bar truss example. The dsoug1.dat example has two subcases. For purposes of this demonstration, the deck has been divided into two separate models, each with a single subcase. The first deck is named cobj and contains the design model as it is in dsoug1 and applies only the second subcase. Also, the DLINK entry has been removed (this was for the purposes of the test and not a requirement). The second deck is called sub2d and applies the first load case and also removes the second DESVAR (and therefore the design of the vertical truss) from the design task. Another difference from the dsoug1.dat deck is the cobj deck has a DESOBJ that points to a DRESP2 that is to be used to combine the two weight objectives from the separate models. (This is a contrived objective that demonstrates how to combine objectives but does not have any physical meaning.) The following input shows portions of the input stream for cobj.dat with the items of interest to this capability highlighted in bold. ID MSC, D200X1 $ V68 G_MOORE 24-MAR-1994 TIME 10 $ diag 8,15 $ SOL 200 $ OPTIMIZATION CEND TITLE = SYMMETRIC THREE BAR TRUSS DESIGN OPTIMIZATION D200X1 SUBTITLE = BASELINE - 2 CROSS SECTIONAL AREAS AS DESIGN VARIABLES label = this run only contains the second subcase of test deck d200x1 $ it is run in conjunction with sub2d.dat ECHO = SORT SPC = 100 dsaprt=all DISP(plot) = ALL STRESS(plot) = ALL DESOBJ(MIN) = 200 $ (DESIGN OBJECTIVE = DRESP2 ID) DESMOD=SUB1 DESSUB = 21 $ DEFINE CONSTRAINT SET FOR BOTH SUBCASES ANALYSIS = STATICS SUBCASE 2 LABEL = LOAD CONDITION 2 LOAD = 310 BEGIN BULK $...DESIGN VARIABLE DEFINITION $DESVAR,ID, LABEL, XINIT, XLB, XUB, DELXV(OPTIONAL) DESVAR, 1, A1, 1.0, 0.1, 100.0 DESVAR, 2, A2, 2.0, 0.1, 100.0 DESVAR, 3, A3, 1.0, 0.1, 100.0 $ $...DEFINITION OF DESIGN VARIABLE TO ANALYSIS MODEL PARAMETER RELATIONS

Main Index


$DVPREL1,ID, TYPE, PID, FID, PMIN, PMAX, $+, DVID1, COEF1, DVID2, COEF2, ... DVPREL1 10 PROD 11 4 +DP1, 1, 1.0 DVPREL1,20, PROD, 12, 4, , , +DP2, 2, 1.0 DVPREL1,30, PROD, 13, 4, , , +DP3, 3, 1.0 $...STRUCTURAL RESPONSE IDENTIFICATION $DRESP1,ID, LABEL, RTYPE, PTYPE, REGION, ATTA, $+, ATT2, ... DRESP1, 20, W , WEIGHT DRESP1, 21, U4, DISP , , , 1, DRESP1, 22, V4, DISP , , , 2, DRESP1, 23, S1, STRESS, PROD, , 2, DRESP1, 24, S2, STRESS, PROD, , 2, DRESP1, 25, S3, STRESS, PROD, , 2, dresp2 200 cobj 200 dtable coef1 cdum2 dresp1 20 21 dtable coef1 1.0 cdum2 0.0 deqatn 200 cobj(c1,cdum2,obj1,odum2) = c1 * obj1 + $ ENDDATA

C0,

,

0.0

+ +DP1

,

,

+DP2

,

,

+DP3

ATTB,

ATT1,

+

, , , , ,

4 4 11 12 13

cdum2 * odum2

The DESVAR/DVPREL1 Bulk Data entries set up design variables for each of the three rod elements in this case. The DESMOD=SUB1 identifies design model as SUB1. The DESOBJ = 200 points to the DRESP2 that is shown at the bottom of the extracted data. It is seen that the objective is perceived as being the weighted sum of a DRESP1 that is the weight response plus a DRESP1 that is a displacement response. Since the weighting terms are 1.0 and 0.0, the objective for this model is actually the weight of the model, but this sets up the combined objective for the merged model. The second model is input from the sub2d.dat input and has a different loading condition and a different (i.e., DESMOD=SUB2) DESMOD value and a different design model from COBJ. A portion of this input file is listed here: TIME 10 $ diag 8,15 $ SOL 200 $ OPTIMIZATION CEND TITLE = SYMMETRIC THREE BAR TRUSS DESIGN OPTIMIZATION D200X1 SUBTITLE = BASELINE - 2 CROSS SECTIONAL AREAS AS DESIGN VARIABLES label = this run contains subcase 1 of d200x1 ECHO = SORT SPC = 100 DISP(plot) = ALL STRESS(plot) = ALL DESOBJ(MIN) = 20 $ (DESIGN OBJECTIVE = DRESP1 ID) DESSUB = 21 $ DEFINE CONSTRAINT SET desmod = SUB2 ANALYSIS = STATICS SUBCASE 1 LABEL = LOAD CONDITION 1 LOAD = 300 BEGIN BULK $ $...DESIGN VARIABLE DEFINITION $DESVAR,ID, LABEL, XINIT, XLB, XUB, DELXV(OPTIONAL)

Main Index


DESVAR, 1, A1, 1.0, 0.1, 100.0 DESVAR, 3, A3, 1.0, 0.1, 100.0 $ $...DEFINITION OF DESIGN VARIABLE TO ANALYSIS MODEL PARAMETER RELATIONS $DVPREL1,ID, TYPE, PID, FID, PMIN, PMAX, C0, , + $+, DVID1, COEF1, DVID2, COEF2, ... DVPREL1 10 PROD 11 4 0.0 +DP1 +DP1, 1, 1.0 DVPREL1,30, PROD, 13, 4, , , , , +DP3 +DP3, 3, 1.0 $ $...STRUCTURAL RESPONSE IDENTIFICATION $DRESP1,ID, LABEL, RTYPE, PTYPE, REGION, ATTA, ATTB, ATT1, + $+, ATT2, ... DRESP1, 20, W , WEIGHT $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ ENDDATA

In this case, only two design variables are defined so that the vertical member of the three bar truss is not being designed. The objective is simply the weight in this case. The command line for submitting this job is of the form: MultiOpt /nast/bin/nast2008 2 cobj sub2d coef 1.0 0.5 scr=yes The coef 1.0 0.5 replaces the DTABLE terms of the cobj.dat shown above so that the combined objective is all of the weight of the first model plus half the weight of the second. Again, this is a contrived objective with no particular physical meaning. Performing this task results in three .f06 files: cobj.f06, sub2d.f06 and merge.f06. The first two contain the results from exercising the individual models and each has a final design optimization history. The final design achieved by this process is not intuitive in that the vertical rod in the cobj model is at its minimum gage and the two angled rods do not have the same value. An inspection of the optimization behavior in the third .f06 file produced by this process, merge.f06, provides assurance that the numbers used in the optimization are correct and that therefore the final result is credible.

Guidelines and Limitations It is necessary to impose some ground rules/limitations on the users to insure that the combining of models is well posed. These include: 1. Each model must have a unique DESMOD Case Control command. 2. Design variables that are to be shared across models must have the same ID. 3. It is an error to have Design Variables in the separate models that share an ID but have different label, XLB,XUB , XVAL or DDVAL information. 4. Designed properties are assumed to be unique even when they are not. This is because it is almost impossible to verify that the design properties are actually identical (e.g; a DVPREL1 that has identical input may actually be referring to a completely different PSHELL entry in terms of its physical meaning.)

Main Index


5. Support for shape optimization is minimal in that it the separate models must have the same topology. 6. Topology optimization is not supported, nor is fully stressed design or ESLNRO (see Optimization of Nonlinear Structural Responses Phase 2 (Pre-release), 327). 7. It is expected that running multiple models with MultiOpt will consume more cpu time than if the identical task could be carried out within a single model. This is primarily due to the overhead of merging and partitioning data from the separate models and this cost is not expected to be large. 8. Up to five separate models can be merged. 9. If the xml form of the input file is used, the separate jobs can be a. Run on separate homogeneous machines b. Have a separate memory request c. Be run serially or in parallel 10. The feature that allows the user to define an overall objective that is the weighted sum of individual objective imposes the additional requirement of defining an objective in the first model that represents the desired final model, but with dummy coefficients and objectives. This is described in the Input , 273. 11. The process has been demonstrated on AIX and Linux 64 bit machines and Windows.

Additional Documentation Using Multiopt in the MD Nastran 2010 Installation and Operations Guide has information on invoking the MultiOpt Utility. More information on the DESMOD Case Control command can be found in DESMOD (p. 271) in the MD Nastran Quick Reference Guide.

Main Index

280 MD Nastran 2010 Release Guide Part Superelement Optimization Enhancements

Part Superelement Optimization Enhancements Introduction Part Superelements are a method for defining superelements by having a completely independent bulk data for each Superelement. One advantage of Part Superelements is that bulk data for various components or subassemblies can be easily assembled without the need to renumber GRIDs, properties, etc. Another advantage is that parameters are independent for each superelement. The method for defining Part Superelements in MD Nastran is by the delimiter BEGIN SUPER=seid, where seid is the user-defined Superelement Identification number. Note that the residual structure is defined in the main Bulk Data Section (BEGIN BULK, or BEGIN SUPER=0). The residual structure is also designated as a Part Superelement with seid=0. The residual structure includes the effects of all the upstream Part Superelements and is used to calculate the solution vector. For more information on Superelements and Part Superelements, refer to the MSC Nastran 2001 Superelement User’s Guide. Part Superelement Optimization was introduced in MD Nastran R3 with the limitation that the design variables, responses, and constraints for SOL 200 optimization were required to be defined in the main Bulk Data Section. With the MD Nastran 2010 release, Part Superelement Optimization extends the design model in SOL 200 to allow design of upstream Part Superelements in addition to the residual structure.

Benefits Part Superelement technology is widely used in the Aerospace and Automotive industry to assemble bulk data models from various sources. Some advantages of Part Superelement technology include automatic connections based on geometry searches and the ability to have completely independent bulk data. Extending the design model to Part Superelements will allow users great flexibility in assembling models and performing design optimization using Part Superelement technology. Design variable, response, and constraint definition for Part Superelement Optimization can include the residual structure and all Part Superelement(s). Design variables can be linked across Part Superelements. In addition synthetic responses can include responses from different Part Superelements are supported with new Bulk Data entries, namely SEDLINK, SEDRSP2, and SEDRSP3.

Input Each Partitioned Superelement may contain traditional Solution 200 bdf entries such as DESVAR, DVPREL1, DRESP1, etc. The new bulk data entries are introduced to support cross boundary Part Superelement design variable linking and synthetic responses. These new bulk data entries are for Part Superelement only and must involve quantities from more than one Part Superelement. See additional comments and remarks for Bulk Data entries SEDLINK, SEDRSP2, and SEDRSP3 (p. 3093) in the MD Nastran Quick Reference Guide. These bulk data entries must be specified in the residual Bulk Data Section.

Main Index


1 SEDLINK

2

3

4

6

7

8

9

IDV1

C1

ID

DSEID

DDVID

C0

CMULT

ISEID1

ISEID2

IDV2

C2

ISEID3

IDV3

C3

ISEID4

IDV4

C4

-etc.-

1

2

3

4

5

6

7

8

9

SEDRSP2

ID

LABEL

EQID or FUNC

REGION

METHOD

C1

C2

C3

“DESVAR”

DVSEID1

DVID1

DVSEID2

DVID2

DVSEID3

DVID3

DVSEID4

DVID4

-etc.-

LBSEID1

LABL1

LBSEID2

LABL2

LBSEID3

LABL3

LBSEID4

LABL4

-etc.-

R1SEID1

NR1

R1SEID2

NR2

R1SEID3

NR3

R1SEID4

NR4

-etc.G2

CMP2

“DTABLE”

“DRESP1”

“DNODE”

“DVPREL1

“DVCREL1”

“DVMREL1”

“DVPREL2”

“DVCREL2”

“DVMREL2”

NDSEID1

G1

CMP1

NDSEID2

NDSEID3

G3

CMP3

-etc.-

P1SEID1

DPIP1

P1SEID2

DPIP2

P1SEID3

DPIP3

P1SEID4

DPIP4

-etc.-

C1SEID1

DCIC1

C1SEID2

DCIC2

C1SEID3

DCIC3

C1SEID4

DCIC4

-etc.-

M1SEID1

DMIM1

M1SEID2

DMIM2

M1SEID3

DMIM3

M1SEID4

DMIM4

-etc.DPI2P2

P2SEID3

DPI2P3

DC12C2

C2SEID3

DC12C3

DMI2M2

M2SEID3

DM12M3

7

8

P2SEID1

PDI2P1

P2SEID2

P2SEID4

DPI2P4

-etc.-

C2SEID1

DC12C1

C2SEID2

C2SEID4

DCI2C4

-etc.-

M2SEID1

DM12M1

M2SEID2

M2SEID4

DMI2M4

-etc.-

1

2

3

4

5

6

SEDRSP3

ID

LABEL

GROUP

TYPE

REGION

“DESVAR”

DVSEID1

DVID1

DVSEID2

DVID2

DVSEID3

DVID3

DVSEID4

DVID4

-etc.-

LBSEID1

LABL1

LBSEID2

LABL2

LBSEID3

LABL3

LBSEID4

LABL4

-etc.-

R1SEID1

NR1

R1SEID2

NR2

R1SEID3

NR3

R1SEID4

NR4

-etc.G2

CMP2

“DTABLE”

“DRESP1

“DNODE”

Main Index

5

NDSEID1

G1

CMP1

NDSEID2

NDSEID3

G3

CMP3

-etc.-

9

10

10

10


“DVPREL1”

P1SEID1

DPIP1

P1SEID2

P1SEID4

DPIP4

-etc.-

“DVCREL1”

C1SEID1

DCIC1

C1SEID2

C1SEID4

DCIC4

-etc.-

“DVMREL1:

M1SEID1

DMIM1

M1SEID2

M1SEID4

DMIM4

-etc.-

“DVPREL1”

P2SEID

DPI2P1

P2SEID2

P2SEID4

DPI2P4

-etc.-

“DVCREL2”

C2SEID1

DC12C1

C2SEID2

“DVMREL2”

C2SEID4

DCI2C4

-etc.-

M2SEID

DMI2M1

M2SEID2

M2SEID4

DMI2M4

-etc.-

“USRDATA”

DPIP2

P1SEID3

DPIP3

DCIC2

C1SEID3

DCIC3

DMIM2

M1SEID3

DMIM3

DPI2P2

P2SEID3

DPI2P3

DCI2C2

C2SEID3

DCI2C3

DMI2M2

M2SEID3

DMI2M3

String -etc.-

For user convenience, specifying PARAM,PSENPCH,YES will write the updated bulk data entries into separate ‘.pch’ files for each Part Superelement, and each design cycle. Note that the number of design cycles that are output is dependant on the value of PARAM,DESPCH. The advantage of specifying PARAM,PSENPCH,YES is that each of the ‘.pch’ files with the updated design bulk data can be used to replace the original model with an ‘INCLUDE’ entry after the appropriate ‘BEGIN SUPER=seid’. If PARAM,SPENPCH,YES is not specified, the updated bulk data entries for all Part Superelements are written to a single ‘.pch’ file which will require the user to manually extract each Part Superelement model from the .pch file and place it in the appropriate ‘BEGIN SUPER=seid’ section of the Bulk Data Section.

PARAM,PSENPCH

Default=NO. Setting PSENPCH to YES causes updated bulk data entries of a Part Superelement for a design cycle punched to a separate file named as follows

JOBNAME_psexx_yy.pch

Where xx is for Part Superelement ID and yy is for design cycle.

Note that PARAM, PSENPCH has no effect for non-Part Superelement run.

Output For SOL 200 with design models in each Part Superelement, the .f06 output is similar to non Part Superelement optimization jobs. There are some minor differences that are specific to Part Superelements only.

Main Index


Comparison Between Input Property Values from Analysis and Design Models This section of the .f06 will repeat for the design model of each Part Superelement. A sample for a Part Superelement is shown as follows:

1 0

DOUBLE FLYSWATTER MODEL $ ANALYSIS USING PART SUPERELEMENTS S.E. STATICS - MULTIPLE LOADS

------

--

JANUARY

13, 2009

MD NASTRAN 1/12/09 PAGE SUPERELEMENT 4

39

COMPARISON BETWEEN INPUT PROPERTY VALUES FROM ANALYSIS AND DESIGN MODELS -----

--------------------------------------------------------------------------------------------------------------------------PROPERTY PROPERTY PROPERTY ANALYSIS DESIGN LOWER UPPER DIFFERENCE SPAWNING TYPE ID NAME VALUE VALUE BOUND BOUND FLAG FLAG --------------------------------------------------------------------------------------------------------------------------PSHELL

4

T

5.000000E-02

5.000000E-02

5.000000E-03

1.000000E+20

NONE

1. THE DIFFERENCE FLAG IS USED TO CHARACTERIZE DIfFERENCES BETWEEN ANALYSIS AND DESIGN MODEL PROPERTIES: IF THE FLAG IS NONE, THEN THERE IS NO SIGNIFICANT DIFFERENCE BETWEEN THE TWO VALUES. IF THE FLAG IS WARNING, THEN THE USER IS ADVISED THAT DIFFERENCES EXIST AND THE DESIGN MODEL IS BEING USED TO OVERRIDE THE ANALYSIS MODEL. IF THE FLAG IS FATAL, THEN THE DIFFERENCES ARE GREATER THAN 1.00000E+35 AND THE RUN WILL BE TERMINATED. 2. THE SPAWNING FLAG (*) INDICATES THAT THE SPAWNED PROPERTY IS DERIVED EITHER FROM THE BEAM CROSS SECTION LIBRARY OR FROM A PBEAM ENTRY. THE PROPERTY ID FOR THE SPAWNED PROPERTY IS IDENTICAL TO ITS PARENT.

Please note that the Part Superelement ID shows up in the title line of a page. In addition, residual Part Superelement will get two versions of above output, first and last. If there are differences between design and analysis model for residual Part Superelement, the differences will show up in the first version.

Main Index


Updated Bulk Data Entries The updated bulk data entries are punched into either a single or multiple ‘.pch’ file(s). It can be controlled by ‘PARAM,PSENPCH,YES’as described previously. A sample punched updated bulk data entries for a Part Superelement is shown as follows: Listing 12-1

Partitioned Superelement punch output for PARAM,PSENPCH,YES

$ ****************************** $ * * $ * PART SE 2 * $ * * $ ****************************** $ $ ************************************************************* $ * * $ * CONTINUOUS DESIGN CYCLE NUMBER = 5 * $ * * $ ************************************************************* $ $ ****************************** $ * * $ * PART SE 2 * $ * * $ ****************************** $ $ UPDATED DESIGN MODEL DATA ENTRIES $ DESVAR * 102T2 1.00000001E-01 1.00000001E-01+D *D 1V 1.00000000E+01 $ ****************************** $ * * $ * PART SE 2 * $ * * $ ****************************** $ $ UPDATED ANALYSIS MODEL DATA ENTRIES $ PSHELL* 2 2 5.00000035E-03 2* * 1.00000000E+00 2 8.33333313E-01 0.00000000E+00* * 0 * *

1V

Guidelines and Limitations 1. For each Part Superelement, the design model specifying design variables, responses, and constraints must be located in the corresponding 'BEGIN SUPER=seid' section. 2. DESVAR, DVxRELi, and DRESPi IDS can be reused in superelements - i.e. each Part Superelement may define DESVAR,1 DRESP1,1, etc. Note that DESIGN VARIABLE HISTORY output will not distinguish the SEID, therefore, it is suggested that unique ids be used whenever practical. 3. SEDLINK, SEDRSP2, and SEDRSP3 must be placed in the main bulk data section before 'BEGIN SUPER=seid' (for seid>0). 4. For Part Superelement, DCONSTR entries can reside in each individual Part Superelement Bulk Data Section starting with ‘BEGIN SUPER=seid’. If DCID is different from a Part Superelement to the next, DCONADD in the main Bulk Data Section can be defined to group DCONSTR entries together for reference by DESSUB. Note that DCONADD entries in ‘BEGIN SUPER=seid’ where seid>0 will be ignored. 5. Part Superelement optimization does not support topology (TOPVAR), topography (BEADVAR), or topometry (TOMVAR) optimization.

Main Index


6. Design Responses for Image Part Superelements (copies, mirrors, etc. via SEBULK Bulk Data entry) are supported in the design model.

Test Cases The following test cases are available in TPL library tpl\pse_200: d200pse1, d200pse2, d200pse3, p200pse6, d200pse7, d200pse8, d200psea and d200pseb TPL Problem d200pse1.dat The double-headed fly swatter model will be used to demonstrate Part Superelement Optimization with the design model including DESVAR from each Part.

Figure 12-2

Main Index

Example problem d200pse1


The case control is similar to case control and design model definition is similar to non Part Superelement optimization files. Note that the DESSUB in the case control points to the DCONSTR in each Part Superelement. Listing 12-2

Partial input for file /pse_200/d200pse7.dat

$ tpl problem d200pse7.dat $ Case control $ ANALYSIS = STATICS $ DESOBJ(MIN)=1001 DESSUB = 100 $ all DCONSTR with ID = 100 will be considered $ $ tpl problem d200pse7.dat BEGIN BULK $ design model for se 0 DCONSTR 100 801 -7.00 DCONSTR 100 802 -7.00 DESVAR 110 T10 1.0 DRESP1 801 RESG12Z DISP DRESP1 802 RESG23Z DISP DRESP1 1001 WEIGHT WEIGHT DVPREL1 10 PSHELL 10 110 .05

7.00 7.00 .1

10.0

T

.005

BEGIN SUPER=1 $ design model for SE 1 DCONSTR 100 101 -7.00 7.00 DCONSTR 100 102 -7.00 7.00 DESVAR 101 T1 1.0 .1 DESVAR 1001 GE_1 1. 0.1 DRESP1 101 S1G57Z DISP DRESP1 102 S1G93Z DISP DVMREL1 1001 MAT1 1 GE ++0000031001 .05 DVPREL1 1 PSHELL 1 T ++000001101 .05 $ each BEGIN SUPER has additions to the

Main Index

10.0 10. .005

3 3

13 23

3 3

57 93

.005 design model


The output is similar to output from non Part Superelement Optimization runs, as an example, the Design Variable History for d200pse1.dat is: Listing 12-3

Design Variable History Partitioned Superelements

TPL Problem d200pse7.dat TPL problem d200pse7.dat provides an example of defining a synthesized response using design components that span multiple Part Superelements. The SEDRSP2 entry is similar to the DRESP2 entry with the exception that an SEID qualifier is required for each design component that is used in the synthesized response. Listing 12-4

Example of SEDRSP2 in file /pse_200/d200pse7.dat

$ tpl problem d200pse7.dat $ design model for se 0 (continued) $ synthesized response across SE SEDRSP2 818 AVERD 108 $ SEID DVID SEID DESVAR 2 102 5 $ SEID const SEID DTABLE 3 CONST3 6 $ SEID RESPID SEID DRESP1 0 801 1 6 601 $ SEID PRELID SEID DVPREL1 4 4 7 $ SEID MRELID DVMREL1 1 1001

DVID 105 const CONST6 RESPID 101

SEID 3

RESPID 301

PRELID 7

GUI Support for Part Superelement Optimization Pre Processing Patran supports Part Superelement and Optimization, however, all the design data will be written to the main bulk data section. The user will have to manually adjust the location of the design entries. Alternatively, the user can use the Patran group option to write out each Part Superelement to an individual bulk data file and then use INCLUDE files to assemble the final models and design models.

Main Index


There is no direct Patran support for the SEDLINK, SEDRSP2, and SEDRSP3 entries, nor PARAM,PSENPCH. These entries could be added via Direct Text Input, or the bdf can be modified before job submission. SimXpert does not currently support SOL 200 Design Optimization. Post Processing With PARAM,POST,-1 the objective, maximum constraint, and design variable history data will be written to the OP2 and available for post-processing by Patran as normal. SimXpert does not currently support Optimization.

Main Index


Optimization - Invariant DRESP3 Gradients Introduction One component of the design model in gradient based design optimization is the design response definition. A design response can be used as an objective or a constraint can be placed on the response to bound the optimization space. A simple example of an objective is to minimize the weight. Constraint can be as simple as “von Mises stress must be less than 20,000 psi,” or as complex as a subroutine that calculates multiple margins of safety based on stress, stability, empirical, and manufacturing considerations. In MD Nastran, there are three types of responses: 1. Direct responses are output quantities generated by a typical MD Nastran analysis. Examples are Weight, Frequency, Stress, Displacement, etc. Direct responses are specified for the design model by specifying DRESP1Bulk Data entries. 2. Equation based responses can be defined by the user based on current design model values and constants. The equation based responses can be quite extensive and allow the user great flexibility in defining a synthesized response. The DRESP2 is used to define equation based results. 3. External responses are available by calling a user supplied subroutine. This type of response gives the user ultimate flexibility by allowing the designer to write his own subroutines that can include empirical based tables, conditional clauses, loops, etc. in defining the response. The DRESP3is used to define the inputs and external response server used to calculate the responses. Sensitivity analysis is performed to calculate the gradient of each response with respect to each design variable. Additional information on design optimization in MD Nastran can be found in the MD Nastran Design Sensitivity and Optimization User’s Guide. The MD Nastran R3 release enhanced DRESP3 by returning multiple responses, providing for analytic gradients, and using a more efficient algorithm when there are many more DRESP1’s in the DRESP3 than there are design variables. The MD Nastran 2010 release has added a feature that allows the user to specify that gradients of the DRESP3 with respect to the design are to be considered invariant during the approximate optimization task.

Benefits In the approximate optimization task, DRESP3 gradients have been calculated using central differencing techniques. For a DRESP3 with 100 arguments, this entails 200 calls to the server for a single gradient calculation. This can be a performance burden if the server call is non-trivial. For this reason, it was decided to implement invariant gradient approach which assumes the gradient is not a strong function of the individual arguments. The approximate optimizer does not have to make any calls to the server.

Input The format of the DRESP3 Bulk Data entry is unchanged. The user is required to modify the R3SGRT server subroutine that supplies MD Nastran with the information on the number of responses and the type

Main Index

290 MD Nastran 2010 Release Guide Optimization - Invariant DRESP3 Gradients

of gradient evaluation desired. Prior to MD Nastran R3, the only gradient option that was supported was finite difference so there was no need for the user to specify the method to be used. MD Nastran R3 provided two options for the gradient type and this was specified in the R3SGRT subroutine by specifying a GRDTYP for each response. With MD Nastran 2010, the number of options is four: • GRDTYP = 1 specifies that analytic gradients will be provided by the user and they will be

computed explicitly during the approximate optimization task • GRDTYP = 2 specifies that analytic gradients will be provided by the user and they will be

considered invariant during the optimization task. • GRDTYP = 3 specifies that finite difference techniques will be required to compute gradient

information and they will be computed explicitly during the approximate optimization task. • GRDTYP = 4 specifies that finite difference techniques will be required to compute gradient

information and they will be considered invariant during the approximate optimization task. The user provided R3SVALD subroutine that evaluates the DRESP3 response does not need to be modified as a result of this enhancement.

Output There is no change to the existing output formats.

Examples There are two tests cases in the TPL subdirectory /tpl/edresp3_08 that demonstrate the invariant dresp3 capability: dresp3fi.dat – This file calculates all the gradients using finite difference methods and considers the gradients to be invariant during the approximate optimization task (i.e., GRDTYP = 4). dresp3fo.dat – This file calculates all the gradients using all four methods. The R3SGRT subroutine in this case has the following specification: Listing 12-5

C

Updated input for subroutine R3SGRT

PARAMETER(NTYPES=5) CHARACTER*8 R3TYPE(NTYPES) DATA R3TYPE/'TYPE88 1 'TYPE94

','TYPE91 '/

', 'TYPE92

ERROR = 0 nresp = 1 DO 100 ITYPE = 1, NTYPES IF (TYPNAM .EQ. R3TYPE(1)) THEN grdtyp(1) = 3 go to 200 else IF (TYPNAM .EQ. R3TYPE(2)) THEN grdtyp(1) = 1 go to 200 else IF (TYPNAM .EQ. R3TYPE(3)) THEN

Main Index

', 'TYPE93

',


100

grdtyp(1) = 2 go to 200 else IF (TYPNAM .EQ. R3TYPE(4)) THEN grdtyp(1) = 3 go to 200 else IF (TYPNAM .EQ. R3TYPE(5)) THEN grdtyp(1) = 4 go to 200 else ERROR = BADTYP END IF CONTINUE

It is seen that the user is able to specify the gradient type as a function of the response name.

Guidelines and Limitations Modifying Existing Server Subroutines The enhanced capability does not require any changes in the MD Nastran input files that have been developed to utilize the DRESP3, but it does require changes in the R3SGRT server subroutine relative to the MD Nastran R3 capability (see the MD Nastran R3 Release Guide to see the changes in this subroutine due to the analytic gradient and multiple response enhancements). To retain the current capability for an existing DRESP3, the changes required in the R3SGRT subroutine are to: 1. Change existing GRDTYP(i) = -2 to GRDTYP(i) = 3 2. Change existing GRDTYP(i)= 2 to GRDTYP(i) = 1 No changes are required to the R3SVALD subroutine relative to the MD Nastran R3 capability.

Other Guidelines In R3SGRT, GRDTYP needs to be defined for all NRESP responses and the values must be either 1, 2, 3 or 4. It is an error if any other value is used. MSC currently does not have test cases that allow an evaluation of the relative performance of the various gradient options. However, one can make the following recommendations: 1. If the DRESP3 evaluations are cheap and simple, GRDTYP = 1 (analytic, variant) is recommended. 2. If the DRESP3 evaluations are simple, but expensive, GRPTYP = 2 (analytic, invariant) is recommended. It would seem that this option would be rarely needed. 3. If the DRESP3 evaluations are not simple, but still cheap, GRDTYP = 3 (finite difference, variant) is recommended. 4. If the DRESP3 evaluation are complex and expensive, GRDTYP = 4 (finite difference, invariant) is recommended.

Main Index

292 MD Nastran 2010 Release Guide Optimization - Invariant DRESP3 Gradients

The invariant gradients will not provide as accurate a calculation as the variable ones so it becomes a trade-off between the time spent performing the optimization and possible more design iterations to reach the final design. It is expected that this new capability will be used sparingly, but will provide a dramatic improvement in CPU time in special circumstances. The current limitation that all GRDTYP’s for a particular TYPE be the same is retained for this project. The GRDTYP’s do not need to all be the same for all the DRESP3’s in an input file. That is, one can specify analytic variant gradients (GRDTYP = 1) for one TYPE and finite difference, invariant gradients (GRDTYP = 4) for another type.

Additional Information Building and Using DR3SERV (p. 253) in the MD Nastran 2010 Installation and Operations Guide has information on installing and running the DR3SERV, the server associated with the DRESP3.

GUI Support for Invariant DRESP3 Gradients Pre Processing Since Invariant DRESP3 Gradients is invoked by modifying the DRESP3 fortran server routine, there is no need for GUI support. Post Processing There are no additional post-processing requirements associated for Invariant DRESP3 Gradients.

Main Index


Design of Monitor Points Introduction Monitor points is a generic name for four types of output requests. The MD Nastran R1 Release Guide provided the most comprehensive discussion of these inputs. Briefly, 1. MONPNT1– The MONPNT1 provides integrated loads at a user defined point in a user defined coordinate system. 2. MONPNT2– The MONPNT2 provides element results (e.g., Stress, Strain, Force) 3. MONPNT3– The MONPNT3 provides a summation of grid point forces at a user specified monito points. 4. MONDSP1– The MONDSP1 allows for the sampling of a displacement vector to create a blended displacement response at a user specified point and coordinate system. With the release of MD Nastran 2010, each of the MONPNT1, MONPNT3 and MONDSP1 quantities can now be specified as design response quantities on the DRESP1entry. The MONPNT2 capability for element results effectively duplicates existing DRESP1 response quantities, so MONPNT2 is not supported.

Benefits The user of this capability is likely to be an investigator who wants to control a load path in an aeroelastic analysis. This is a sophisticated application that is related to aeroelastic tailoring, implying that it will be done in conjunction with composites. It’s likely that our users will find other applications that are currently undefined.

Input The existing DRESP1 entry now has 5 additional options. The following is extracted from the description of the entry DRESP1 (p. 1644) in the MD Nastran Quick Reference Guide: Response Type

Main Index

ATTA

ATTB

ATTi

STMONP1

Component (see Remark 36.)

Blank

Blank

STMOND1


Blank

Blank

MONPNT3


Blank

Blank

AEMONP1


Blank

Blank

AEMOND1


Blank

Blank

294 MD Nastran 2010 Release Guide Design of Monitor Points

36. For monitor point responses (RTYPE = STMONP1, STMOND1, MONPNT3 AEMONP1 or AEMOND1) the ATTA field specifies the components to be extracted. These can be any subset of the integers 1 through 6 that appear on the monitor quantity with the NAME provided in the PTYPE field. All of these responses can be invoked in a static aeroelastic (ANALYSIS=SAERO) subcase. STMONP1, STMOND1 and MONPNT3 can be invoked from a static (ANALYSIS=STAT) subcase. The responses are not available in a dynamic response or normal modes subcase. The response types have the following meaning: a. STMONP1 – A structural MONPNT1 b. STMOND1 – A structural MONDSP1 c. MONPNT3 – A MONPNT3 d. AEMONP1 – An aerodynamic MONPNT1 e. AEMOND1 – An aerodynamic MONDSP1 For all but the STMONP1, the response is the elastic monitor point value. For the STMONP1, it is the elastic “minus” inertial “plus” elastic applied load value.

Output The various response outputs have been modified to clearly identify Monitor Points.

Main Index


Listing 12-6

Sample Monitor Point Response output identification.

-----

DESIGN CONSTRAINTS ON RESPONSES

-----

(MAXIMUM RESPONSE CONSTRAINTS MARKED WITH **) --------------------------------------------------------------------------------------------------------INTERNAL EXTERNAL INTERNAL INTERNAL DCONSTR RESPONSE DRESPx RESPONSE L/U REGION SUBCASE ID ID ID ID TYPE FLAG ID ID VALUE --------------------------------------------------------------------------------------------------------1 100 10 3456 STMOND1 UPPER 0 10 2.3412E-01 2 100 11 4567 MONPNT3 LOWER 0 10 -2.7536E-01 3 100 8 5678 GPFORCE LOWER 5678 10 -2.7536E-01 4 100 8 5678 GPFORCE UPPER 5678 10 2.6273E-01** 5 100 9 5679 GPFORCE LOWER 5679 10 5.7648E-02 6 100 9 5679 GPFORCE UPPER 5679 10 -6.6978E-02 7 100 1 6543 EQUA UPPER 6543 10 6.6703E-02

---------------------------------------------------------------------| R E S P O N S E S IN D E S I G N M O D E L | --------------------------------------------------------------------------

MONITOR POINT RESPONSES

-----

-----------------------------------------------------------------------------------------------------------INTERNAL DRESP1 RESPONSE NAME COMPONENT LOWER UPPER ID ID LABEL NO. BOUND VALUE BOUND -----------------------------------------------------------------------------------------------------------10 3456 STIP SWTIP 3 N/A 3.0853E+00 2.5000E+00 11 4567 SMP3 SPOINT 3 1.0000E+00 1.2754E+00 N/A

**************************************************************************** * * * D E S I G N S E N S I T I V I T Y M A T R I X O U T P U T * * * * * * R E S P O N S E S E N S I T I V I T Y C O E F F I C I E N T S * * * **************************************************************************** ---------------------------------------------------------------------------------------------------------------DRESP1 ID= 3456 RESPONSE TYPE= STMOND1 NAME = SWTIP COMP NO= 3 SEID= 0 SUBCASE RESP VALUE DESIGN VARIABLE COEFFICIENT DESIGN VARIABLE COEFFICIENT ---------------------------------------------------------------------------------------------------------------10 3.0853E+00 1 INBD -8.0550E-01 2 SNDD -6.8049E-01 ---------------------------------------------------------------------------------------------------------------DRESP1 ID= 4567 RESPONSE TYPE= MONPNT3 NAME = SPOINT COMP NO= 3 SEID= 0 SUBCASE RESP VALUE DESIGN VARIABLE COEFFICIENT DESIGN VARIABLE COEFFICIENT ---------------------------------------------------------------------------------------------------------------10 1.2754E+00 1 INBD 3.6495E+00 2 SNDD -3.9502E+00

Guidelines and Limitations These new responses are only available for static and/or static aeroelastic subcases (ANALYSIS=STATIC or ANALYSIS=SAERO). The extracted response value is typically the “elastic” value printed in the .f06 file. An exception is the STMONP1. In this case, the response value is the sum of “elastic restrained” minus the “inertial” plus the “restrained applied” values.

Main Index


Test Cases Three test cases are provided in the tpl subdirectory /tpl/ue_mdr4 that demonstrate this new capability: TPL problem dmpa.dat TPL problem dmpa.dat is a design sensitivity analysis with a single static aeroelastic subcase. The model is a classic test case of a half-span 15 degree swept wing studied in NASA TN D-1824. The boundary conditions are a wind tunnel mount and the ANALYSIS=SAERO is performed at a Mach Number of 0.45. Further description of the model and aeroelastic capabilities of MD Nastran can be found in the Aeroelastic Analysis User’s Guide, example problem ha144c.dat.

Figure 12-3

Example problem dmpa

The subcase invokes constraints on each type of monitor responses with constraints contrived to force their retention. This test case is used to test the quality of the sensitivities. A part of the bulk data file which contains the monitor points, the design response and their constraints is shown here: Listing 12-7

Design Response definition for Monitor Points

mondsp1 swtip 35 aecomp swtip set1 840

Main Index

transverse disp and twist at wing tip swtip 2.515 5.525 set1 840 8 16 24 32 40

23


mondsp1 awtip 123456 aecomp acaero aelist 101124 monpnt3 spoint 3 set1 5 set1 6 set1 50 set1 60 set1 15 set1 16 set1 25 set1 26 monpnt1 outbd 123456 aecomp otbd set1 1234 21 40 monpnt1 aoutbd 35 aecomp aotbd aelist 1234 dresp1 1234 dresp1 1235 dresp1 1236 dresp1 3456 dresp1 4567 dresp1 6789 8 $constr 200 dconstr 200 dconstr 200 dconstr 200 dconstr 200 dconstr 200 dconstr 200 doptprm desmax delb

pitch and plunge at the wing tip acaero 2.3 4.7 aelist 101124 101 thru 124 contains results at a single grid 5 6 1.88124 3.1572 0. 21 12 19 5 13 21 29 37 5 12 19 26 2 10 18 26 34 2 9 16 23 1 9 17 25 33 1 8 15 22 contains from the three outboard strips otbd 1.88124 3.1572 set1 1234 5 thru 8 13 thru 16 thru 24 29 thru 32 38 contains the three outboard aerodynamic strips aotbd 1.88124 3.1572 aelist 1234 113 thru 124 oaero aemonp1 aoutbd 3 tiptran aemond1 awtip 3 ostru stmonp1 outbd 3 stip stmond1 swtip 3 smp3 monpnt3 spoint 3 tipdis disp 3 16 32 40 23 1234 1.0 1.01 1234 1.0 3.0 1235 1.0 3.0 1236 1.0 3.0 3456 1.0 3.0 4567 1.0 3.0 6789 1.0 3.0 20 p1 1 p2 15 iprint .01

37 39

24

7

It is seen that five monitor points are constructed, one for each of the available monitor types. In this example, only the “TZ” (component 3) of each of the monitor points is being designed even though multiple components are available from monitored quantities. A number of displacement constraints are also specified to provide a qualitative assessment of the MONDSP1 results and their sensitivities. TPL Problem dmoncants.dat TPL problem dmoncants.dat is a variation of the TPL problem dmpa.dat and contains both a static aeroelastic and a static subcase. In this example, constraints are placed on monitor point results that require redesign in order to provide an optimal design. The weight is minimized while satisfying all the imposed constraints. The bulk data sample shown in Listing 12-8 indicates that aeroelastic subcase (ANALSYIS=SAERO with DESSUB=200) has placed upper bound limits on structural and aerodynamic MONPNT1 responses, an aerodynamic MONDSP1 and a lower bound on a structural MONDSP1. The static subcase (ANALYSIS=STATIC with DESSUB=100) applies a single, more stringent limit on the structural MONDSP1.

Main Index


Listing 12-8

Partial listing of TPL problem dmoncants.dat

mondsp1 swtip 35 aecomp swtip set1 840 mondsp1 awtip 123456 aecomp acaero aelist 101124 monpnt3 spoint 3 set1 5 set1 6 set1 50 set1 60 set1 15 set1 16 set1 25 set1 26 monpnt1 outbd 123456 aecomp otbd set1 1234 21 40 monpnt1 aoutbd 35 aecomp aotbd aelist 1234 dresp1 1234 dresp1 1235 dresp1 1236 dresp1 3456 dconstr 200 dconstr 200 dconstr 200 dconstr 200 dconstr 100

transverse disp and twist at wing tip swtip 2.515 5.525 set1 840 8 16 24 32 40 pitch and plunge at the wing tip acaero 2.3 4.7 aelist 101124 101 thru 124 contains results at a single grid 5 6 1.88124 3.1572 21 12 19 5 13 21 29 37 5 12 19 26 2 10 18 26 34 2 9 16 23 1 9 17 25 33 1 8 15 22 contains from the three outboard strips otbd 1.88124 3.1572 set1 1234 5 thru 8 13 thru thru 24 29 thru 32

23

0.

16 38

37 39

contains the three outboard aerodynamic strips aotbd 1.88124 3.1572 aelist 1234 113 thru 124 oaero aemonp1 aoutbd 3 tiptran aemond1 awtip 3 ostru stmonp1 outbd 3 stip stmond1 swtip 5 1234 6.5 1235 2.0 1236 6.5 3456 -2.5 3456 -2.0

TPL Problem dmp3.dat TPL problem dmp3.dat is another variant of TPL problem dmpa.dat that provides an example of using monpnt3 as a design quantity. Listing 12-9

Partial listing of TPL problem dmpa.dat

MONPNT3 SPOINT CONTAINS RESULTS AT A SINGLE GRID 3 5 6 1.88124 3.1572 DRESP1 4567 SMP3 MONPNT3 SPOINT 3

0.

Reference Documents The MD Nastran Quick Reference Guide provides a description of the input required for these new responses while the Design Sensitivity and Optimization User’s Guide is a good resource for learning about design optimization in MD Nastran.

Main Index


GUI Support for MONPNTi Optimization Pre Processing Neither Patran nor SimXpert supports MONPNTi definition or optimization.

Main Index

300 MD Nastran 2010 Release Guide Parallel Sensitivities

Parallel Sensitivities Introduction Design sensitivity and optimization in MD Nastran requires sensitivity calculation of the design responses w.r.t. each design variable. Design sensitivity calculations can be a very costly portion of a SOL 200 run for models with large numbers of design variables and large numbers of design responses. The Design Sensitivity and Optimization User’s Guide provides great detail about design sensitivity calculations in MD Nastran. In MD Nastran 2010, design sensitivity calculations have been enhanced to be performed in a distributed parallel (dmp) environment in SOL 200 of MD Nastran. The parallel implementation divides the sensitivity task across a number of processors so that each processes a subset of the total number of design variables. Following the sensitivity analysis and before optimization, the separate sensitivity data are appended into a global sensitivity set.

Benefits Parallel Sensitivity Analysis is aimed at users who have design optimization tasks that spend significant time in the sensitivity calculation phase. This typically occurs for models with large dof, or there are many (perhaps thousands) of design variables and the adjoint method of sensitivity analysis is either unavailable or still time consuming.

Inputs 1. Specify the DOMAINSOLVERExecutive Control statement with the new DSA keyword. For example: DOMAINSOLVER DSA Other DOMAINSOLVER options like ACMS, FREQ, and MODES may also be specified or modified along with DSA. For example, DOMAINSOLVER DSA ACMS Note: DOMAINSOLVER options MODES and FREQ are defaults on with dmp keyword on the Nastran submittal command, but the DSA option must be explicitly specified. 2. Specify the dmp=n keyword on the Nastran submittal command; where n is the number of available processors.

Outputs There are no new outputs. It should be noted that with dmp=n, by default, only the master processor’s output (f04 and f06) is saved. “slaveout=yes” may be specified on the Nastran submittal command to request the slaves’ output.

Main Index


Test Cases TPL problem /ugdesopt/dsoug7.dat involves a frequency response sizing optimization problem. As an example, the Executive Control Section is modified as follows: domainsolver acms dsa SOL 200 cend and the job is submitted with: nastran dsoug7 dmp=2 The job converges after five design cycles and compares exactly with the serial results demonstrating that the parallel sensitivity calculations provide the same answers. Listing 12-10

Design Variable History for TPL problem ugdesopt/dsoug7.dat

DESIGN VARIABLE HISTORY --------------------------------------------------------------------------------------------------------------------------------INTERNAL | EXTERNAL | | DV. ID. | DV. ID. | LABEL | INITIAL : 1 : 2 : 3 : 4 : 5 : --------------------------------------------------------------------------------------------------------------------------------1 | 1 | T1 | 8.0000E-02 : 9.6000E-02 : 9.6301E-02 : 9.9607E-02 : 9.8070E-02 : 1.0022E-01 : 2 | 2 | T2 | 8.0000E-02 : 7.7291E-02 : 8.4733E-02 : 8.3555E-02 : 8.5617E-02 : 8.3472E-02 : 3 | 3 | T3 | 8.0000E-02 : 6.6729E-02 : 6.6797E-02 : 7.0123E-02 : 6.9962E-02 : 6.8825E-02 : 4 | 4 | T4 | 8.0000E-02 : 6.7694E-02 : 5.6433E-02 : 4.8899E-02 : 4.5751E-02 : 4.3705E-02 : 5 | 5 | T5 | 8.0000E-02 : 7.3645E-02 : 6.4645E-02 : 5.6491E-02 : 5.1688E-02 : 4.9985E-02 : 6 | 6 | T6 | 8.0000E-02 : 7.9524E-02 : 7.4968E-02 : 7.1886E-02 : 7.3299E-02 : 7.4792E-02 : 7 | 7 | T7 | 8.0000E-02 : 8.5560E-02 : 8.6633E-02 : 8.6667E-02 : 8.9316E-02 : 9.1213E-02 : 8 | 8 | T8 | 8.0000E-02 : 9.4564E-02 : 1.0857E-01 : 1.1484E-01 : 1.1281E-01 : 1.1295E-01 : 9 | 9 | T9 | 8.0000E-02 : 9.5853E-02 : 1.1502E-01 : 1.3803E-01 : 1.5202E-01 : 1.5574E-01 : 10 | 10 | T10 | 8.0000E-02 : 9.6000E-02 : 1.1416E-01 : 1.3621E-01 : 1.6346E-01 : 1.8296E-01 : *** USER INFORMATION MESSAGE 6464 (DOM12E) RUN TERMINATED DUE TO HARD CONVERGENCE TO AN OPTIMUM AT CYCLE NUMBER = 5.

Testing on larger models has demonstrated that the implementation of parallel sensitivity scales well for statics. Similar performance is expected for other analysis disciplines and on all platforms that support dmp.

Figure 12-4

Main Index

Example problem dspdsa1 run with MEM=2Gb on IBM Power5

302 MD Nastran 2010 Release Guide Parallel Sensitivities

GUI Support for Parallel Sensitivity Pre Processing Neither Patran nor SimXpert supports the DOMAINSOLVER command for Parallel Sensitivity. Direct text input can be used to specify DOMAINSOLVER DSA and the job can be submitted with the additional command line argument DMP=n. Post Processing There are no additional post-processing requirements associated for the parallel sensitivity enhancement.

Main Index


DTABLE Enhancement for Dynamic Analysis Introduction As discussed in Optimization - Invariant DRESP3 Gradients, 289, one component of the design model in gradient based design optimization is the design response definition. The advanced response definitions are available via the equation based response DRESP2, or the external program response DRESP3. In addition to using design variables and direct responses, the user may want to define constants to use in the advanced response equations. These constants can be defined with a DTABLEentry for subsequent use by the DRESP2 or DRESP3. Additional information on design optimization in MD Nastran can be found in the MD Nastran Design Sensitivity and Optimization User’s Guide. The DTABLE enhancement for MD Nastran 2010 allows the DTABLE entry to reference a TABLEDi entry. In MD Nastran 2010, when the DTABLE encounters an Integer input for VALUi, it will use the Real values found on TABLEDi. When the corresponding LABLi is used in a synthesized response DRESP2, the data defined on the TABLEDi entries will be used.

Benefits The DTABLE enhancement benefits dynamic optimization problems that use the MATCH function by greatly simplifying the input. The integer input for DTABLE in MD Nastran 2010 reduces the input to 1 TABLEDi, 1 DRESP1 with ATTB field left blank and a DRESP2 with a single LABLi under DTABLE and a single NRid under DRESP1. Prior to this enhancement, the user would need to define 1. DTABLE with LABLi for each forcing frequency 2. DRESP1 for each forcing frequency 3. A DRESP2 with MATCH function with DTABLE calls out each LABLi and DRESP1 ID involved For a frequency response SOL 200 job with, say, 50 forcing frequencies, one will need DATBLE with 50 (LABLi,VALUi) pairs, 50 DRESP1 each with a single frequency specified and a DRESP2 which has 50 LABLi under DTABLE flag and 50 NRid under DRESP1 flag. The old-style vs. new-style simplified input will be demonstrated in the sample section.

Input The DTABLEBulk Data entry now accepts integer input for a VALUi. The integer value invokes a TABLEDi which carries (freq,value) or (time,value) pairs for a number of frequencies or times, respectively. The TABLEDi will be interpolated for frequency or time values that are not explicitly defined in the table.

Main Index

304 MD Nastran 2010 Release Guide DTABLE Enhancement for Dynamic Analysis

1

2

3

4

5

6

7

8

9

DTABLE

LABL1

VALU1

LABL2

VALU2

LABL3

VALU3

LABL4

VALU4

LABL5

VALU5

LABL6

VALU6

LABL7

VALU7

LABL8

VALU8

10

-etc.-

Output No new output.

Guidelines and Limitations 1. Integer input for DTABLE can be utilized with RTYPE of FRxxxx, PSDxxxx, ACxxxx and Txxxx when the MATCH function selected on DRESP2. 2. For dynamic analysis with DRESP2 selecting MATCH function, spawning of DRESP2 of single frequency (or time) will not be performed. Instead, DRESP2 will include all responses of DRESP1 ID specified. 3. Multiple DTABLE entries are allowed and LABLi on DTABLE must be unique among all DTABLE entries.

Test Cases There are two tests cases in the TPL subdirectory /tpl/dtabl200 that demonstrate the DTABLE enhancement TPL Problem d200tbi1.dat TPL problem d200tbi1.dat is a design optimization job including normal modes (ANALYSIS=MODES) and modal frequency response (ANALYSIS=MFREQ) subcases. For the MFREQ subcase, there are 61 forcing frequencies. To use MATCH function on DRESP2 prior to Nastran 2010, the following table (abridged) shows the input entries involved: Listing 12-11 DTABLE

Main Index

c30 c34 c38 c42 c46 c50 c54 c58 c62 c66 c70 c74 c78 c82 c86 c90

Old-style DTABLE input for MATCH function 1.e+10 1.e+10 1.e+10 1.e+10 1.e+10 1.e+10 1.e+10 1.e+10 1.e+10 1.e+10 1.e+10 1.e+10 1.e+10 1.e+10 1.e+10 1.e+10

c31 c35 c39 c43 c47 c51 c55 c59 c63 c67 c71 c75 c79 c83 c87

1.e+10 1.e+10 1.e+10 1.e+10 1.e+10 1.e+10 1.e+10 1.e+10 1.e+10 1.e+10 1.e+10 1.e+10 1.e+10 1.e+10 1.e+10






$ dresp1,130,f130,frvelo,,,1,30.,701001 dresp1,131,f131,frvelo,,,1,31.,701001 dresp1,132,f132,frvelo,,,1,32.,701001 . . (55 DRESP1 removed) . dresp1,188,f188,frvelo,,,1,88.,701001 dresp1,189,f189,frvelo,,,1,89.,701001 dresp1,190,f190,frvelo,,,1,90.,701001 $ dresp2,330,f330,MATCH +,dtable,c30,c31,c32,c33,c34,c35,c36, +, ,c37,c38,c39,c40,c41,c42,c43, +, ,c44,c45,c46,c47,c48,c49,c50, +, ,c51,c52,c53,c54,c55,c56,c57, +, ,c58,c59,c60,c61,c62,c63,c64, +, ,c65,c66,c67,c68,c69,c70,c71, +, ,c72,c73,c74,c75,c76,c77,c78, +, ,c79,c80,c81,c82,c83,c84,c85, +, ,c86,c87,c88,c89,c90 +,dresp1,130,131,132,133,134,135,136, +, ,137,138,139,140,141,142,143, +, ,144,145,146,147,148,149,150, +, ,151,152,153,154,155,156,157, +, ,158,159,160,161,162,163,164, +, ,165,166,167,168,169,170,171, +, ,172,173,174,175,176,177,178, +, ,179,180,181,182,183,184,185, +, ,186,187,188,189,190

With the DTABLE enhancement, the input for MD Nastran 2010 is shown as follows Listing 12-12

MD Nastran 2010 DTABLE enhanced input for MATCH function

tabled1 530 20. 1.e+10 2000. 1.e+10 DTABLE const 1.e+10 const2 530 $ dresp1,130,f130,frvelo,,,1, ,701001 $ dresp2,330,f330,MATCH +,dtable,const2 +,dresp1,130

endt

Note that this example happens to have a constant matching function. Usually, the matching function in dynamic analysis is not constant and TABLED1 entry may have many more physical lines to define the response curve.

GUI Support for DTABLE Enhancement Pre Processing Neither Patran nor SimXpert supports the MD Nastran 2010 DTABLE Enhancement. Post Processing There are no additional post-processing requirements associated with the DTABLE Enhancement.

Main Index

306 MD Nastran 2010 Release Guide Constants with DTABLE2

Constants with DTABLE2 Introduction As discussed in Optimization - Invariant DRESP3 Gradients, 289, one component of the design model in gradient based design optimization is the design response definition. The advanced response definitions are available via the equation based response DRESP2, or the external program response DRESP3. In addition to using design variables and direct responses, the user may want to define constants to use in the advanced response equations. These constants can be defined with a DTABLE entry for subsequent use by the DRESP2 or DRESP3. Additional information on design optimization in MD Nastran can be found in the MD Nastran Design Sensitivity and Optimization User’s Guide. Historically, the DTABLE entry was used to associate a real constant to a label for subsequent use in design property relations (DVCREL2, DVMREL2, DVPREL2) or advanced design responses (DRESP2, DRESP3). The DTABLE has a simple input that is a paired label / constant (LABLi/VALUi). The DTABLE2 Bulk Data entry extends this capability to “lookup” constant values defined on property, connectivity, and material entries.

Benefits DTABLE2 provides a direct access to fields with real value on property, connection and material entries. This allows the user to change the input file properties without having to redefine all of the values associated to the properties that are defined on a DTABLE entry. The LABLi on DTABLE2 entries can be used interchangeably with LABLi on DTABLE for level 2 property relations: DVCREL2, DVMREL2, and DVPREL2as well as advanced responses: DRESP2and DRESP3.

Input The new Bulk Data entry for DTABLE2 is: Format: 1 DTABLE2

2

3

4

5

LABL1

PNAME1

PID1

FNAME1

LABL3

PNAME3

PID3

FNAME3

PTHK10

PSHELL

10

T

CBARX1

CBAR

3888

X1

6 LABL2

7 PNAME2

8 PID2

9 FNAME2

Example: DTABLE2

Main Index

MAT1E

MAT1

38

E

10


Field

Contents

LABLi

Label for the constant. (Character)

PNAMEi

Property, material or connection bulk data entry name. (Character)

PIDi

ID of PNAMEi entry. (Integer > 0)

FNAMEi

Field name of PNAMEi. (Character)

Output No new output for DTABLE2.

Guidelines and Limitations 1. LABLi on DTABLE2 and DTABLE must be unique among all DTABLE and DTABLE2 entries. 2. LABLi on DTABLE2 can be referenced under DTABLE flag of DVxREL2 (where x=P, M or C) /DRESP2/DRESP3. 3. Value for FNAMEi field of PNAMEi Bulk Data entry with the ID of PIDi are taken from analysis model before updating analysis values with the designed values. If the designed value is desired, use DVxREL2 flag on DRESP2 or DRESP3 entries instead. 4. DATBLE2 is accessible from IFPNEW only. IFPNEW can be turned on with ‘NASTRAN SYSTEM(444)=1’.

Test Cases TPL Problem d200tb2b.dat TPL problem tpl/dtabl200/d200tb2b.dat is modified to use DTABLE2 for the DRESP2 reference. The label DVP11 is associated to PBAR with ID 11, “A” for area. The PNAME “A” is taken directly from the Bulk Data entry PBAR: 1 PBAR

Main Index

2

3

4

5

6

7

8

PID

MID

A

I1

I2

J

NSM

D2

E1

E2

F1

C1

C2

D1

K1

K2

I12

Field

Contents

PID

Property identification number. (Integer > 0)

MID

Material identification number. (Integer > 0)

A

Area of bar cross section. (Real; Default = 0.0)

9 F2

10

308 MD Nastran 2010 Release Guide Constants with DTABLE2

Field

Contents

I1, I2, I12

Area moments of inertia. (Real; I1 > 0.0, I2 > 0.0, I1*I2 > I12 2 ; Default = 0.0)

J

Torsional constant. (Real; Default = 1---  I 1 + I 2  for SOL 600 and 0.0 for all other 2 solution sequences)

NSM

Nonstructural mass per unit length. (Real)

Ci, Di, Ei, Fi

Stress recovery coefficients. (Real; Default = 0.0)

K1, K2

Area factor for shear.(Real or blank)

Listing 12-13

DTABLE2 example input

$ with DTABLE2 $ dtable2 DVP11 pbar dvc110 cbar dvm113 mat1 dvc21 cbar dresp2 1000 rtest desvar 1 dtable l1 dvp23 dresp1 1 dresp2 999

11 1 1 1 1010 2 l2 dvc21

A x1 rho x3

DVP12 dvc111 dvp23 dvm214

PBAR cbar pbar mat1

11 1 11 1

J x2 i1 E

dvp11 dvm214

dvp12

dvc110

dvc111

dvm113

DRESP2,1000 has 10 LABLi including 8 defined via DTABLE2. All 10 LABLi will be considered as constants during design cycles. Note that if these were considered as designed properties instead of design constants, the setup should be as shown in following table for DRESP2,1000. Listing 12-14

Old-style input for using properties as constants

DVPREL1 1 1 DVPREL1 2 1 DVCREL1 10 1 DVCREL1 11 1 DVMREL1 13 1 DVPREL2 3 DESVAR DTABLE DVCREL2 12 DESVAR DTABLE DVMREL2 14 DESVAR DTABLE L1 dresp2 1000 desvar dtable dresp1 dvprel1

Main Index

PBAR 1.0 PBAR 1.0 CBAR 1.0 CBAR 1.0 MAT1 1.0 PBAR 1 L1 CBAR 1 L1 MAT1 1 rtest 1 l1 1 1

11

A

11

J

1

X1

1

X2

1

RHO

11 2 L2 1 2 L2 1

I1

100

X3

100

E

200

1000 2 l2 2

.1

12.

1.5

.1

12.

1.5


dvcrel1 dvmrel1 dvprel2 dvcrel2 dvmrel2 dresp2

10 13 3 12 14 999

11

GUI Support for DTABLE2 Pre Processing Currently, neither Patran nor SimXpert supports DTABLE2. Post Processing There are no additional post-processing requirements associated with DTABLE2.

Main Index

310 MD Nastran 2010 Release Guide New Optimizer - IPOPT

New Optimizer - IPOPT Introduction MSC Software conducts surveys of optimizer technologies from industry and academia. This has lead to the integration of optimizer IPOPT. IPOPT implements an interior point line search filter method that aims to find a local optimal solution for large scale nonlinear optimization. It was originally developed by Carnegie Mellon University in 2002 and now is supported by IBM. Interior point method as one of barrier methods was first proposed in the sixties. Barriers methods are used to transform a “difficult” constrained problem into a sequence of “easy” unconstrained problems. MSCADS SUMT method is one of this classical barrier method and BIGDOT is also based on this approach. Barrier methods were popular during the sixties. However, this classical barrier method has its shortcomings, practitioners of nonlinear programming lost interest and switched to newly emerging, apparently more efficient MMFD and SQP-like methods (MSCADS and DOT) in the mid-seventies and eighties. In the mid-eighties, a modern interior-point revolution started with the well-known Karmarkar linear programming algorithm which can be interpreted as a barrier method. Since then, interior point algorithms have emerged as one of most important and useful algorithms for mathematical programming. In particular, these interior point methods provide an attractive alternative to active constraint set methods in handling problems with large numbers of design variables and inequality constraints. IPOPT is a software package for large scale nonlinear optimization. This code has been shown to be capable of handling tens of thousands of design variables. It can be used to solve SOL 200 sizing, shape, topology, topometry, and topography problems. Currently, SOL 200 has two license options, Design Optimization and Topology Optimization (IPOPT requires the Topology Optimization license feature). In MD Nastran 2010, IPOPT has been made the default optimizer for topology, topometry, and topography design optimization problems. This is done because testing indicates that IPOPT provides a more robust solution than the MSCAD SUMT method. The choice of optimizers can be made with the OPTCOD feature on the DOPTPRMBulk Data entry, or with MD Nastran System Cell OPTCOD (413)). See also notes in the .Licensing, 313.

Benefits In theory, the interior point method is a very robust algorithm that provides an alternative to SOL 200 existing optimizers, in particular, MSCADS SUMT method. The IPOPT optimizer not only enables performing practical topology, topometry, and topography optimization tasks but can also be used to perform standard shape and sizing optimization for design tasks.

Theory In this section, a very brief discussion about the interior point method implemented in IPOPT is presented. More detail can be read on paper “On the implementation of a primal-dual interior point filter

Main Index


line search algorithm for large-scale nonlinear programming”, Mathematical Programming, 106(1):25– 57, 2006 by A. Wachter and L. T. Biegler. To simplify the description of the interior point method, we consider a problem with equality constraints as

minimize

fx

subject to

Cj  X  = 0

j = 1 2   m

Xi  0

i = 1 2 n

(12-1)

where X L and X U are the lower and upper bounds on the design variables X . n is the number of design variables, and m is the number of equality constraints. The objective function f  X  and the inequality constraints C j  X  are assumed to be twice continuously differentiable. Inequality constraints can be transformed to equality constraints by introducing slack variables. In general, gradient-based optimization algorithms have a common strategy as below: A general optimization algorithm loop • Start k = 0 , X = X 0 • Evaluate f  X  and C j  X  • Calculate gradients of f  X  and g j  X  • Determine a search direction d k • Perform a one-dimensional search to find  * that will minimize f  X + d k  subject to the

constraints. • Set X k + 1 = X k +  * d k • Check for convergence. If satisfied, exit. Otherwise repeat the loop

Two critical parts of the optimization task consists of determining a search direction and finding a best one-dimensional search step. The determining a search direction is the most time consuming part and one of major difference between the interior method and SOL 200 other optimization methods.

Main Index


As a barrier method, the interior point algorithm computes (approximates) solutions for a sequence of barrier problems n

  x  = f  x  – 

minimize:



i

ln  x 

(12-2)

i =1

subject to:

Cj x  = 0

j = 1  m

for a decreasing sequence of barrier parameters µ converging to zero. Equivalently, this can be interpreted as applying a homotopy method to the primal-dual equations, f  x  + c  x  – z = 0 cx = 0

(12-3)

XZe – e = 0 with the homotopy parameter  which is driven to zero. Here, R m and zR n correspond to the Lagrangian multipliers for the equality constraints and the bound constraints, respectively. Note, that Eq. (12-3) for  = 0 together with “x; z  0 are the Karush-Kuhn-Tucker (KKT) conditions for the original problem Eq. (12-2). Those are the first order optimality conditions for Eq. (12-1) if constraint qualifications are satisfied Eq. (12-3). In order to solve the barrier problem Eq. (12-2) for a given fixed value  j of the barrier parameter, a damped Newton's method is applied to the primal-dual Eq. (12-3). Here, a search direction is obtained from solving a symmetric linear system Wk + k + w I Ak T

Ak

–c I

x

dk  dk

=

   x k  + A k  k j c  xk 

(12-4)

where Jacobian A k = c  x k  and W k denotes the Hessian  2xx L  x k  k z k  of the Lagrangian function T

L  x  z  = f  x  + c  x   – z

The choice of scalars w and c is discussed in Wachter's paper. The overall efficiency of the interior point method is dependent on solving a  n + m    n + m  sparse linear system Eq. (12-4).

Main Index


Input There are two ways to select the optimizer IPOPT code. One way is by modifying the Nastran system cell OPTCOD (413))as shown in Table 12-1. Table 12-1

System Cell Summary

System Cell Number

System Cell Name

413

OPTCOD

Description and Default Values Specifies which optimization code to be used in SOL 200 (Default = 0, automatic selection for a better performance based on number of design variaables, number of constraints, number of active/violated constraints and computer memory) 3 - MSCADS 4 - IPOPT Optimizer

The second way is by a parameter OPTCOD on a DOPTPRM Bulk Data entry that has options shown in Table 12-2. Table 12-2

DOPTPRM Design Optimization Parameters

Name OPTCOD

Description, Type and Default Values OPTCOD (Character; Default= Blank) = Blank (taken from system cell number 413) = “MSCADS”: MSCADS is used = “IPOPT”: IPOPT is used

.Licensing MSC provides two optimization license options: 1. Optimization (license file FEATURE line MD_Optimization) 2. Topology Optimization (license file FEATURE line MD_Topology_Optimization). The default behavior is as follows: • If both MD_Optimization and MD_Topology_Optimization licenses are found:

The default behavior is that the optimizer and METHOD will be automatically selected for a better performance based on number of design variables, number of constraints, number of active/violated constraints and computer memory. • If MD_Optimization is found but MD_Oopology_Optimization license is NOT found:

The default behavior is that the MSCADS optimizer will be used for models with any sizing, shape design variables, topology, topometry, or topography design variables. The method used in MSCADS is automatically selected.

Main Index


• If MD_Topology_Optimization license is found but MD_Optimization is NOT found:

The default behavior is that the IPOPT optimizer will be used for models with any sizing, shape design variables, topology, topometry, or topography design variables.

Output If default OPTCOD and/or METHOD is used, the program prints injobname.f06 what optimizer and method is used. For example, ***SYSTEM INFORMATIN MESSAGE 6649 (ADS9D) MSCADS METHOD = 1 (MMFD) HAS BEEN SELECTED FOR DESIGN CYCLE= 1. ***SYSTEM INFORMATION MESSAGE 6649 (DOMIP9D) IPOPT HAS BEEN SELECTED FOR DESIGN CYCLE= 1.

There are no outputs that are affected by optimizer selection with the exception that the optimizer output produced using the IPRINT > 0 parameter on the DOPTPRM entry is written to a file “msc_ipopt.out”.

Guidelines and Limitations The optimization results from IPOPT are expected to be comparable to those from other optimizers. Numerical results show IPOPT is a robust optimizer. However, unlike MSCADS, IPOPT does not support active constraint sets. Thus, IPOPT may be slow for problems with many constraints, in particular, many constraints are inactive. If this is the case, the OPTCOD parameter can be used to invoke the MSCADS SUMT optimizer for problems with many design variables and many constraints.

Examples There are several example files in the TPL that can be used to demonstrate the new IPOPT performance.

Main Index


TPL Problem /optim68/icwse01.dat TPL problem icwse01.dat is and intermediate complexity wing shown in Figure 12-5 was solved using MSCADS and IPOPT.

Figure 12-5

Intermediate Complexity Wing Model

This composite structure is modeled with 62 CQUAD4 elements, 55 CSHEAR elements, 39 CROD elements, and 39 CONM2 elements. Two static load cases are imposed along with an eigenvalue load case. The objective was to minimization. There are 153 sizing design variables and 414 stress and failure index constraint and a lower and upper bounds on the first fundamental frequency. To use IPOPT, a parameter OPTCOD=IPOPT is added on Bulk Data entry DOPTPRM such as

DOPTPRM APRCOD delx

2 0.49

DESMAX p1

30 1

DELP p2

0.50

DPMIN 12 OPTCOD

0.001 Ipopt

Table 12-3 shows the IPOPT results for this example and all results are comparable.

Table 12-3

Intermediate Complexity Wing Optimization Results Initial Value

Optimum MSCADS (MMFD)

Objective

1.6892+2

1.9277+2

1.9414+2

Max Con

5.8425+2

8.7297-04

1.3169-03

21

20

# Cycles

Main Index

Optimum IPOPT


TPL Problem /topography/ip3dbeam.dat TPL problem ip3dbeam.dat, shown in Figure 12-6, is used to demonstrate IPOPT for topology optimization. The 3D beam is modeled with 48,000 six-sided solid elements (CHEXA). The geometry, mesh, and loads are shown in Figure 12-6. The structural compliance is minimized with a mass target 0.2 (i.e., 80% material savings).

. Figure 12-6

TPL file /topography/ip3dbeam.dat Beam Finite Element Model

The input data for this example related to topology optimization model is given in Listing 12-5. A Bulk Data entry TOPVAR =1 is used to define a topological design region. Type one design responses DRESP1 = 2 and 10 identify compliance and fractional mass respectively. OPTCOD=IPOPT on the Bulk Data entry DOPTPRM selects the new optimizer IPOPT for solving this optimization problem. SMETHOD= ELEMENT is used to select CASI iterative solver that can provide a major speedup in the solution of large static analyses for solid element models. Listing 12-15

Partial input for file /topography/ip3dbeam.dat

DESOBJ = 10 DESGLB = 1 ANALYSIS = STATICS SMETHOD=ELEMENT $ DIRECT TEXT INPUT FOR GLOBAL CASE CONTROL DATA

Main Index


SUBCASE 1 $ SUBCASE NAME : RUN1_LOAD_CASE SUBTITLE=RUN1_LOAD_CASE SPC = 2 LOAD = 3 BEGIN BULK DCONSTR 1 DOPTPRM, OPTCOD, TOPVAR 1 DRESP1 2 DRESP1 10

2 IPOPT PSOLID FRM COMP

.2 PSOLID .2 FRMASS COMP

1

Figure 12-7 shows the topology optimized result that is smoothed and smoothed by using MD Patran.

This optimal design is very clear without any checkerboard effect.

Figure 12-7

TPL file /topography/ip3dbeam.dat Proposed Topology Design Concept

GUI Support for IPOPT Post Processing Patran supports IPOPT. There are no additional post-processing requirements associated for IPOPT.

Main Index

318 MD Nastran 2010 Release Guide Topology and Topometry Enhancements

Topology and Topometry Enhancements Introduction Topometry optimization is a special form of sizing optimization most commonly used for shell elements whereby each shell element in a property region is allowed to change thickness independently of its neighboring element. This provides the user an insight to the optimum material distribution to achieve the objective while satisfying constraints. Additional element types commonly supported by topometry optimization are non-volume elements such as CWELD, CBUSH, and CFAST. Topology optimization adjusts each elements’ “effectivity” by adjusting the modulus of Elasticity and density to determine a optimum material distribution. Topology optimization can be applied to solid, shell, and beam elements. The two methods are describe in further detail in the MD Nastran Design Sensitivity and Optimization User’s Guide. MD Nastran 2010 contains a few enhancements for SOL 200 topometry and topology optimization capabilities. The enhancements include 1. density constraint method for topology minimum member size control 2. composite (PCOMP) topometry optimization 3. discrete topometry optimization. 4. enhanced TOPVAR entry and casting constraints

Benefits Topology Optimization Density Constraint Method A density constraint method is implemented for topology minimum member size control. This approach is more efficient than the filtering method for topology problems with a very fine mesh and a relatively large predefined minimum member size. Composite (PCOMP) Topometry Optimization This new feature enables SOL 200 to support composite ply-by-ply thickness optimization. The ply-byply means each ply thickness (or orientation angle) per composite element is treated as an independent design variable. The ply thickness can be linked together to support element-by-element thickness optimization. Although topometry optimization is not recommended for topology optimization tasks, it is observed topometry optimization can be used to get “similar topological results” for many cases. Since SOL 200 topology optimization does not support PCOMP entries, this composite TOMVAR can be used to decide which composite element should be retained and which composite element should be discarded from the design space.

Main Index


Discrete Topometry Optimization The discrete optimization capability is expanded to support topometry optimization. This capability enhances the simplicity of the design and hence its manufacturability. Enhanced TOPVAR entry and casting constraints Topology initial value XINIT has a default in MD2010. It is easier and recommended that the user use the default value of XINIT. Aligned mesh option is added to topology casting and extrusion constraints. When aligned mesh is used for topology designed properties with casting/extrusion constraints, a smaller tolerance is used to process casting constraints during optimization. Thus, a better/sharper topology design proposal may be produced. In addition, topology casting constraint capabilities are significantly enhanced in MD 2010.

Input for Topometry Enhancements A review of the topometry and topology optimization section in the MD Nastran R3 and the MSC Nastran 2005 r2 Release Guide is recommended if you are new to MSC.Nastran’s implementation of the topometry and topology technology. The enhanced topometry TOMVAR Bulk Data entry format is: 1

2

3

4

5

6

7

8

9

TOMVAR

ID

TYPE

PID

PNAME/ FID

XINIT

XLB

XUB

DELXV

“DLINK” “DDVAL”

TID

C0

C1

DSVID

Field

Contents

TYPE

Property entry type. Used with PID to identify the elements to be designed. (Character: “PBAR”, “PSHELL”, “PSOLID”, and “PCOMP”, etc.)

“DDVAL”

Indicates that this line defines discrete TOMVAR variables

DSVID

DDVAL entry identifier (Integer > 0)

“DLINK”

Indicates that this line relates a ply thickness to another ply thickness

TID

TOMVAR entry identifier (Integer > 0).

C0

Constant term (Real; Default = 0.0)

C1

Coefficient term (Real; no Default)

Input for Minimum Member Size Enhancements The density constraint approach can be selected by a parameter TCHECK on Bulk Data entry DOPTPRM.

Main Index

10


DOPTPRM Design Optimization Parameter: TCHECK Name

Description, Type and Default Value

TCHECK

Topology Checkerboarding/minimum member size control option. (Integer > -1) -1

Automatic selection of filtering or density constraint for a better result.

1

Filtering algorithm (Default)

2

Density constraint

0

No control

Input for Topology Enhancements The enhanced topology TOPVAR Bulk Data entry format is: Format: 1

2

3

4

5

6

7

8

9

TOPVAR

ID

LABEL

PTYPE

XINIT

XLB

DELXV

POWER

PID

CS

NCS

“SYM”

CID

MSi

MSi

MSi

“CAST”

CID

DDi

DIE

ALIGN

“EXT”

CID

EDi

ALIGN

“TDMIN”

TV

10

Field

Contents

XINIT

Initial value. (Blank or Real, XLB < XINIT < 1.0 Default=blank). Typically, XINIT is defined to match the mass constraint on DRESP1=FRMASS, so the initial design does not have violated constraints. In this case, the default is set to the constraint value. If the mass (DRESP1=FRMASS or WEIGHT) is the objective, the default is 0.9. The default of XINIT is 0.6 for the other cases.

ALIGN

Indicates whether the designed property finite element mesh is precisely aligned with the draw direction or extrusion direction. (Character: “YES” or “NO” or Blank; Default = blank = “NO”)

Output The only change in output for these features is for the Composite Topometry optimization. In this case, a element result file jobname.plyxxx (where xxx is a PCOMP ply identifier) contains the optimal design values for each composite ply. The element result file can be imported into Patran or third party postprocessor to display composite topometry optimization results.

Main Index


Guidelines and Limitations • DISCOD = 3 and 4 (discrete processing method) is recommended for discrete topometry

optimization tasks since topometry Optimization usually involves many design variables and DISCOD = 4 is the fast discrete processing method. • The density constraint approach is more efficient. However, this approach may result in more

unexpected intermediate density elements than the filtering approach.

Examples TPL Problem /topography/tomex5.dat TPL problem /topography/tomex5.dat is a 2D Composite Plate example intended to demonstrate a plyby-ply thickness optimization using the TOMVAR entry. This composite plate has 640 CQUAD4 element as shown in Figure 12-8. The ply layup is symmetric: 0°, 90°, 45°, -45°,-45°,45°,90°,0°. The objective is to minimize structural compliance and lower/upper bounds are applied on each ply thickness. since the composite is modeled with the “SYM” option, there are 4 independent design variables. The problem is treated as a planar problem an dofs 3456 are permanently constrained on a GRDSET entry. The input data for this example pertinent to the composite lay up and topometry optimization model is given in Listing 12-16. The TOMVAR Bulk Data entries 1-4 define the ply-by-ply thickness optimization. It is noticed that all four ply thickness per element are independent variables. Thus, there are 640x4 independent design variables.

Figure 12-8

A Composite Plate example tomex5.dat

Listing 12-16

Partial Input File for tomex5.dat

$COMPOSITE TOPOMETRY OPT EXAMPLE DESOBJ = 10

Main Index


ANALYSIS = STATICS $ DIRECT TEXT INPUT FOR GLOBAL CASE CONTROL DATA SUBCASE 1 $ SUBCASE NAME : RUN1_LOAD_CASE SUBTITLE=RUN1_LOAD_CASE SPC = 2 LOAD = 3 BEGIN BULK PCOMP 1 -.0105 0.0 0.65E6 TSAI 70 1.000 0.0 YES 70 1.000 90. 70 1.000 45. YES 70 1.000 -45. DOPTPRM, OPTCOD, IPOPT DRESP1 10 COMP COMP $...DESIGN TOPOMETRY DESIGN DEFINITION TOMVAR, 1 , PCOMP, 1, T1 , .5, 1.25-3, 1.0 TOMVAR, 2 , PCOMP, 1, T2 , .5, 1.25-3, 1.0 TOMVAR, 3 , PCOMP, 1, T3 , .5, 1.25-3, 1.0 TOMVAR, 4 , PCOMP, 1, T4 , .5, 1.25-3, 1.0

SYM YES YES

In addition to the standard .f04, .f06 and .pch output files, the final ply thickness distributions are contained in files tomex5.ply0001, tomex5.ply0002, tomex5.ply0003, tomex5.ply0004. To post process these in Patran, they must be read from the tools menu, and then the results can be displayed using standard Patran fringe plots.

Figure 12-9

Main Index

Importing ply topometry results in Patran


Figure 12-10 through Figure 12-13 show the optimized ply thickness distribution for all elements.

Main Index

Figure 12-10

Ply 1 Thickness Distribution of 0° plies

Figure 12-11



Figure 12-12


Figure 12-13

Ply 4 Thickness Distribution -45° plies

The DLINK feature can be used to relate one ply thickness to another ply thickness in order to support composite element-by-element thickness optimization. The input data for this example is given in Listing 12-17. The DLINK line is used to explicitly link the thickness of plies 2, 3, and 4 to ply 1. Thus, each composite element has only one independent design variables.

Main Index


Listing 12-17

Input File for tomex6.dat with DLINK

$...DESIGN TOPOMETRY DESIGN DEFINITION TOMVAR, 1 , PCOMP, 1, T1 , .5, TOMVAR, 2 , PCOMP, 1, T2 , .5, , DLINK, 1, 0.0, 1.0 TOMVAR, 3 , PCOMP, 1, T3 , .5, , DLINK, 1, 0.0, 1.0 TOMVAR, 4 , PCOMP, 1, T4 , .5, , DLINK, 1, 0.0, 1.0

1.25-3, 1.25-3,

1.0 1.0

1.25-3,

1.0

1.25-3,

1.0

Figure 12-14 shows the optimized element-by-element thickness distribution. Note that only 1 ply output file is generated: tomex6.ply0001.

Figure 12-14

Composite Element Combined Thickness Distribution

GUI Support for PCOMP Topometry Pre Processing Patran supports topometry optimization, but the DLINK,DDVAL options are not yet supported. The current “Quick” topology, topometry, topography optimization setup can be read in the Patran 2008R2 Release Guide.

Main Index


Post Processing Patran supports post processing of PCOMP Topometry enhancements as described previously in Output, 320.

Main Index


Optimization of Nonlinear Structural Responses Phase 2 (Pre-release) Introduction MSC Software’s MD Nastran R3 introduced a basic nonlinear response optimization capability (ESLNRO) that is based on the Equivalent Static Loads concept. It allows the user to perform sizing and shape optimization tasks by including geometry and/or material nonlinearities and leverages the linear multidisciplinary design optimization capability in SOL200 (Ref.1). For example, a large-scale nonlinear response optimization task of a joined-wing problem was solved with the MD Nastran R3 capability (Ref.2). The MD Nastran 2010 release has further extended this capability in the following areas: 1. Support of 3D contact in addition to geometry and material nonlinearities; 2. Support of topology optimization applications; 3. Support of new response types = SPCFORCE, FRMASS, COMP. Now with all three nonlinearities are supported in the nonlinear response optimization tasks and the design space covers sizing, shape or topological changes, the capability should open up more and more application possibilities. Since the ESLNRO capability is still a fairly new product, it will require a combined effort of the users and developers to make it a better product. The users are encouraged to apply the new capability and to share experience and provide feedback that can lead to future enhancements. The following describes the current status of the ESLNRO for MD Nastran 2010. What is supported: • Analysis = NLSTATIC, • Geometry (large displacement), material and boundary nonlinearities, • Nonlinear stress responses are available from the basic nonlinear elements: CBEAM, CROD,

CTUBE, CQUAD4, CQUADR, CTRIA3, CTRIA6, CHEXA, CPENTA, CTETRA. • Enhanced Nonlinear Elements (PBEMN1, PSNL1D, PSNL2D, PSLDN1) can be included in the

analysis model as long as no TOPVAR is present. The stress responses of these elements may also be optimized if they can be mapped to that of the basic nonlinear elements. • RTYPE = DISP, STRESS, WEIGHT, VOLUME, SPCFORCE, FRMASS, COMP. • DRESP2 • DESVAR, DVPRELx, TOPVAR

What is not supported: • TOMVAR, BEADVAR • DVMRELx, DVCRELx

Main Index

328 MD Nastran 2010 Release Guide Optimization of Nonlinear Structural Responses Phase 2 (Pre-release)

• CASI solver in linear response optimization for displacement and stress responses • Both TOPVAR and enhanced Nonlinear Elements in the same job

Benefits • Allow all three nonlinearities of geometry, material and boundary in an ESLNRO design task. • Leverage the advanced nonlinear analysis capability in SOL 400 and the powerful linear

multidisciplinary design optimization capability in SOL 200 • Enable to solve large-scale nonlinear optimization tasks (thousands of design variables and

constraints).

Methodology Basic Optimization Statement A general nonlinear response optimization problem can be stated as below:

Find:

X

Minimize:

F  X U NL  g  X U N L   0

Subject to: and

XL  X  XU K  X U NL U NL = P and   U  = 0 for contact conditions

where F  X UNL  is the objective function such as structural weight, nonlinear compliance, maximum displacement or any user defined response, g  X UNL  is the design constraint such as displacement, stress, fractional mass in topology optimization or any user defined constraint. Since the finite element based nonlinear analysis solver is used, the basic equilibrium equation, K  X U NL U NL = P and the contact condition is any,   U  = 0 must also be satisfied. Notice the solution to the equilibrium equation requires iterative process in addition to the optimization design loop. ESLNRO In the ESLNRO, the nonlinear response optimization problems is first transformed into a linear problem using the equivalent static loads that are obtained from a nonlinear analysis and the original problem is indirectly solved by a linear response optimization procedure. The whole process repeats until it converges.

Main Index


The ESLNRO approach involves three-iterative-procedures: K  X U NL U NL = P U = 0

P eq = K L U NL

K L  X U L = P e q U = 0

ESLNRO Loop

Find:

X

Minimize:

F  X U L 

Subject to:

K L  X U L = P eq

Nonlinear analysis

Transformation to ESL

Linear contact analysis with ESL

U = 0 UL  U *

L  

Al l o w a b l e

Linear response optimization including contact conditions

Allowable

*

 L ' =    L   =  N L   L Notice U L = U NL and  L =  NL at start of linear response optimization The main solution driver, or the ESLNRO loop controls the executions of two sub-iterative solutions for nonlinear analysis and linear response optimization. The following three sub-sections will discuss several topics that are critical to a successful ESLNRO process.

The Enhanced Convergence Criteria for ESLNRO An ESLNRO job will be terminated if one of the conditions is satisfied. The design cycle here refers the ESLNRO design cycle (or the outer loop) not the design cycle in the linear response optimization (or the inner loop).

Main Index


1. the maximum change among all design variables between the current and previous design cycles is less than a given tolerance (CONVDV) for two consecutive design cycles or 2. the linear response optimization task achieves hard convergence in a single inner design cycle for two consecutive ESLNRO design cycles or 3. the percentage of design variables that have their relative changes satisfy the tolerance (CONVDV) exceeds the user-supplied tolerance (TOPOCONV) for two consecutive design cycles. This only applies to topology optimization applications or 4. the maximum number of design cycles (DSMXESL) is reached For an ESLNRO job terminated due to conditions 1 through 3, the following message will be printed out in the f06 file: **************************************************************************** ESLNRO CONVERGENCE ACHIEVED ON THE FOLLOWING CRITERIA (HARD CONVERGENCE DECISION LOGIC) 1)

MAXIMUM OF RELATIVE D.V. CHANGES = EEEEEEEEEEEE IS LESS THAN EEEEEEEEEEEE FOR 2 CONSECUTIVE ESLNRO DESIGN CYCLES;

2)

TWO CONSECUTIVE LINEAR RESPONSE OPTIMIZATION RUNS ACHIEVED HARD CONVERENCE IN A SINGLE DESIGN CYCLE.

--- OR ---

--- OR --3)FFFFFFFF% OF DESIGNED ELEMENTS OR IIIIIIII DESIGNED ELEMENTS HAVE THE RELATIVE VALUE CHANGE THAT IS LESS THAN THE EEEEEEEE (CONVDV). THE HARD CONVERGENCE IS ARCHIEVED IF IT EXCEEDS FFFFFFFF% (TOPOCONV). ****************************************************************************

Figure 12-15

Special Strategy to Handel Divergent Nonlinear Analyses

During a topology optimization process, the program adds density to the element with higher strain energy and reduces density from the element with lower strain energy to minimize the compliance while maintaining the weight constraint. Iteratively, this will result in a collection of elements with lower strain energy or ‘empty’ elements. Although creating empty and non-empty element groups is the goal of topology optimization, the empty elements introduce singular behaviors to the analysis itself. When enough ‘empty’ elements exist in the structure, the nonlinear analysis tends to fail to converge. In MD Nastran 2010, a simple strategy has been implemented to handle divergent nonlinear analyses. If a nonlinear analysis fails to converge at the initial design cycle, the job is terminated with appropriate message for the user to improve the model. However, if a divergent analysis is encountered for design cycles greater than 1, the design move produced by previous design cycle is cut by half and a new analysis is performed on the reduced design. This heuristic strategy will be consecutively for five design cycles. If the nonlinear analysis still fails to converge, the job will be terminated. Special Move Limit Scheme for topology optimization tasks For topology optimization tasks, only the scaled-back scheme is supported (See Ref.1 for discussions of move limits).

Main Index


Implementation The ESLNRO capability is implemented using a multiple invocation strategy to bring SOL400 and SOL200 together to provide an integrated solution for nonlinear response optimization tasks. From the user point of view, a single user input file is required to specify both nonlinear analysis model and the design model set up. Behind the scenes, communications between the ESLNRO driver, SOL400 and SOL200 are through various intermediate files. You may consult Release Guide for MD Nastran R3 (Ref.1) for more detailed discussion how to manage these files. Input The following are the new parameters introduced in MD Nastran 2010 for ESLNRO. ESLLCOMP Default = NO ESLLCOMP selects types of compliance response to be included in the design task. The nonlinear compliance response is defined using a DRESP1 entry with RTYPE=COMP for the ESLNRO topology optimization tasks. As the default, it is computed by the product of the applied nonlinear loads and corresponding nonlinear displacement components. Alternatively, ESLLCOMP=YES selects a linear compliance response that computed as the total work done by the equivalent static loads on the linear system. ESLMPC1 Default = 0 This parameter applies only to the ESLNRO jobs with 3D contact. Its default has different meanings depending on the type of contact applications. As the default, for a glued contact ESLNRO job, a linear response optimization task will include a set of MPC entries that are created from the nonlinear analysis. For a touching contact ESLNRO job, the linear response optimization task will not include the MPC entries by default. Setting ESLMPC1 to a positive number will turn on the MPC inclusion. ESLMPC1 = 1: uses the MPC entries created from the nonlinear analysis at the converged nonlinear analysis. ESLMPC1 = 2 uses the MPC entries created at the beginning of the very first nonlinear analysis ESLOPTEX Default = 0 The parameter allows the user to perform an ESLNRO job at a targeted exit point. The allowable values of ESLOPTX are listed below with their description. 0 - Do not exit. Proceed with ESLNRO nonlinear response optimization. 1 - Exit after the initialization of the analysis and design model but before nonlinear FE analysis begins. 2 - Exit after nonlinear FE analysis ends.

Main Index


3 - Exit after design constraint evaluation and screening. ESLPRT Default = 0 ESLPRT specifies how often the ESLNRO results are printed in the f06 file and saved in the xdb file. By default, the program will print the results to the f06 file at the first and the last design cycles and save the results to xdb (or op2) at the first and last design cycles on the disk (See ESLPRT1 for selection of result contents). ESLPRT > 0, then the results are printed at the first design cycle; at every design cycle that is a multiplier of ESLPRT; and the last design cycle. ESLPRT < 0, the no results are printed and saved. ESLPRT1 Default = 7 ESLPRT1 specifies what type of results to be written to the f06 and to xdb (or op2). It may take any of the following base values or to a combination of these base values. ESLPRT1 = 0, write no data. ESLPRT1 = 1, write the nonlinear analysis results to the f06 file. ESLPRT1 = 2, write the optimization data controlled by P1 and P2 to the f06 file. ESLPRT1 = 4, save the nonlinear analysis results to the xdb (or op2) file. ESLPRT1 = 8, save the linear response optimization results to the xdb (or op2) file. For example, by default, results from the nonlinear analysis, the optimization data will be written to the f06 file and result data will be written to xdb or op2. ESLUNT1, ESLUNT2 Default = 53, 54 File units are used to store and retrieve design variables and design properties for ESLNRO topology optimization tasks. TOPOCONV Default = 80 Parameter TOPOCONV is applicable only to ESLNRO topology optimization tasks. It sets a lower bound for the percentage of the design variables whose maximum relative changes are within the tolerance specified by CONVDV on the DOPTPRM entry. By default, when more than 80% of the design variables show their maximum relative changes are within CONVDV, the job will be terminated.

Main Index


Output The output created by an ESLNRO job can be divided into following types: 1. results from nonlinear analysis run and linear optimization run arranged in the design cycle order. 2. xdb (or op2) fiel per nonlinear design cycle: one for nonlinear analysis results and another for linear optimization results. 3. For sizing and shape optimization jobs, the design history of objective, maximum constraints and design variables in the CSV format and a complete updated Bulk Data section are always created in the pch file based on the final design. 4. for topology optimization jobs, a .des file is created that can be used to show the optimized configuration. 5. a new ASCII file with a comprehensive summary of design history. Results from nonlinear analysis run and linear optimization run By default, the nonlinear analysis results at the initial and the last design cycles are printed to the f06 file. The following listing shows a sample output for the initial design cycle.

Main Index


******************************************************* * * * I N I T I A L E S L N R O D E S I G N C Y C L E * * * ******************************************************* ^^^ A NONLINEAR ANALYSIS JOB INITIATED WITH FOLLOWING COMMAND: /nast/md2009t1/linux64/nastran /scratch/shz/deslo1_nlsol400 scr=yes bat=no rcf=eslonc out=/scratch/shz/deslo1_nlsol400

...... 0

*********************************************** * * * I N I T I A L A N A L Y S I S (S T A R T) * * * *********************************************** N O N - L I N E A R

LOOP CONTROLS FOR :

SUBCASE

I T E R A T I O N 1,

S O L U T I O N

STEP

SOLUTION CONTROL PARAMETERS FROM : NLPARM

……

1, ID :

Number of Increments (NINC) ............. Incremental Time for Creep (DT) ......... Matrix Update Option (KMETHOD) .......... Matrix Update Increment (KSTEP) ......... Maximum Number of Iterations (MAXITER) .. Convergence Options (CONV) .............. Intermediate Output Flag (INTOUT) ....... - Displacement (EPSU) ...... Tolerance - Residual Force (EPSP) ...... - Work (EPSW) ...... Divergence Limit (MAXDIV) ...............

10 0.00E+00 AUTO 10 25 P V NO 1.00E-02 1.00E-02 1.00E-02 3

Maximum Incremental Rotation (RTOLB) .... Minimum Number of Iterations (MINITER) ..

2.00E+01 0

*** USER INFORMATION MESSAGE 6204 (NL3EMA) 9.999990E-03 SECONDS REQUIRED TO DECOMPOSE MATRIX.

1

NASTRAN MODEL - NLC013B IS THE MARC MODEL 0 0 N O N - L I N E A R ............................................. ............................................. .............................................

C O N T R O L

SUBSTEP

I T E R A T I O N

P A R A M E T E R S

0

1

AUGUST M O D U L E

28, 2009

MD NASTRAN

8/28/09

PAGE

33

O U T P U T

*********************************************** * * * I N I T I A L A N A L Y S I S (E N D) * * * ***********************************************

By default, the printout from a linear optimization run, controlled by P1 and P2 on the DOPTPRM entry is printed to the f06 file. The following listing shows a sample output for the initial design cycle.

Main Index


^^^ A LINEAR OPTIMIZATION JOB INITIATED WITH FOLLOWING COMMAND: /nast/md2009t1/linux64/nastran /scratch/shz/deslo1nn_eslsol200 scr=yes bat=no r cf=eslonc out=/scratch/shz/deslo1nn_eslsol200 /nast/md2009t1/linux64/nastran /scratch/shz/deslo1nn_eslsol200 scr=yes bat=no rcf=eslonc out=/scratch/shz/deslo1nn_eslsol200 -----

DESIGN OBJECTIVE

-----

---------------------------------------------------------------------------------------------------INTERNAL MINIMIZE RESPONSE RESPONSE OR SUPERELEMENT SUBCASE ID DRESPx TYPE MAXIMIZE ID ID VALUE ---------------------------------------------------------------------------------------------------1 DRESP2 N/A MINIMIZE N/A N/A 1.4707E+04 -----

1 0

DESIGN VARIABLES

-----

--------------------------------------------------------------------------------------------------------INTERNAL DESVAR LOWER UPPER ID ID LABEL BOUND VALUE BOUND --------------------------------------------------------------------------------------------------------1 3 PSHELL:1 5.0000E-03 1.0000E-01 1.0000E+01 2 4 PSHELL:2 5.0000E-03 1.2500E-01 1.0000E+01 3 1 PSHELL:1 5.0000E-03 1.0000E-01 1.0000E+01 4 2 PSHELL:2 5.0000E-03 1.2500E-01 1.0000E+01 AUGUST 28, 2009 MD NASTRAN 8/28/09 PAGE NASTRAN MODEL - NLC013B IS THE MARC MODEL SUBCASE1 -----

DESIGNED PROPERTIES

-----

---------------------------------------------------------------------------------------------------------PROPERTY PROPERTY PROPERTY TYPE OF LOWER UPPER TYPE ID NAME PROPERTY BOUND VALUE BOUND ---------------------------------------------------------------------------------------------------------PSHELL 1 T DVPREL1 N/A 1.0000E-01 N/A PSHELL 2 T DVPREL1 N/A 1.2500E-01 N/A PSHELL 11 T DVPREL1 N/A 1.0000E-01 N/A PSHELL 22 T DVPREL1 N/A 1.2500E-01 N/A -----

DESIGN CONSTRAINTS ON RESPONSES

-----

(MAXIMUM RESPONSE CONSTRAINTS MARKED WITH **)

1

Main Index

--------------------------------------------------------------------------------------------------------INTERNAL EXTERNAL INTERNAL INTERNAL DCONSTR RESPONSE DRESPx RESPONSE L/U REGION SUBCASE ID ID ID ID TYPE FLAG ID ID VALUE --------------------------------------------------------------------------------------------------------1 200 9 1 STRESS UPPER 200000000 1 1.4529E-01 2 200 10 2 STRESS UPPER 200000000 1 1.4432E-01 3 200 11 3 STRESS UPPER 200000000 1 7.5701E-02 4 200 12 21 STRESS UPPER 200000000 1 1.4644E-01 5 200 13 22 STRESS UPPER 200000000 1 1.4371E-01 6 200 14 23 STRESS UPPER 200000000 1 1.3030E-02 7 200 15 41 STRESS UPPER 200000000 1 1.4735E-01** 8 200 16 42 STRESS UPPER 200000000 1 1.4343E-01 9 200 17 61 STRESS UPPER 200000000 1 1.4735E-01** 10 200 18 62 STRESS UPPER 200000000 1 1.4343E-01 11 200 19 81 STRESS UPPER 200000000 1 1.4644E-01 12 200 20 82 STRESS UPPER 200000000 1 1.4371E-01 13 200 21 83 STRESS UPPER 200000000 1 1.3025E-02 14 200 22 101 STRESS UPPER 200000000 1 1.4529E-01 15 200 23 102 STRESS UPPER 200000000 1 1.4432E-01 16 200 24 103 STRESS UPPER 200000000 1 7.5693E-02 17 200 25 160 STRESS UPPER 200000000 1 1.5630E-02 18 200 26 180 STRESS UPPER 200000000 1 4.8893E-02 19 200 27 200 STRESS UPPER 200000000 1 4.8889E-02 20 200 28 220 STRESS UPPER 200000000 1 1.5615E-02 21 200 2 1001 DISP LOWER 1001 1 -3.6981E-02 22 200 3 1001 DISP LOWER 1001 1 -3.6980E-02 23 200 4 1001 DISP LOWER 1001 1 -3.6979E-02 24 200 5 1001 DISP LOWER 1001 1 -3.6978E-02 25 200 6 1001 DISP LOWER 1001 1 -3.6978E-02 26 200 7 1001 DISP LOWER 1001 1 -3.6979E-02 27 200 8 1001 DISP LOWER 1001 1 -3.6980E-02 AUGUST 28, 2009 MD NASTRAN 8/28/09

152


1. If PARAM, POST, n is requested in the user input file, the analysis results will be stored in a separate xdb or op2 file with a new name: fn_postxxx where fn is the initial user input file name, post is the reserved key word and xxxx is the design cycle number at which the results are created. For example, assume the user input file has a job name as myjob, the job is terminated at design cycle 25 with PARAM,POST,0, by default, new files named as myjob_post0000.xdb and myjob_post0025.xdb will be generated after the job is run successfully. 2. A New ASCII File with Comprehensive Summary of Design History This file will be useful to monitor the ESLNRO job. **************************************************************************************** C O M P R E H E N S I V E S U M M A R Y O F D E S I G N C Y C L E H I S T O R Y **************************************************************************************** Totycle NL.DSCycle LinearDSCycle Objective Maxconst 1 1 0 3.219942E+04 3.929590E-03 2 1 1 7.717369E+03 -8.570094E-02 3 1 2 6.356784E+03 -3.654086E-02 4 1 3 5.621113E+03 0.000000E+00 5 1 4 5.621083E+03 0.000000E+00 6 2 0 9.169358E+04 2.975586E-04 7 2 1 9.911871E+03 -8.711449E-06 8 2 2 9.855386E+03 -8.711449E-06 9 2 3 9.855385E+03 -8.711449E-06 10 3 0 8.065990E+04 5.532227E-04 11 3 1 8.765772E+03 3.244820E-01 12 3 2 9.714928E+03 -1.352803E-02 13 3 3 9.714928E+03 -1.352803E-02 14 4 0 5.646795E+04 1.196680E-03 15 4 1 7.785467E+03 -3.360441E-03 16 4 2 7.708911E+03 -3.360441E-03 17 4 3 7.708912E+03 -3.360441E-03

Guidelines and Limitations 1. Familiarity of SOL400 and SOL200 is required to use ESLNRO. 2. Specify nonlinear stress item codes on the atta field on a DRESP1 entry for nonlinear stress quantities. These codes can be found in the Appendix of the Quick Reference Guide. 3. Add keyword sdir=mydir in your command line to redirect all your intermediate files generated from your job to a designated location to better maintain those files. 4. Use PARAM, ESLRCF, rcfnam to customize the separate Nastran runs. One of its use is to include a dmap alter. For example, Mem=120m $ allocate 120 Million words of memory #debug:my.alter $ include a dmap alter for intermediate runs. If DRSPAN is used, PARAM, ESLLCOMP, YES must be included in your job for a job with a compliance response (i.e., RTYPE=COMP on a DRESP1 entry). 5. Use smaller design move limits (both delxesl and delx) for the highly nonlinear ESLNRO tasks such as topology optimization with large deformation.

Main Index


6. For the design tasks that have a contact body relying on other contact body to prevent rigid body motion, the MPC equations should be included in the linear optimization using PARAM, ESLMPC1, 1. However, this setting does not produce good results as expected and requires more studies.

Examples Example 1 Designing Cantilevers With General Contact (deslo1.dat) in /tpl/nlropt2427 This problem consists of two cantilever plates modeled with CQUAD4 elements and fixed at both ends and the top surface of the cantilever is loaded with the pressure load and the bottom surface is loaded at the free tip as shown in Figure 12-16. Originally, two beams are separate. Without including the contact condition, the problem would treat the top beam as a simple cantilever under a pressure load as if the bottom beam is disjoined. However, when the general contact is considered, the intensity of the pressure load on the top surface eventually forces the top beam to touch the bottom one. Then, the bottom cantilever acts a flexible supporting mechanism to slow the downward movement of the top beam. In addition, a different plastic material is specified for each surface with MATS1. The detailed MATS1 entries and 3D contact entries can be found in the user input file, deslo1.dat.

Pressure loads applied on the whole top

Figure 12-16

Main Index

Model definition for Example 1


Figure 12-17

Initial Deformed Stress Contour

Figure 12-17 plots the stress contour on the deformed shapes of two beams. The higher stress occurs at two fixed ends of the beams (1.76E+05) whereas the maximum displacement occurs at the free end of the bottom cantilever.

The design task is to minimize the structural weight while limiting the deformation at given grid points and all the element stresses by varying the thicknesses of top and bottom surfaces. Notice the gap constraint is imposed to ensure the distance between the middle planes of the top and bottom beams. The job starts with an infeasible design and takes 7 design cycles to converge to a feasible design as shown in Figure 12-18. Figure 12-19 plots the design variable history. Both xy-plots are created using CSV file saved in the punch file for an ESLNRO job.

Weight

Designing Cantilevers w ith Contact 17500

0.30

17000

0.25

16500

0.20

16000

0.15

15500

0.10

15000

0.05

14500

0.00 0

Figure 12-18

Main Index

2

4

6

8


Design Variable History

Thick ness

0.15 0.14 0.13 0.12 0.11 0.10

0

2

4

6

8

De sign Cycle T of Bottom Cantilever

T of Top C antile ver

Figure 12-19

Figure 12-20

Final Stress Contounr

Figure 12-20 plots the final stress contour on the deformed structure. The maximum stress still occurs at the fixed end of the bottom beam but has been reduced to 1.41E5 from 1.76E5 whereas the maximum deformation is reduced to 0.09 from 0.11.

Main Index


Example 2 Topology Optimization Problem with Large Deformation (deslo9.dat, deslo9a.dat, deslo10.dat, deslo10a.dat and deslo9l.dat, deslo9al.dat) This problem is originally published in Ref. 3 that shows the necessity to include nonlinear analysis with topology optimization when large deformation is involved. A rectangular plate is modeled with CQUAD4 elements (not shown) and has the dimension of 0.8m by 0.2m by 0.001m (width by height by thickness). The middle points at both ends are fixed except the z-rotational degree of freedom. A concentrated force is applied at the middle point on the top as shown in Figure 12-21.

200.N

0.2m

0.8m

Main Index

Figure 12-21

A Rectangular Plate Model

Figure 12-22

Initial Deformation Plot


The deformation of the initial model is plotted as shown in Figure 12-22. The maximum displacement occurs at the loading point with the value of is 0.249m, about 2.5 times of the height of the plate. So this is a nonlinear problem with a large deformation behavior. The design task is to find an ‘optimal’ distribution of materials on this rectangular plate to minimize the nonlinear compliance while maintaining 20% of the original weight under the large displacement condition. First, a linear topology optimization job of the same model is solved with SOL 200 (deslo9l.dat). It converges in 39 design cycles. The final configuration with is shown in Figure 12-23. The plot is created using Patran’s DesignTool/Post-Process with the threshold value of 0.2. Let us call it the updated linear structure (or FE model). One can see that the right and left arms of the updated linear structure are in compression under the original loading condition.

Figure 12-23

Final configuration from linear topology optimization

Next, the same job is solved by the new ESLNRO capability under the large displacement condition (deslo9.dat). The job converges in 89 design cycles. Its final configuration is shown in Figure 12-24 that is created using Patran’s Design Tool/Post-Process/Display Results with the threshold value of 0.2. We will call it the updated nonlinear structure (or FE model). Notice the updated structure is in always tension.

Figure 12-24

Final configuration from nonlinear topology optimization

It is clear that the updated linear and nonlinear structures are very different. One may notice that under the current loading condition (see Figure 12-21), a part of the updated linear structure is under compression while the updated nonlinear structure is all in the tension. To verify which structure is more capable of sustaining the nonlinear load condition, first Patran’s Group techniques are used to create an updated FE model for both the linear and nonlinear structures as shown in Figure 12-23 and Figure 12-24. Next, the nonlinear analysis is performed on each of two structures with the original loading (deslo9al.dat and deslo9a.dat).

Main Index


The final results are very interesting: the updated linear FE structure collapses due to local buckling because the right and left arms are in compression. On the other hand, the updated nonlinear FE model performs well. Figure 12-25 plots the deformation from the updated nonlinear FE model under the original loading. The maximum displacement of 0.0184m occurs at the loading point.

Figure 12-25

Displacement plot of the updated nonlinear structure

This example shows that it is necessary to perform the topology optimization by including nonlinear analysis responses. Notice Ref. 3 published a final configuration that is given in Figure 12-26. It is significantly different from both the updated linear structure and the updated nonlinear structure as shown in Figure 12-23 and Figure 12-24. According to Ref.3, this updated nonlinear structure also performs well under the original loading.

Figure 12-26

Final configuration obtained by Ref.3

It is natural to ask why it is significantly different from the updated nonlinear structure obtained by ESLNRO (Figure 12-24). One explanation lies in that the objective function used by Ref.3 is nonlinear mean compliance that is the sum of nonlinear strain energy and complementary energy. However, the nonlinear compliance response in the ESLNRO is the sum of the product of applied loads and the corresponding nonlinear displacement components or the work done. In the linear analysis, the strain energy and its complementary energy are same. So the total work done is twice the strain energy.

Main Index


However, in the geometrically nonlinear analysis, the above relation does not hold. The nonlinear compliance response defined in ESLNRO is different from the mean compliance response. To carry out the study further, a new ESLNRO job is performed by setting DESMAX to 1. This enforces that the linear optimization job is only carried out in one design cycle and it then immediately returns the proposed new design back to the ESLNRO loop. A new set of equivalent static loads will be generated from the updated nonlinear analysis. The purpose of this exercise is to update the equivalent static loads as much as possible since the equivalent static loads in a linear optimization is invariant. The final configuration based on this strategy is shown in Figure 12-25. The final configuration agrees well with the published results (See Figure 12-26) except two small closed loops are formed at the bottom of the structure. Figure 10 is created using Patran’s Design Tool/Post-Process/Display Results with the threshold value of 0.2. It should be pointed out that this run does not achieve hard convergence. In stead, it is terminated after 5 consecutive nonlinear analyses unable to find a converged solution.

Figure 12-27

Plot of displacement for the alternate updated nonlinear structure

Furthermore, an independent nonlinear analysis is performed for the updated nonlinear FE model under the original loading (deslo10a.dat). The deformation plot from this nonlinear analysis is shown in Figure 12-28 with the maximum displacement of 0.021m that occurs at the loading point.

Figure 12-28

Main Index

Plot of displacement for the alternate updated nonlinear structure


From this example, we have learned that it is important and necessary to perform the topology optimization by including large displacement as nonlinear responses. In addition, if measured in terms of the maximum displacement, both updated nonlinear structures from Figure 12-24 and Figure 12-27 are close, 0.0184m vs. 0.021m. However, their configurations are significantly different. Therefore, the nonlinear topology optimization tasks are more difficult to solve than the linear ones because it not only tends to show the local minima phenomenon but also the nonlinear analyses may not lead to convergent solution because the collection of elements with lower strain energy or ‘empty’ elements.

References 1. MD Nastran R3 Release Guide, 2008. 2. S. Zhang, E. H. Johnson, D. Chou, L. Proctor & G.J. Park, “Optimization of Nonlinear Structural Responses with MD Nastran,” Proceedings of the 12th AIAA/ISSMO Multidisciplinary Analysis and Optimization Conference, 10-12 Sept. 2008 3. H. C. Gea and J. Luo, “Topology optimization of structures with geometric nonlinearities,” Computers & Structures 79(2001) 1977-1985

Main Index


Build External Servers Using the SCons Tool Introduction MD Nastran provides the external server capability (beam library, DRESP3 and Spline servers) to allow the client to create their custom applications without modifying the Nastran program. Prior to MD Nastran 20101, the binary server executables are built using make utilities. Starting this release, they will be built using the SCons tool.

Overview SCons is a Software Construction tool. Its major benefits are given below. It is expected that SCons tool provide same or better experience to build an external server. 1. Automatically to resolve source code dependencies; 2. Fairly easy to build binary programs on various platforms with different operating systems. It is particular true for building external server programs on Windows; 3. Easy to develop applications that use combined Python scripts and other source codes written in C or Fortran because SCons configuration files are written in Python scripts; 4. Easy to extend the server template codes by simply adding your source codes to the target directory without the need to modify SConscript. Although DRESP3 server is used to describe the procedures to build an external server, they can be applied directly to beam library and spline servers.

The Installation Directory for External Server programs The location of a server directory has been changed and is placed under install_dir/md20101/nast/ directory. Three external servers are placed in three separate directories, respectively. The root directory for beam library server: install_dir/md20101/nast/beamlib The root directory for dresp3 server: install_dir/md20101/nast/dr3 The root directory for spline server: install_dir/md20101/nast/spline_server The DRESP3 server directory can be located in install_dir/md20101/nast/dr3 on UNIX and install_dir\md20101\nast\dr3 on Windows. Its structure is shown in the figure below that is borrowed from Directory for dr3 server (p. 11) in the MD Nastran 2010 Installation and Operations Guide. It contains three SCons construction files and 3 subdirectories: include, lib and src. Notice that the library subdirectory contains a set of predefined libraries and object files that architecture dependent. The src directory contains the source codes that are used together with the library and object files to build server programs.

Main Index

346 MD Nastran 2010 Release Guide Build External Servers Using the SCons Tool

The SCons tool requires a subdirectory be created for each server program. For example, directory dr3serv is created for server dr3serv that contains a SConscript file and Fortran files r3sgrt, r3svald, r3svals. It is convenient to use the program name as the directory name but is not required. Data Structure of DRESP3 Server ---- dr3 (root) | --- SConopts --- SConscript --- SConstruct --- Include |-- ftncalls.h |-- stdmsc.h |-- stdsystm.h --- lib | ----- < ARCH 1> | ----- linux64 | -- libdr3srv.a, libdr3main.a | -- cnxx.o | -- initgmsrvcmns.o | -- main.o | -- semd.o ----- win64 | -- dr3srv.lib, dr3main.lib | -- cnxx.obj | -- getlserm.obj | -- initgmsrvcmns.obj | -- main.obj | -- semd.obj ------ ---- src | -- SConscript | -- dr3serv | | -- SConscript | | -- r3sgrt.F | | -- r3svald.F | | -- r3svals.F | -- dr3serva | |… | -- other sample dresp3 server directories

Build a DRESP3 Server The simplest way to build a server is to enter the command from the install_dir/md20101/nast/dr3 directory scons dr3serv where dr3serv is the program name you want to build. The command creates dr3serv on UNIX or dr3serv.exe on Windows. By default, the command saves the program in the directory dr3/Apps/arch/bin

Main Index


that is architecture dependent. For example, arch=LX8664 indicates Linux 64 bit machine or arch=WIN8664 a Window 64 bit machine. If you do not have the write privilege to the install_dir, you have two options: 1. Define APPS_LOCAL and SCA_OBJECT construction variables to redirect the output to another writable location. To learn more about the SCons build environment, please consult Subsection of 'Build External Servers using SCons tools' Under the External Response Section in the DS&O's User Guide. 2. Copy the entire dr3 directory to another location that you have the write access to. This option is particularly useful when you want to create your server program in a new subdirectory. Guidelines to Build a DRESP3 Server Building an external server requires your computer to have Software Development Kit installation (SDK) and MD Nastran installation with the external server option. To create a new server program, you may either work in a new subdirectory under the src to develop required SConscript and Fortran template files or work in an existing subdirectory to modify the required files. If your server program requires additional source codes, you can simply include them in the target directory without the need change in SConscript. However, if you want to add your custom library or object file, you need to place them in the lib/ directory and to update the SConscript file to reference the library and/or object files. To learn more about customizing the SCons build environment and advanced build scenarios, please see Build External Servers using SCons Tool (p. 294) in the Design Sensitivity and Optimization User’s Guide or SCASCons Build System (p. 403) in the SCA Framework User’s Guide.

Using Server Program Consult the External Responses (p. 191) in the Design Sensitivity and Optimization User’s Guide for more information on how to use the server program in a Nastran job.

Main Index

348 MD Nastran 2010 Release Guide Deactivation of Original Design Sensitivity (DSA)

Deactivation of Original Design Sensitivity (DSA) MSC deployed a capability to provide design sensitivities for SOLs 101, 103 and 105 results over 20 years ago. This capability was characterized by a DVAR entry that defined design variables, an associated DVSET that defined the properties that could be varied and a DSCONS entry to define the response and the constraint limits. This capability has been absent from the Quick Reference Guide since the MSC Nastran 2004 release but has still been available in the code. With the release of MD Nastran 2010, this capability is no longer available. The extensive Design Sensitivity and Optimization capability that is contained in MD/MSC Nastran and that is documented in the MD Nastran 2010/MSC Nastran 2010 Design Sensitivity and Optimization User’s Guide provides all the functionality of the Original Design Sensitivity Analysis plus many other features as detailed in this document and the User’s Guide.

Main Index

Chapter 13: Aeroelasticity

13

Main Index


Aeroelasticity



Input of Pressures on an Aerodynamic Mesh



Aeroelasticity - Output of Trimmed Loads



CSV Output of Trim Results



CSV Output of Stability Derivatives



SUBCOM/SUBSEQ with Static Aeroelasticity



Upper Hessenberg Complex Eigenanalysis No Longer Supported for Flutter Analysis

350 MD Nastran 2010 Release Guide Aeroelasticity

Input of Pressures on an Aerodynamic Mesh Introduction In MD Nastran 2010 the user can now apply pressures at aerodynamic grid (AEGRID) points.

Benefits It is now possible to input pressures that come from an external source, such as CFD analyses or wind tunnel tests, onto an aerodynamic mesh and Nastran will transform these pressures to forces that can be included in a static aeroelastic analysis.

Feature Description A new Nastran module has been provided that combines information input on the AEPRESS/DMIJ entries with geometry provided on AEGRID/AEQUAD4/AETRIA3 entries and coordinate systems data to produce forces at the aerodynamic mesh points. Spline input can then be used to transfer these forces to structural grid points so that they can be included in a standard SOL 144 static aeroelastic analysis. No new input commands or entries are required to invoke this capability.

Guidelines and Limitations 1. Pressure is input at the grids of the aerodynamic mesh and is converted to forces using the same techniques as are applied with a PLOAD4 entry. That is, the forces are computed using a combination of connected elements (AEQUAD4 and/or AETRIA3 in this case) to define the area over which the pressure is acting in conjunction with systems to determine the direction in which the forces are acting. The forces are computed at the AEGRID locations. 2. Pressure can be input in all three directions at the aerodynamic grid and they do not need to act in a direction normal to the surface. The aerodynamic coordinate system defined by the AEROS Bulk Data entry defines the directions in which the pressures act. 3. There is no aeroelastic effect associated with the AEPRESS input in this case. Only rigid aerodynamic loads are produced. In the example given above, deformations are produced at the structural grid points but there is no aerodynamic correction due to these deformations. 4. It should be apparent that an application of this technique is to input results from a CFD analysis into a Nastran static aeroelastic analysis. To do this, the user needs to define the aerodynamic mesh using AEGRID/AEQUAD4/AETRIA3, the pressure vector using a combination of AEPRESS/UXVEC and DMIJ entries and the appropriate spline methods. 5. The AEPRESS data can be used in combination with AEFORCE/AEDW input to directly input aerodynamic forces or downwashes on the same aerodynamic mesh.

Main Index

CHAPTER 13 351 Aeroelasticity

6. It is not possible to combine aerodynamic mesh input with Doublet Lattice like aerodynamics in a single run. However, it is possible to have separate meshes using the “RIGID/Flexible Mesh” concepts introduced in MSC Nastran 2005 R3. This entails making an initial run with only the rigid aerodynamic mesh and then, in a subsequent run, attaching the database from this run and using the AERCONFIG case control command to identify the rigid mesh results in a static aeroelastic analysis that would obtain its flexible increments from a doublet lattice based analysis. 7. Currently, this technology is only available in static aeroelasticity (SOL 144 or the ANALYSIS=SAERO option in SOL 200). Support for SOL 146 (dynamic response) is not provided at this time.

Test Cases The following test cases are available on the TPL in subdirectory /tpl/aero_asm: cyl144b.dat TPL Problem cyl144b.dat TPL file cyl144b.dat provides an example of the loads on a cylinder spinning in an airstream. Textbooks on introductory fluid mechanics such as Chapter 4.8 of Reference 1. provide a closed form solution for this airflow. The aerodynamic mesh is depicted in Figure 13-1. The cylinder has a radius of 1.0 and a length of 10.0. Length units are in inches. Data are input at angles of 22.5 degrees at five spanwise stations ranging from -5.0 to 5.0. The structural model consists of 10 CBAR elements that reference a PBARL entry that creates TUBE cross sections that have an outer radius of 1.0 and an inner radius of 0.95. From the reference, pressure per unit dynamic pressure in a uniform stream can be expressed as: 2

p  q = 4sin  + 2 sin   r  V   +  r  V  

2

where  is the rotation speed in radians/sec. r is the radius of the cylinder and V  is the freestream velocity. The pressure acts radially while Nastran requires input in rectangular coordinates at the grid points. With a coordinate system that has positive x in the direction of the flow and the z axis normal to the flow, the radial pressure at each point has components in the x and z directions. For irrotational flow, the net force in the streamwise direction is zero so that it is only necessary to input the z component of the pressure. Note that 3D effects of the flow are neglected so there is no spanwise component.

Main Index


Figure 13-1

The Aerodynamic and Structural Model for the Flow Around a Spinning Cylinder.

A section of the pressure input is given shown in Figure 13-2. The AEPRESS entry identifies a UXVEC entry that indicates the state of the pressure input. In this case, the state includes the intercept and a CIRC value of 0.1, where CIRC is the r  V  parameter. The AEPRESS data at the UXVEC condition is input as a vector using the DMIJ format that lists the grid and component for each real number that provides the pressure at the mesh point. Since the three dimensional aspects of the flow are ignored in this analysis, the same pressure distribution in input at the 5 spanwise cuts.

Main Index


aepress 0.45 asymm uxvec 102 intercpt 1.0 dmij circ1 0 DMIj circ1 1 2 3 4 3 6 3 8 3 10 3 12 3 14 3 16 3

Figure 13-2

asymm

102

circ 0.1 9 1 1 .2866 3.505 3.505 .2866 -.1694 -2.8221 -2.8221 -.16942

circ1 0 1 3 5 7 9 11 13 15 101

0 3 3 3 3 3 3 3 3 3

1 .0 1.6213 4.41 1.6213 0.0 -1.2213 -3.61 -1.2213 0.0

A Portion of the Input Bulk Data that Provides Pressure Data on the Aerodynamic Mesh

Figure 13-3 provides an additional snippet with splining and boundary condition information. The SPLINE7 is a 6 DOF spline that uses a finite beam technique to connect all the aerodynamic mesh points to the structural grids that are defined along the axis of the tube. The GRDSET entry constrains the motion in the 1256 directions at all the structural grid points while the SPC condition invokes symmetry about the x-axis and the SUPORT entry allows the tube to move in the 3 direction.

$ $ $ $ aelist

* 6DOF FINITE BEAM SPLINE

EID 101 201 404 set1 101 SPLINE7 100

CAERO 1 thru thru 1001 1

BOX1 thru 216 416 thru 101

spc suport grdset

1006 3

4

1 1006

Figure 13-3

BOX2 16 301 1011 both

$ $ $

*

SETG 101 thru

DZ thru 316

101

1.0

116 402

401 403

1256

Spline and Boundary Condition Input for the Spinning Cylinder

The goal of the analysis is to determine the rate of rotation necessary to create a lift force that is equal to the weight (URDD3 = 1.0) of the aluminum tube when immersed in an airstream moving at M = .45 (Velocity = 6031.8 inches/sec) at sea level. The .f06 file indicates that the value of the CIRC parameter at “trim” is 1.214E-3. The rotational rate is then 1.214E-3  6031.8   2    = 1.16 cycles/second.

References 1. Kuethe, A.M and Schetzer, J.D., Foundations of Aerodynamics, John Wiley & Sons, New York, Second Edition, 1959.

Main Index


Aeroelasticity - Output of Trimmed Loads Introduction MD Nastran now supports the creation of bulk data force/moment entries for trim loads.

Benefits A primary reason for performing a static aeroelastic analysis is to determine the aeroelastic loads acting on the free-flying vehicle. With this new capability it is now possible to output the loads from the trim solution in the familiar FORCE/MOMENT Bulk Data entry format so that these loads could be passed to the group performing detailed stress analysis. In another application, these loads could be viewed in a graphical fashion using, for example, MD Patran.

Input The TRIMF Case Control command is used to invoke this new capability. The user can provide an ASSIGN statement to direct the results to a special purpose file, or they will go to the .pch file by default. The TRIMF command is quite flexible in that it can output load components or total loads. It is also possible to limit the output to a set of user defined grid points. TRIMF Format: TRIMF    UNIT = i    LOADSET = n   LARGE   INERTIA   APPLIED   AIR   ALL   NOSUM   RIGID  , NOELASTIC   QNORM    =    n 

Example: TRIMF(LOADSET=10001,LARGE)=ALL TRIMF(UNIT=59,INERTIA,NOSUM)=1

Main Index

Describer

Meaning

UNIT

Fortran unit to which data are written. (Optional; Default = 7) (punch file).

LOADSET

Load set id for output bulk data entries. If the TRIMF specification results in multiple load sets, then the defined ID will be used for the first and each subsequent load set has an ID incremented by 1. (Optional; Default = 1)

LARGE

Write the output data in large field format (16 characters per field). The default is 8 characters per field.

INERTIA

Write out inertial loads as a separate load set. By default, the separate load set will not be written.


Describer

Meaning

APPLIED

Write out applied loads as a separate load set. By default, the separate load set will not be written.

AIR

Write out aerodynamic loads as a separate load set. By default, the separate load set will not be written.

NOSUM

By default, the sum of the inertial, applied, and aerodynamic loads will be written as a separate load set. This option suppresses the writing of that set of loads.

RIGID

Write out rigid instances of the selected loads (Inertial, Applied, Air and/or Sum) as separate load sets. By default, the separate load set will not be written.

NOELASTIC

By default, the sum of the rigid and elastic increment loads will be written as a separate load set. This option suppresses the writing of that set of loads.

QNORM

Normalize the load by the dynamic pressure used in the trim analysis. By default, the loads are not normalized.

ALL

Loads for all points will be output

n

Set identification of a previously appearing SET command. Only loads on points with identification numbers that appear on this SET command will be output (Integer > 0)

Remark: 1. By default, the loads are written to the punch file (Fortran unit 7). If the user specifies an alternate Fortran unit number on the TRIMF entry, by default the loads will be written to a file name that is machine specific (i.e. ‘fort.53’ on many UNIX platforms). The user may connect the Fortran unit to a user-defined file name by using an ASSIGN entry in the FMS Section of the input file. For example: ASSIGN USERFILE='load13.inc',STATUS=UNKNOWN,FORMATTED,UNIT=53 2. Up to eight loads sets are available: Rigid Inertial, Rigid Applied, Rigid Air, Rigid Sum and four more with the sum of the rigid and elastic increment. 3. Care must be taken if LOADSET is specified in a run with multiple subcases. There are no checks that the load set IDs which are generated by one subcase are not also used for another subcase. For example, consider the following Case Control commands: SUBCASE 1 TRIM = 1 TRIMF(RIGID) = ALL $ SUBCASE 2 TRIM = 2 TRIMF(LOADSET=2) = ALL Subcase 1 will generate two load sets with set IDs 1 and 2. Subcase 2 will also output a load set ID 2. 4. The LOADSET option should not be specified in a TRIMF entry that is located above the subcase level. For example, consider the following:

Main Index


TRIMF(LOADSET=101) = ALL SUBCASE 1 TRIM = 1 SUBCASE 2 TRIM = 2 Here, both subcases will output trim loads with load set ID = 101.

Output The output of TRIMF are FORCE and MOMENT bulk data entries. The output is to either the punch file or user defined file. See test case below for sample output.

Guidelines and Limitations The TRIMF request can be placed above all subcases, in which case it is in effect until overwritten or at the subcase level to make a subcase dependent request.

Test Cases The following test cases are available in the TPL in directory /tpl/ue6_09a: trimf.dat TPL file trimf.dat is a variation of the ha144e.dat test file documented in the MD Nastran Aeroelastic User’s Guide. The variation is to add the following trimf commands in two of the five subcases: assign userfile='abrupt.inc', status=unknown,formatted,unit=53 ... ... SUBCASE 1 TRIM = 1 $ HIGH SPEED LEVEL FLIGHT SUBCASE 2 TRIM = 2 $ HIGH SPEED ROLLING PULLOUT SUBCASE 3 trimf(unit=53,loadset=1,rigid)=all TRIM = 3 $ HIGH SPEED PULLOUT WITH ABRUPT ROLL SUBCASE 4 trimf(loadset=10,inertia,air,rigid) = 100 TRIM = 4 $ HIGH SPEED SNAP-ROLL ENTRY SUBCASE 5 TRIM = 5 $ HIGH SPEED CLIMBING TURN

The test case in contrived to test a number of the features of the new capability. For example, the assign statement is used to capture the output from the third subcase while the data from the fourth subcase goes to the .pch file. It is seen that the output only goes to a set of grids in the fourth subcase. This feature could be used, for example, if only the loads on the wing are of interest.

Subcase 3 output is to the user defined file “abrupt.inc”$...............................................................................

Main Index


$ $ TRIM CASE: 3 $ RIGID (AERODYNAMIC + APPLIED - INERTIAL) LOADS $ FORCE 1 97 0 1.0 0.0 0.0 -14400. FORCE 1 98 0 1.0 0.0 0.0 6408.71 FORCE 1 99 0 1.0 0.0 -5.97767-16280.6 FORCE 1 100 0 1.0 0.0 -849.963-17073.7 FORCE 1 111 0 1.0 0.0 0.0 7102.12 FORCE 1 112 0 1.0 0.0 0.0 -9393.04 FORCE 1 121 0 1.0 0.0 0.0 35721.3 FORCE 1 122 0 1.0 0.0 0.0 -33645.6 FORCE 1 211 0 1.0 0.0 0.0 6736.25 FORCE 1 212 0 1.0 0.0 0.0 -2391.09 FORCE 1 221 0 1.0 0.0 0.0 -20757.3 FORCE 1 222 0 1.0 0.0 0.0 28125.5 FORCE 1 311 0 1.0 -1.84-11-832.2 -288. FORCE 1 312 0 1.0 -1.23-11 272.795-192. MOMENT 1 98 0 1.0 -645.697 0.0 0.0 MOMENT 1 99 0 1.0 -645.697 0.0 0.0 $............................................................................... $ $ TRIM CASE: 3 $ ELASTIC (AERODYNAMIC + APPLIED - INERTIAL) LOADS $ FORCE 2 97 0 1.0 0.0 0.0 -14400. FORCE 2 98 0 1.0 0.0 0.0 6958.1 FORCE 2 99 0 1.0 0.0 95.7669-14832.1 FORCE 2 100 0 1.0 0.0 -762.642-16588.3 FORCE 2 111 0 1.0 0.0 0.0 16858.9 FORCE 2 112 0 1.0 0.0 0.0 -10494. FORCE 2 121 0 1.0 0.0 0.0 46718.8 FORCE 2 122 0 1.0 0.0 0.0 -34359.8 FORCE 2 211 0 1.0 0.0 0.0 11975.7 FORCE 2 212 0 1.0 0.0 0.0 -2332.64 FORCE 2 221 0 1.0 0.0 0.0 -17538. FORCE 2 222 0 1.0 0.0 0.0 28513.3 FORCE 2 311 0 1.0 -1.84-11 526.924-288. FORCE 2 312 0 1.0 -1.23-11 139.951-192. MOMENT 2 98 0 1.0 -515.146 0.0 0.0 MOMENT 2 99 0 1.0 -515.146 0.0 0.0

Subcase 4 output goes to the default unit (punch file) $............................................................................... $ $ TRIM CASE: 4 $ RIGID INERTIAL LOADS $ FORCE 10 100 0 1.0 -1.65-12-33147.4-21.0849 FORCE 10 111 0 1.0 1584.39-4922.53-298.03 FORCE 10 112 0 1.0 1056.26-4337.95 954.982 FORCE 10 121 0 1.0 4753.18-3093.03 844.847 FORCE 10 122 0 1.0 3168.79-3118.28 1716.9 $............................................................................... $ $ TRIM CASE: 4 $ ELASTIC INERTIAL LOADS $ FORCE 11 100 0 1.0 -1.65-12-32947.6 44.9123 FORCE 11 111 0 1.0 1584.39-4922.53-369.264 FORCE 11 112 0 1.0 1056.26-4337.95 1861.03 FORCE 11 121 0 1.0 4753.18-3093.03 661.133 FORCE 11 122 0 1.0 3168.79-3118.28 1832.56 $............................................................................... $ $ TRIM CASE: 4

Main Index


$ RIGID AERODYNAMIC LOADS $ FORCE 12 100 0 1.0 0.0 416.853-16643.4 FORCE 12 111 0 1.0 0.0 0.0 9339.64 FORCE 12 112 0 1.0 0.0 0.0 -16832.9 FORCE 12 121 0 1.0 0.0 0.0 18282.9 FORCE 12 122 0 1.0 0.0 0.0 -4692.2 $............................................................................... $ $ TRIM CASE: 4 $ ELASTIC AERODYNAMIC LOADS $ FORCE 13 100 0 1.0 0.0 166.317-15698.5 FORCE 13 111 0 1.0 0.0 0.0 24597.3 FORCE 13 112 0 1.0 0.0 0.0 -19263.1 FORCE 13 121 0 1.0 0.0 0.0 33389. FORCE 13 122 0 1.0 0.0 0.0 -5317.57 $............................................................................... $ $ TRIM CASE: 4 $ RIGID (AERODYNAMIC + APPLIED - INERTIAL) LOADS $ FORCE 14 100 0 1.0 -1.65-12-32730.5-16664.5 FORCE 14 111 0 1.0 1584.39-4922.53 9041.61 FORCE 14 112 0 1.0 1056.26-4337.95-15877.9 FORCE 14 121 0 1.0 4753.18-3093.03 19127.7 FORCE 14 122 0 1.0 3168.79-3118.28-2975.3 $............................................................................... $ $ TRIM CASE: 4 $ ELASTIC (AERODYNAMIC + APPLIED - INERTIAL) LOADS $ FORCE 15 100 0 1.0 -1.65-12-32781.3-15653.6 FORCE 15 111 0 1.0 1584.39-4922.53 24228.1 FORCE 15 112 0 1.0 1056.26-4337.95-17402.1 FORCE 15 121 0 1.0 4753.18-3093.03 34050.1 FORCE 15 122 0 1.0 3168.79-3118.28-3485.

GUI Support Patran currently does not support the TRIMF case control SimXpert does not have an aeroelastic workspace.

Main Index


CSV Output of Trim Results Introduction MD Nastran 2010 contains a new feature that allows the user to create a summary of the trim results in a CSV (Comma Separated Values) file suitable for viewing and manipulating in a spreadsheet application.

Benefits The CSV file provides a convenient summary of the trim results that would otherwise have to be gleaned from disparate parts of the .f06 file. This is particularly valuable when hundreds of subcases are being analyzed in a single run.

Input The CSV feature in activated by PARAM LDSUM (Ch. 5) in the MD Nastran Quick Reference Guide. The unit the CSV file is written to is specified by PARAM XYUNIT. An assign statement such as: assign userfile='aecsv1.csv' status=unknown form=formatted unit=52 defines the file where the results are stored. The unit 52 corresponds to PARAM XYUNIT 52.

PARAM LDSUM Default = 0 Dictates what information is to be stored on a CSV (comma separated values) file in a SOL 144 (static aeroelasticity) task. The unit the CSV file is stored to is specified by param XYUNIT. LDSUM has the following options: • = 0 (Default) – Do not create a CSV file for static aeroelasticity • =1 Create a CSV file that contains for each static aeroelastic subcase:

a. Subcase ID b. Mach number c. Dynamic Pressure d. Trim Values e. Mass and CG information (mass, xcg,ycg,zcg, IXX,IYY,IZZ,IXY,IXZ and IYZ) • =2

Same as 1 plus net structural monitor point (MONPNT1, MONDPS1, MONPNT2, MONPNT3) results

• = 3 Same as 2 plus the output of RIGID AIR, ELASTIC RESTRAINED, and INERTIAL,

RIGID APPLIED and ELASTIC APPLIED components for the structural MONPNT1 results

Main Index


Output The output is a csv file as shown in the test case below.

Guidelines and Limitations 1. PARAM LDSUM can appear in case control or in the bulk data portion of the input file. Only one PARAM LDSUM can appear. 2. The first row in the spreadsheet provides titles for the columns that contain the results. Each subsequent row contains all the requested results for a single subcase. This means that there is a potential for more columns in the row than standard spreadsheet programs like Microsoft Excel can accommodate. This implies it may be necessary to use a special purpose spreadsheet tool to take full advantage of the new capability. 3. The PARAM XYUNIT is also used in SOL 200 to provide design optimization results. If the SOL 200 run includes static aeroelastic subcases and PARAM LDSUM is used, the resulting spreadsheet will have a row for each static aero subcase for each design iteration followed by the design optimization results.

Test Cases The following test cases are available in the TPL in directory /tpl/ue_csv09: aecsv1.dat, aecsv4.dat TPL Problem aecsv1.dat TPL example problem aecsv1 uses PARAM,LDSUM,1 to provide a summary of the trim results without any monitor points results. assign userfile='OUTDIR:aecsv1.csv' status=unknown, form=formatted unit=52 SOL 144 $ STATIC AERO CEND param ldsum 1 $ control for csv output param xyunit 52 $ output unit for csv file TITLE = EXAMPLE HA144F: FSW WITH FUSELAGE, 3 CONTROLS & 2 STOR HA144F SUBTI = UNSYMMETRIC FLIGHT CONDITIONS, DOUBLET-LATTICE AERO LABEL = FULL-SPAN MODEL WITH DISPLACED CANARD ECHO = BOTH SPC = 1 $ SYMMETRIC CONSTRAINTS MPC = 10 $ CANARD/FUSELAGE STRUCTURAL CONNECTIONS DISP = ALL $ PRINT ALL DISPLACEMENTS MONITOR = ALL SUBCASE 1 TRIM = 1 $ HIGH SPEED LEVEL FLIGHT BEGIN BULK

Partial listing of the resulting CSV file: Sub Case,Mach,Dynamic Pressure ,INTERCEPT ,ANGLEA ,P ... 1, 9.000000E-01, 1.200000E+03, 1.000000E+00 ...

Main Index


TPL Problem aecsv4.dat TPL problem aecsv4.dat is a more comprehensive example geometry with PARAM,LDSUM,4 to provide a summary of the trim results including comprehensive monitor point results.

Figure 13-4

TPL Problem aecsv4.dat

assign userfile='OUTDIR:aecsv4.csv' status=unknown, form=formatted unit=52 SOL 144 TIME 600 END param ldsum 4 $ control for csv output param xyunit 52 $ output unit for csv file SEALL = ALL SUPER = ALL ECHO = SORT MAXLINES = 999999 AECONFIG = Freedom4 SUBCASE 1 $ Subcase name : Mach .4 Level Flight SUBTITLE=Mach .4 Level Flight DISPLACEMENT(SORT1,REAL,plot)=ALL SPCFORCES(SORT1,REAL)=ALL OLOAD(SORT1,REAL,plot)=ALL STRESS(SORT1,REAL,VONMISES,BILIN,plot)=ALL TRIM = 1 AESYMXZ = Asymmetric AESYMXY = Asymmetric SUPORT1 = 1 AEROF = ALL APRES = ALL BEGIN BULK PARAMAESMETHRITZ

GUI Support Patran currently does not support PARAM,LDSUM SimXpert does not have an aeroelastic workspace.

Main Index


CSV Output of Stability Derivatives Introduction MD Nastran has a new feature that allows the user to write out the stability derivatives from a Solution 144 job to a CSV (Comma Separated Values) file that is suitable for viewing in a spreadsheet program.

Benefits This new capability will allow the user to examine how the stability derivatives change as a function of the flight or trim condition.

Input The name of the file to which the stability derivatives will be written is controlled by the Nastran ASSIGN statement using standard Nastran syntax. For example:

ASSIGN USERFILE='stabder.csv' STATUS=UNKNOWN FORM=FORMATTED UNIT=53 Two new Nastran parameters were created to control the CSV output: SDUNIT and SDCSV. SDUNIT – This parameter defines the Fortran unit number to which the stability derivatives will be written. This unit number should coincide with that from the ASSIGN statement that defines the name of the CSV file. For example: PARAM SDUNIT 53 SDCSV – This parameter controls which stability derivative data are written:

Value

Derivative

0

No derivatives will be output

1

Rigid Aero

2

Rigid splined

4

Elastic Restrained

8

Elastic Unrestrained

16

Inertial Restrained

32

Inertial Unrestrained

To output more than one type, the value flags can be summed. For example, to output all stability derivatives:

Main Index


PARAM

SDCSV

63

For each type, derivatives for all controllers will be written.

Outputs A new file will be created that contains the stability derivative information. The file will look similar to the following: SUB CASE,MACH,DYNAMIC PRESSURE,REFERENCE_ID,INTERCPT_REF,SIDES_REF, ... ,REF.COEFF_SD_A_CZ_RA,REF.COEFF_SD_S_CZ_RS, ... 1, 8.300000E-01, 2.577100E+00, 0, 1.000000E+00 , 0.000000E+00 , ... , 1.970288E+05 , 1.970288E+05 , ... 2, 8.300000E-01, 2.577100E+00, 0, 1.000000E+00 , 0.000000E+00 , ... , 1.970288E+05 , 1.970288E+05 , ... 3, 8.300000E-01, 2.581900E+00, 0, 1.000000E+00 , 0.000000E+00 , ... , 1.970288E+05 , 1.970288E+05 , ... 4, 8.300000E-01, 2.581900E+00, 0, 1.000000E+00 , 0.000000E+00 , ... , 1.970288E+05 , 1.970288E+05 , ... 5, 8.300000E-01, 2.588200E+00, 0, 1.000000E+00 , 0.000000E+00 , ... , 1.970288E+05 , 1.970288E+05 , ... 6, 8.300000E-01, 2.588200E+00, 0, 1.000000E+00 , 0.000000E+00 , ... , 1.970288E+05 , 1.970288E+05 , ... 7, 8.300000E-01, 2.595900E+00, 0, 1.000000E+00 , 0.000000E+00 , ... , 1.970288E+05 , 1.970288E+05 , ... 8, 8.300000E-01, 2.595900E+00, 0, 1.000000E+00 , 0.000000E+00 , ... , 1.970288E+05 , 1.970288E+05 , ... 9, 8.300000E-01, 2.597200E+00, 0, 1.000000E+00 , 0.000000E+00 , ... , 1.970288E+05 , 1.970288E+05 , ... 10, 8.300000E-01, 2.597200E+00, 0, 1.000000E+00 , 0.000000E+00 , ... , 1.970288E+05 , 1.970288E+05 , ...

The format of the stability derivative column headers is: ____ Where: name

Name of the controller

type

SD

mesh

A = aerodynamic S = structural

axis

CX, CY, CZ, CMX, CMY, CMZ

component

RA = rigid aero RS = rigid splined ER = elastic restrained EU = elastic unrestrained IR = inertial restrained IU = inertial unrestrained

Guidelines and Limitations Nastran will not prevent the user from writing the stability derivatives to the same CSV file as the monitor points. However, no merging of similar columns is attempted. Instead, the CSV file will contain two independent sections: one for the monitor points, and one for the stability derivatives.

Main Index


Test Case The aecsvsd63.dat test case is available in the TPL in directory tpl/ue_csv09. This test case will output all stability derivatives (SDCSV=63) to a CSV file named aecsvsd63.csv. assign userfile='OUTDIR:aecsvsd63.csv' status=unknown form=formatted, unit=53 SOL 144 CEND TITLE = MSC/NASTRAN Aeroelastic job created on 01-Jun-99 at 16:00:58 SUBCASE 1 SUBTITLE=Mach .4 Level Flight TRIM = 1 SUPORT1 = 1 BEGIN BULK PARAM SDUNIT 53 PARAM SDCSV 63 PARAM POST 0 . . . . . .

Main Index


SUBCOM/SUBSEQ with Static Aeroelasticity Introduction The SUBCOM/SUBSEQ commands that were previously limited to statics problems have been extended to static aeroelasticity problems (both in SOL 144 and in SOL 200 with ANALYSIS=SAERO).

Benefits The motivation for this task is to allow a scaling of the results (displacements and element responses) from a static aeroelastic trim analysis as a post-processing operation. This is particularly of benefit in an optimization task where one desires to explore applying different limit factors to the results in a design task.

User Inputs The existing SUBCOM/SUBSEQ case control commands have been activated for a static aeroelastic analysis. Typically, a single SUBSEQ coefficient is used to scale the results of the previous subcase, although multiple coefficients are supported. In a SOL 200 job, the SUBCOM subcase needs to be accompanied by an ANALYSIS=SAERO command to designate that this subcase is to be grouped with the static aeroelastic subcases.

Outputs Data recovery occurs for the SUBCOM subcases in the same way as any other subcase. The SUBCOM ID appears on the right hand side of the page to indicate that the results are associated with the SUBCOM

Guidelines and Limitations Only element and grid responses are affected by the SUBCOM. Trim results and stability derivative results are neither computed or output. In SOL 200, it is illegal to invoke a DRESP1 with RTYPE = STABDER or TRIM from a SUBCOM subcase that has ANALYSIS=SAERO.

Example A variation of the familiar HA144A test case for the forward swept wing is used to demonstrate the new SUBCOM capability in a SOL 144 test case. The test case is available in the TPL in directory /tpl/ue_csv09: subcoma.dat. The case control is shown below and it is seen that there is a SUBCOM 4 that requests output that is 50% greater than that of subcase 3. TITLE = EXAMPLE HA144A: 30 DEG FWD SWEPT WING WITH CANARD HA14 HA144A SUBTI = SYMMETRIC FLIGHT CONDITIONS, DOUBLET-LATTICE AERO LABEL = HALF-SPAN MODEL, STATIC SYMMETRIC LOADING

Main Index


ECHO = BOTH SPC = 1 $ DISP = ALL $ STRESS = ALL $ FORCE = ALL $ AEROF = ALL $ APRES = ALL $ SUBCASE 1 TRIM = 1 $ SUBCASE 2 TRIM = 2 $ SUBCASE 3 TRIM = 3 $ subcom 4 subseq(1.5) BEGIN BULK

SYMMETRIC PRINT ALL PRINT ALL PRINT ALL PRINT ALL PRINT ALL

CONSTRAINTS DISPLACEMENTS STRESSES FORCES AERODYNAMIC FORCES AERODYNAMIC PRESSURES

1 G LEVEL FLIGHT (LOW SPEED) 1 G LEVEL FLIGHT (HIGH SUBSONIC SPEED) 1 G LEVEL FLIGHT (LOW SUPERSONIC SPEED)

A snippet of the output from this job is shown below. It is seen that the displacements of SUBCOM 4 are 50% greater than those of SUBCASE 3.

1 0

EXAMPLE HA144A: 30 DEG FWD SWEPT WING WITH CANARD HA14 HA144A SYMMETRIC FLIGHT CONDITIONS, DOUBLET-LATTICE AERO HALF-SPAN MODEL, STATIC SYMMETRIC LOADING D I S P L A C E M E N T

1 0

POINT ID. TYPE T1 T2 T3 90 G 0.0 0.0 0.0 97 G 0.0 0.0 -5.984770E-03 98 G 0.0 0.0 -8.086921E-04 99 G 0.0 0.0 -8.673837E-04 100 G 0.0 0.0 -9.000074E-03 110 G 0.0 0.0 -2.312949E-03 111 G 0.0 0.0 2.641245E-03 112 G 0.0 0.0 -7.267144E-03 120 G 0.0 0.0 1.953165E-02 121 G 0.0 0.0 2.512188E-02 122 G 0.0 0.0 1.394143E-02 EXAMPLE HA144A: 30 DEG FWD SWEPT WING WITH CANARD HA14 HA144A SYMMETRIC FLIGHT CONDITIONS, DOUBLET-LATTICE AERO HALF-SPAN MODEL, STATIC SYMMETRIC LOADING D I S P L A C E M E N T POINT ID. 90 97 98 99 100 110 111 112 120 121 122

Main Index

TYPE G G G G G G G G G G G

0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0

T1

0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0

T2

T3

0.0 -8.977155E-03 -1.213038E-03 -1.301076E-03 -1.350011E-02 -3.469424E-03 3.961868E-03 -1.090072E-02 2.929747E-02 3.768281E-02 2.091214E-02

OCTOBER

21, 2009

MD NASTRAN

10/20/09

PAGE

62

PAGE

63

SUBCASE 3 V E C T O R R1 R2 0.0 0.0 0.0 0.0 -6.176078E-04 0.0 0.0 -3.176077E-04 0.0 0.0 3.528226E-04 0.0 0.0 1.363732E-03 0.0 6.497581E-04 1.981678E-03 0.0 6.497581E-04 1.981678E-03 0.0 6.497581E-04 1.981678E-03 0.0 1.088872E-03 2.236090E-03 0.0 1.088872E-03 2.236090E-03 0.0 1.088872E-03 2.236090E-03 0.0 OCTOBER 21, 2009 MD NASTRAN

R3

10/20/09 SUBCOM 4

V E C T O R R1 0.0 0.0 0.0 0.0 0.0 9.746371E-04 9.746371E-04 9.746371E-04 1.633308E-03 1.633308E-03 1.633308E-03

R2 0.0 -9.264118E-04 -4.764115E-04 5.292339E-04 2.045598E-03 2.972517E-03 2.972517E-03 2.972517E-03 3.354135E-03 3.354135E-03 3.354135E-03

0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0

R3


Upper Hessenberg Complex Eigenanalysis No Longer Supported for Flutter Analysis The original implementation of the PK flutter analysis utilized an Upper Hessenberg algorithm for extracting complex eigenvalues. In MSC Nastran 2005 R3, a QZ algorithm was introduced that had the advantage of being able to accommodate a singular matrix. For several releases, the Upper Hessenberg algorithm could still have been used if NASTRAN SYSTEM(108)=1 was specified. This option is no longer available and the use of SYSTEM(108)=1 will cause a User Information Message to be printed:

*** USER INFORMATION MESSAGE 5282 (FA1PKE) SYSTEM(108) HAS A NONZERO VALUE, IMPLYING THERE IS A preference TO USE THE UPPER HESSENBERG METHOD FOR PK FLUTTER ANALYSIS. User information: THIS IS NO LONGER SUPPORTED AND THE DEFAULT QZ ALGORITHM WILL BE USED.

Main Index


Main Index

Chapter 14: Elements MD Nastran Release Guide

14

Main Index

Elements



Enhancements to Connector Elements



Element Enhancements - Heat Shell Element with Linear/Quadratic Temperature Distribution Across the Element Thickness



Concentric half cylinder with view factor calculations with imposing heat flux with thermal thick shell



Axisymmetrical Mechanical and Heat Transfer Shell Elements



Axisymmetrical Shell Elements



Multi-Dof Heat Shell Elements



Herrmann Elements

370 MD Nastran 2010 Release Guide Enhancements to Connector Elements

Enhancements to Connector Elements Introduction A finite element modeler has many ways of modeling structural connections and fasteners. Spot welds, seam welds, bolts, screws, and so on can be represented, depending on the modeling goals, either with flexible springs or bars (CBUSH, CBAR), rigid elements (RBAR, RBE2, RBE3), or multipoint constraints (MPC). Though generally, these elements are sometimes difficult to use; singularities may be introduced particularly in the out-of-plane rotational direction for shells, rigid body invariance may not be assured, and data preparation and input can be a formidable task in real-world applications. Increasing mesh refinement can also introduce further stiffness errors; point-to-point connections in which effective cross-sectional areas are larger than 20% of the characteristic element lengths can often lead to significant underestimation of connector stiffness. Connector elements are a special class of elements that were introduced to MSC Nastran in V2001. The first implementation was for elements that represent spot welds. These elements are convenient to define by the user because all that is necessary to define the elements a geometric location in space. Subsequent versions of MSC Nastran and MD Nastran have provided many enhancements and now include elements that can model bolts and seam welds. In MD Nastran 2010, there have been further enhancements to the existing elements to allow data recovery in dynamic solution sequences, calculate displacements and stresses for seam weld elements and support user defined coordinate systems for spot weld elements the way that user defined coordinate systems are used for bolt elements.

Benefits The following features are included in MD Nastran 2010. 1. Support auxiliary displacement output for frequency response and transient analysis for CWELD, CFAST and CSEAM elements. 2. Generate eight auxiliary grids internally and compute their associated displacements for CSEAM elements. 3. Provide stress and strain output for CSEAM elements. 4. Support user defined element coordinate system for CWELD elements.

Theory Mathematical Model to Construct the CSEAM Auxiliary Points The four auxiliary vertex points of the cross section at start point GS are constructed by the following s

s

equations (see Figure 14-1), where t 1 and t 2 are tangent vectors of the element coordinate system at

Main Index

CHAPTER 14 371 Elements

s

start point GS, W is the width of the seam, and T is the thickness of the seam. For a continuous seam, t 1 s

and t 2 vectors are adjusted to a common face for the two consecutive seam elements. Therefore, the four auxiliary grids at the start point S of the ith seam should be coincident with the four auxiliary grids at the end point E of the (i-1)th seam, if both elements have same width and thickness. W s T s x S A1 = x s – ----- t 1 – --- t 2 2 2 W s T s x S A2 = x s – ----- t 1 – --- t 2 2 2 W s T s x S B1 = x s – ----- t 1 – --- t 2 2 2 W s T s x S B2 = x s – ----- t 1 – --- t 2 2 2 s

t2 GSB1

GSB2

T/2 s

GS

T/2

t1

GSA1

GSA2 W/2

Figure 14-1

W/2

Seam Weld Cross Section at Start Point S

The four auxiliary vertex points of the cross section at end point GE are calculated in the same way as that for the start point GS. These eight auxiliary points form an auxiliary HEXA element with the following vertex points.

Main Index

1

2

3

4

5

6

7

8

GSA1

GSA2

GSB2

GSB1

GEA1

GEA2

GEB2

GEB1


Input The only new input is related to the element coordinate system on the CWELD entry. The relevant changes are shown in the following CWELD entry (other items that did not change are not shown). The other enhancements are to extend the solution sequences and provide additional output for the CSEAM.

Main Index


CWELD

Weld or Fastener Element Connection

Defines a weld or fastener connecting two surface patches or points. Large displacement and large rotational effects are supported when using SOL 600 and MD Nastran SOL 400 only. Format: 1

2

3

4

5

6

7

CWELD

EWID

PWID

GS

“PARTPAT”

8

9

GA

GB

MCID

PIDA

PIDB

XS

YS

ZS

101

8

203

21

33

GA

GB

MCID

GA

GB

MCID

GA

GB

Example: CWELD

PARTPAT

Alternate formats and examples: Format ELPAT: CWELD

EWID

PWID

GS

“ELPAT”

SHIDA

SHIDB

XS

YS

ZS

103

5

403

ELPAT

309

511

GS

“ELEMID”

403

ELEMID

GS

“GRIDID”

Example: CWELD

Format ELEMID: CWELD

EWID

PWID

SHIDA

SHIDB

103

5

309

511

Example: CWELD

Format GRIDID: CWELD

Main Index

EWID

PWID

SPTYP

MCID

10


GA1

GA2

GA3

GA4

GA5

GA6

GA7

GA8

GB1

GB2

GB3

GB4

GB5

GB6

GB7

GB8

7

29

233

GRIDID

15

28

31

35

46

51

3

5

8

Example: CWELD

QT 55

60

Format ALIGN: CWELD

EWID

PWID

“ALIGN”

GA

GB

7

29

ALIGN

103

259

MCID

Example: CWELD

Field

Contents

Type

Default

MCID

Specifies the element stiffness coordinate system. See Remark 15.

Integer > -1 or Default = -1 blank

Remarks: 15. MCID = -1 or blank (Default), then the coordinate system is as defined in Remark 12. If MCID > 0, then a “beam” like coordinate system is defined. The x ele m axis direction of the connector defined as 1

xB – xA = --------------------xB – xA

Output The results of CWELD and CFAST elements are stored in standard beam and standard bush formats respectively; while the results of CSEAM elements are displayed in hexa format with the eight auxiliary grids as vertex points. For frequency response, the output data may be in rectangular or polar format. The examples below will give a description of the output.

Test Cases The following test cases are available in the TPL in directory /tpl/rg4_conn: r4_conn_exa.dat, r4_conn_exb.dat

Main Index


TPL example model r4_conn_exa.dat This example demonstrates the modeling of frequency response for CWELD elements with user defined element coordinate system and the ELPAT format:

Figure 14-2

Example r4_conn_exa.dat geometry

SOL 108 END DISPL= ALL FORCE=1 STRESS=1 SUBCASE 1 SUBTITLE= shear the weld dload=1 method= 400 freq=11 BEGIN BULK $ Spot weld cweld, 30, 30, 300, elpat, , , , 755, +CW1 +CW1, 11, 10 pweld, 30, 10, 0.1 $ cord2r, 755, , 0., 0., 0., 0., 0., -1., , 0., 1., 0.

Note:

Main Index

Turning on additional diagnostics with SWLDPRM,PRTSW,1 will provide information about the auxiliary GRID locations and ids. The displacement printout shown afterwards gives the auxiliary GRID displacements.


CWELD EID= 30 WITH ELPAT OR PARTPAT GS IS MOVED FROM ( 1.0000E+00, 4.0000E-01, 5.0000E-01) TO ( 1.0072E+00, 3.9841E-01, 2.3848E-01) AUXILIARY POINTS= ( 9.8328E-01, 3.6349E-01, 4.3080E-01) ( 1.0718E+00, 3.6307E-01, 4.2595E-01) ( 1.0714E+00, 4.5062E-01, 4.1219E-01) ( 9.8294E-01, 4.5104E-01, 4.1704E-01) ( 9.7227E-01, 3.5413E-01, 4.8613E-02) ( 1.0608E+00, 3.5407E-01, 5.3039E-02) ( 1.0608E+00, 4.4269E-01, 5.3042E-02) ( 9.7233E-01, 4.4275E-01, 4.8616E-02) NUMBER OF TIMES GS MOVES= 1 NUMBER OF TIMES DA IS REDUCED= 0 ANGLE BETWEEN TWO SHELL NORMALS= 10.77 GS=( 1.007E+00, 3.984E-01, 2.385E-01) GA=( 1.027E+00, 4.071E-01, 4.215E-01) GB=( 1.017E+00, 3.984E-01, 5.083E-02) T_BE MATRIX: -2.9113E-02 9.9958E-01 0.0000E+00 -2.3310E-02 -6.7890E-04 -9.9973E-01 -9.9930E-01 -2.9105E-02 2.3320E-02 GA ID = 101000001 GB ID = 101000002 PATCH A: EID= 11 GIDS= 111 112 113 114 0 0 0 0 EID= 11 GIDS= 111 112 113 114 0 0 0 0 EID= 11 GIDS= 111 112 113 114 0 0 0 0 EID= 11 GIDS= 111 112 113 114 0 0 0 0 PATCH B: EID= 10 GIDS= 101 102 104 0 0 0 0 0 EID= 10 GIDS= 101 102 104 0 0 0 0 0 EID= 10 GIDS= 101 102 104 0 0 0 0 0 EID= 10 GIDS= 101 102 104 0 0 0 0 0

The displacement, element force and stress results are shown as follows.

0

0

FREQUENCY =

POINT ID. 101

1.000000E+01

TYPE G

0

102

G

0

104

G

0

111

G

0

112

G

0

113

G

0

114

G

0

300

G

0

101000001

G

0

101000002

G

0

Main Index

SUBCASE 1 C O M P L E X

T1 -7.791607E+00 5.248972E-07 -7.795311E+00 -3.276013E-06 -8.547235E+00 1.220098E-05 -7.810302E+00 2.649062E-06 -7.806551E+00 8.092410E-07 -8.705634E+00 -8.982315E-06 -8.569546E+00 1.027111E-07 0.0 0.0 -8.114884E+00 -7.519017E-07 -8.094540E+00 3.244864E-06

T2 -6.924270E-01 1.286137E-05 8.285373E-01 -1.135917E-05 -6.924270E-01 1.286628E-05 -6.437430E-01 -7.254856E-06 7.064308E-01 1.905125E-06 8.381162E-01 3.584831E-06 -6.340333E-01 -8.022997E-06 0.0 0.0 1.247901E-01 -2.020528E-06 8.064318E-02 5.525994E-07

D I S P L A C E M E N T (REAL/IMAGINARY) T3 1.487187E-02 -3.858250E-05 8.895068E-02 3.686814E-05 -8.223225E-02 -3.003202E-05 1.438998E-02 1.925463E-05 8.188874E-02 -1.219865E-05 -2.708165E-02 -1.199635E-05 -8.270818E-02 2.709107E-05 0.0 0.0 1.340001E-02 3.345231E-06 1.383702E-02 3.173882E-06

V E C T O R

R1 -9.710412E-02 8.550648E-06 -9.710412E-02 8.550648E-06 -9.710412E-02 8.550648E-06 -9.709817E-02 7.837443E-06 -9.706381E-02 3.714137E-06 -9.705853E-02 3.080924E-06 -9.709751E-02 7.757903E-06 0.0 0.0 -9.707516E-02 5.076566E-06 -9.710412E-02 8.550648E-06

R2 -3.703940E-02 -3.772603E-05 -3.703940E-02 -3.772603E-05 -3.703940E-02 -3.772603E-05 -3.749770E-02 1.728056E-05 -3.750144E-02 1.772999E-05 -3.752504E-02 2.056146E-05 -3.751689E-02 1.958415E-05 0.0 0.0 -3.750778E-02 1.849139E-05 -3.703940E-02 -3.772603E-05

R3 7.556269E-01 -1.167940E-05 7.556269E-01 -1.167940E-05 7.556269E-01 -1.167940E-05 7.554925E-01 4.460259E-06 7.554878E-01 5.025620E-06 7.554884E-01 4.950366E-06 7.554936E-01 4.324563E-06 0.0 0.0 7.554896E-01 4.807756E-06 7.556269E-01 -1.167940E-05 SUBCASE 1


0

02

FREQUENCY =

ELEMENT ID 30

SUBCASE 1 F O R C E S

FREQUENCY =

ELEMENT ID 30

I N W E L D E L E M E N T S (REAL/IMAGINARY)

( C W E L D P )

BEND-MOMENT END-A BEND-MOMENT END-B - SHEAR PLANE 1 (MZ) PLANE 2 (MY) PLANE 1 (MZ) PLANE 2 (MY) PLANE 1 (FY) PLANE 2 (FZ) -1.196586E-01 5.743172E-03 -3.431428E-03 3.061221E-03 -3.133458E-01 7.230475E-03 1.436048E-02 -6.890686E-04

03 0

1.000000E+01 C O M P L E X

1.000000E+01 C O M P L E X

AXIAL STRESS 1.147757E+00 -1.376786E-01

4.131643E-04 -3.671607E-04

3.760163E-02 -8.678561E-04

AXIAL FORCE FX 9.014460E-03

TORQUE MX -1.499722E-

-1.081325E-03

1.800308E-

SUBCASE 1 S T R E S S E S

MAX STRESS END-A 1.278480E+03 1.531557E+02


MIN STRESS END-A -1.276184E+03 -1.534311E+02

MAX STRESS END-B 6.728133E+01 7.810646E+00

( C W E L D P )

MIN STRESS END-B -6.498582E+01 -8.086003E+00

MAXIMUM BEARING SHEAR STRESS STRESS 1.297688E+02 3.134292E+01 1.557555E+01 3.761164E+00

TPL Problem r4_conn_exb.dat TPL problem r4_conn_exb.dat demonstrates the static analysis for CSEAM elements with displacement and stress output requests. In this case there are several overlapping plates connected with CSEAM. The CSEAM model has internally generated auxiliary grid IDs starting from 90001.

Figure 14-3

Example r4_conn_exb.dat geometry

sol 101 cend load = 10 spc = 10 disp = all set 4 = 10001,10002,10003,10004,10005 stress = 4 begin bulk ... swldprm prtsw 1 $ cseam100011000se0elem113214 1000110002 cseam100021000se010elem330440 1000310004 cseam100031000se1010elem5030060400 1000510006

Main Index


cseam100041000sl1030pshell70200 1000710008 cseam100051000sl1030 pshell70200 1000910010 $ $23456 pseam 1000 200.2 $

The displacement and stress results are shown as follows.

0 D I S P L A C E M E N T POINT ID. 509 10001 10002 10003 10004 10005 10006 10007 10008 10009 10010 101000001 101000002 101000003 101000004 101000005 101000006 101000007 101000008 101000009 101000010 101000011 101000012 101000013 101000014

TYPE G G G G G G G G G G G G G G G G G G G G G G G G G

T1 2.805908E-02 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 7.372772E-03 7.673701E-03 6.849292E-03 6.850486E-03 7.376085E-03 7.677149E-03 6.851723E-03 6.853319E-03 2.237370E-02 2.267277E-02 2.469706E-02 2.469634E-02 2.237715E-02 2.267609E-02

T2 -2.599996E-04 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 3.151977E-03 3.151946E-03 -2.230086E-04 -2.224528E-04 -3.603303E-03 -3.603285E-03 -2.002655E-04 -2.007576E-04 3.150388E-03 3.150356E-03 -2.220506E-04 -2.216082E-04 -3.602424E-03 -3.602407E-03

T3 -2.023823E-01 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 -3.154194E-02 -3.261929E-02 -3.259117E-02 -3.151381E-02 -2.985591E-02 -3.093446E-02 -3.090637E-02 -2.982783E-02 -1.297074E-01 -1.325928E-01 -1.326306E-01 -1.297368E-01 -1.284061E-01 -1.313060E-01

V E C T O R R1 6.784551E-05 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0

R2 1.449939E-02 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0

R3 -6.875442E-07 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0

0 0

ELEMENT-ID 0 10001 0 0 0 0 0 0 0 0 0

Main Index

CORNER GRID-ID 0GRID CENTER X Y Z 101000001 X Y Z 101000002 X Y Z 101000003 X Y Z 101000004 X Y Z 101000005 X Y Z 101000006 X Y Z 101000007 X Y Z 101000008 X Y Z

S T R E S S E S I N S E A M E L E M E N T S ( C S E A M ) ------CENTER AND CORNER POINT STRESSES--------DIR. COSINES NORMAL SHEAR PRINCIPAL -A- -B- -CCS 8 GP 7.490945E+02 XY 3.996807E-02 A 7.490945E+02 LX 1.00 0.0 0.0 2.938447E-01 YZ -7.958079E-13 B 1.469501E-01 LY 0.00 0.0 0.0 0.0 ZX 9.094947E-12 C 1.469501E-01 LZ 0.00 0.0 0.0 1.635867E+03 XY 7.365383E-02 A 1.635867E+03 LX 1.00 0.00 0.00 1.320214E+02 YZ -2.318950E-02 B 1.320214E+02 LY 0.00 1.00 0.00 3.053776E+02 ZX -3.091930E-04 C 3.053776E+02 LZ 0.00 0.00-1.00 1.635903E+03 XY 7.365383E-02 A 1.635903E+03 LX 1.00 0.00 0.00 1.320599E+02 YZ 2.318950E-02 B 1.320599E+02 LY 0.00 1.00 0.00 3.054590E+02 ZX -3.091930E-04 C 3.054590E+02 LZ 0.00 0.00-1.00 -1.369259E+02 XY 6.282309E-03 A -1.311691E+02 LX 0.00 0.00-1.00 -1.311691E+02 YZ 2.318950E-02 B -3.053584E+02 LY 1.00 0.00 0.00 -3.053584E+02 ZX -3.091930E-04 C -1.369259E+02 LZ 0.00 1.00 0.00 -1.370004E+02 XY 6.282309E-03 A -1.312972E+02 LX 0.00 0.00-1.00 -1.312972E+02 YZ -2.318950E-02 B -3.054782E+02 LY 1.00 0.00 0.00 -3.054782E+02 ZX -3.091930E-04 C -1.370004E+02 LZ 0.00 1.00 0.00 1.636985E+03 XY 7.365383E-02 A 1.636985E+03 LX 1.00 0.00 0.00 1.326195E+02 YZ -2.318950E-02 B 1.326195E+02 LY 0.00 1.00 0.00 3.062530E+02 ZX 3.091930E-04 C 3.062530E+02 LZ 0.00 0.00-1.00 1.636935E+03 XY 7.365383E-02 A 1.636935E+03 LX 1.00 0.00 0.00 1.325717E+02 YZ 2.318950E-02 B 1.325717E+02 LY 0.00 1.00 0.00 3.061331E+02 ZX 3.091930E-04 C 3.061331E+02 LZ 0.00 0.00-1.00 -1.395096E+02 XY 6.282309E-03 A -1.322068E+02 LX 0.00 0.00-1.00 -1.322068E+02 YZ 2.318950E-02 B -3.062338E+02 LY 1.00 0.00 0.00 -3.062338E+02 ZX 3.091930E-04 C -1.395096E+02 LZ 0.00 1.00 0.00 -1.394977E+02 XY 6.282309E-03 A -1.322486E+02 LX 0.00 0.00-1.00 -1.322487E+02 YZ -2.318950E-02 B -3.061523E+02 LY 1.00 0.00 0.00 -3.061523E+02 ZX 3.091930E-04 C -1.394977E+02 LZ 0.00 1.00 0.00

MEAN PRESSURE

VON MISES

-2.497961E+02

7.489476E+02

-6.910887E+02

1.425098E+03

-6.911407E+02

1.425078E+03

1.911511E+02

1.713834E+02

1.912586E+02

1.714006E+02

-6.919526E+02

1.425502E+03

-6.918799E+02

1.425529E+03

1.926500E+02

1.704930E+02

1.926329E+02

1.703949E+02



Main Index

380 MD Nastran 2010 Release Guide Element Enhancements - Heat Shell Element with Linear/Quadratic Temperature Distribution Across the

Element Enhancements - Heat Shell Element with Linear/Quadratic Temperature Distribution Across the Element Thickness Introduction Through the thickness temperature distributions in shell elements is a common physical phenomena experienced by structures subjected to rapid temperature gradients. In MD Nastran 2010, simulating constant, linear, or quadratic temperature distribution across the thickness for thermal analysis of thinwalled structure is now possible in heat transfer analysis.

Benefits Through thickness temperature solutions provide a more accurate simulation across the shell thickness compared with that of the classical element that provides only a constant temperature. The heat transfer temperature solutions provide a better temperature distribution for mechanical analysis. Through thickness temperature solutions also provide ease of modeling compared to alternative modeling with brick elements.

Input Through thickness temperature distributions are turned on by specifying the NLMOPTS,TEMPP Bulk Data entry. There are three possible values: • NLMOPTS,TEMPP,CONS - constant distribution (default) • NLMOPTS,TEMPP,LINE - linear distribution • NLMOPTS,TEMPP,QUAD - quadratic distribution

Only one TEMPP option is allowed in a job. The GRIDs defined on the element are used for the TOP temperature. The BOT or MID temperature will be held by the internally created grids.The user can access the internally generated GRID IDs via the NLMOPTS, TEMPGO option • NLMOPTS,TEMPGO,NO - do not print internally generated GRID IDs (default) • NLMOPTS,TEMPGO,YES -print internally generated GRID IDs

Main Index


Figure 14-4

NLMOPTS TEMPP locations for TOP, MID, BOT w.r.t. element coordinate system

To accommodate the through thickness capabilities, temperature boundary conditions specified with SPC,SPC1,SCPD have been extended to specify condition at the TOP/BOT/MID position by specify dof 1, 2, or 3 respectively. Internal calculations map the boundary conditions to the internally generated GRID IDs component 1. Heat boundary conditions can be defined on surface elements with CHBDYE. Note that only CHBDYE is supported among the CHBDY elements when NLMOPTS,TEMPP is not CONS. This is because the TOP/BOT position is related to element normal direction. This entry is extended to allow user specifying bottom surface by specifying TYPE=6. Internally the entry that references bottom surface will be converted to a standard CHBDYG with the associated grids. Initial temperature can be defined with the existing TEMP or new TEMPN1 entries. The TEMP entry will define initial temperatures at the TOP, whereas TEMPN1 can be used to define temperatures at the TOP (dof 1), BOT (dof 2), or MID (dof 3).

Main Index


TEMPN1 - MD Only

TOP/BOT/MID Grid Point Temperature Field for Heat Shell Element in SOL 400

Defines initial temperature at grid points of heat shell elements with linear or quadratic temperature distribution across the thickness direction. Format: 1

2

3

4

5

6

7

8

TEMPN1

SID

G1

C1

T1

G2

C2

T2

10

100

123

1300.

9

10

Example: TEMPN1

Field

Contents

SID

Temperature set identification number. (Integer > 0)

Gi

Grid point identification number. (Integer > 0)

Ci

Component numbers. (0 < Integer < 3; up to 3 unique Integers may be placed in the field with no embedded blanks.) 1=TOP, 2=BOT, 3=MID. (Integer > -1; Default = 1)

Ti

Temperature. (Real)

Point heat fluxes can be defined with existing SLOAD or new SLOADN1 entries. The SLOAD entry will define the point flux at the TOP, whereas the SLOADN1 entry can be used to define point flux at the TOP (dof 1), BOT (dof 2), or MID (dof 3).

Main Index


SLOADN1 - MD Only

Describes TOP/BOT/MID Scalar Load for Heat Shell Element in SOL 400

Defines concentrated flux on grid points of heat shell elements with linear or quadratic temperature distribution through the thickness direction. Format: 1

2

3

4

5

6

7

8

SLOADN1

SID

G1

C1

Q1

G2

C2

Q2

10

10

12

1300.

20

2

1300.

9

10

Example: SLOADN1

Field

Contents

SID

Load set identification number. (Integer > 0)

Gi

Grid point identification number. (Integer > 0)

Ci

Composite numbers. (0 < Integer < 3; up to 3 unique Integers may be placed in the field with no embedded blanks.) 1=TOP, 2=BOT, 3=MID. (Integer > -1; Default = 1)

Qi

Power. (Real)

Output The output for NLMOPTS,TEMPGO,YES provides a mapping for internal GRID IDs relative to the nominal GRID which is defined as the TOP.

U S E R TOP BOT MID TOP BOT MID

G R I D

P O I N T (T O P)

M A P P I N G

T O

B O T/M I D

I N T E R N A L

The output for temperatures and heat flow are unaffected.

Main Index

G R I D

1 2 3 4 5 6 7 8 9 10 101000001 101000002 101000003 101000004 101000005 101000006 101000007 101000008 101000009 101000010 0 0 0 0 0 0 0 0 0 0 11 12 13 14 15 16 17 18 19 20 101000011 101000012 101000013 101000014 101000015 101000016 101000017 101000018 101000019 101000020 0 0 0 0 0 0 0 0 0 0


Guidelines and Limitations • The element connectivity orientation (n) will determine the TOP and BOT location as illustrated

below.

• Edge load does not support yet BOT and MID components • For mechanical analysis, the following should be noted: • For bidirectional coupling, all nodal temperatures are mapped to layer-wise temperatures if

ANALYSIS = ISH is used on PSHLN1 card. Only top temperatures are passed in if ANALYSIS = IH is used . • For chained analysis, only the TOP temperature will be passed into the mechanical analysis.

Test Cases There are several test cases available in the TPL subdirectories /tpl/mdr4s400a/hsb*.dat and /tpl/mdr4s400b/hshell*.dat TPL Problem hshell_dc_2.dat Example problem hshell_dc_2.dat demonstrates a linear through thickness temperature distribution for a static heat transfer analysis on a QUAD4, QUAD8, and TRIA3 mesh. The input heat flux loading is applied to the TOP face of the elements, and the radiation to a 20 degree fixed temperature is allowed from the TOP face of the elements.i

Figure 14-5

TPL example hshell_dc_2.dat geometry and loading.

In the model a linear through thickness distribution is specified with NLMOPTS,TEMPP,LINE

Main Index


.

Figure 14-6

TPL example hshell_dc_2.dat Temperatures (BOT)

TPL Problem hshell_dc_4.dat Test problem hshell_dc_4.dat is a cylinder with a quadratic through thickness temperature capability. It is loaded with a surface heat flux of 30 W/in^2 directed outwards from the TOP surface; radiating to a 20 degree fixed temperature with an emissivity factor of 0.8

Main Index


Figure 14-7

Main Index

TPL example hshell_dc_4.dat geometry and loading.


Figure 14-8

TPL example hshell_dc_4.dat Temperatures at MID.

GUI Support SimXpert supports the pre-processing of through thickness heat shell elements. SimXpert supports the post-processing of the through thickness as shown in the examples above. Patran currently only supports post-processing of the TOP surface.

Main Index

388 MD Nastran 2010 Release Guide Concentric half cylinder with view factor calculations with imposing heat flux with thermal thick shell

Concentric half cylinder with view factor calculations with imposing heat flux with thermal thick shell

Figure 14-9

SimXpert model

Geometry 1. The inner radius is 1 meter with depth of 10 meter 2. The outer radius is 2 meter with the depth of 10 meter

Applications We are imposing a constant heat flux of 500 watt/m2 along the entire outer cylinder, and the generated heat is transfer to the inner cylinder through radiation exchange. The loss radiation goes to the opening at -273.15 degree C.

Main Index


Since we are using thermal thick shell element for the outer shell, and we want to apply heat flux at the outer surface. We will see thermal gradients (drop in temperatures) along the thickness. The thermal - thick shell element is activated using the advanced nonlinear formulations: PSHLN1: PSHELL PSHLN1

1 1

2 2

0.1 2

2

ISH

2

outer outer

Also you will need a global setting called : NLMOPTS,TEMPP,QUAD This means a quadratic temperature distribution is assumed. The top ,middle, and bottom temperature per a single grid point are now available. Previous for the membrane CQUAD4 element, only a single temperature is allowed per grid . Top surface definition is based on the normal direction on the nodal connectivity of the CQUAD4 entry.

Objective We want to find the resulting temperature due to the laser heating imposed on the outer cylinder. In this exercise, we will use the new hemi-cube view factor calculations in SOL 400, and the geometry was build entirely within SIMX/version 3086 under the structure workspace.

Limitation Currently SIMX does not support the heating on the top or bottom surface because it required the addition of CHBDYE element. Update: SIMX does support the pre-processing using QBDY3, CONV, RADBC for the top and bottom surfaces using SIMX version 2010-83. Similarly you can have radiation, convection on top or bottom of shell element.

Main Index


The reason is that we will want to apply the heat flux on the bottom face of the outer cylinder: There is a total 600 CQUAD4 elements. The numbers of CQUAD4 element is from element ID 401 to 1000. CHBDYE,3001,401,6 ,*1,*1,== =598 QBDY3,6,500.0,,3001,THRU,3600

Here we have shown the NASTRAN replication command: This will automatically generated the CHBDYE from 3001 to 3600. The number 6 in field 4 on the CHBDYE ID 3001 represent the bottom side for the CQUAD4 401 . We are incrementing each field by 1, and we have to repeat 598 times, or total number of CHBDYE cards is from element 3001 to 3600.

Boundary Conditions 1. Heat flux (500 watt/m2) is applied on the entire outer cylinder 2. View factor is exchange between the inner cylinder to the outer cylinder 3. The loss radiation goes to -273.15 degree C 4. Sigma is 5.67e-8 watt/m2.K**4 5. Offset temperature is 273.15, the input temperature is degree C

Materials

Main Index

K (watt/m.C)

Shell Thickness

emissivity

Inner cylinder

100

0.002

0.8

Outer cylinder

10

0.1

1.0


SIMXpert file: cylinder3_flux.SimXpert Active side for View factor

Figure 14-10

Front side and backside for the shell elements

As you can see the gray color indicates this is the backside, and in our case the active side is green for the inside, blue color for the outside. Henceforth, we can select the active side as the front side.

Shading flag In this case the inner cylinder can potential block the view from outer cylinder, and therefore shading flag for the view factor calculations is set to BOTH so that program will detect potential blockers in this model.

Main Index


Figure 14-11

Main Index

Outer Cylinder


Figure 14-12

Main Index

Inner Cylinder


Main Index

Figure 14-13

Heat Lux Load

Figure 14-14

Browser Tree


Figure 14-15

Radiation Parameters

We will want to use the new NLSTEP with fixed increments:

Main Index


Figure 14-16

Main Index

Select ITER Method


Figure 14-17

Convergence on UPW

Figure 14-18

Fix Increments

The initial runs using the SIMX with heating applied on the top side of the cylinder, the top side here is the side facing the inner cylinder, we will get a constant temperature of 141.6 degree C on all layers for the outer cylinder.

Main Index


Next will modified the test deck so that the heating is applied on the bottom side of the cylinder, this way we will see the gradients through the thickness.

Main Index


NASTRAN test deck: half_flux_tempp2.dat

Figure 14-19

Main Index

Temperature Contour


Figure 14-20

Main Index

Outer Cylinder - Top Layers


Figure 14-21

Main Index

Middle Layers


Figure 14-22

Bottom Layers

Outer cylinder

Top

Middle

Bottom

Temp(max)

141.6

144.1

146.6

Temp(min)

77.78

80.56

83.15

The top here is the element that faces the inward inner cylinder.

Main Index


Figure 14-23

Inner Cylinder Temperature Contour

We can see due to the heating of outer cylinder, the inner cylinder sees the hot spot along the center that has temperature variations from 138.3 degree C to 28.71 degree C. The reason that we see the temperature is cooler near the end is because radiation loss to the cold space at -273.15 degree C.

Summary We built the entire model in SimXpert 2010 using the THERMAL GUI inside of the structures work space. We demonstrate the temperature gradients through thickness are supported in MD Nastran 2010.

Main Index

404 MD Nastran 2010 Release Guide Axisymmetrical Mechanical and Heat Transfer Shell Elements

Axisymmetrical Mechanical and Heat Transfer Shell Elements Introduction This functionality simulates mechanical or thermal axisymmetrical structures subject to axisymmetrical loading.

Benefits The model size is significantly smaller compared with that of 3-D shell modeling.

Feature Description CAXISYM, PAXISYM, PLOADX1, SLOADN1, TEMPN1, SPC, SPC1, SPCD, NLMOPTS. To input moment load, FORCE entry with 0,0,1 component vectors. The rotation output in the .f06 file is located under the T3 column. For thermal analysis, constant/linear/quadratic nodal temperature distribution is supported using NLMOPTS,TEMPP option. For linear distribution, TOP and BOT temperature can be specified on a grid using component 1 and 2, respectively. The MID temperature (for quadratic distribution) is assigned using component 3. The TOP/BOT attribute is defined based on element normal. For thermal analysis, internally generated grid is created to store the BOT/MID temperature. At this moment this grid is also used to present the output in f06 file. It is planned to give TOP/BOT/MID attribute to the user grid output in the .f06 file. At this moment the stress output is given at the centroid and top surface of the element. It is planned to output more element results.

Test Cases There are several test cases available in the TPL subdirectories /tpl/mdr4s400/axishell*.dat TPL Problem .dat A cylindrical shell under pressure and axial loading. To demonstrate the basic modeling technique how to use this feature. sol 400 cend title=testing CAXISYM element subcase 1 analysis=lnstatics nlparm=10 displacement=all stress=all

Main Index


spc=1 load=2 begin bulk NLPARM,10,10,,PFNT,-1 grid,1,,5., 0., 0. grid,2,,5., 10., 0. grid,3,,5., 20., 0. caxisym,1,1,1,2 caxisym,2,1,2,3 paxisym,1,1,,1. MAT1 1 210000. spc1,1,2,1 force,2,3,,100.,0.,1.,0. ploadx1,2,1,10.,10.,1,2 ploadx1,2,2,10.,10.,2,3 enddata

Main Index

.3

7.86-9

406 MD Nastran 2010 Release Guide Axisymmetrical Shell Elements

Axisymmetrical Shell Elements Introduction This project extends the capability of MD Nastran to simulate mechanical or thermal axisymmetrical structure subject to axisymmetrical loading. These elements will support contact, material nonlinearity, and geometrical nonlinearity.

Benefits The typical benefit of this feature is that the simulation process can be set up and run faster compared to that using the 3-D shell elements. Offers a new possibility for MD Nastran 2010 users to simulate slender axisymmetrical structure with axisymmetrical loading. The elements can be used as a preliminary step before general 3D shell elements are chosen. Since models are normally smaller and faster to run, more variation in the design parameters of the structure can be studied.

Feature Description CAXISMY, PAXISYM, PLOADX1, NLMOPTS, SLOADN1, TEMPN1, SPC, SPC1, SPCD For stress analysis, the number of nodal degrees of freedom is 3. The first two are translational displacement the third one is rotation which is located as the 6th degree of freedom. SPC’s and Load’s and nodal output have to be interpreted with this convention. For thermal analysis, constant/linear/quadratic nodal temperature distribution is supported using NLMOPTS,TEMPP option. Please refer to the Multi-dof Heat Shell element project for more detail description about this feature.

Example The following example (for the complete model please refers to axishell_pls.dat) will demonstrate this feature. A cylindrical shell under pressure loading will be analyzed. The material is elasto-plastic. sol 400 cend subcase 1 analysis=nlstatics nlparm=10 displacement=all stress=all spc=10 load=20 begin bulk param,lgdisp,1 NLPARM,10,10,,PFNT,-1,,UPV,, ,,,,,,1,,, ,0 CAXISYM, 1, 1, 1, 5

Main Index


… GRID, 1, , 5.0, 0.0, 0.0 ... mat1, 1, 60000., , 0.3 matep, 1, table, , 10 tables1, 10, 2 , 0., 240., 1.0, 4240., endt paxisym, 1, 1, , 0.15 spc1, 10, 2, 1 … ploadx1, 20, 1 , -10., -10., 1, 5 … ENDDATA

An excerpt of the .f06 file is shown below for stress and nodal output.

LOAD STEP = 1.00000E+00 N O N L I N E A R S T R E S S E S

...

ELEMENT FIBER ID DISTANCE 11 -7.480408E-02 7.480408E-02

D I S P L A C E M E N T

...

POINT ID. 1 2

TYPE

I N

STRESS-XX

A X I S Y M STRESS-YY

2.509646E+02 2.464789E+02

E L E M E N T S STRESS-XY

2.421699E+02 5.841080E+01

( C A X I S Y M ) STRAIN-XX

STRAIN-YY

-1.324018E+00 3.865741E-03 -1.887177E+00 3.815957E-03

STRAIN-XY

3.557906E-03 -2.567605E-04

-8.177767E-05 -8.177767E-05

V E C T O R G G

T1

8.829507E-02 2.648748E-02

T2 0.0 1.140616E-02

0.0

T3 0.0

0.0

R1 0.0

0.0

R2 0.0

R3 0.0 -2.933693E-02

Product Dependencies SimXpert and Patran need modifications to use the new or updated entries: CAXISYM, PAXISYM, PLOADX1, NLMOPTS, SPC, SPC1, SPCD, SLOADN1, TEMPN1. These GUI’s should also support the post-processing of TOP/BOT/MID attribute of the nodal temperature.

Documentation Dependencies None.

Limitations • Offset is not yet supported. • For chained analysis, only the top temperature will be passed into the mechanical model. • Moment carrying glue is not yet implemented for the axisymmetric shells.

Main Index

408 MD Nastran 2010 Release Guide Multi-Dof Heat Shell Elements

Multi-Dof Heat Shell Elements Introduction This project extends the current capability of the heat shell elements where the temperature distribution across the thickness can be set as constant, linear or quadratic.

Benefits This functionality provides more accurate simulation across the shell thickness compared with that of the classical element when it is expected that temperature is not constant through the thickness. Another benefit is ease of modeling. For thin wall structure, modeling with shell is much easier compared to that when using brick elements.Without this feature, shell elements have to converted into brick elements and the boundary and load conditions have to be redefined. This functionality also offers a better representation of the temperature distribution for mechanical analysis (only for bidirectional coupled analysis).

Feature Description The following features need extra attention when using multi-dof heat shell elements. For more detail description please refer to the MD Nastran Quick Reference Guide. NLMOPTS Bulk Data Entry This feature requires modified NLMOPTS Bulk Data. NLMOPTS,TEMPP,LINE (CONS,QUAD) is used to activate LINEar (CONSTant, QUADratic) temperature distribution across the shell thickness. The user grid holds the TOP temperature. Only one option is allowed in a job. The BOT or MID temperatures are held by the internally created grids. To print this information on the f06 file, users have to set NLMOPTS, TEMGO, YES. PSHLN1 Bulk Data Entry Shell elements have to reference PSHLN1. Please note that using LINE or QUAD option for NLMOPTS,TEMPP means that fully 3-D material data are required. SPC, SPC1, SPCD Bulk Data Entry The temperature boundary conditions with SPC, SPC1, and SPCD are extended. Component 1, 2 and 3 are now used to assign temperature at TOP, BOT and MID position.

Main Index


SLOAD or TEMP Bulk Data Entries These entries will assign value at the TOP position of the grids. To assign value at other position please use SLOADN1 or TEMPN1. SLOADN1 or TEMPN1 Bulk Data Entries SLOADN1 and TEMPN1 are the extension of the existing entries SLOAD and TEMP, respectively. With these entries it is now possible to assign component 1, 2, and 3 values for the TOP, BOT and MID position. CHBDYE Bulk Data Entry The SIDE field of CHBDYE is extended to allow user defining TOP, BOT and MID surface for shell elements using side 1, 6, and 7, respectively.

Example The following example (hshell4_radbc.dat) will demonstrate this feature. A plate has constant temperature on the top surface and exchanges heat to the ambient through radiation. The temperature distribution through the thickness is chosen to be linear. The results show that the temperature at the top surface differs from that of the bottom surface. SOL 400 CEND TITLE = Testing new heat shell element TEMP(INIT) = 20 SPC = 30 load = 10 THERMAL = ALL flux = ALL ANALYSIS = HSTAT NLPARM = 100 BEGIN BULK PARAM,SIGMA,5.67E-8 PARAM,TABS,0.0 nlmopts,TEMPP,LINE, ,TEMGO,YES, ,SPCRMPT,1 NLPARM,100,1,,PFNT,,,PU,,+NLP +NLP,1.0E-03,1.e-03 GRID,1,,0.0,0.0,0.0 GRID,2,,10.0,0.0,0.0 GRID,3,,10.0,10.0,0.0 GRID,4,,0.0,10.0,0.0 GRID,5,,0.0,10.0,0.0 GRID,8,,5.0,5.0,0.0 ctria3,1,1,1,2,8 ctria3,2,1,2,3,8 ctria3,3,1,8,3,4 ctria3,4,1,1,8,4 PSHELL,1,1,1. PSHLN1,1,,,,IH MAT4,1,200.0,,,1.2

Main Index

410 MD Nastran 2010 Release Guide Multi-Dof Heat Shell Elements

spc1,30,,1,2,3,4,5,8 spcd,10,1,,1300.,2,,1300. spcd,10,3,,1300.,4,,1300. spcd,10,8,,1300. spcd,10,5,,300. TEMPD,20,1300.0 RADBC,5,1.0,,100001,100002,100003,100004 RADM,45,1.0,1.0 chbdye,100001,1,6,,,45 chbdye,100002,2,6,,,45 chbdye,100003,3,6,,,45 chbdye,100004,4,6,,,45 ENDDATA

An excerpt of the F06 file is shown bellow. First the mapping of the user grids to the internally created ones is shown. From the temperature vector, it is obviously seen that the grids have different TOP (1,2, etc.) and BOT (101000001, 101000002, etc.) temperatures.

U S E R TOP BOT MID

G R I D

P O I N T (T O P)

101000001

M A P P I N G

T O

B O T/M I D

1 2 3 101000002 101000003 101000004 101000005 0 0 0

I N T E R N A L …

4 0

G R I D 5 0

… …

LOAD STEP = 1.00000E+00 T E M P E R A T U R E V E C T O R POINT ID. 1 101000001

TYPE S

ID S

VALUE

ID+1 VALUE ID+2 VALUE ID+3 VALUE … 1.300000E+03 1.300000E+03 1.300000E+03 1.300000E+03 1.008747E+03 1.008747E+03 1.008747E+03 1.008747E+03 ...

...

Product Dependencies SimXpert and Patran need modifications to use the new or updated entries: NLMOPTS, SPC, SPC1, SPCD, CHBDYE, SLOADN1, TEMPN1. These GUI’s should also support the post-processing of TOP/BOT/MID attribute of the nodal temperature.


Limitations • Edge load on the BOTTOM or MID nodes are not supported yet. It will be supported in the next

release. • For mechanical anaylsis it should be noted that for bidirectional coupling, all nodal temperatures

are mapped to layer-wise temperatures if ANALYSIS = ISH is used on a PSHLN1 card and only top temperatures are passed on if ANALYSIS = IH is used. • For chained analysis, only the TOP temperature will be passed into the mechanical model.

Main Index


Herrmann Elements Introduction This project supports linear Herrmann elements which can be used for incompressible or nearly incompressible materials. A plane strain, an axisymmetric, and a tetrahedral element is available.

Benefits The Herrmann elements can be used for incompressible elasticity, rubber elasticity and elasto-plasticity. For elasto-plastic material behavior update Lagrange formulation based on multiplicative decomposition must be used (NLMOPTS,LRGSTRN,2). Supported is a tetrahedron element for 3D analyses, a triangular element for plane strain analyses, and a triangular element for axisymmetric analyses.

Feature Description The Herrmann element type can be activated on the nonlinear property extension entries as follows: Tetrahedron

Plane Strain

Axisymmetric

PSLDN1

PSHLN2

PSHLN2

C4, ISOL, L

C3, IPS, L

C3, IAX, L

Note that these elements are selected automatically when they have rubber or elasto-plastic material behavior. This is controlled in NLMOPTS,SPROPMAP (on by default).

Product Dependencies This property type needs to be added to SimXpert and Patran.


Limitations • Initial velocities, accelerations and volumetric loads will not work correctly in transient dynamic

analyses since these elements use internally an extra grid point which does not yet get this contribution.

Main Index

412 MD Nastran 2010 Release Guide Herrmann Elements

Main Index

Chapter 15: MiscellaneousMD Nastran 2010 Release Guide

15

Main Index

Miscellaneous 

Enhanced MONSUM



PARAM,NONCUP Usage Extended to SOL 111



Application Regions



New Input File Reader - IFPSTAR



Contact Rigid Body Growth



Brake Squeal Analysis



Results and Output Changes



MSC.Nastran Error List

414 MD Nastran 2010 Release Guide Enhanced MONSUM

Enhanced MONSUM Introduction The MONSUM Bulk Data entry was introduced in MD Nastran R2 to enable the linear combination of monitor results or the updating in place of a monitor result. The MD Nastran R2 implementation imposed the restriction that the results to be summed must be of the same type. This restriction has been relieved in the current delivery.

Benefits The MONSUM feature of MD Nastran R2 allowed to user to perform such tasks as units conversion on a monitor result or to combine similar types on monitor results. Users also felt a need to combine different types of monitor points to create a special purpose response that is meaningful in the analysis task at hand. This extension of the MONSUM provides this added capability.

Feature Description The enhanced MONSUM, 2527 Bulk Data entry is described in the MD Nastran Quick Reference Guide. “Legacy” input files are supported in that the alternate format shown in the guide is identical to the standard format of earlier releases. A remark in the MONSUM description indicates that the summed quantities must be of a similar type, specifically: Force and moment summation monitor points: AMONPNT1, SMONPNT1, MONPNT3 Displacement monitor points: AMONDSP1 and SMONDSP1

Example Two examples are provided in the TPL: Monsum2.dat – This is a SOL 144 file that has five MONSUM entries. Three of these demonstrate the legacy feature while one combines an aerodynamic monpnt1 and a monpnt3 and another combines a structural monpnt1 with an aerodynamic monpnt1. Monsum4.dat – This is another SOL 144 file that has a single MONSUM entry that combines a structural mondsp1 with an aerodynamic mondsp1.

Guidelines and Limitations The MD Nastran R2 Release Guide and the previous examples imply this is a SOL 144 capability. This is not the case in that it can also be used in SOLs 101, 103, 108, 109, 111, 112 and 200. Summing a MONPNT1 and MONPNT3 in the dynamic solution sequences is currently misleading since the MONPNT1 support inertia results while the MONPNT3 does not.

Main Index

CHAPTER 15 415 Miscellaneous

The summed results are printed as one of the monitor types with the following order of precedence: smonpnt1, smondsp1, monpnt3, amonpnt1, amondsp1. E.g., an amonpnt1 and a monpnt3 appearing on the same entry will result in a monpnt3 regardless of which appears first. If different monitor results are being summed, the NAME appearing on the MONSUM should be unique with respect to other names. For the update in place, the name can be the same.

Main Index

416 MD Nastran 2010 Release Guide PARAM,NONCUP Usage Extended to SOL 111

PARAM,NONCUP Usage Extended to SOL 111 Until now, the usage of PARAM,NONCUP was allowed only in SOL 112, not in SOL 111. In MD Nastran 2010, usage of this parameter is allowed in SOL 111 also. In both SOLs 111 and 112, PARAM,NONCUP has the same meaning as follows:

Main Index

NONCUP = -1

Use uncoupled solution if there are no off-diagonal terms in any of the modal matrices (MHH, BHH, and KHH); otherwise use coupled solution.

NONCUP > -1

Use coupled solution regardless of the existence of off-diagonal terms in the modal matrices.

NONCUP = -2

Use uncoupled solution regardless of the existence of off-diagonal terms in the modal matrices.


Application Regions Introduction A new set concept called SET3 has been added which allows one to group together a list of nodes, elements, properties or a list of points and associate them with a unique id.

Benefits Application region can be used for group the elements or nodes. It is necessary for total heat load, contact loads, super element radiation load, and primitive radiation load. It is more convenient for the translator to process the groups of FEM data.

Input SET3 entry is used to define the application regions.

Main Index

418 MD Nastran 2010 Release Guide New Input File Reader - IFPSTAR

New Input File Reader - IFPSTAR The IFPStar component is MSC Software’s enhanced bulk data processor that is introduced in MD Nastran 2010 and MSC Nastran 2010. IFP stands for Input File Processor. The IFPStar component utilizes MSC’s Simulation Component Architecture (SCA) framework, and provides a robust mechanism to verify that the your input is both correct and accurate.

Benefits The benefits of the IFPStar component include: • Faster input processing (up to 40% faster for typical large models) • SORT is not required before interpretation • Significantly lower memory requirements • Clearer error messaging • Rule based definition identifies exact entry and field of illegal data • Identification of which INCLUDE file / line number of an illegal entry • Uses Quick Reference Guide rule base • Provides consistent and rigorous rule checking • Template definition of fields provides easier implementation of new features, thus reducing

development time. • Higher precision of input tables – 64bit maintained • The higher precision may cause slightly different answers compared to previous versions or

models run with the old Input File Processor (IFP) • Replaces IFP, RMDUPBK, and XSORT modules with a single more efficient module • Extensible and Pluggable to in-house or external applications (future) • Simplifies the process of adding new entries

IFPStar significantly improves developers’ ability to add or modify Nastran bulk data entries in a very short amount of time (less than 3 hours for a very complex entry, comparing to days using legacy IFP module). Rather than ad-hoc parsing rules buried in multiple layers of code, within the application, IFPStar utilizes template-based definitions for entries, which simplifies the process of adding new fields, putting proper checks in place on the fields within an entry, adding boundary conditions, etc … Another advantage of IFStar component is that it leverages the “component” capability of the SCA framework, which means the component can be used in any SCA enabled application (in house or external), and can easily be updated in the field, without the need for updating the entire installation.

Detailed error messages The error messages that are created in the IFPStar component are aimed to better help engineers pinpoint their input errors. For example, let’s assume that a user makes the following mistake in a MPC entry:

Main Index


SPC1

IO

12

1

3

1

3

The correct entry is: SPC1

10

12

Both IFPStar component and legacy IFP module catch the user’s error, and below is how each one issues the error messages: Legacy IFP module: *** USER FATAL MESSAGE 315 (IFPDRV) FORMAT ERROR ON BULK DATA ENTRY SPC1 SPC1 IO 12 1 3 *** USER FATAL MESSAGE 316 (IFPDRV) ILLEGAL DATA ON BULK DATA ENTRY SPC1 SPC1 IO 12 1 3 IFPStar Component: *** USER FATAL MESSAGE 9994 (BULKPM) Term Violation for Entity: SPC1 near line 27 SID:IO is an illegal integer value.

Potential Behavior Differences Note that IFPStar enforces the current Bulk Data rule set in the Quick Reference Guide. This means that legacy models that may have worked in previous versions may fail with IFPStar. Typical causes are illegal input that was not previously trapped, undocumented features or obsolete input entries. Note that there are several entries that are only supported by the IFPStar component in MD Nastran 2010 and MSC Nastran 2010. These entries include:

Main Index

PRJCON

MAXBRG

FSICTRL

WETLOAD

WETSURF

WETELMG

WETELME

MATUDS

PRPUDS

BCONUDS

ELEMUDS

QUDS

RCPARM

MAT6

MATT6

RADC

RADCT

VIEWEX

PCONV1

PRIM1

PRIM2

PRIM3

PRIM4

PRIM5

PRIM6

PRIM7

PRIM8

TABLEU1

TABLEU2

ENTUDS

RADCOL

DTABLE2

MATUSR

MATTUSR

420 MD Nastran 2010 Release Guide New Input File Reader - IFPSTAR

In RESTART runs, the “/” bulk data has been enhanced to have more user friendly commands. Previously, the only options on the “/” bulk data entry were to remove specific sorted bulk data line numbers, but with IFPStar the delete directives are more user friendly. Please refer to the Quick Reference Guide for more details. The sorted bulk data (print/punch) will have a slightly different look. In future versions of MD Nastran and MSC Nastran new bulk data entries will only be supported by the IFPStar component.

Known Issues In addition to the entries listed above, there are a few items that will not work with the IFPStar component. MSGMESH is no longer supported. Basic replication entries are supported, but some advanced replication applications may not work. In this case, it is recommended to use the old IFP processor with the case control command ECHO=PUNCH to generate a bulk data input without replications. Since this is a brand new component, and Nastran has 30+ years of legacy, while all attempts have been made to support the legacy, it is possible that some client models may not work with-in the bounds of IFPStar component rules and definitions. When this rare situation occurs with your existing models, you can get around this problem by using the old IFP by adding the following system cell nastran system(444)=0 to the top of your input file (see next paragraph for more details).

Changing the Defaults The NASTRAN System cell 444 is reserved to select the input file processor options. SYSTEM(444)=1 is the new default for the IFPStar component, SYSTEM(444)=0 is old IFP. These settings can be changed in the Patran Translation Parameters form and in the SimXpert Generic Solver Parameters form. In Patran 2010 and SimXpert 3.2 and earlier versions, the default can be changed in the Direct Text Input system cell section by adding "NASTRAN SYSTEM(444)=0" - without the quotes

If You Find Errors If you encounter an entry that follows the Quick Reference Guide rules and does not contain undocumented fields, but fails in the IFPStar component, please contact MSC support.

Main Index


Contact Rigid Body Growth An additional contact enhancement in MD Nastran 2010 release is the rigid body contact growth. This is particularly important for analysis of biomedical components like stents. A typical stent application places a stent in a blocked artery and then uses a balloon to expand the device. The main challenge in simulating stent growth in FEA is by expanding the stent internal surface by growing the rigid body with time increment. MD Nastran 2010 solves this issue by providing rigid body contact growth.

Additional information can be found in the MD Demonstration Problem Chapter 64.

Main Index

422 MD Nastran 2010 Release Guide Brake Squeal Analysis

Brake Squeal Analysis The brake squeal option available in MD Nastran R3 was limited to (1) linear finite elements and (2) a single rotation axis. Since there are quite some applications where quadratic finite elements are preferred to linear finite elements, in MD Nastran 2010 both linear and quadratic finite elements are supported in a brake squeal analysis. Moreover, in Sol600, the limitation of a single rotation axis has been removed, so that it is possible to model e.g. multiple gear wheel combinations in a single analysis, where per pair of contact bodies a different rotation axis can be specified. To this end, an alternate format of the BSQUEAL entry has been introduced, where the field entry "BODY" signals the start of data for a pair of contact bodies.

Main Index


Results and Output Changes Change of Solution Method for Dynamic Enforced Motion Analysis Using SPC/SPCD The total solution of a dynamic enforced motion analysis using SPC/SPCD can be regarded as a combination of a static enforced motion solution (similar to what is done in SOL 101) and a dynamic enforced motion solution that is relative to this static-based solution. Two methods are employed for obtaining the solution in Nastran. In the total or absolute (TOTAL/ABS) motion method, the program solves directly, in one step, for the TOTAL solution of the dynamic analysis which includes both the static-based solution and the dynamic solution that is relative to the static-based solution. In the relative (REL) motion method, the program obtains the total solution of the dynamic analysis in two steps, by first solving for the static-based solution and then solving separately for the dynamic solution RELATIVE to the static-based solution. The TOTAL/ABS solution method is computationally more efficient. This is also the only method that is meaningful and that should be employed when a problem involves the use of NOLINi or NLRGAP entries. An important point to note regarding this method is that, for modal dynamic analysis, residual vectors are absolutely critical in order for this method to get correct answers. The REL solution method, though less efficient, may be more accurate for transient solutions and for modal frequency response solutions at very low forcing frequencies. Also, for modal dynamic analysis, this method is not as critically dependent on residual vectors as the TOTAL/ABS solution method. In pre-MD 2010 versions of Nastran, the TOTAL/ABS method did not support modal damping and fluid structure problems. These problems are now fully resolved. With these enhancements, the TOTAL/ABS and REL solution methods both yield essentially the same results. In earlier versions of Nastran, the REL method was the implied default solution method. However, because of efficiency and other considerations outlined above, the TOTAL/ABS method has been chosen to be the default solution method in MD 2010. (See also related discussion below.)

New ENFMETH Parameter There is a parameter called ENFMETH that controls the solution method when dynamic enforced motion analysis via SPC/SPCD is used in SOLs 108, 109, 111, 112, 146 and 200. This parameter was an undocumented parameter in earlier versions and was used internally with a implied default value of REL, implying the use of the REL solution method mentioned above. This parameter is now documented in the ENFMETH (p. 723) in the MD Nastran Quick Reference Guide and the default value has been changed to TOTAL (or ABS) to reflect the new default of the TOTAL/ABS solution method indicated above. It should be emphasized here that the new ENFMETH parameter is completely separate, independent and distinct from the similarly sounding ENFMOTN parameter. These two parameters should not be confused with each other. The former controls the solution method when dynamic enforced motion analysis via SPC/SPCD is used while the latter controls how the results of such an analysis are output.

Main Index

424 MD Nastran 2010 Release Guide Results and Output Changes

Details will be clear from the descriptions of these parameters in the ENFMETH and ENFMOTN (p. 724) in the MD Nastran Quick Reference Guide.

NEW OPTMIZER Optimization tasks that previously used the BIGDOT optimization algorithm now employ the IPOPT optimization algorithm (See The IPOPT Algorithm (App. C) in the Design Sensitivity and Optimization User’s Guide). These are typically topology optimization tasks or tasks with many design variables. If the user explicitly selects the BIGDOT algorithm using OPTCOD=BIGDOT on the DOPTPRM bulk data entry, the IPOTPT algorithm will be used in its place and a User Information Message will be printed that indicates this. It is expected that the results from the two algorithms will be similar, but not exactly the same.

Main Index


MSC.Nastran Error List The current error lists for MD Nastran can be obtained from the MSC Software Simcompanion website: http://simcompanion.mscsoftware.com/infocenter/index?page=content&id=KI8008006

Main Index

426 MD Nastran 2010 Release Guide MSC.Nastran Error List

Main Index

Ap. A: Connectors MD Nastran 2010 Release Guide

A

Connectors



Main Index

Connectors Output

428 MD Nastran 2010 Release Guide Connectors Output

Connectors Output Example A - Element Force and Element Stress 0

FREQUENCY =

ELEMENT ID 30 0

BEND-MOMENT END-A PLANE 1 (MZ) PLANE 2 (MY) -1.808122E-01 -1.966379E-02 2.170022E-02 2.359719E-03

FREQUENCY =

ELEMENT ID 30 0

BEND-MOMENT END-A PLANE 1 (MZ) PLANE 2 (MY) -1.808791E-01 -1.966534E-02 2.171652E-02 2.360096E-03 1.000000E+01 C O M P L E X

AXIAL STRESS 3.525211E+00 -4.228557E-01

FREQUENCY =

ELEMENT ID 30

Main Index

2.000000E+01 C O M P L E X

FREQUENCY =

ELEMENT ID 30 0

1.000000E+01 C O M P L E X


BEND-MOMENT END-B PLANE 1 (MZ) PLANE 2 (MY) -3.561784E-03 2.373087E-03 4.290746E-04 -2.845342E-04 F O R C E S

S T R E S S E S


- SHEAR PLANE 1 (FY) PLANE 2 (FZ) -3.980280E-01 -4.946850E-02 4.777317E-02 5.934670E-03



AXIAL FORCE FX TORQUE MX 2.765457E-02 2.769116E-02 -3.313215E-03 3.328268E-03 SUBCASE 1

( C W E L D P )




AXIAL FORCE FX TORQUE MX 2.768694E-02 -2.765884E-02 -3.321101E-03 3.320390E-03 SUBCASE 1

( C W E L D P )



S T R E S S E S

( C W E L D P )

- SHEAR PLANE 1 (FY) PLANE 2 (FZ) -3.979684E-01 -4.947790E-02 4.775866E-02 5.936962E-03


BEND-MOMENT END-B PLANE 1 (MZ) PLANE 2 (MY) -3.602137E-03 2.367348E-03 4.389053E-04 -2.831364E-04


2.000000E+01 C O M P L E X

AXIAL STRESS 3.521090E+00 -4.218517E-01

SUBCASE 1 F O R C E S

MAXIMUM SHEAR STRESS 2.092356E+02 2.511545E+01

BEARING STRESS 4.010323E+01 4.812626E+00 SUBCASE 1

( C W E L D P )


MAXIMUM SHEAR STRESS 2.094103E+02 2.515803E+

BEARING STRESS 4.010902E+01

Appendix A 429 Connectors

Example B - Element Stress Output 0 ELEMENT-ID 10001

10002

Main Index

CORNER GRID-ID 0GRID CENTER X Y Z 90001 X Y Z 90002 X Y Z 90003 X Y Z 90004 X Y Z 90005 X Y Z 90006 X Y Z 90007 X Y Z 90008 X Y Z 0GRID CENTER X Y Z 90009 X Y Z 90010 X Y Z 90011 X Y Z

S T R E S S E S I N S E A M E L E M E N T S ( C S ------CENTER AND CORNER POINT STRESSES--------DIR. COSINES NORMAL SHEAR PRINCIPAL -A- -B- -CCS 8 GP 7.747896E+05 XY -3.827610E+03 A 7.748116E+05 LX 1.00 0.00-0.01 1.074136E+05 YZ 1.673470E-10 B 2.502929E-09 LY-0.01 0.00-1.00 2.328306E-09 ZX 1.746230E-09 C 1.073916E+05 LZ 0.00 1.00 0.00 1.711155E+06 XY -7.739222E+03 A 1.711200E+06 LX 1.00 0.00-0.01 3.764584E+05 YZ -3.868169E+03 B 3.602726E+05 LY-0.01 0.23-0.97 3.611997E+05 ZX -5.157554E+01 C 3.773406E+05 LZ 0.00 0.97 0.23 1.707039E+06 XY -7.739222E+03 A 1.707084E+06 LX 1.00 0.00-0.01 3.646422E+05 YZ 3.868169E+03 B 3.572576E+05 LY-0.01-0.47-0.88 3.592958E+05 ZX -5.157554E+01 C 3.666358E+05 LZ 0.00 0.88-0.47 -1.638654E+05 XY 8.400235E+01 A -1.563204E+05 LX 0.01 0.00-1.00 -1.563954E+05 YZ 3.868169E+03 B -3.583610E+05 LY 1.00-0.02 0.01 -3.582869E+05 ZX -5.157554E+01 C -1.638663E+05 LZ 0.02 1.00 0.00 -1.655750E+05 XY 8.400235E+01 A -1.580980E+05 LX 0.01 0.00-1.00 -1.581723E+05 YZ -3.868169E+03 B -3.622819E+05 LY 1.00 0.02 0.01 -3.622085E+05 ZX -5.157554E+01 C -1.655759E+05 LZ-0.02 1.00 0.00 1.727548E+06 XY -7.739222E+03 A 1.727593E+06 LX 1.00 0.00-0.01 3.830623E+05 YZ -3.868169E+03 B 3.659432E+05 LY-0.01 0.22-0.98 3.668194E+05 ZX 5.157554E+01 C 3.838939E+05 LZ 0.00 0.98 0.22 1.722568E+06 XY -7.739222E+03 A 1.722612E+06 LX 1.00 0.00-0.01 3.703815E+05 YZ 3.868169E+03 B 3.612509E+05 LY-0.01-0.39-0.92 3.628978E+05 ZX 5.157554E+01 C 3.719841E+05 LZ 0.00 0.92-0.39 -1.698541E+05 XY 8.400235E+01 A -1.598039E+05 LX 0.01 0.00-1.00 -1.598779E+05 YZ 3.868169E+03 B -3.639800E+05 LY 1.00-0.02 0.01 -3.639066E+05 ZX 5.157554E+01 C -1.698548E+05 LZ 0.02 1.00 0.00 -1.706989E+05 XY 8.400235E+01 A -1.607165E+05 LX 0.01 0.00-1.00 -1.607901E+05 YZ -3.868169E+03 B -3.658836E+05 LY 1.00 0.02 0.01 -3.658106E+05 ZX 5.157554E+01 C -1.706996E+05 LZ-0.02 1.00 0.00 CS 8 GP 7.406084E+05 XY 9.462977E+02 A 7.406120E+05 LX 1.00 0.00 0.00 -2.130364E+04 YZ 4.292815E-10 B -2.130482E+04 LY 0.00 1.00 0.00 -1.583248E-08 ZX 1.333328E+03 C -2.400266E+00 LZ 0.00 0.00-1.00 1.623490E+06 XY 1.970375E+03 A 1.623494E+06 LX 1.00 0.00 0.00 8.306726E+04 YZ 9.464031E+02 B 8.306052E+04 LY 0.00 1.00 0.00 2.947562E+05 ZX 1.612613E+03 C 2.947584E+05 LZ 0.00 0.00-1.00 1.623357E+06 XY 1.970375E+03 A 1.623361E+06 LX 1.00 0.00 0.00 8.317433E+04 YZ -9.464031E+02 B 8.316755E+04 LY 0.00 1.00 0.00 2.942068E+05 ZX 1.612613E+03 C 2.942091E+05 LZ 0.00 0.00-1.00 -1.337316E+05 XY -7.777978E+01 A -1.233649E+05 LX-0.01-0.01-1.00 -1.233709E+05 YZ -9.464031E+02 B -2.949047E+05 LY 1.00 0.01-0.01 -2.948834E+05 ZX 1.612613E+03 C -1.337162E+05 LZ-0.01 1.00-0.01

E A M ) MEAN PRESSURE

VON MISES

-2.940678E+05

7.270885E+05

-8.162711E+05

1.342475E+06

-8.103257E+05

1.345162E+06

2.261826E+05

1.983753E+05

2.286519E+05

2.005495E+05

-8.258101E+05

1.352764E+06

-8.186157E+05

1.356026E+06

2.312129E+05

1.993407E+05

2.324332E+05

2.003621E+05

-2.397683E+05

7.514921E+05

-6.671043E+05

1.446252E+06

-6.669126E+05

1.446268E+06

1.839953E+05

1.666055E+05


0 ELEMENT-ID

10003

0 ELEMENT-ID 10004

Main Index

S T R E S S E S I N S E A M E L E M E N T S ( C S E ------CENTER AND CORNER POINT STRESSES--------DIR. COSINES NORMAL SHEAR PRINCIPAL -A- -B- -CX -1.333445E+05 XY -7.777978E+01 A -1.228786E+05 LX-0.01-0.01-1.00 Y -1.228843E+05 YZ 9.464031E+02 B -2.941010E+05 LY 1.00-0.01-0.01 Z -2.940796E+05 ZX 1.612613E+03 C -1.333288E+05 LZ 0.01 1.00-0.01 90013 X 1.608190E+06 XY 1.970375E+03 A 1.608193E+06 LX 1.00 0.00 0.00 Y 7.755697E+04 YZ 9.464031E+02 B 7.755026E+04 LY 0.00 1.00 0.00 Z 2.916883E+05 ZX 1.054044E+03 C 2.916916E+05 LZ 0.00 0.00-1.00 90014 X 1.608294E+06 XY 1.970375E+03 A 1.608298E+06 LX 1.00 0.00 0.00 Y 7.790112E+04 YZ -9.464031E+02 B 7.789438E+04 LY 0.00 1.00 0.00 Z 2.916921E+05 ZX 1.054044E+03 C 2.916954E+05 LZ 0.00 0.00-1.00 90015 X -1.357683E+05 XY -7.777978E+01 A -1.230557E+05 LX-0.01-0.01-1.00 Y -1.230615E+05 YZ -9.464031E+02 B -2.918279E+05 LY 1.00 0.01-0.01 Z -2.918155E+05 ZX 1.054044E+03 C -1.357617E+05 LZ-0.01 1.00-0.01 90016 X -1.356183E+05 XY -7.777978E+01 A -1.228063E+05 LX-0.01-0.01-1.00 Y -1.228120E+05 YZ 9.464031E+02 B -2.915773E+05 LY 1.00-0.01-0.01 Z -2.915649E+05 ZX 1.054044E+03 C -1.356115E+05 LZ 0.01 1.00-0.01 0GRID CS 8 GP CENTER X 1.284104E+03 XY -4.129671E+01 A 1.285049E+03 LX 1.00 0.02 0.00 Y -5.206752E+02 YZ 6.457412E-10 B -5.216197E+02 LY-0.02 1.00 0.00 Z -2.142042E-08 ZX 8.847564E-08 C -2.142039E-08 LZ 0.00 0.00-1.00 90017 X 2.416318E+03 XY -5.225373E+01 A 2.417096E+03 LX 1.00 0.01 0.00 Y -1.092519E+03 YZ -4.401031E+01 B -1.094830E+03 LY-0.01 1.00 0.03 Z 1.684483E+02 ZX -5.868064E-01 C 1.699818E+02 LZ 0.00 0.03-1.00 90018 X 2.495232E+03 XY -5.225373E+01 A 2.496019E+03 LX 1.00 0.02 0.00 Y -9.753662E+02 YZ 4.401031E+01 B -9.776510E+02 LY-0.02 1.00-0.03 Z 3.143401E+02 ZX -5.868064E-01 C 3.158376E+02 LZ 0.00-0.03-1.00 90019 X -8.759534E+01 XY -3.033968E+01 A -2.349008E+01 LX-0.42-0.08-0.91 Y -5.015059E+01 YZ 4.401031E+01 B -1.968506E+02 LY 0.88-0.30-0.38 Z -1.829433E+02 ZX -5.868064E-01 C -1.003486E+02 LZ 0.24 0.95-0.19 90020 X -1.375186E+02 XY -3.033968E+01 A -7.612272E+01 LX-0.44 0.04-0.90 Y -9.965966E+01 YZ -4.401031E+01 B -3.093700E+02 LY 0.88 0.21-0.42 Z -2.998451E+02 ZX -5.868064E-01 C -1.515307E+02 LZ-0.17 0.98 0.13 90021 X 2.982642E+03 XY -5.225373E+01 A 2.983355E+03 LX 1.00 0.01 0.00 Y -8.465572E+02 YZ -4.401031E+01 B -8.487935E+02 LY-0.01 1.00 0.03 Z 4.219966E+02 ZX 5.868065E-01 C 4.235193E+02 LZ 0.00 0.03-1.00 90022 X 2.948929E+03 XY -5.225373E+01 A 2.949649E+03 LX 1.00 0.01 0.00 Y -8.420306E+02 YZ 4.401031E+01 B -8.444359E+02 LY-0.01 1.00-0.04 Z 3.050948E+02 ZX 5.868065E-01 C 3.067800E+02 LZ 0.00-0.04-1.00 90023 X -2.039378E+02 XY -3.033968E+01 A -1.402171E+02 LX-0.43-0.02-0.90 Y -1.611178E+02 YZ 4.401031E+01 B -4.434710E+02 LY 0.90-0.16-0.42 Z -4.364915E+02 ZX 5.868065E-01 C -2.178590E+02 LZ 0.13 0.99-0.09 90024 X -1.412352E+02 XY -3.033968E+01 A -7.500764E+01 LX-0.41 0.04-0.91 Y -9.800105E+01 YZ -4.401031E+01 B -3.004030E+02 LY 0.89 0.22-0.39 Z -2.905998E+02 ZX 5.868065E-01 C -1.544254E+02 LZ-0.18 0.98 0.12

CORNER GRID-ID 90012

CORNER GRID-ID 0GRID CENTER X Y Z 90025 X Y Z 90026 X Y Z 90027 X Y Z 90028 X Y Z 90029 X Y Z 90030 X Y Z 90031 X Y Z 90032 X Y Z

S T R E S S E S I N S E A M E L E M E ------CENTER AND CORNER POINT STRESSES--------NORMAL SHEAR PRINCIPAL CS 8 GP 2.857427E+00 XY -5.724032E-02 A 7.595094E+00 7.594403E+00 YZ -5.420588E-10 B 1.257286E-08 1.257285E-08 ZX -6.053597E-09 C 2.856735E+00 1.577084E+00 XY 5.002377E+00 A 6.410882E+00 1.218060E+00 YZ 1.910919E-01 B -3.610427E+00 4.063272E+00 ZX 2.547832E-03 C 4.057961E+00 -5.694098E+00 XY 5.002377E+00 A -8.618130E-01 -6.043215E+00 YZ -1.910919E-01 B -1.292361E+01 -1.291273E+01 ZX 2.547832E-03 C -1.086462E+01 3.802032E+00 XY -5.116858E+00 A 1.589757E+01 1.373110E+01 YZ -1.910919E-01 B -4.134058E+00 -4.131593E+00 ZX 2.547832E-03 C 1.638033E+00 1.120986E+01 XY -5.116858E+00 A 2.345315E+01 2.131121E+01 YZ 1.910919E-01 B 9.069369E+00 1.298105E+01 ZX 2.547832E-03 C 1.297959E+01 -5.801891E+00 XY 5.002377E+00 A -9.705124E-01 -6.152861E+00 YZ 1.910919E-01 B -1.313789E+01 -1.312748E+01 ZX -2.547842E-03 C -1.097383E+01 1.536345E+00 XY 5.002377E+00 A 6.378676E+00 1.195284E+00 YZ -1.910919E-01 B -3.641881E+00 3.985157E+00 ZX -2.547842E-03 C 3.979991E+00 1.171584E+01 XY -5.116858E+00 A 2.348970E+01 2.126247E+01 YZ -1.910919E-01 B 9.489802E+00 1.305916E+01 ZX -2.547842E-03 C 1.305798E+01 4.514247E+00 XY -5.116858E+00 A 1.643190E+01 1.423316E+01 YZ 1.910919E-01 B -3.919224E+00 -3.916836E+00 ZX -2.547842E-03 C 2.317893E+00

A M ) MEAN PRESSURE 1.834361E+05

VON MISES 1.662438E+05

-6.591450E+05

1.435601E+06

-6.592958E+05

1.435494E+06

1.835484E+05

1.627915E+05

1.833317E+05

1.627466E+05

-2.544763E+02

1.610510E+03

-4.974160E+02

3.080820E+03

-6.114019E+02

3.040780E+03

1.068964E+02

1.504556E+02

1.790078E+02

2.061600E+02

-8.526937E+02

3.380599E+03

-8.039978E+02

3.369357E+03

2.671824E+02

2.728479E+02

1.766120E+02

1.980148E+02

N T S ( C S E A M ) DIR. COSINES MEAN -A- -B- -CPRESSURE LX-0.01 0.00-1.00 LY 1.00 0.00-0.01 LZ 0.00 1.00 0.00 LX 0.72-0.69 0.05 LY 0.69 0.72 0.03 LZ 0.06-0.02-1.00 LX 0.72-0.04 0.69 LY 0.69 0.06-0.72 LZ-0.01 1.00 0.07 LX-0.39 0.01-0.92 LY 0.92 0.01-0.39 LZ-0.01 1.00 0.01 LX-0.39 0.92-0.02 LY 0.92 0.39 0.01 LZ 0.02-0.02-1.00 LX 0.72 0.04 0.69 LY 0.69-0.05-0.72 LZ 0.01 1.00-0.06 LX 0.72-0.69-0.05 LY 0.69 0.72-0.03 LZ-0.06 0.02-1.00 LX-0.40 0.92 0.03 LY 0.92 0.40-0.01 LZ-0.02 0.02-1.00 LX-0.39-0.01-0.92 LY 0.92-0.01-0.39 LZ 0.01 1.00-0.01

VON MISES

-3.483943E+00

6.644488E+00

-2.286139E+00

9.076537E+00

8.216681E+00

1.117548E+01

-4.467181E+00

1.785942E+01

-1.516737E+01

1.288174E+01

8.360745E+00

1.124266E+01

-2.238929E+00

9.062510E+00

-1.534583E+01

1.260059E+01

-4.943524E+00

1.805928E+01

Appendix A 431 Connectors

Main Index


Main Index

Ap. B: Thermo-Mechanical Theory MD Nastran 2010 Release Guide

B

Thermo-Mechanical Theory



Main Index

Coupled Thermo-Mechanical Theory

434 MD Nastran 2010 Release Guide Coupled Thermo-Mechanical Theory

Coupled Thermo-Mechanical Theory Introduction Many problems encountered in industry require the analysis of a fully coupled thermo-mechanical problem. In general the observed phenomena need to be modelled like this if one or more of the following situations occur: • The structure undergoes large deformation so that there is a change in the geometry and

boundary conditions associated with the heat transfer problem. • Deformation converts mechanical work into heat through an irreversible process which can not

be neglected relative to other heat sources. • Changing contact conditions influence the heat flow between parts that are contacting each other. • Relative sliding of different parts contacting each converts frictional work into heat through an

irreversible process which can not be neglected relative to other heat sources. In either case the changes in the temperature distribution contribute to the deformation of the structure, through thermal strains and through changes of the temperature dependent material properties. In the following a short overview is given of the basic equations governing the thermo-mechanical problem and their weak form to make their solution feasible by means of the finite element method.

A Short Overview Of The Basic Equations Of Continuum Thermo-mechanics Before discussung some of the implementation details of the coupled thermal/mechanical analysis capability in MD Nastran, a short overview is given of the basic equations of continuum thermomechanics in order to recognize the different sources of coupling between the thermal and the mechanical phases of the deformation process. The description here is necessarilly brief and only intends to point out the related physical concepts. For more details the reader is referred to the works of J.F. Besseling and E. van der Giessen 1., of H. Ziegler 2. and of Y.C. Fung 3., among the many sources available on this topic. The following notational conventions are used in this overview. Summation is implied over repeated indices in expressions, where the range is 3 for Latin indices and 2 for Greek indices. A superimposed dot means taking the material time derivative.  ij denotes the Kronecker delta defined as  ij = 1 when i = j , otherwise it is zero.  ij k denotes the permutation tensor defined as  ij k = 1 when i  j  k is an even permutation,  ij k = – 1 when i  j  k is an odd permutation, otherwise it is zero. The kinematics of the continuum is described in a Cartesian reference frame, where the undeformed configuration serves as the reference configuration. The material points in this configuration are represented by their Cartesian coordinates X i . Their coordinates in the deformed configuration are represented by x i , which can be regarded as a functions of time, t, and their initial position:

Main Index

Appendix B 435 Thermo-Mechanical Theory

x i = x i  t X 1 X 2 X 3 

(2-1)

The displacements, u i , of any material point are thus given as: ui = xi – Xi

(2-2)

To describe the process with plastic deformations, the deformation gradient x F i j = --------i X j

(2-3)

is assumed to be the product (cf. E.H. Lee,”Elastic-plastic deformation at finite strains”, J. Appl. Mech., 36, e

p

1-6, 1969., 450) of an elastic (or recoverable) part, F i j , and a plastic (or non-recoverable) part, F i j : e

p

(2-4)

F i j = F i k F kj

With this assumption a number of tensors are defined that can be used as measures for the elastic and plastic deformations and they are valid for arbitrary finite deformations. The total elastic strain tensor is given as: e 1 e e E i j = ---  F ki F k j –  ij  2

(2-5)

The rate of total deformation tensor is given as: u· 1 u· d ij = ---  -------i + -------j , 2  x j x i

(2-6)

which is the symmetric part of the velocity gradient u· –1 e p L ij = F· ik F k j = -------i = L i j + L ij x j

,

(2-7)

which is decomposed in an elastic part –1

e e e L i j = F· ik F k j

(2-8)

and a plastic part p

e

p

e

–1

L i j = F ik  kl F l j with

Main Index

(2-9)


–1

p p p  ij = F· ik F k j

(2-10)

The rate of elastic deformation tensor is given as: e e 1 e d ij = ---  L i j + L ji  2

(2-11)

The material time derivative of the elastic strain tensor and the rate of elastic deformation tensor are thus related by. e e e e E· i j = d kl F k i F l j

(2-12)

The rate of plastic deformation tensor is given as: p p 1 p d ij = ---  L i j + L ji  2

(2-13)

The rate of total deformation therefore is the sum of the elastic and plastic rates of deformation: e

p

d ij = d i j + d i j

(2-14)

The balance equations summarized below are formulated with respect to the deformed configuration and are valid for any amount of deformation. With  as the mass density, u· i and, u·· i as the material components of velocity and accelleration, ij as the Cauchy sress tensor components, fi as the external volume force vector components, pi as the external pressure force vector components, T as the absolute temperature, q as the external heat flux per unit area, qi as the heat flux vector components, ni as the vector components of the outward unit normal, s as the entropy per unit mass,  as the entropy production per unit mass, and e as the internal energy per unit mass, the following basic equations of continuum thermo-mechanics are listed for a closed system: 1. conservation of mass: d  dV = 0 d t V

=>

u· i ·  +  ------- = 0 x i

(2-15)

2. balance of momentum: d u· dV = d t V i

Main Index





p d p i

+

V f i dV

=>


 ij ---------- + f i = u·· i in V and  ij n j = p i on p x j

(2-16)

3. balance of moment of momentum: d  x u· dV = d t V ij k i j





 x p d p i jk i j

+

V  ij k x i f j dV

=>

 ij =  ji

(2-17)

4. conservation of energy: 1 d   e + --- u· i u· i dV =    2 dt V



p

 

q

 p i u· i + q  d +

V f i u· i dV

q e· =  ij d i j – -------i in V and q i n i = – q on q x i

=>

(2-18)

5. law of entropy production: d s dV = d t V



--q- d +



qT

V  dV

and   0 =>

 q i  T   = s· + -------------------0 x i

(2-19)

It is furthermore postulated that the specific internal energy, e, and the specific entropy, s, are state variables of the system, so their expressions represent equations of state. Equation (2-15) expresses the fact that the total mass of the system remains constant. Equation (2-16) expresses the fact that the change in momentum of the system is caused by the external forces acting on the system. Equation (2-17) expresses the fact that the change in moment of momentum of the system about the origin of the coordinate system is caused by the moments of the external forces about this origin. Equation (2-18) expresses the first law of thermodynamics, which states that the rate of work done by the external loading plus the heat flux supplied to the system through its external boundaries is equal to the change in internal energy plus the change in kinetic energy of the system. Equation (2-19) expresses the second law of thermodynamics, which states that the difference between the total entropy change and the entropy flow through the external boundaries, i.e. the entropy production, is always non-negative. Only for reversible thermo-mechanical processes it is zero, for all others it is positive. With (2-18) the law of entropy production can be put in the following form: q i T T = – ---- ------- +  i j d ij –   e· – Ts·   0 T x i

Main Index

(2-20)


So far no assumptions have been made about the constitutive behaviour of the material and the above expressions are still very general. It will be assumed that the internal energy can be given as a function e

of entropy, s, and the components of elastic strain, E i j : e

e = e (s,E i j) ,

(2-21)

Furthermore Fourier’s law of heat conduction is assumed: T q i = –  ij ------x j

(2-22)

where  ij are the coefficients of the thermal conductivity tensor. The law of entropy production then takes the following form:  ij T T p T = ------ ------- ------- +  i j d ij T x i x j     e e e e e – T s·  0 +   ij –  ---------- F i k F jl d ij –   ----e    s  E kl e     E s ij

(2-23)

Since equation (2-23) must hold for every conceivable thermo-mechanical process in the material it can p

be concluded, that the tensor  ij must be positive definite and that  ij d ij must always be positive. This reflects our notions of irreversibility, that heat can only flow “by itself” from a region of higher temperature to a region of lower temperature and that work done in plastic deformations is not recoverable as mechanical work. Furthermore it is necessary that: e e e  ij =  ---------- F ik F jl e E kl

(2-24)

e T = ----s e

(2-25)

s

and

E

ij

The reasoning behind the last two equations is as follows. Assume for instance, that the constitutive relation of the material is such that the “equal” sign in (2-25) must be a “smaller than” sign. Now it is always possible to conceive a process such that there are no temperature gradients, there is no plastic deformation, the elastic deformations remain constant, but the entropy is increasing, by supplying heat over its boundaries. If this heat supply is slow enough, there will be no temperature gradients. This process would result in a negative entropy production, thus violating (2-19). For similar reasons the

Main Index


“larger than” sign is also impossible, leaving the equal sign as only possibility that never violates the entropy production law. The same line of reasoning applies to (2-24). These last two equations give the thermodynamic definitions of stress and temperature. Since temperature is often better apprehended as a state variable to describe the process than entropy, the so-called free energy per unit mass, f, is often used, instead of the internal energy. The specific free energy is defined as: (2-26)

f = e – Ts The entropy production equation of (2-20) is now written as: q i T · T = – ---- ------- +  i j d ij –   f + sT·   0 T x i

(2-27)

The free energy is a function of state and is written as a function of temperature and elastic strains: e

(2-28)

f = f (T,E ij) The law of entropy production then takes the following form:  ij T T p T = ------ ------- ------- +  i j d ij T x i x j     e e e f f + s T·  0 +   ij –  ---------- F i k F jl d ij –   -----   T  e E k l e     E T ij

,

(2-29)

from which the same conclusions can be drawn with respect to the entropy productive mechanisms as from equation (2-23) and furthermore it is necessary that: e e f  ij =  ---------- F ik F j l , and e E kl

(2-30)

f s = – -----T e

(2-31)

T

Ei j

With equations (2-28), (2-30) and (2-31) and also noting equation (2-14), the energy balance equation (2-18) can now be brought to the following form: q p Ts· =  ij d ij – -------i , x i Since the entropy, s, is a function of state:

Main Index

(2-32)


e

s = s (T,E ij) ,

(2-33)

equation Figure 2-32 can be written as: q e p s s T -----T· + T ---------- E· i j =  ij d ij – -------i e T e x i E i j E T ij

(2-34)

and by employing equation (2-25), (2-30) and (2-31) this finally becomes:  ij q e p e  -----T· – T ---------d =  ij d ij – -------i T e T e ij x i E

E

ij

(2-35)

ij

The heat capacity, c, of the material is defined as: 2

s  f ec = ----= T -----= – T --------2 T e T e T e E ij E E

ij

(2-36)

ij

The final form of the energy equation then becomes:  ij q e p cT· = T ---------d ij +  i j d ij – -------i T e x i E

(2-37)

ij

The equations of motion as given by equation (2-16) are:  ij u·· i = --------- + f i x j

(2-38)

Furthermore the system is subjected to mechanical boundary conditions i j nj = pi ui  t  = ui  t 

, on 

p

, on 

u

(2-39)

and thermal boundary conditions qi ni = –q

, on 

q

T t = Tt

, on 

T

and to mechanical initial conditions

Main Index

(2-40)


0

ui  t = 0  = ui 0 · u i  t = 0  = u· i

(2-41)

and thermal initial conditions Tt = 0 = T p

0

(2-42)

u

Here  and  are resp. the regions on the outer boundary of the structure where the external forces q

T

and the displacemenst are prescribed and  and  are resp. the regions on this outer boundary where the external fluxes and the temperatures are prescribed. The first term in the right hand side of equation (2-37) accounts for the termo-elastic effects in the material, the second term accounts for the dissipative effects due to irreversible deformation processes. The differential equations (2-37) and (2-38) together with the boundary conditions (2-39) and (2-40) and initial conditions (2-41) and (2-42) fully describe the thermal and mechanical behaviour of the system in terms of absolute temperature, T, and displacements, u i , provided that they can be supplemented with adequate constitutive relations. In particular it is necessary to provide more details about the form of the free energy function, f, and to provide the laws that govern the plastic deformation process. These details are not pursued in this overview.

Weak Formulation Of The Thermo-mechanical Problem Including Contact To arrive at the finite element equations of the coupled thermo-mechanical problem, the governing differential equations together with their boundary conditions are cast in a weak form. This form allows to easily include the constraint relations resulting from contact. It also clearly shows the structure of the set of extremely nonlinear ordinary differential equations and how the coupling terms appear in this set of equations. The equations are first presented in their strongly coupled form. The solution of this set of equations is extremely complicated and computationally expensive. By making a number of judicious assumptions the structure of the equations can be greatly simplified, resulting in a weakly coupled set of equations. This latter set of equations suffices in most practical applications to obtain an accurate solution of the coupled thermo-mechanical problem. When some regions of the external boundary contact each other, it is necessary to add non-penetration constraints to the set of mechanical equations. If furthermore friction is included it is necessary to split the contact region into two distinct regions, one where the friction stress is less than the friction stress limit and no relative sliding can occur, i.e. a sticking region, and one where the friction stress equals the friction stress limit and relative sliding can occur, i.e. a slipping region. In regions of contact, heat flow over the contacting interfaces takes place and due to slip frictional work is converted into heat. The contacting interface can be such that ideal heat conduction takes place, meaning that the temperature fields on both sides of the interface are the same, or it can be such that some hypothetical medium conducts heat between the two sides of the interface and the properties of this medium are determined

Main Index


c

by a one-dimensional heat flow law. The different contact regions are denoted as follows:  represents all regions where contact takes place, 

st ic k

denotes the sticking region, 

sl ip

denotes the slipping

cond

fl ow

region,  denotes the region where ideal heat conduction takes place over the interface and  denotes the region where the heat flow over the interface is controlled by some one-dimensional heat flow law. Note that these different regions are not static, but are all subject to change during the deformation process.

For the equation of motion the following expression for its weak form, augmented with terms emerging from contact, is obtained:

V  u·· i u i +  ij  i j  dV – V f i u i dV – 





n



c

  pu  d –





t   t  u   d st ick

–





p u d p i i

–

m ax t t   u   d sli p 

(2-43) = 0

This expression is the well-known virtual work equation including inertia terms and augmented with additonal contact constraint terms. Here u i are the virtual displacement components,   ...  is the first variation of the term within the parenthesis and  ij is the virtual strain w.r.t the current configuration: u 1 u  ij = ---  -----------i + -----------j 2  x j x i 

(2-44)

Note that this last term is not the first variation of some finite strain quantity. The first term in the first volume integral represents the intertia of the system. The second term in this volume integral represents the internal force contributions to the system resulting from nonlinear material behaviour, internal material damping and thermal effects like thermal expansion and temperature dependent material p

properties. The second volume integral and the surface integral over  represent the external forces c

acting on the system. The surface integral over  represents the non-penetration contact constraint, n

where p is the unknown contact pressure and u is the difference in normal displacements on both sides of the interface. The surface integral over 

st ic k

represents the sticking constraint, where t  is the

t

unknown tangentional stress and u  is the difference in tangential displacements on both sides of the interface. These two integrals represent the “hard” mechanical contact conditions, where the displacement fields are made identical on both sides of the interface. The surface integral over  m ax

accounts for the slipping condition, where t  Coulomb’s law of friction.

Main Index

sl ip

is the friction stress limit, which is often determined by


For the energy equation the following expression for ist weak form, augmented with terms emerging from contact, is obtained: 

·

 i j e

T T

- d –  ij d ij T +  ij ------- --------- dV –  V   cT – T -------- x i x j  T i j





cond

  gT  d –

p





f lo w

h  T  d –







q

q T d  –

max · t av t u  T d sl ip 

(2-45) = 0

Here T is the virtual temperature and   ...  is again the first variation of the term within the parenthesis. The first term in the volume integral represents the heat capacity of the system. The second term represents the thermo-elastic effects. The third term represents the heat as a result of the irreversible deformation process. The fourth term represents the thermal conductivity of the system. The surface q

integral over  represents the external heat flux into or out of the system, which may be from direct heat sources or from convective boundary conditions. The surface integral over 

cond

represents the

ideal heat conduction constraint, where g is the unknown heat flux over the interface and T is the difference in temperatures on both sides of the interface. This integral represents the “hard” thermal contact conditions, where the temperature fields are made identical on both sides of the interface. The fl ow

surface integral over  represents the heat flow over the interface through some hypothetical medium, where h is a linear or nonlinear heat flow law depending on the difference in temperatures on both sides of the interface. The surface integral over 

sl ip

represents the heat as a result of friction,

t av where u·  is the relative tangential velocity in the interface and T is the average of the virtual temperatures on both sides of the interface.

Equations (2-43) and (2-45) form the basis to arrive at the finite element equations for the unknown temperatures and displacements. Making suitable assumptions for the spatial distributions of the temperature and displacement fields the following strongly coupled system of equations is obtained for the mechanical, (2-46), and thermal, (2-47), problem: int ex t sl ip Mu·· + F (u,T) – F  u  – F (u,T) = 0 ˜ ˜ ˜ ˜ ˜ ˜ ˜ ˜ ˜ p C  T T· + K  T T – E  u T T – Q  u T  – ˜ ˜ ˜ ˜ ˜ ˜ ˜ ˜ q fl ow slip Q  u T  – Q  u T  – Q  u T  = 0 ˜ ˜ ˜ ˜ ˜ ˜ ˜ ˜

(2-46)

(2-47)

Here u and u·· are the vectors of unknown displacements and accellerations and T and T· are the vectors ˜ ˜ ˜ ˜ of unknown temperatures and their time derivatives. In equation (2-46) M is the mass matrix of the

Main Index


int

system, F is the internal force vector accounting for nonlinear and temperature dependent material ˜ e xt behaviour, geometric nonlinearities, and thermal expansion, F is the external force vector, possibly ˜ s lip accounting for follower force effects and F is the external force vector resulting from slipping ˜ friction, where the friction properties may be temperature dependent. Force contributions due to internal and external damping, i.e. velocity dependent terms, could also be present, but this has not been made explicit in equation (2-46). In summary, thermal effects enter the mechanical problem through temperature dependent material properties, temperature dependent friction properties and thermal expansion. In equation (2-47) C is the temperature dependent heat capacity matrix, K is the temperature p

dependent conductivity matrix, E is the matrix accounting for thermo-elastic effects, Q is the heat flux ˜ q vector accounting for plastic work conversion, Q is the heat flux vector accounting for external heat ˜ fl ow sli p sources, Q is the heat flux vector accounting for heat flow over contact interfaces and Q is the ˜ ˜ heat flux vector accounting for frictional work conversion. Heat transfer due to radiation could also be present, but this has not been made explicit in equation (2-47). In summary, mechanical effects enter the thermal problem through geometry changes, plastic and frictional work to heat conversions, thermoelastic effects and heat flow over contacting interfaces. The hard contact constraints get incorporated in these equations by splitting the vectors with displacement and temperature degrees of freedom in two parts, a part with the dependent and a part with the independent degrees of freedom. The dependent degrees of freedom are related to the independent ones through the hard contact constraint relations of the mechanical or thermal problem and they can be condensed out of the global system of eqautions. Equations (2-46) and (2-47) represent an extremely nonlinear set of coupled equations and this set can only be solved in an incremental fashion through an iterative process like the Newton-Raphsen process. In order to carry out this process suitable linearizations have to be made of all the terms in these equations. Since vectors in the mechanical problem have a temperature dependence and vectors in the thermal problem have a displacement dependence a number of cross-coupling matrix terms will appear in the global system matrix. The computation of all these terms is very expensive and they also result in a nonsymmetric system matrix making its solution very expensive. Displacements are usually measured in meters and in many applications are of the order 10 2

–2

or less, whereas temperatures are usually 3

measured in Kelvin or Celsius and are of the order 10 or 10 , so the order of magnitude of the degrees of freedom of the mechanical and the thermal problem may differ substantially making the equations numerically very sensitive. The following assumtions are made to simplify the structure of the equations without loss of much accuracy. It is assumed that the temperature field is constant in the mechanical set of equations and the displacement field is constant in the thermal set of equations. This completely eliminates all cross-coupling terms in the system matrix and completely decouples the thermal and the mechanical problem resulting in a weakly coupled set of equations that has to be solved in a staggered way. First a solution is obtained for the thermal problem, while the deformations are held constant. Then a solution is obtained for the mechanical problem, while the updated temperatures are held constant. With these new displacements the next thermal increment is solved on the updated geometry and this procedure is repeated over and over again. This procedure is, of course, only justified if the incremental changes for each phase are relatively small, but this is not a real limitation, since the incremental Newton-

Main Index


Raphson process already requires this. Since the mechanical behaviour is assumed to be constant during the thermal phase, the effects of mechanical work being converted to heat only result in additional contributions to the external heat flux vector of the thermal problem, namely one for the plastic work and one for the frictional work. In practice not all mechanical work is converted to heat and conversion factors are introduced to account for this. Thermo-elastic effects are usually very small and are disregarded in most practical applications. Conversely, since the thermal behaviour is assumed to be constant during the mechanical phase, the effects of temperature dependent material properties and thermal expansion result in additional contributions to the external force vector of the mechanical problem. For many practical applications it is not necessary to include inertia effects. The decoupled sets of equations eliminate the numerical sensitivity and the resulting equations for the thermal and mechanical problems often remain symmetric, so these simplifications greatly reduce the computational cost of the coupled analysis without sacrificing too much accuracy. With all these assumptions, the staggered solution process of the weakly coupled set of incremental eqautions for the quasi-static problem (i.e. no inertia) can be summarized as follows: start of weakly coupled thermo-mechanical analysis u = u ˜ ˜

0

T = T ˜ ˜ repeat

0

start of thermal phase n = 0 n

T = T ˜ ˜ repeat n = n+1 n–1

n

Q

HT  u T = R  T ˜ ˜ ˜ ˜ ˜ n n–1 n + T T = T ˜ ˜ ˜ until converged n

T = T ˜ ˜ end of thermal phase start of mechanical phase n = 0 u ˜ Main Index

n

= u ˜

n–1

 u ˜


repeat n = n+1 n–1

n

F

KT  u T = R  T ˜ ˜ ˜ ˜ n n–1 n + u u = u ˜ ˜ ˜ until converged u = u

n–1

 u ˜

n

end of mechanical phase until finished end of weakly coupled thermo-mechanical analysis The barred quantities denote they are constant during the particular solution phase, i.e. u is constant ˜ during the thermal phase and T is constant during the mechanical phase. H is the system matrix of the ˜ Q thermal problem and R is the flux vector including residual terms from the iteration process, flux terms ˜ from the external heat sources and flux terms from mechanical work conversions and contact. K is the F

system matrix of the mechanical problem and R is the force vector including residual terms from the ˜ iteration process, force terms from the external loads and force terms from thermal expansion, temperature dependent material properties and friction.

An Example: Metal Plasticity As an example of the general theory discussed in A Short Overview Of The Basic Equations Of Continuum Thermo-mechanics. It is applied to the case of metal plasticity, which is probably one of the most important application areas of the theory. It is assumed that the material is isotropic and that all deformations and strains remain small. Two aspects need to be made specific. The free energy function needs to be defined and the relations describing the plastic deformations need to be defined. The assumption of small strains reduces the multiplicative decomposition of the deformation gradient as given in (2-4) to an additive decomposition of the total strain into an elastic and plastic part. The deformation gradients appearing in (2-4) are written as F i j =  ij +  i j e

e

p

p

F i j =  ij +  i j F i j =  ij +  i j

Main Index

(2-48)


e

where all the  ij terms (total, elastic and plastic) are all very small w.r.t. unity, i.e.  ij « 1 ,  ij « 1 p

and  ij « 1 . The total deformation gradient therefore can be approximated by e

p

F i j   ij +  ij +  ij ,

(2-49)

where the products of strain terms are ignored, so the additive decomposition of the total strain into an elastic and a plastic part is obtained: e

p

 ij =  ij +  ij

(2-50)

The Green-Lagrange total strain tensor, E i j , is defined from the deformation gradient as follows: 1 1 E i j = ---  F ki F k j –  ij  = ---  U i k U k j –  ij    ij 2 2

(2-51)

It thus serves as a good approximation for the strain tensor  ij and the same holds for the elastic and plastic parts of the strain. With the assumption of isotropic material behaviour the free energy, f, as a function of absolute e

temperture, T, and elastic strain, E i j can be represented by the following expression: 2 T T 1 T- – 1 ---- 0 f =  0 cT 0  ----– - ln  ------  – --- K    T – T 0   + T    T T 2 0 0 0 2 1 --- K  I 1 –   T – T 0   + 2GI 2 2

(2-52)

I1 and I2 are the first and second invariants of the elastic strain tensor defined as: e

I 1 = E ii , 1 e e I 2 = --- e ij e i j 2

(2-53)

where e e 1 e ij = E i j – --- I 1  ij 3

(2-54)

is the deviatoric part of the elastic strain tensor. T0 and 0 are the initial temperature and density of the reference configuration. K, G,  and c are the familiar material constants, K is the bulk modulus, G is the shear modulus,  is the coefficient of thermal expansion and c is the heat capacity of the material. In absence of thermal effects, the last two terms in (2-52) together are recognized as the elastic strain energy

Main Index


function per unit undeformed volume for a linear elastic material. With presence of thermal effects, the elastic strains should actually be understood as recoverable strains, since they also may include contributions from thermal expansion. With equations (2-52) the stresses and entropy are found from equations (2-30) and (2-31) as: e e f f  i j =  ---------- F ik F jl   0 ---------- = e e E kl E ij T T

(2-55) e

K  I 1 –   T – T 0   ij + 2Ge ij K T fs = – ----= c ln  ------ + -------- I 1   0 T T e 0 E

(2-56)

ij

For plasticity the stress state is limited by a yield surface, where a stress state inside the yield surface is elastic and a stress state outside the yield surface is unreachable. The yield surface is a function,  , of stress and temperature and for many metals can accurately be described by the von Mises yield function. 2

 =    T  = J 2 –  v  T 

(2-57)

1 J 2 = --- s i j s ij 2

(2-58)

1 s i j =  ij – ---  k k  i j 3

(2-59)

where

with

as the deviatoric part of ij and  v is the yield stress in shear of the material as a function of temperature. The criteria for the stress state are: · Elastic when   0 or  = 0 and   0 · Plastic when  = 0 and  = 0 When plastic flow takes place the stress state remains on the yield surface and the resulting rate of plastic deformation is given by a flow rule. For associative plasticity this flow rule states that the plastic deformation rates are normal to the yield surface in the stress point. This type of flow rule accurately describes the plastic flow of many metals. In addition there can be so-called hardening rules, that describe the change of the yield surface as a function of the plastic deformation, but for brevity this will not be considered here. The plastic deformation rate given by the flow rule is:

Main Index


p  E· i j =  --------- ij

(2-60)

where  is a yet unknown proportionality factor called the plastic multiplier, which is set to zero when the stress state is elastic. The value of this multiplier is determined by the condition that during plastic flow the stress state remains on the yield surface:  ·  ·  = ----------  ij + ------ T· = 0 T  ij

(2-61)

The stress rate in this expression is given as: 2

2

e  f  f ·  ij =  0 --------------------- E· kl +  0 ---------------- T· e e e E ij E k l E i j  T

(2-62)

Employing the fact that e  E· i j = E· i j –  ---------- ,  ij

(2-63)

the plastic multiplier can be solved as: 2

2

   f  f  - · ---------- --------------------- E· k l +  ---------- ---------------- + ----T e   ij E e E e   T  ij E ij T ij kl  = --------------------------------------------------------------------------------------------------2  f   ------------ ------------------------ ---------- a b E e E e  cd ab

(2-64)

cd

The stress rate can now be written as: ·  ij = L ij kl E· kl + H ij T·

(2-65)

where 2

2

 f  f   ---------------------- ------------ ----------- ---------------------e e e e     2 E ij E p q p q r s E rs E k l  f L i jk l =  --------------------- – ----------------------------------------------------------------------e e 2 E i j E kl   f  ------------ ------------------------ ---------- a b E e E e  cd ab

and

Main Index

cd

(2-66)


2 2     f  f  ---------------------- ------------  ----------- ----------------- + ----- e e e  p q   rs E T T 2 E   E  f ij pq rs H i j =  ---------------- – ------------------------------------------------------------------------------------e 2 E i j T  f   ------------ ------------------------ ---------- a b E e E e  cd ab

(2-67)

cd

For large strains and deformations the usual assumption is that the elastic strains remain very small, but the plastic strains can be large. In this case the changes of the geometry must also be considered. Similar expression as for the small strain case are obtained, but they must be given in terms of objective stress and strain rates.

References 1. J.F. Besseling and E. van der Giessen, Mathematical modelling of inelastic deformation, Chapman & Hall, 1993. 2. H. Ziegler, An introduction to thermomechanics, North-Holland publishing company, 1983. 3. Y.C. Fung, Foundations of solid mechanics, Prentice-Hall Inc., 1965. 4. E.H. Lee,”Elastic-plastic deformation at finite strains”, J. Appl. Mech., 36, 1-6, 1969.

Main Index

Ap. C: Thermal Contact Theory MD Nastran 2010 Release Guide

C

Thermal Contact Theory



Main Index

Thermal Contact Theory

452 MD Nastran 2010 Release Guide Thermal Contact Theory

Thermal Contact Theory Introduction In thermal contact a distinction is made between hard contact glued, hard contact convective and near contact. Hard contact glued means that two bodies contact each other mechanically and the temperature fields on both sides of the interface must be made identical. Hard contact convective means that two bodies contact each other mechanically, but the heat flow between the two sides of the interface is through some hypothetical medium, so the temperatures on both sides do not have to be identical. The heat flow through this hypothetical medium is controlled by a one-dimensional linear heat flow law. Near contact means that two bodies are not in contact mechanically, but are close enough to exchange heat. The heat flow between the two interfaces is controlled by a linear or nonlinear one-dimensional heat flow law, so it is assumed that the bodies are already relatively close to each other as compared to their sizes. Two types of bodies are considered in a thermal contact analysis, meshed bodies and rigid bodies. Meshed bodies are defined by finite elements and can conduct heat, so they can have a nonuniform temperature distribution. Meshed bodies can also exchange heat with an environment in regions that are not contacting other bodies. Various convective heat transfer laws are possible. Rigid bodies are defined by geometrical entities and have a constant temperature everywhere. Rigid bodies can have a heat capacity, in which case they can exchange heat with meshed bodies or they have a prescribed temperature, so they act as a heat source when contacted by meshed bodies. When a meshed body contacts another meshed body, the grids of the slave (or touching) body touch entities of a master (or touched) body. These entities are element edges in two-dimensional analysis, like plane strain or axisymmetric analysis or they are element faces in three-dimensional analysis. In either case each constraint relation controlling the heat transfer is between one slave grid and a set of master grids of the touched entity. When a meshed body contacts a rigid body the grids of the slave body touch geometric entities of the master body. These geometric entities all have the same temperature and each constraint relation is between one slave grid and the rigid body having the constant temperature. In the next sections the equations are discussed that describe the different kinds of thermal interactions when meshed bodies contact other meshed bodies or when they contact rigid bodies.

Mesh to Mesh Contact Mesh to Mesh Hard Contact Glued In this case a grid is in contact with a face of an element. The contact condition becomes a MPC condition. If the contacting grid temperature is T A and the face grid temperatures are T B , the condition i

is a simple linear MPC: N

T A = T B     =

 i = 1

Main Index

 i    T B

i

(3-1)

Appendix C 453 Thermal Contact Theory

TA

is the dependent grid, T B are the independent grids. The weight factors  i depend on the location i

where the T A grid touches the face and are simply the shape function values to interpolate the temperatures inside the face. This may be written as TA TA T B  

=

TB

1 0  0 0 1  N

1

. TB

= ST

(3-2)

N

The MPC equation can alternatively be expressed as: TA 1 –1  –N

TB

1

. TB

T

= HM P C  T = 0

(3-3)

N

Mesh to Mesh Convective Heat Transfer (Hard or Near Contact) In this case the heat flow between two bodies is controlled by a one-dimensional heat flow law. The heat leaving body A is: Q A =   q =   h   T A – T B     

(3-4)

where  is the area contribution for grid A, q the heat flow per unit area and h is the heat transfer coefficient, which may be composed of several contributions. The heat entering body B is Q B = – Q A . For each grid that is in contact with a master face, a conductive heat transfer element matrix gets created of the following form: T

Kc o n t a c t =   h  S 

1 –1  S , –1 1

(3-5)

TA

where the element dof vector is:

TB

1

. TB

N

This can be interpreted as a one dimensional heat link with one grid being grid A and its other grid B being on the touching element face, so its temperature is computed from the face grid temperatures by the linear MPC equation.

Main Index


The heat transfer coefficient h can have several contributions, coming from different heat flow types: q 1 = h 1  T A – T B      q 2 = h 2  T A – T B      2

(3-6) EXPF

 T A – T B     

2

q 3 =   T A + T B       T A + T B       T A – T B      EX P F

(3-8)

E X PF

 TA – T B      q 4 = h 4 ----------------------------------------------------------------  T A – T B       T – T      A

(3-7)

(3-9)

B

d d q 5 = h 5 A  1 – ------------- + h 5 B -------------  T A – T B       dn e a r d n e a r

(3-10)

Equation (3-6) is just a linear heat flow law with a constant heat transfer coefficient. Equations (3-7), (3-8) and (3-9) represent some nonlinear heat flow laws, where Equation (3-8) is a radiation law. Equation (3-10) allows to have a distance dependent heat flow between the two bodies in case of near contact, where dnear is the near contact distance tolerance. When bodies are separated by a distance larger than dnear, they are not in contact. The total flux per unit area is the sum of these contributions: 5

q =



qi

(3-11)

i = 1

For hard convective contact only the first flux type is used. For near contact it may be a combination of all five. All relations are of the form: q = h  T A  T B        T A – T B     

(3-12)

where the heat transfer coefficient is some nonlinear function of the body temperatures in the contact point. Note that for the radiative condition  q 3  the temperatures should always be absolute temperatures.

Mesh to Geometry Contact Mesh to Geometry Hard Contact Glued A grid of the meshed body is contacting a rigid surface. In this case the grid temperature is set equal to the rigid geometry temperature. This can be done in two ways: As a SPCD condition: T A = T BODY As a MPC condition: T A – T BODY = 0

Main Index


In the latter case an extra scalar point for the rigid contact body is created, which may obtain either a prescribed temperature or it may be loaded with an external flux. A simple MPC between this scalar point and each grid that contacts the rigid body is created. With this extra scalar point it is possible to associate a total heat capacity C MB (S.I. units: J/K) of the rigid body, which simply represents a lumped heat capacity contribution to the scalar point. Mesh to Geometry Convective Heat Transfer (Hard or Near Contact) This situation is similar to the mesh-to-mesh case, but the temperature T B is the everywhere constant temperature of the rigid geometry, T BODY . The film condition at grid A is: Q A =   h   T A – T B OD Y 

(3-13)

Again two ways are distinguished as discussed in Mesh to Geometry Hard Contact Glued: 1. The body temperature is applied directly. In this case a concentrated conductivity matrix term: K contact =   h  T A and a load term Q co ntact =   h  T BODY for grid A are obtained. 2. An extra scalar point is created. In this case a simple conductivity matrix arises: Kc o n t a c t =   h 

1 – 1  and the element dof is: T = –1 1

TA T B OD Y

(3-14)

This latter relation is similar to the one in Mesh to Mesh Convective Heat Transfer (Hard or Near Contact), but now their is only one master degree of freedom, which is the temperature of the scalar point associated with the rigid body.

No Contact A face of a meshed body not being contacted or only partially being contacted may exchange heat with its environment according to similar laws as the first four in Mesh to Mesh Convective Heat Transfer (Hard or Near Contact), but the temperature T B is replaced by an ambient temperature T AMB , which is the same for all faces of a contact body and T A now represents the surface temperature. The flux per unit are is: q =   h   T A – T AM B  ,

(3-15)

where  is an area contribution factor for the face  0    1  . The total contribution is determined by the integration over the element face (this is similar to an elastic foundation in mechanical terms): Q f ilm =  A

Main Index

 fac e

T

h     T A – T A M B dA = H A  T A – Q AM B

(3-16)


where  is the vector of shape functions that interpolate the temperatures inside the element face. From above expression a conductivity matrix contribution and a load vector contribution arise. The conductivity matrix is: HA =  A

T



h   dA

(3-17)

face

The load vector is: QA M B = 



hT AM B  dA

(3-18)

A fac e

Treatment of MPC Equations The MPC equations that can arise as a result of the contact conditions are imposed with the help of Lagrange multipliers. This is relatively easy, since the heat transfer MPC equations are all linear of the form: TA gT =

1 –1  –N

TB

. .. . TB

1

T

= HM P C  T = 0

(3-19)

N

For each MPC constraint an additional Lagrange multiplier dof is created. The constraint is furthermore augmented with a penalty term. The system matrix contribution for this constraint becomes: T

T

pH M P C H M P C H M P C , T HM P C 0

KM P C =

(3-20)

where p is the penalty factor used in the constraint. The associated incremental dof’s are: dT , d where  is the Lagrange multiplier dof. The residual vector contribution for this constraint becomes: RM P C =

Main Index

–   + pg H M P C –g

(3-21)


When a grid touches a rigid body that has no scalar point associated with it, the SPCD-like constraint is simulated by a simple MPC equation with a non-homogeneous term  C non  . In this MPC there are no independent grids. g = T A – T B O DY = 0

(3-22)

The iteration process repeatedly solves for: dT A = – g = –  T A – T B O DY  = C n o n

(3-23)

and H M P C is the trivial unit vector with one component, so computing K M P C and R M P C becomes almost trivial.

Mechanical Coupling Frictional heat The heat generated by sliding friction in the contact interfaces gets evenly distributed over the two bodies that contact each other and can be expressed as: 1 Q A = Q B = ---  F w   rel , 2

(3-24)

where F w is the magnitude of the friction force at grid A and  rel is the magnitude of the relative velocity between the two bodies at grid A. Q A can be applied directly as a concentrated heat flux to the contacting grid. Q B is distributed over the grids of the master face being contacted: Q B =  i      Q B The i

scale factor  may be used to accommodate different unit systems in the heat transfer and mechanical analysis or to accommodate a loss to the environment, in which case not all heat generated is available as a loading heat source.

Main Index


Main Index

MD Nastran 2010 Release Guide

Recommend Documents