Mech UCO Lect 06 Using APDL 1

Chapter 6 Using APDL in Mechanical 1

ANSYS Mechanical Advanced ((Using g Command Objects) j ) ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.

6-1

June 2009 Inventory #002669

Using APDL in Mechanical 1

Overview

Training Manual

• Using an understanding of Mechanical APDL acquired from the previous chapters, this section will demonstrate how to use APDL commands to access advanced functionality within Mechanical. • Consider the APDL commands as a scripting language to: – Manipulate the mesh directly – Access advanced solver functionality – Access advanced postprocessing capabilities

• In this chapter, using “Commands” Commands objects in the Geometry, Remote Points, and Connections branches will be explored.

ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.

6-2



A. Preliminaries

Training Manual

• Before diving into the details of using “Commands” objects in Mechanical, some general topics will be reviewed: – – – –

Solver unit system Saving the Mechanical APDL database Creating/deleting elements and other entities Branches in the Outline Tree applicable to “Commands” objects


6-3



… Unit System

Training Manual

• APDL commands may involve the input of values that are unitdependent, such as piezoelectric coefficients. Because “Commands” objects are general, there is no mechanism to convert entered arguments off APDL commands iff a user decides to change the active unit system from the “Units” menu. • Consequently, it is strongly recommended to manually specify the solver l unit i system in i the h Details D il view i off the h “Analysis “A l i Settings” S i ” branch. “Solver Units: Manual” allows the user to specify the unit system for the Mechanical APDL solver – B By setting tti “S “Solver l U Units: it Manual” M l” with ith “Solver “S l Unit System” set appropriately, the user-specified unit system will always by used by the Mechanical APDL solver,, regardless g of what the active unit system is in Mechanical – This ensures that, if another user obtains the Workbench project, their solution will be in the correct unit i system ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.

6-4



… Saving the Mechanical APDL database

Training Manual

• Mechanical uses the file.rst result file for postprocessing. Most postprocessing operations can be done in Mechanical using User Results, dicussed later. However, there may be unforeseen circumstances where a user may wish to postprocess results in Mechanical APDL – Postprocessing in Mechanical APDL was covered in an earlier chapter

• Because of this reason, it is highly recommended to save the Mechanical APDL database (file.db). – In the Details view of the “Analysis Settings” b branch, h sett “Save “S ANSYS db db: Y Yes” ” – The default is not to save file.db, so this must be specified by the user


6-5



… Creating/Deleting Elements

Training Manual

• When elements or nodes are created or deleting using APDL commands, please note that Mechanical will not be aware of these changes to the mesh. – If elements/nodes need to be created using APDL commands in a “Commands” branch, postprocessing of these elements must be done inside of Mechanical APDL – If possible, possible avoid deleting elements via APDL commands commands. Consider modifying the geometry/mesh to omit regions that are not of interest


6-6



… Inserting Commands Objects

Training Manual

• The following branches in the Outline tree allow users to insert “Commands” objects: – – – – – – – – –

Any Body under a “Geometry” branch Any Remote Point under a “Remote Points” branch Any Contact Region under “Connections” branch Any Spot Weld under “Connections” branch Any Joint under “Connections” branch Any Spring under “Connections” branch Any Beam under “Connections” branch Directly under any analysis branch Directly under the “Solution” branch

• The details of each of these options will be covered in this chapter


6-7



… Supplementary Branches

Training Manual

• Two branches that do not use “Commands” objects directly but are quite helpful are the “Coordinate Systems” and the “Named Selections” branches – As will be discussed later, a Coordinate System can be assigned a manual coordinate system ID number, which can be used in APDL commands. For example, this is useful for selecting a node near a coordinate system or transforming results in a particular coordinate system in Mechanical APDL. – Named Selections will appear pp as nodal or element components in Mechanical APDL, where a “component” is a “group” of nodes or elements. This allows users to conveniently reference entities without having to worry about geometry, geometry node/element ID number, etc., and this method can be used for updated geometry as well.


6-8



… Other Branches

Training Manual

• Other branches, such as “Construction Geometry”, “Virtual Topology”, “Symmetry”, “Mesh”, and “Solution Combination” branches, are not applicable to APDL commands, so “Commands” C objects are not inserted under those branches.


6-9



B. Geometry Branch

Training Manual

• A “Commands” object may be inserted under a Body under the “Geometry” branch – Note that a “Commands” object cannot be inserted directly under the “Geometry” branch or directly under a multibody part. It can only be inserted under a particular body – Point Masses are also not applicable for “Commands” Commands objects

• The below lists some reasons to use a “Commands” Commands object associated with a Body: – Definition of composite materials – Solving other types of physics not native to Mechanical – Adding nonlinear material models, such as creep or y or anisotropic p hyperelasticity yp y viscoelasticity


6-10



… Geometry Branch

Training Manual

• Once a “Commands” object is inserted, APDL commands can be pasted or typed into the text area. • The “Commands” object inserted under a Body can be used to change the following element attributes for that Body: – – – –

Element type Material Properties Real Constants/Section Properties Element Coordinate System

• Use the APDL p parameter MATID to reference the element type, yp material property, real constant, or section property ID number. – The Element Coordinate System ID will typically be “0” (default) unless a Coordinate System has been associated with that body


6-11



… Geometry Branch: Element Type

Training Manual

• As discussed in a previous chapter, changing element types is done via the following two commands: – ET,MATID,… – KEYOPT,MATID,…

• Changing the element type allows a user to solve different physics or use a specialized element. However, the nodal connectivity must be the same between the original and target element type – The “Mesh” branch controls whether the element will be higher- or lowerorder. The Mesh Method also dictates what the element shape will be ( (e.g., hexahedral, h h d l tetrahedral) t t h d l)

• If any element-specific options (“keyoptions”) need to be set, use the KEYOPT command


6-12




Training Manual

• Caution concerning pyramid elements: – Note that while most higher-order elements have a pyramid shape, not all lower-order elements have a pyramid shape. Hence, check the Elements R f Reference t ensure that to th t the th selected l t d element l t type t supports t pyramids. id For example, p the structural 8-node brick element SOLID185 does not show a pyramid form, so a user should not attempt to use this element if pyramids are present • Pyramids appear when a Mesh Method of “Hex-Dominant Meshing” or “MultiZone” (with Free Mesh Type set) is used used. • When pyramids are present, this also typically means that tetrahedrons are present as well. Mechanical will generate tetrahedrons as a 10-node tet while pyramids and wedges are degenerate 20-node hex elements. Hence, in these case, MATID will ill representt the th 10-node 10 d tet t t elements l t while hil MATID+1 1 will ill refer f to t the 20-node hex element type ID. ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.

6-13




Training Manual

• Note about Element Control: – In the Details view of the “Geometry” branch, the user can change “Element Control” • By default, this is set to “Program Controlled,” where the Mechanical APDL solver may change keyoptions automatically prior to solution • Currently y applicable pp to structural elements • APDL Command is ETCONTROL • See the Commands Reference for ETCONTROL for additional details


6-14




Training Manual

• Note about Element Control (continued): – During solution, the following will be printed in the “Solution Information” branch: • If automatic resetting of keyoptions is not desired, be sure to set “Element Control: Manual” in the Details view of the “Geometry” branch

Notice that certain keyoptions have been automatically reset by Mechanical APDL. Although Alth h the th automatic t ti setting tti off options is meant to aid the user in selecting appropriate element formulations, etc., the k knowledgeable l d bl user may nott wantt keyoptions automatically overridden. In this case, set “Element Control: Manual” prior t solution. to l ti


6-15



… Geometry Branch: Material Properties

Training Manual

• Deleting all existing material properties for the particular body is done via the following commands: – MPDELE,Label,MATID – TBDELE,Label,MATID

• As a review, defining linear elastic material properties: – MP,Label,MATID,… (constant materials) – MPTEMP,… and MPDATA,Label,MATID,… (temperature-dependent)

• To define nonlinear material properties, use: – TB,Label,MATID,… , , , to activate a p particular material table – TBTEMP,… and TBDATA,… or TBPT,… to define the parameters

• In all of the above cases cases, Label refers to the material property name name. See the MP or TB help in the Commands Reference for details.


6-16




Training Manual

• Material Properties are the only element attribute which allows superimposing multiple definitions. • For example, to define density and elastic modulus, one would repeat the MP command as follows: – MP,EX,MATID,10e6 – MP,DENS,MATID,0.1/386.1

• To define bilinear isotropic plasticity and creep, one would do the following: – – – – – –

MP,EX,MATID,200e3 MP,NUXY,MATID,0.3 TB,BISO,MATID,1 TBDATA,1,300,2e3 TB,CREEP,MATID,1,3,10 TBDATA,1,3.125E-14,5,0

Defines linear elastic properties Defines bilinear plasticity constants Defines creep law and its coefficients

• For o nonlinear o ea structural st uctu a material ate a co combinations, b at o s, see “Section Sect o 2.6 6 Material Model Combinations” in the Elements Reference for details ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.

6-17




Training Manual

• Points to keep in mind: – When adding creep material properties via TB,CREEP,MATID, note that Mechanical, by default, will not request creep strains to be saved. By adding ddi OUTRES,EPCR,ALL O S C i a “Commands” in “C d ” object bj t under d the th analysis l i branch (discussed later), one can ensure that creep strains are stored for postprocessing. (Note that, in the specific case of creep, RATE,ON must also be added in the “Commands” object j under the analysis y branch.)) – For user-defined materials with TB,USER,MATID or user-defined creep with TB,CREEP,MATID,,,100, state variables are often defined via TB,STATE,MATID. As with the above case, the user should add OUTRES,SVAR,ALL in i a “Commands” “C d ” object bj t under d the th analysis l i branch b h to t ensure that state variables are stored in the result file for postprocessing.


6-18



… Geometry Branch: Section Properties

Training Manual

• The Elements Reference in the Mechanical APDL help system describes whether a particular element uses real constants or section properties – In either case, the APDL scalar parameter MATID can be used to reference the real constant and section property ID number of that particular Body.

• Deleting existing real constants or section properties: – RDELE,MATID – SDELETE,MATID

• Recall the definition of a new real constant or section property: – R,ID,… – SECTYPE,ID,… and SECDATA,…

• Modification of a real constant: – RMODIF,ID,… – (No equivalent functionality is present for sections. One must delete an existing section and define a new section instead.)


6-19



… Geometry Branch: Section Properties

Training Manual

• Tip for composite (layered) elements: – Composite elements define the material properties for each layer via real constants or section properties. There is no need to redefine or modify th material the t i l ID number b associated i t d with ith the th Body. B d • Note, however, that structural damping (MP,DAMP) and reference temperature for thermal strains (MP,REFT) are defined via the material ID number, not per layer. y

– For composite elements, one must define the material ID numbers used in each layer within the Commands object • Use material ID numbers that are larger than the number of parts present when d fi i defining the th material t i l ID number b for f each h layer l • The actual material property definition used in layers only needs to be performed once in the event that multiple bodies have composite definition

– From the Workbench Project Schematic, link the “Model” Model to a “Mechanical APDL” system. Then, verify the composite definition inside of Mechanical APDL using /ESHAPE,1 to visualize the 3D cross-section, including layeres.


6-20



C. Remote Points

Training Manual

• Remote Points are an integral part of many features in Mechanical: – – – – – –

Point Mass Joints Springs Moment Remote Force Remote Displacement

• Each Remote Point has an ((x, y y, z)) location and is scoped to a geometric entity. One can think of Remote Points as “tying” nodes on a geometric entity to the remote point location, either with a ‘deformable’ or ‘rigid’ behavior. • Understanding how Remote Points work allows users to take advantage of them with “Commands” objects ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.

6-21



… Uses for Remote Points

Training Manual

• The below are some reasons why one may wish to use “Commands” objects with Remote Points: – Reduce the interface nodes for creation of CMS superelements for more efficient system-level analyses – Define monitor locations, such as the average deformation of a given surface – Create C t an MNF fil file ffor use with ith Ad Adams/Flex /Fl †

†

Adams is developed by and is a registered trademark of MSC Software


6-22



… Remote Point Representation

Training Manual

• A Remote Point consists of contact and target elements – The target element is a 1-node element, representing the remote point location – The contact elements are associated with the vertex, edge, or surface that is scoped in the Remote Point Definition – This is an example of surface-based constraints using contact elements. For details, details see Chapter 9 of the Contact Technology Guide Guide. TARGE170 Element (circled)

CONTA174 Elements (purple) ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.

6-23



… Remote Point Behavior

Training Manual

• To better understand the “deformable” and “rigid” behavior, consider the simple 2D plate with a remote force (via remote point) applied to the center hole: Deformable behavior: circle does not retain shape p

Rigid behavior: circle maintains shape ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.

6-24



… Remote Points

Training Manual

• Insert a “Commands” object under a Remote Point: – The parameter _npilot reflects the node ID number. One can define a new parameter to keep track of this node ID number for later use, such as d fi i defining master t DOF: DOF MY_INTERFACE_NODE = _npilot m,MY_INTERFACE_NODE,all

– The parameter TID is the target element’s element s element type ID number number. For example, if one may wish to constrain only UX and UY DOF rather than all 6 (or all 3, if 2D), one can use the following command: keyopt,TID,4,11


6-25



… Remote Points

Training Manual

• Tips on using APDL with Remote Points: – Keep in mind that APDL parameters are persistent throughout the Mechanical APDL run. Hence, per the previous slide, the parameter MY_INTERFACE_NODE C O will ill have h the th value l off the th node d ID number b and d can be used in postprocessing as well. – Most functionality with regards to Remote Points, such as load application postprocessing displacements or reaction forces, application, forces spring/joint definition, are already built into the Mechanical GUI. Hence, prior to using “Commands” objects with Remote Points, consider whether or not the sought capability already exists within Mechanical.


6-26



D. Contact Regions

Training Manual

• “Commands” objects may also be inserted under any Contact Region • There are many situations where APDL commands can access advanced controls: Definition of debonding/delamination with CZM Use of fluid pressure-penetration loading Near-field contact radiation and convection Definition of multiphysics contact (coupled thermal-electric-structural) with frictional heat generation ti – Inclusion of orthotropic friction or dynamic coefficient of friction, along with cohesion – Changing contact detection locations …other options available as well! – – – –


6-27



… Contact Regions

Training Manual

• Most of the commonly-used contact options are present in the Mechanical GUI. • However, ANSYS contact elements have a plethora of options to allow users to simulate many different scenarios • To understand the various contact capabilities p that are available,, refer to the following sections in the Help documentation: – Contact Technology Guide > Chapter 3: Surface-to-Surface Contact – Contact Technology gy Guide > Chapter p 7: Multiphysics p y Contact – Contact Technology Guide > Chapter 12: Debonding


6-28



… Contact Regions

Training Manual

• Insert a “Commands” object of the Contact Region of interest: – The parameters CID and TID are used to refer to the contact and target element type IDs, respectively. – To apply fluid pressure-penetration loading where pressure loading occurs when a contact status opens, use the following: esel,s,type,,CID sfe all 1 pres 120 sfe,all,1,pres,,120 allsel,all

– To change the contact detection type to “normal from target”, use keyopt,CID,4,2


6-29



… Contact Regions

Training Manual

• Tips on Contact Regions and APDL: – Because Contact Regions are not included in Named Selections, to reference a contact region for later use, use either of the following: • Define a parameter(s) with the CID (and TID) values • Create an element component (group) for later use via ESEL and CM commands

– Understand the situations where symmetric and asymmetric contact pairs exist exist. If “Behavior: Behavior: Symmetric” Symmetric is set for “Pure Pure Penalty” Penalty or “Augmented Lagrange” algorithms, ensure that any change real constants or material properties are reflected for both CID and TID.


6-30



E. Joints

Training Manual

• Typical uses of “Commands” objects inserted for Joints include the following: – Definition of Screw Joints and other joints not available in the Mechanical GUI – Incorporation of nonlinear stiffness, nonlinear damping, and/or Coulomb friction1 – Obtaining Obt i i more detailed d t il d control t l over joint j i t behavior, such as applying rotational stops and locks on a General Joint

Note that, at release 12.0, the hysteretic friction capability of Joints (MPC184) has been removed in favor of the Coulomb friction model.

1


6-31



… Joints

Training Manual

• Many sophisticated joint functionality are present in Mechanical: – Torsional stiffness and damping for Cylindrical and Revolute Joints – Bushing Joint, which can be thought of as a General Joint where a user may input stiffness and damping relationships between all 6 relative DOF – Joint stops and locks for many joint types

• Prior to implementing “Commands” objects for Joints, review the Help system to ensure that the capability is not already present: – “Mechanical (formerly Simulation) > Using the Mechanical Application Features > Geometry in the Mechanical Application > Joints”


6-32



… Joints

Training Manual

• If it is deemed necessary to include a “Commands” object to access functionality via APDL commands, review the following Help manual: – “Multibody Analysis Guide > Chapter 2. Modeling in a Multibody Simulation > Section 2.3 Connecting Multibody Components with Joint Elements” – “Elements Reference > Element Library > MPC184”

• The element type used for joints is MPC184. Note that the joint (MPC184 element) is connected to the solid model via Remote Points. – If the connection between the joint and solid part needs to be modified, define a Remote Point with a “Commands” object, as discussed in an earlier section of this chapter. – Only insert a “Commands” Commands object under a “Joint” Joint branch if the joint property will be modified. This includes constraining relative DOF, adding stops/locks, or defining joint “material properties”


6-33



… Joints

Training Manual

• The APDL parameter “_jid” refers to the element type, material, real constant, and section ID number of the MPC184 element: – To define nonlinear stiffness for a Translational Joint: tb,join,_JID,1,4,jnsa tbpt,,U1,F1 • …repeat (Each TBPT command defines pair of displacements Ui and forces Fi)

– T To add dd a rotational t ti l stop t for f relative l ti Z-rotation Z t ti for f a General G l Joint J i t between b t -45° and 45°: secstop,6,-acos(-1)/2,acos(-1)/2 • (Notice input is in radians, and “6” 6 refers to relative DOF 6 or ROTZ)


6-34



… Joints

Training Manual

• Tips on using APDL commands with Joints: – The SECTYPE command is required to define the joint behavior and is typically defined by Mechanical. Hence, to add stops/locks, one should nott use the th SECTYPE S C command d if it already l d defined d fi d by b Mechanical, M h i l but b t one can just add SECLOCK and SECSTOP commands, as the particular joint ID will already be “active”. – Not all Joints support stops stops, locks locks, and joint “material” material definition (friction, stiffness, damping) – for example, the Spherical Joint supports neither. Consult the Elements Reference for details on each Joint type prior to using APDL commands to ensure that the feature is available for that joint type – Modifying the local coordinate system which defines the orientation of the relative joint DOF is highly discouraged since Mechanical will incorrectly report results for that joint joint. – The DJ command applies joint constraints while the FJ command applies loading to the joints. However, when possible, use of “Joint Loads” in Mechanical is recommended over using g APDL commands,, as the former is much easier to implement. ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.

6-35



F. Springs and Beams

Training Manual

• In addition to Contact Regions and Joints, the “Connections” branch allows use of Springs and Beams – Springs are longitudinal springs and/or dampers with preload capabilities – Beams have circular cross-sections and are meant to represent structural connections that carry bending loads

• As with Joints, Springs and Beams are connected to 2D or 3D bodies via Remote Points – If a Remote Point is not explicitly used, the underlying finite element representation is still using surface-based constraints of contact and target elements, as elaborated in the Remote Points section of this chapter


6-36



… Springs and Beams

Training Manual

• A Spring is represented with a COMBIN14 element, and a Beam is modeled with a single BEAM188 element. – Line Bodies are also represented with BEAM188 elements, and the two should not be confused with each other. • When modeling beam structures, use line bodies (number of beam elements per line body is controlled via Mesh Sizing). • To model a connection that can carry bending loads, loads a Beam connection may be applicable.

• Using “Commands” objects for Springs and Beams is not as common as its usage g in other branches,, although g a few reasons for doing so are listed below: – Changing the longitudinal Spring to a torsional one via keyoption – Replacing the Beam with a rigid beam (MPC184) – Replacing the Spring with nonlinear or other types of spring elements


6-37




Training Manual

• For Springs, after inserting a “Commands” object, use the parameter _sid to reference the spring’s element type, material, and real constant ID number – Example of changing to a torsional spring: keyopt,_SID,3,1 – Note that ‘stiffness’ and ‘force’ will refer to ‘torsional stiffness’ and ‘moment’ – Springs do not use a section ID, so the section ID number will be “1”

• For Beams, the parameter _bid refers to the beam’s element type, material, real constant, and section ID number – To replace the deformable beam with a rigid one, use the following: mpdele,all,_BID et,_BID,184,1,0 – Note that the Beam has material properties, so density and thermal expansion may be used, if present. To prevent these materials from being used, used MPDELE is included in the above example to delete the material definition for _BID (beam’s material ID). ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved.

6-38




Training Manual

• 1D springs may be required for an analysis, where the stiffness in a particular direction is known beforehand. – 1D springs should be modeled with COMBIN14 and KEYOPT(2)=1 through 6. The best practice is to model 1D springs with coincident nodes. – Because Springs in Mechanical are longitudinal springs, they must have finite length. Hence, Springs should not be converted to 1D springs. – To T create t 1D springs i b between t bodies, b di define d fi 2 Remote R t Points P i t att the th same location but scoped to the 2 bodies’ geometric entities. Add “Commands” objects under both Remote Points to record the pilot node parameters. Using g “Commands” object j in the analysis y ID number as p branch (described shortly), 1D spring(s) can be defined using the two pilot node locations. – Springs operate in the nodal coordinate system. Hence, if Remote Points are used, d ensure that th t the th referenced f d coordinate di t systems t are the th same.


6-39


Mech UCO Lect 06 Using APDL 1

Recommend Documents