Unioni bullonate con Abaqus

ABAQUS: Selected Topics


University of Sydney 28 Feb 2006 – 02 Mar 2006 Copyright 2005 ABAQUS, Inc.


2

Day 1 • Lecture 1

Overview of ABAQUS

– Workshop 1 • Lecture 2

Introduction to Non-linear Analysis

– Workshop 2 • Lecture 3

Linear Static Analysis of Cantilever Beam Non-linear Analysis of Skew Plate

Materials – Metal

– Workshop 3a

Plasticity and Hardening – 2D Cantilever Beam

– Workshop 3b

Skew Plate with Plasticity

• Lecture 4

Materials – Concrete

– Workshop 4

Copyright 2006 ABAQUS, Inc.

Collapse of a Concrete Slab


3

Day 2 • Lecture 5

Eigenvalue Buckling Analysis

– Workshop 5a

Cargo Crane – Critical Load Estimation

– Workshop 5b

Eigenvalue Buckling of a Square Tube

• Lecture 6

Static Post-buckling Analysis

– Workshop 6a

Cargo Crane – Riks Analysis

– Workshop 6b

Buckling of a Square Tube with Imperfections

• Lecture 7

Damped Static Post-buckling Analysis

– Workshop 7a

Cargo Crane – Stabilized Static Analysis

– Workshop 7b

Cargo Crane – Dynamic Analysis



4

Day 3 • Lecture 8

Introduction to Contact Modeling

– Workshop 8a

Hinge Model

– Workshop 8b

Clip and Plate Model

• Lecture 9

Bolted Connection Modeling

– Workshop 9a

Pump Model – Bolt Loading

– Workshop 9b

Beam-Column Connection with Fasteners

• Lecture 10

Including Initial Stresses (Optional)

• Question Session



Legal Notices The information in this document is subject to change without notice and should not be construed as a commitment by ABAQUS, Inc. ABAQUS, Inc., assumes no responsibility for any errors that may appear in this document. The software described in this document is furnished under license and may be used or copied only in accordance with the terms of such license. No part of this document may be reproduced in any form or distributed in any way without prior written agreement with ABAQUS, Inc. Copyright  ABAQUS, Inc., 2005. Printed in U.S.A. All Rights Reserved. ABAQUS is a registered trademark of ABAQUS, Inc. The following are trademarks of ABAQUS, Inc.: ABAQUS/Aqua; ABAQUS/CAE; ABAQUS/Design; ABAQUS/Explicit; ABAQUS/Foundation; ABAQUS/Standard; ABAQUS/Viewer; ABAQUS Interface for MOLDFLOW; ABAQUS Interface for MSC.ADAMS; and the ABAQUS, Inc., logo. All other brand or product names are trademarks or registered trademarks of their respective companies or organizations.


5


Lecture 1

Overview of ABAQUS



Overview • Introduction • Components of an ABAQUS Model • Structure of an ABAQUS Input File • ABAQUS Conventions • Workshop 1: Linear Static Analysis of a Cantilever Beam


L1.2


What is ABAQUS?



Introduction ABAQUS is a suite of finite element analysis modules


L1.4


L1.5

Introduction • The heart of ABAQUS are the analysis modules, ABAQUS/Standard and ABAQUS/Explicit, which are complementary and integrated analysis tools. – ABAQUS/Standard is a general-purpose, finite element module. • It provides a large number of capabilities for analyzing many different types of problems, including many nonstructural applications. – ABAQUS/Explicit is an explicit dynamics finite element module. – ABAQUS/CAE incorporates the analysis modules into a Complete ABAQUS Environment for modeling, managing, and monitoring ABAQUS analyses and visualizing results.



L1.6

Introduction • ABAQUS/CAE – Complete ABAQUS Environment for modeling, managing, and monitoring ABAQUS analyses, as well as visualizing results. – Intuitive and consistent user interface throughout the system. – Based on the concepts of parts and assemblies of part instances, which are common to many CAD systems. – Parts can be created within ABAQUS/CAE or imported from other systems as geometry (to be meshed in ABAQUS/CAE) or as meshes. – Built-in feature-based parametric modeling system for creating parts. Copyright 2004 ABAQUS, Inc.

ABAQUS/CAE main user interface


L1.7

Introduction • Solver modules – ABAQUS/Standard and ABAQUS/Explicit provide the user with two complementary analysis tools. ABAQUS/Standard’s capabilities: – General analyses • Static stress/displacement analysis: – Rate-independent response – Rate-dependent (viscoelastic/creep/viscoplastic) response • Transient dynamic stress/displacement analysis • Transient or steady-state heat transfer analysis • Transient or steady-state mass diffusion analysis



Introduction • Steady-state transport analysis • Coupled problems: – Thermo-mechanical (sequentially or fully coupled) – Thermo-electrical – Pore fluid flow-mechanical – Stress-mass diffusion (sequentially coupled) – Piezoelectric (linear only) – Acoustic-mechanical


L1.8


L1.9

Introduction – Linear perturbation analyses • Static stress/displacement analysis: – Linear static stress/displacement analysis – Eigenvalue buckling load prediction • Dynamic stress/displacement analysis: – Determination of natural modes and frequencies – Transient response via modal superposition – Steady-state response resulting from harmonic loading • Includes alternative “subspace projection” method for efficient analysis of large models with frequency-dependent properties (like damping) – Response spectrum analysis – Dynamic response resulting from random loading



L1.10

Introduction ABAQUS/Explicit’s capabilities: – Explicit dynamic response with or without adiabatic heating effects – Fully coupled thermo-mechanical analysis – Structural-acoustic analysis – Annealing for multistep forming simulations – Automatic adaptive meshing allows the robust solution of highly nonlinear problems



L1.11

Introduction Comparing ABAQUS/Standard and ABAQUS/Explicit – ABAQUS/Standard • A general-purpose finite element program. • Can solve for true static equilibrium in structural simulations. • Provides a large number of capabilities for analyzing many different types of problems, including many nonstructural applications.



L1.12

Introduction – ABAQUS/Explicit • Solution procedure does not require iteration. • Solves highly discontinuous high-speed dynamic problems efficiently. • Does not require as much disk space as ABAQUS/Standard for larger problems. • Contact calculations are easier with ABAQUS/Explicit. Applications such as quasi-static metal forming simulations are easier. • Provides an adaptive meshing capability.



L1.13

Introduction – Documentation • Unless otherwise indicated, all documentation is available both online and in print. • ABAQUS Analysis User’s Manual • ABAQUS/CAE User’s Manual • ABAQUS Example Problems Manual • ABAQUS Benchmarks Manual (online only) • ABAQUS Verification Manual (online only) • ABAQUS Theory Manual (online only)



L1.14

Introduction – Additional reference materials • Installation and Licensing Guide – (Installation instructions) • Release Notes – (Explains changes since previous release) • Advanced lecture notes on various topics (print only) • Tutorials – Getting Started with ABAQUS – Getting Started with ABAQUS/Standard: Keywords Version (online only) – Getting Started with ABAQUS/Explicit: Keywords Version (online only) • ABAQUS Home Page www.abaqus.com



Components of an ABAQUS Model



L1.16

Components of an ABAQUS Model – The ABAQUS analysis modules run as batch programs. The primary input to the analysis modules is an input file • A text file which contains options from element, material, procedure, and loading libraries. – When working in ABAQUS/CAE, this input file is created “behind the scenes” when an analysis job is submitted • For many analyses, the user need never see the input file • In some cases, the user may need to manually edit the input file before submitting the analysis – A basic understanding of the ABAQUS input file format and contents is beneficial



L1.17

Components of an ABAQUS Model – The input file is divided into two parts: model data and history data. Model data

Geometric options—nodes, elements Material options Other model options

History data

Procedure options Loading options Output options



L1.18

Components of an ABAQUS Model • History subdivided into analysis steps – Steps are convenient subdivisions in an analysis history. – Different steps can contain different analysis procedures—for example, static followed by dynamic. – Distinction between general and linear perturbation steps: • General steps define a sequence of events that follow one another. – The state of the model at the end of the previous general step provides the initial conditions for the start of the next step. This is needed for any history-dependent analysis. • Linear perturbation steps provide the linear response about the base state, which is the state at the end of the most recent general step.



L1.19

Components of an ABAQUS Model • Example: bow and arrow simulation

Step 3 = natural frequency extraction

Step 1 = pretension

Step 2 = pull back

Step 4 = dynamic release

Step 1: String the bow Step 2: Pull back on the bow string Step 3: Linear perturbation step to extract the natural frequencies of the system— has no effect on subsequent steps Step 4: Release the arrow Copyright 2004 ABAQUS, Inc.


Structure of an ABAQUS Input File



L1.21

Structure of an ABAQUS Input File • Option blocks – All data are defined in “option blocks” that describe specific aspects of the problem definition, such as an element definition, etc. Together the option blocks build the model.

Property reference option block

Node option block

Model data

Material option block

Element option block

Contact option block

History data

Analysis procedure option block

Boundary conditions option block

Initial conditions option block

Loading option block

Output request option block



L1.22

Structure of an ABAQUS Input File – Each option block begins with a keyword line (first character is *). – Data lines, if needed, follow the keyword line. – Comment lines, starting with **, can be included anywhere. • Keyword lines – Begin with a single * followed directly by the name of the option. – May include a combination of required and optional parameters, along with their values, separated by commas. • Example: A material option block defines a set of material properties.


*MATERIAL, NAME=material name keyword

parameter parameter value

The first line in a material option block


L1.23

Structure of an ABAQUS Input File • Data lines – Define the bulk data for a given option; for example, element definitions. – A keyword line may have many data lines associated with it. • Example: An element option block defines elements by specifying the element type, the element numbers, and the nodal connectivity.

*ELEMENT, 560, 101, 564, 102, 572, 103, ⋅ ⋅



ABAQUS Conventions


TYPE=B21 102 103 104

keyword line data lines

node numbers (as required for beam B21 elements) element numbers


L1.25

ABAQUS Conventions • Units – ABAQUS uses no inherent set of units. – It is the user’s responsibility to use consistent units.

Common systems of consistent units



ABAQUS Conventions • Time measures – ABAQUS keeps track of both total time in an analysis and step time for each analysis step. – Time is physically meaningful for some analysis procedures, such as transient dynamics. – Time is not physically meaningful for some procedures. In rateindependent, static procedures “time” is just a convenient, monotonically increasing measure for incrementing loads.


L1.26


L1.27

ABAQUS Conventions • Coordinate systems – For boundary conditions and point loads, the default coordinate system is the rectangular Cartesian system.

local rectangular coordinate system with YSYMM boundary conditions

• Alternative local rectangular, cylindrical, and spherical systems can be defined. • These local directions do not rotate with the material in large-displacement analyses.

Boundary conditions on a skew edge



L1.28

ABAQUS Conventions – For material directions (i.e., directions associated with each element’s material or integration points) the default coordinate system depends on the element type: • Solid elements use global rectangular Cartesian system.

Default material directions for solid elements

• Shell and membrane elements use a projection of the global Cartesian system onto the surface.

Default material directions for shell and membrane elements



L1.29

ABAQUS Conventions – Alternative rectangular, cylindrical, and spherical coordinate systems may be defined. • Affects input: anisotropic material directions. • Affects output: stress/strain output directions. • Local material directions rotate with the material in large-displacement analyses.



ABAQUS Conventions • Degrees of freedom – Primary solution variables at the nodes. – Available nodal degrees of freedom depend on the element type. – Each degree of freedom is labeled with a number: 1=x-displacement, 2=y-displacement, 11=temperature, etc.


L1.30


Workshop 1: Linear Static Analysis of a Cantilever Beam



Workshop 1: Linear Static Analysis of a Cantilever Beam •

Workshop tasks 1. Follow detailed instructions to create a simple cantilever beam model using the ABAQUS/CAE modules. 2. Submit a job for analysis. 3. View the analysis results.


L1.32


Lecture 2

Nonlinear Analysis in ABAQUS/Standard



Overview • Equilibrium Equations • Linear Analysis • Nonlinearity in Structural Mechanics • Solving Nonlinear Equilibrium Equations • Including Nonlinear Effects in an ABAQUS Simulation • Convergence Issues • Diagnostics • Workshop 2: Nonlinear Analysis of a Skew Plate


L2.2


Equilibrium Equations



L2.4

Equilibrium Equations • The finite element method seeks to find the displacements of a structure, u, such that: – The solution is continuous across element boundaries. – Equilibrium is achieved, and the prescribed boundary conditions are satisfied. • Static equilibrium – The basic statement of static equilibrium is that the internal forces exerted on the nodes, I, resulting from the element stresses and external forces, P, acting at every node must balance:

P (u ) − I (u ) = 0

(Eq. 2.1)

– Equation 2.1 is general, and makes no assumptions about the forms of P(u) and I(u).



L2.5

Equilibrium Equations



L2.6

Linear Analysis • Linear assumptions – If we assume • the deflections, rotations and strains are small • the material behaves linearly, and • the loads and boundary conditions do not change as the structure deforms then P is constant and I = Ku where K is constant – The equilibrium equation is then linear in u and the solution can be found directly:

u = K-1P



L2.7

Linear Analysis • Characteristics of a linear analysis – Results (stress, strain, displacement) vary in proportion to the applied loads. • Eg twice the load gives twice the displacement • If the problem is solved once, the results can be scaled – For a given set of boundary conditions, the results from distinct loads can be superimposed to find the combined effect



Linear Analysis • Linear analysis has historically been widely used – Linear methods are easy and fast to solve – ABAQUS can solve linear problems • But… – Real world problems are only approximately linear – Linear analysis is often inappropriate: • Non-linear material response • Large deformations • Loads or boundary conditions dependent on solution • In these cases, a nonlinear analysis is required to correctly model the structural response.


L2.8


Nonlinearity in Structural Mechanics



L2.10

Nonlinearity in Structural Mechanics • Sources of nonlinearity – Material nonlinearities: • Nonlinear elasticity • Plasticity • Material damage • Failure mechanisms • Etc. – Note: material dependencies on temperature or field variables do not introduce nonlinearity if the temperature or field variables are predefined.


Some examples of material nonlinearity


L2.11

Nonlinearity in Structural Mechanics – Boundary nonlinearities: • Contact problems – Boundary conditions change during the analysis. – Extremely discontinuous form of nonlinearity.

An example of self-contact: “Compression of a jounce bumper,” Example Problem 1.1.16 in the ABAQUS Example Problems Manual



L2.12

Nonlinearity in Structural Mechanics – Geometric nonlinearities: • Large deflections and deformations • Large rotations • Structural instabilities (buckling) • Preloading effects

An example of a load-displacement curve from a buckling analysis



L2.13

Nonlinearity in Structural Mechanics – Typical nonlinear problems have all three forms of nonlinearity. • Must include the nonlinear terms in the equations.

An example of with nonlinearity— elastomeric keyboard dome



Solving Nonlinear Equilibrium Equations


Video Clip


L2.15

Solving Nonlinear Equilibrium Equations • Static equilibrium – As before, we have

P = Ku – However, now P and K can depend on u :

P = P(u) and K = K(u) • It is no longer possible to solve for u directly – Nonlinear problems are generally solved using an incremental and iterative numerical technique



L2.16

Solving Nonlinear Equilibrium Equations • Incremental solution scheme – For a static problem a fraction of the total load is applied to the structure and the equilibrium solution corresponding to the current load level is obtained. • The load level is then increased (i.e., incremented) and the process is repeated until the full load level is applied. P

Increments in applied load

Final equilibrium solution at total load

u Intermediate equilibrium solutions Copyright 2004 ABAQUS, Inc.


L2.17

Solving Nonlinear Equilibrium Equations – To solve for equilibrium in nonlinear problems, ABAQUS/Standard uses an incremental-iterative solution, based on the Newton-Raphson technique. – Assume that the solution to the previous load increment, u0, is known. – Assume that after an iteration, i, an approximation, ui, to the solution has been obtained. Let ci+1 be the difference between this solution and the exact solution to the discrete equilibrium equation, Equation 2.1, so that

P (ui + ci +1 ) − I (ui + ci +1 ) = 0.

(Eq. 2.2)

– Expanding the left-hand side of Equation 2.2 in a Taylor series about the approximate solution, ui, then gives

 ∂P(ui ) ∂I (ui )  P(ui ) − I (ui ) +  −  ci +1 + .... = 0. ∂u   ∂u

(Eq. 2.3)



L2.18

Solving Nonlinear Equilibrium Equations – By ignoring higher-order terms, the equation can be written as

K i ci +1 = P (ui ) − I (ui ), where K i =

∂I (ui ) ∂P (ui ) is the tangent stiffness. − ∂u ∂u

– The next approximation to the solution is

ui +1 = ui + ci +1. – Note that if the load depends on displacement (e.g., pressure on a surface that rotates), the stiffness matrix includes a load stiffness contribution.



L2.19

Solving Nonlinear Equilibrium Equations – ABAQUS then forms Ki+1 and calculates Ii+1 based on the updated state of the model, ui+1. – The difference between the total applied force, PTOTAL, and the internal force, Ii+1, is called the force residual, Ri+1: Ri+1= PTOTAL− Ii+1. – If R1 is very small (within the tolerance limit) at every degree of freedom in the model, the structure is in equilibrium. • The default tolerance is that R1 must be less than 0.5% of the time averaged force in the structure. • ABAQUS automatically calculates the time averaged force. – If the iteration does not produce a converged solution, ABAQUS will perform another iteration in an attempt to find a converged solution.



L2.20

Solving Nonlinear Equilibrium Equations – This procedure is repeated until force residuals are within the tolerance limits. Each iteration, i, requires: 1. Formulation of tangent stiffness, Ki. 2. Solution of simultaneous system of equations for ci+1. • Update the estimate of the solution: ui+1 = ui + ci+1. 3. Calculation of internal force vector Ii+1 based on ui+1. 4. Judgment of equilibrium convergence: • Is Ri+1 within the “tolerance”? # iter

• Is ci +1 <<

∑c ? j

j =1



L2.21

Solving Nonlinear Equilibrium Equations – The method can be understood quite easily (in one dimension) from a load-displacement diagram:

Two convergence criteria: Small residuals Residual

Small corrections 1

Internal force

2 Correction



Solving Nonlinear Equilibrium Equations • Steps, increments, and iterations – Analysis steps • The load history for a simulation consists of one or more steps. – Increments • An increment is part of a step. – In static problems the total load applied in a step is broken into smaller increments so that the nonlinear solution path may be followed. – In dynamic problems the total time period is broken into smaller increments to integrate the equations of motion. – Iterations • An iteration is an attempt at finding the equilibrium solution in an increment.


L2.22


L2.23

Solving Nonlinear Equilibrium Equations • Automatic time incrementation – ABAQUS automatically adjusts the size of the increments so that nonlinear problems are solved easily and efficiently. • Heuristic algorithm (based on many years of experience). – In static problems it is based on number of iterations required to converge. • Convergence is easily achieved: ⇒increase increment size

• Convergence difficult or divergence occurs: ⇒cut back increment size

• Otherwise: ⇒maintain same increment size

– Tip: For highly nonlinear problems, it is recommended that the initial time increment be chosen as a small fraction (e.g., 10%) of the total step time.



L2.24

Solving Nonlinear Equilibrium Equations • Incrementation data: ABAQUS/Standard

Automatic time incrementation chosen by default.

– Specify the initial increment size and the number of increments allowed.

Default maximum number of increments allowed for the step.

– ABAQUS will stop if: • The maximum number of increments is reached before the total load is applied or • If increment sizes smaller than the minimum are required.


Suggested initial increment size. Default is the time period.

Minimum and maximum increment sizes. Defaults based on time period for step.


Including Nonlinear Effects in an ABAQUS Simulation



Including Nonlinear Effects in an ABAQUS Simulation • Material nonlinearity – Define a nonlinear material model (e.g., plasticity, hyperelasticity, etc). – Examples are discussed in Lectures 3 and 4 • Boundary nonlinearity – Define contact interactions between bodies. – Discussed further in Lecture 8. • Geometric nonlinearity – Set the Nlgeom option when defining the analysis step.


L2.26


L2.27

Including Nonlinear Effects in an ABAQUS Simulation • Geometric nonlinearity – Include all nonlinear geometric effects due to: • Large deflections, rotations, deformation.

Specify time period of the step.

• Preloading (initial stresses). • Load stiffness. – If the above are not important, the answer will be the same as with Nlgeom set to Off but the analysis will be more expensive.

Set Nlgeom to On to include include all nonlinear geometric effects.



Convergence Issues


Edit Step dialog box


L2.29

Convergence Issues (Noncontact Related) • What does convergence mean? – For an implicit solver such as ABAQUS/Standard: • Equilibrium state has been obtained based on predefined criteria (small residuals, small solution corrections, etc.). • Non-convergence – If ABAQUS is unable to converge to the equilibrium state in an acceptable number of iterations, the analysis will terminate at that point – Information is available to help diagnose convergence problems • Error and warning messages • Detailed information about the solution progress – Available in • Message file (*.msg) • Job Monitor and Job Diagnostics in ABAQUS/CAE



L2.30

Convergence Issues (Noncontact Related) • Some common warning messages ABAQUS/Standard Numerical singularities

These indicate that so many digits are lost during linear equation solution that the results are not reliable. The most common cause is an unconstrained rigid body mode in a static stress analysis.

Zero pivots

These occur during linear equation solution when there is a force term but no corresponding stiffness. Common causes are unconstrained rigid body modes and overconstrained degrees of freedom.

Negative eigenvalues

Negative eigenvalues indicate that the stiffness matrix is not positive definite. For example, a buckling load may have been exceeded.



Diagnostics



L2.32

Diagnostics – Job Monitor • Summarizes the solution progress. • The same information is also printed to the status (.sta) file. – Job Diagnostics • Provides details of each iteration for an ABAQUS/Standard analysis. • The same information is also printed to the message (.msg) file.



L2.33

Diagnostics • Understanding the Job Monitor – Summarizes how analysis proceeds—shows automatic time incrementation at work. – You can check the status file while the job is running. – One line written after each successful increment.



Diagnostics • Understanding Job Diagnostics in ABAQUS/Standard – Includes: • All iteration details. • Solver messages. • Useful troubleshooting information: – Locations of highest residuals. – Locations of excessive deformation. – Locations of contact changes. – The locations can be highlighted in the model.


L2.34


L2.35

Diagnostics

Tools Job Diagnostics

Initial time increment



L2.36

Diagnostics

A similar display is given for rotational degrees of freedom

Toggle on to see the locations in the model where the largest residuals and displacement increments and corrections occur.



L2.37

Diagnostics

× 0.005 0.012



L2.38

Diagnostics

× 0.005 0.012



L2.39

Diagnostics

4 or fewer iterations (do this again and ∆t can increase)



L2.40

Diagnostics no increase

Two consecutive increments with 4 or fewer iterations: ∆ t = 1.5∆ told


∆ t = 1.5∆ told


L2.41

Diagnostics



Workshop 2: Nonlinear Analysis of a Skew Plate



L2.43

Workshop 2: Nonlinear Analysis of a Skew Plate •

Workshop tasks

1. Create model. a. Local material directions. b. Local boundary condition directions. 2. Run static analysis: a. Linear b. Geometric nonlinearity 3. Postprocess the results.

Video Clip



Lecture 3

Materials - Metal



Overview • Introduction • Typical Metal Behaviour • Linear Elasticity • Metal Plasticity • Yield Functions • Hardening • Input of Material Data for Plasticity • Workshop 3a: Plasticity and Hardening • Workshop 3b: Skew Plate with Plasticity


L3.2


Introduction



Introduction • ABAQUS has a wide variety of built-in material models designed to be used to model – Metals, ceramics, rubbers, foams, plastics, soils, concrete and other geotechnical materials • Phenomenological Approach – Most material models (for metal and concrete) are based upon experimental observations. – Capture critical material behaviour within a usable and stable continuum description • Material Input – Key material parameters (eg Youngs Modulus) must be entered by the user – ABAQUS has no inbuilt library of material parameters


L3.4


L3.5

Introduction • This course provides general information about modeling two particular materials in ABAQUS – Metals – Concrete • The focus of this lecture is on modeling Metals – Conrete is discussed in the next lecture



Typical Metal Behaviour



L3.7

Typical Metal Behaviour – Consider a uniaxial tension test performed on a metal specimen at relatively low temperature. B

stress

A

E 1 C

strain

Uniaxial stress-strain data for a metal Copyright 2005 ABAQUS, Inc.


L3.8

Typical Metal Behaviour – The material initially exhibits stiff linear response to the applied load: • Young’s modulus E quantifies the material stiffness. • The deformation is fully recoverable—if the load is released, the specimen will return to its original configuration. – At point A the material yields, and the deformation beyond this point is not fully recoverable—it is no longer purely elastic. – Yield is usually accompanied by a drastic reduction in the stiffness of the material: • Response to further loading follows a much lower work hardening modulus. • In extreme cases the material exhibits no stiffness beyond the initial yield point and is considered perfectly plastic.



L3.9

Typical Metal Behaviour – If the strain is reversed at point B, the material immediately recovers its elastic stiffness. – If the specimen is completely unloaded, the strain at point C represents the permanent deformation in the material. – If the unloading does not continue beyond the elastic range and the specimen is again loaded in the original direction, the material yields at, or very close to, point B.



L3.10

Typical Metal Behaviour – If the unloading is continued so that yield occurs in the opposite direction, the yield stress is reduced compared to that of the original specimen. This is known as the Bauschinger effect. B

stress

A

C strain

D A−

The Bauschinger effect Copyright 2005 ABAQUS, Inc.


L3.11

Typical Metal Behaviour – Discussion thus far has been limited to uniaxial stress-strain measurements at one temperature and one strain rate. For most metals: • As the material temperature increases, the yield stress decreases. • As the strain rate increases, the yield stress increases. – Varying the temperature and strain rate provides results similar to those shown in the figure below. stress

stress temperature increasing

strain

Effect of temperature and strain rate on stress-strain data Copyright 2005 ABAQUS, Inc.


Linear Elasticity


strain rate increasing

strain


L3.13

Linear Elasticity – Most metals have some range of deformation in which their behavior remains elastic and linear – The linear elastic material model: • Is valid for small elastic strains (normally less than 5%); • Can be isotropic, orthotropic, or fully anisotropic; and • Can have properties that depend on temperature and/or other field variables. – Orthotropic and anisotropic material definitions require the use of local material directions.



L3.14

Linear Elasticity – For a linear elastic material, Hooke's law states:

stress ∝ strain. – The generalized form of the law is written as

σ = D el : ε el – where σ is the Cauchy (or “true”) stress, D el is the fourth-order elasticity el tensor, and ε is the elastic log strain.

1

Uniaxial stress-strain curve for a linear elastic material Copyright 2005 ABAQUS, Inc.


L3.15

Linear Elasticity • Defining linear elasticity in ABAQUS

*Material, name=steel *Elastic 2.e11, 0.3

Temperaturedependence



Metal Plasticity



L3.17

Metal Plasticity – When inelastic material models are used in ABAQUS, the total strain in the model, ε, is decomposed into elastic, plastic, and creep strains:

ε = ε el + ε pl + ε cr . – ABAQUS plasticity models are usually formulated in terms of a yield surface, a flow rule, and hardening. • A yield surface is a test function that determines if the material responds purely elastically at a particular stress state. • A flow rule defines the plastic deformation that occurs if the material is no longer responding purely elastically. • Hardening defines the way in which the yield and/or flow definitions change as inelastic deformation occurs.



Yield Functions



L3.19

Yield Functions

(

)

0 – The yield function of the metal plasticity models, f σ ,σ , defines when the metal begins to deform inelastically.

• When f = 0, the metal is yielding. • σ is the true stress in the metal (it is a tensor quantity). • σ 0 is the yield stress (usually a scalar quantity). – The yield function is often written in terms of stress invariants. The commonly used stress invariants are

1 3 3 Mises equivalent stress, q = ( S : S ), 2

equivalent pressure stress, p = − trace (σ ) ,

where S is the deviatoric stress, defined as σ = S − pI . • Note that for uniaxial loading, q = σuniaxial. Copyright 2005 ABAQUS, Inc.


L3.20

Yield Functions – There are two yield functions available for the classical metal plasticity models in ABAQUS: • The Mises yield function,

f = q − σ 0. • Hill’s anisotropic yield function,

(

f = F σ yy − σ zz

)

2

2

(

+ G (σ zz − σ xx ) + H σ xx − σ yy

F, G, H, L, M, and N are material constants


)

2

2 2 2 + 2 Lσ yz + 2 M σ zx + 2 Nσ xy − σ 0.


L3.21

Yield Functions – The Mises yield function is suitable when: • The metal is subjected to monotonic loads, such as crash analyses and forming simulations. • The material has isotropic yielding. – Hill’s yield function is intended for metals that have initial anisotropy in their yield behavior. • The anisotropy does not evolve with plastic deformation of the material.



Yield Functions – Defining Mises plasticity in ABAQUS

*Material, name=steel *Elastic Linear elasticity 2.e11, 0.3 *Plastic Plastic strain at 4.e8, 0.0 initial yield = 0.0 4.2e8, 0.02 5.e8, 0.2 6.e8, 0.5

True stress and log plastic strain


L3.22


L3.23

Yield Functions – Defining Hill’s plasticity in ABAQUS *Material, name=steel *Elastic 2.e11, 0.3 *Plastic 4.e8, 0.0 4.2e8, 0.02 5.e8, 0.2 6.e8, 0.5 *Potential 1.5, 1., 1., 1., 1., 1.

Stress ratios; can be functions of temperature and field variables.



L3.24

Yield Functions – ABAQUS calculates the values of the constants F, G, H, L, M, and N of Hill’s yield function from stress ratios:

R11 = σ 11 σ 0 , R22 = σ 22 σ 0 , R33 = σ 33 σ 0 R12 = σ 12 τ 0 , R13 = σ 13 τ 0 , R23 = σ 23 τ 0

where σ 11, σ 22 , K are the yield stress values when σ ij is the only nonzero component of stress, σ 0 is the reference yield stress value and

τ0 =σ0

3.

σ 0 is given on the *PLASTIC option or in the Plastic definition area of the material editor; it is usually chosen as one of the three direct yield stress magnitudes. Copyright 2005 ABAQUS, Inc.


L3.25

Yield Functions • Example: cylindrical cup deep drawing with transverse anisotropy – We examine two cases: one in which the material is considered isotropic, another in which transverse anisotropy is assumed. This example is modeled using the ∗POTENTIAL option within the material block: ∗POTENTIAL 1., 1., 1.1511, 1., 1. , 1.

– Plots of blank thickness in the final formed configuration for both cases are shown in the figures on the next page.



L3.26

Yield Functions – The effect of the anisotropy on the thickness is readily apparent, as the increased strength in the thickness direction results in less thinning of the blank.

isotropic

anisotropic

Effect of transverse anisotropy on blank thickness Copyright 2005 ABAQUS, Inc.


Hardening



L3.28

Hardening • Yield surface must be coupled to a hardening relationship – The yield surface may change as a result of plastic deformation. The change in the yield surface is defined by the hardening law. – The following hardening laws are available in ABAQUS: • Perfect plasticity • Isotropic hardening

Intended for applications such as crash analyses, metal forming, and general collapse studies.

• Kinematic hardening

Intended for applications involving cyclic loading.

• Combined isotropic/kinematic hardening • Johnson-Cook plasticity


Well suited to model high-strainrate deformation of metals; only available in ABAQUS/Explicit.


L3.29

Hardening • Perfect plasticity (no hardening) – Simplest definition of plasticity – In perfect plasticity the metal’s yield function, f, does not evolve as the metal accumulates plastic strains. – Perfect plasticity can be used with either the Mises or the Hill yield function. – Perfect plasticity is defined by providing only one value for the yield stress of the metal, σ 0.



Hardening – Defining perfect plasticity in ABAQUS

*Material, name=steel *Elastic 2.e11, 0.3 *Plastic 4.e8, 0.0

One value of the yield stress of the metal, σ 0, is provided.


L3.30


L3.31

Hardening • Isotropic hardening (default) – Isotropic hardening is used to model gross plastic straining or when straining at a point is essentially in the same direction in strain space. – The yield stress increases (or decreases) uniformly in all stress directions as plastic straining occurs – With isotropic hardening the metal’s yield stress evolves as the metal accumulates plastic strains, σ 0 ε pl .

( )

ε

pl

is the equivalent plastic strain, defined as

ε

pl

=

t

∫  0

2 pl pl  ε& : ε& dt. 3 



L3.32

Hardening • ε

pl

is obtained through the variable PEEQ in ABAQUS.

– It is obtained by integrating the equivalent plastic strain rate over the history of the deformation. – Thus, it always grows with any plastic deformation.



L3.33

Hardening – Define isotropic hardening by providing tabular data of σ 0 and ε

pl

.

– Isotropic hardening can be used with either Mises or Hill’s yield function.

*Material, name=steel *Elastic 2.e11, 0.3 *Plastic 4.e8, 0.0 4.2e8, 0.02 5.e8, 0.2 6.e8, 0.5



L3.34

Hardening • Linear kinematic hardening – Linear kinematic hardening is used to model the behavior of metals subjected to cyclic loading. – The linear kinematic model defines the yield function as

f = q ( σ − α ) − σ 0 = 0.

α is the backstress tensor that describes how the center of the yield surface moves in stress space as plastic strains accumulate. • q (σ − α ) can be either Mises or Hill’s yield potential (function).



L3.35

Hardening

• Pick the second data point from stabilized cyclic test data. • The linear kinematic hardening data can be a function of θ only. • No field variable ( fi ) or rate dependence is allowed

(σ

0

,ε

pl

)

1.0

[×103]

(σ

0

, 0)

0.5

Stress—S11

– Define linear kinematic hardening by providing the initial yield stress, σ 0 , and the yield stress, σ 0(ε pl), at some finite plastic strain.

0.0

−0.5

−1.0 −10.

−5.

0.

Strain—E11

5.

10.

[×10−3]

Calibrating the linear kinematic hardening model



Hardening – Sample usage:

*Material, name=steel *Elastic 200.E3,.3 *Plastic, hardening=kinematic 200., 0.0 220., 0.0009


L3.36


L3.37

Hardening – The linear kinematic model can provide a first-order approximation of the anisotropic hardening that occurs in metals when they are loaded cyclically. • The model accounts for the translation of the yield surface with plastic deformation but does not consider any change in the size of the yield surface. • The linear kinematic model is valid only for relatively small strains (ε < 0.05). • Approximates the Bauschinger

stress

A Y

effect seen in cyclic loading.

B O

strain

C Y −

The Bauschinger effect Copyright 2005 ABAQUS, Inc.


Input of Material Data for Plasticity



L3.39

Input of Material Data for Plasticity – Experimental measurements are often reported in terms of nominal (engineering) stress versus nominal strain. For approximately incompressible material behavior, a simple conversion to true stress and logarithmic strain can be carried out:

σ true = σ nom (1 + ε nom ) , ε ln = ln (1 + ε nom ) . – These expressions relate true stress versus logarithmic total strain. ABAQUS requires true stress versus logarithmic plastic strain to be defined with the plasticity model options. Logarithmic plastic strain can be obtained from logarithmic total strain using

ε lnpl = ε ln −

σ true E

.



Workshop 3a: Plasticity and Hardening Workshop 3b: Skew Plate with Plasticity



Lecture 4

Materials - Concrete



Overview • Introduction • Mechanical Behavior of Plain Concrete • ABAQUS Constitutive Models for Concrete • Concrete Smeared Cracking • Usage • Calibration • Modeling Aspects • Reinforcement Modeling • Workshop 4: Collapse of a Concrete Slab


L4.2


Introduction



Introduction • ABAQUS offers a variety of constitutive material models suited for the analysis of concrete structures. • This lecture is intended as an introduction to the Smeared Cracking Model in ABAQUS/Standard. – Suitable for modeling reinforced concrete under low confining pressures and monotonic loading. – Other models are available, but are beyond the scope of this course. • This lecture also provides an overview of modeling reinforcement.


L4.4


L4.5

Introduction • Typical applications – Collapse load calculations of structural components, such as reinforced beams, columns, shear walls, etc. – Nuclear reactor engineering: Failure analysis of reinforced concrete containment by overpressurization – Road and bridge engineering



Mechanical Behavior of Plain Concrete



L4.7

Mechanical Behavior of Plain Concrete • Concrete behaves as a quasi-brittle material except under high triaxial compression. • Unlike classically brittle solids, concrete can undergo inelastic deformation that may be significantly larger than the elastic strains. • What follows are general observations about the macroscopic behavior of typical plain concrete. – These observations are useful for constructing and understanding constitutive models – No attempt is made to discuss the highly complex microscopic behaviour of concrete



L4.8

Mechanical Behavior of Plain Concrete • Uniaxial behavior – Beyond some stress threshold, concrete behaves nonlinearly, exhibiting progressive and irreversible damage until complete collapse occurs. – Strain softening results from the formation of micro-cracks.

Uniaxial compression behavior

Uniaxial tension behavior

Karsan and Jirsa (1969)

Mazars and Pijaudier-Cabot (1989)



L4.9

Mechanical Behavior of Plain Concrete • Dilatancy: Volume increase that results from the formation and growth of cracks parallel to the direction of the greatest compressive stress.

Typical plot of compressive stress vs. axial, lateral, and volumetric strain



L4.10

Mechanical Behavior of Plain Concrete • Biaxial loading – Under biaxial compressive loading, concrete strength is greater than the one observed in uniaxial tests.

Compressive stress vs. strain components and volumetric strain under biaxial-compressive loading Kupfer et al. (1969)



L4.11

Mechanical Behavior of Plain Concrete • Biaxial strength envelope

Biaxial strength envelope of concrete

Failure modes of biaxially loaded concrete

Kupfer et al. (1969)



L4.12

Mechanical Behavior of Plain Concrete • Triaxial loading – Under high confining pressure, crack propagation is prevented. The brittle behavior disappears and is replaced by ductility with work hardening.

Triaxial concrete behavior Chen (1982)



L4.13

Mechanical Behavior of Plain Concrete • Cyclic behavior – Plasticity and stiffness degradation – Stiffness recovery upon load reversal (unilateral effect)

Stress-deformation curve under cyclic loading (small compressive stress)

Stress-deformation curve under cyclic loading (large compressive stress)

Reinhardt and Cornelissen (1984)

Reinhardt and Cornelissen (1984)



ABAQUS Constitutive Models for Concrete



L4.15

ABAQUS Constitutive Models for Concrete • ABAQUS uses a continuum description of the concrete material response instead of tracking discrete “macro” cracks. Constitutive calculations are performed independently at each integration point. • Models for concrete at low pressure stress – Smeared cracking model (ABAQUS/Standard) – Brittle cracking model (ABAQUS/Explicit) – Concrete damaged plasticity model • Models for concrete under high compression – Cap model • This lecture will only cover the smeared cracking model



L4.16

ABAQUS Constitutive Models for Concrete • Modeling reinforcement – “Tension Stiffening” – In ABAQUS reinforcement in concrete structures is typically provided by means of rebar and/or embedded elements. – With this modeling approach, the concrete behavior is considered independently of the rebar. – Effects associated with the rebar/concrete interface, such as bond slip and dowel action, are modeled approximately – This is done by introducing some “tension stiffening” into the postcracking concrete response to simulate load transfer across cracks through the rebar.



L4.17

ABAQUS Constitutive Models for Concrete • Brittle cracking model – Intended for applications in which the concrete behavior is dominated by tensile cracking and compressive failure is not important. – Includes consideration of the anisotropy induced by cracking. – The compressive behavior is assumed to be always linear elastic. – A brittle failure criteria allows the removal of elements from a mesh. – This material model is not discussed further in this class. • For more information see “Cracking model for concrete,” section 11.5.2 of the ABAQUS Analysis User's Manual.



ABAQUS Constitutive Models for Concrete • Concrete Damaged Plasticity Model – Intended as a general capability for the analysis of concrete structures under monotonic, cyclic, and/or dynamic loading – Scalar (isotropic) damage model, with tensile cracking and compressive crushing modes – Degradation of elastic stiffness in both tension and compression – Takes into account stiffness recovery effects in cyclic loading – This material model is not discussed further in this class. • For more information see “Concrete damaged plasticity,” section 11.5.3 of the ABAQUS Analysis User's Manual.


L4.18


Smeared Cracking Model



L4.20

Smeared Cracking Model – Intended for applications in which concrete is subjected to essentially monotonic straining and a material point exhibits either tensile cracking or compressive crushing. – Plastic straining in compression is controlled by a “compression yield” surface. – Tensile cracking occurs when the stress reaches the “crack detection” surface. – Cracking is assumed to be the most important aspect of the behavior, and the representation of cracking and post-cracking anisotropic behavior dominates the modeling.



L4.21

Smeared Cracking Model • Features of smeared cracking model • Compressive response – Elastic-plastic with hardening/softening – Undamaged elastic stiffness • Tensile response – Elastic with failure – Post-failure softening and damaged elasticity Unixaxial behaviour of plain concrete Copyright 2005 ABAQUS, Inc.


L4.22

Smeared Cracking Model • Multiaxial response – Yield and failure surfaces are fitted to experimental data

Yield and failure surfaces in the (p–q) plane


Yield and failure surfaces in plane stress


L4.23

Smeared Cracking Model • Tensile Crack Detection – Cracking is assumed to occur when the stress reaches “crack detection surface.” – Cracks are irrecoverable: they remain for the rest of the calculation (but may open and close). – No more than three orthogonal cracks can occur at any point (in 3D). – Following crack detection, the crack affects the calculations because a damaged elasticity model is used. – Stiffness degradation affects the normal stiffness and optionally the shear stiffness as well (using the Shear Retention option).



L4.24

Smeared Cracking Model • Post-cracking Response – Defined by “tension stiffening” curve input by user – This is the mechanism by which the rebar/concrete interaction is modeled – Also includes damaged elasticity normal to crack – Optionally, can include degradation of shear stiffness Post-failure response in tension



Usage



Usage • Isotropic Linear Elasticity for undamaged elastic response *** ** MATERIALS ** *Material, name=concrete *Elastic 29000., 0.18


L4.26


L4.27

Usage • Defining the plastic response in compression – User enters the uniaxial stress-strain response – Give tabular data defining yield stress as a function of plastic strain – Data is usually readily available from a uniaxial compression test



Usage • Plastic response in compression *** ** MATERIALS ** *Material, name=concrete *Elastic 29000., 0.18 *Concrete 18.4, 0. 32., 0.0013

Yield stress as function of plastic strain


L4.28


L4.29

Usage • Post-cracking tensile response – “tension stiffening” – The post-crack response is defined by a tension stiffening curve – Two possible ways of specifying tension stiffening: • Postfailure stress-strain relation • Fracture energy cracking criterion (stress-displacement relation) – The default is to define a Postfailure stress-strain relation (Type=Strain) • Give tabular data defining fraction of stress remaining versus postcracking strain Ratio of stress to failure stress

1.0

Crack opening strain



L4.30

Usage • Tension stiffening – continued… – When there is no reinforcement in the concrete, the stress-strain softening approach introduces unreasonable mesh sensitivity. – To deal with this, we assume that the fracture energy to open a unit area of crack, Gf , is a material property. – With this approach the concrete’s brittle behavior is characterized by a stress-displacement response rather than a stress-strain response. – Use Type=Disp to activate this approach • Specify the displacement, u0, at which linear loss of strength gives zero stress Ratio of stress to failure stress

1.0

u0 Crack opening displacement



L4.31

Usage Mesh sensitivity for unreinforced concrete: P u

Constant softening slope (σ−ε)

P

P

Constant fracture energy (σ−u)

1 element

8

4

1, 2, 4, and 8 elements

2 elements

u

*Tension Stiffening, Type=Strain

u

*Tension Stiffening, Type=Disp



Usage • Tension stiffening – continued… – The user must specify the tension stiffening behaviour; it cannot be omitted. – However, this data is not easily specified since the tension stiffening behaviour depends on the amount an orientation of reinforcement – But it is very important to the behaviour of the model – See later comments on Calibration and Modelling Aspects


L4.32


L4.33

Usage • Tension stiffening *** ** MATERIALS ** *Material, name=concrete *Elastic 29000., 0.18 *Concrete 18.4, 0. 32., 0.0013 *Tension Stiffening 1., 0. 0., 0.0008

Fraction of remaining stress

Postcracking strain



Usage • Defining the yield/failure surfaces – The user can enter four ratios to define the yield and failure surfaces • Ratio of ultimate biaxial compressive stress to ultimate uniaxial compressive stress • Ratio of uniaxial tensile stress at failure to ultimate uniaxial compressive stress • Ratio of magnitude of principal plastic strain at ultimate stress in biaxial compression to plastic strain at ultimate stress in uniaxial compression • Ratio of tensile principal stress at cracking in plane stress (when the other principal stress is at the ultimate compressive value) to the tensile cracking stress in uniaxial tension – If this data is not specified, default values are used


L4.34


L4.35

Usage • Failure ratios *** ** MATERIALS ** *Material, name=concrete *Elastic 29000., 0.18 *Concrete 18.4, 0. 32., 0.0013 *Tension Stiffening 1., 0. 0., 0.0008 *Failure Ratios 1.16, 0.0625, 1.28, 0.3333



Usage • Shear retention – The user can specify data to define how the shear modulus degrades in the presence of cracking. – The data required is • Fraction of shear modulus applicable to a closed crack • Crack opening strain at which the shear modulus is zero – If this option is omitted, the default is for full shear retention (i.e. the shear modulus is unaffected by cracking)


L4.36


L4.37

Usage • Shear retention *** ** MATERIALS ** *Material, name=concrete *Elastic 29000., 0.18 *Concrete 18.4, 0. 32., 0.0013 *Tension Stiffening 1., 0. 0., 0.0008 *Failure Ratios 1.16, 0.0625, 1.28, 0.3333 *Shear Retention 0.9, 0.002



Calibration



L4.39

Calibration • Minimum of two experiments are required to calibrate the simplest version of the concrete model (using all possible defaults) – Uniaxial compression test – Uniaxial tension test • Uniaxial compression – This test gives the compressive stress-strain curve • Uniaxial tensile test – This test is difficult to perform, and data is often not available – Assumption required for tensile failure strength (usually about 7-10% of compressive strength) – Calibration of post-failure response depends on nature of reinforcing



Calibration • Shear Retention – Combined tension and shear experiments are required to calibrate the post-cracking shear behaviour – Tests are difficult so default (full shear retention) is often used • Failure Ratios – Biaxial experiments are required to calibrate the Failure Ratios – Tests are difficult so default values are generally used


L4.40


Modeling Aspects



L4.42

Modeling Aspects • Choice of material properties – The user’s success in analyzing concrete problems depends significantly on making sensible choices regarding the concrete material parameters. – The values chosen for tension stiffening are the most important item when analyzing problems that involve cracking failure of the concrete. Generally, the more tension stiffening is included, the easier it is to obtain numerical solutions. – The tensile postfailure behavior is not easily specified: the loss of strength depends on such factors as the density of reinforcement and the quality of the bond between the rebar and the concrete. – Some trial and error may be required to calibrate the tension stiffening in each particular case



L4.43

Modeling Aspects – A reasonable starting point for reinforced concrete is to assume that the strain softening after failure reduces the stress linearly to zero at a total strain about 10 times the strain at failure. σt σ t0

ε t0

∼10×ε t0

– The strain at failure is typically 10-4, so a total strain of 10-3 is reasonable



L4.44

Modeling Aspects • Elements – ABAQUS offers a variety of elements for use with the concrete cracking model including beam, shell, plane stress, plane strain, axisymmetric, and three-dimensional continuum elements. – For general shell analysis more than the default number of 5 integration points through the thickness of the shell should be used; 9 thickness integration points are commonly used to model progressive failure of the concrete through the thickness with acceptable accuracy.



L4.45

Modeling Aspects • Output – In addition to the standard output identifiers available in ABAQUS, the following variables relate specifically to material points in the smeared crack concrete model: CRACK

Unit normal to cracks in concrete

CONF

Number of cracks at a concrete material point

– These variables are only available in the printed results file (*.dat) – Not currently supported through ABAQUS/CAE • Must be manually requested *El Print, Elset=concrete_elems CONF, CRACK



Modeling Aspects • Other considerations – Considerable nonlinearity is expected in the response of concrete structures, including the possibility of unstable regimes as the concrete cracks. The following is recommended to alleviate possible convergence difficulties: • Use automatic stabilization in static steps, ∗STATIC, STABILIZE. In problems with global instabilities, use the modified Riks method, ∗RIKS. • Since the overall convergence of the solution is expected to be nonmonotonic, use ∗CONTROLS, ANALYSIS=DISCONTINUOUS to prevent premature termination of the equilibrium iteration process because the solution may appear to be diverging.


L4.46


Reinforcement Modeling



Reinforcement Modeling • Reinforcement in ABAQUS – In ABAQUS, concrete reinforcement is modeled using REBAR LAYERS – Shell, membrane, and surface elements are reinforced by directly specifying a rebar layer in the element. • Surface elements do not have any element properties other than the rebar layer and are used primarily as place-holders for rebar layers. – Solid elements are reinforced using the embedded element constraint. • In this technique, either surface or membrane elements reinforced with rebar layers are embedded in the solid host elements.


L4.48


L4.49


Reinforcement

Solid elements

Embedded element constraint

Rebar layers in membranes

Structural elements

Rebar layers in membranes

Rebar layers in shells

Rebar layers in surface elements

Rebar layers in various element types in ABAQUS Copyright 2005 ABAQUS, Inc.


L4.50

Reinforcement Modeling – Rebars layers are used for modeling uniaxial reinforcement in shell, membrane and surface elements. – Rebars layers have the following properties: • Their material properties are independent of those of the underlying elements. • As many different combinations and orientations of rebar layers as are needed can be defined within a single element. • The rebar layer volume is not subtracted from the volume of the element to which the rebar layer is added. – Thus, rebar layers should be used only when the volume fraction of reinforcement is small (such as with reinforced concrete where the volume fraction of the rebar is between 1% and 4%).



L4.51

Reinforcement Modeling • Specification of rebar layers – The ∗REBAR LAYER option is used in conjunction with the ∗SHELL SECTION, ∗MEBRANE SECTION, or ∗SURFACE SECTION

options to specify reinforcement layers in shell, membranes, and surface elements, respectively.



L4.52

Reinforcement Modeling – Sample usage: *SHELL SECTION, ELSET=... *REBAR LAYER, ORIENTATION=ORI1 name, a, s, f, mat, alpha, 1

name

mat

a

s

alpha

*SHELL SECTION, ELSET=... *REBAR LAYER, ORIENTATION=ORI1 name, a, s, f, mat, alpha, 1


f


L4.53

Reinforcement Modeling – For each rebar layer, specify • rebar layer name (used to identify the layer in the list of section points when postprocessing with ABAQUS/Viewer); • the rebar material name; • cross-sectional area a of each rebar; • the rebar spacing s in the plane of the membrane, shell, or surface element; • the angular orientation alpha, in degrees, measured relative to the local 1-direction, positive in the direction of the element normal; and • the position of the rebars in the thickness direction f (for shell elements only), measured from the midsurface of the shell (positive in the direction of the positive normal to the shell). – Repeat the data to define each rebar layer – Similar method is used to define rebar in membrane and surface element Copyright 2005 ABAQUS, Inc.


L4.54

Reinforcement Modeling • Prestresses in rebar layers – Prestress can be defined in the rebars using the *INITIAL CONDITIONS, TYPE=STRESS, REBAR option, with or without using the *PRESTRESS HOLD option. • With the *PRESTRESS HOLD option the initial stress defined in the rebar is held constant. – While equilibrium iterations are performed to obtain the corresponding (self-equilibrating) stresses in the matrix material, the rebar layer will strain, but this strain is not allowed to cause changes in the stress in the rebar layer. • Without the *PRESTRESS HOLD option, the initial stresses are allowed to change during an equilibrating static analysis step as both the matrix and the rebar stresses adjust to the equilibrium configuration.



L4.55

Reinforcement Modeling • For example, in reinforced concrete: – The rebar are initially stretched to a desired tension before being covered by concrete. – After the concrete cures and bonds to the rebar, release of the initial rebar tension transfers load to the concrete, introducing compressive stresses in the concrete. – The resulting deformation in the concrete reduces the stress in the rebar.



L4.56

Reinforcement Modeling • Output – ABAQUS/CAE supports visualization of rebar layer orientations and results in rebar layers. – Output of variables such as stresses and strains at the rebar integration points is available • Results can be viewed on a layer-by-layer basis. • To display results for a given rebar layer, select the named rebar layer from the list of available section points.



L4.57

Reinforcement Modeling – The force in the rebar is available at the layer integration points as RBFOR, which is the rebar stress times the current cross-sectional area (see the figure on the following page). – RBANG and RBROT identify the current orientation of rebar within the element and the relative rotation of the rebar layer as a result of finite deformation. – Sample output request: *Element output, rebar S, E, RBANG, RBROT, RBFOR



Reinforcement Modeling • Rebar force output


L4.58


L4.59

Reinforcement Modeling • Embedding Rebar Layers – Membrane and surface elements reinforced with rebar layers can be embedded in continuum (solid) elements in an arbitrary manner such that the two meshes need not match. • This is accomplished using an EMBEDDED REGION constraint.



Reinforcement Modeling • Usage: *EMBEDDED ELEMENT, HOST ELSET=tread, ROUNDOFF TOLERANCE=1.e-6 belt1, belt2

– The ROUNDOFF TOLERANCE parameter is used to adjust the position of embedded nodes such that they lie exactly on a host element face or edge. – This reduces the number of constraint equations required, allowing for a more economical solution.


L4.60


L4.61


rebar orientation embedded membrane element

host solid element

Reinforced solid element using the embedded element technique Copyright 2005 ABAQUS, Inc.


Workshop 4: Concrete Slab Analysis



L4.63

Workshop 4: Collapse of a Concrete Slab – This workshop illustrates reinforced concrete modeling of typical slab-type structures. – The square slab is supported at its four corners and loaded by a point load at its center. – The slab is reinforced in two directions at 75% of its depth. – Noteworthy features: • Reinforced concrete shell modeling using rebar layer • Tension stiffening is modeled assuming a linear loss of strength beyond the cracking failure of concrete • Use of the Riks solution algorithm for globally unstable response



L4.64

Workshop 4: Collapse of a Concrete Slab

Geometry of the square slab and reinforcement



L4.65

Workshop 4: Collapse of a Concrete Slab • Load-deflection response:

ABAQUS/Standard

Load-deflection response for three different values of tension stiffening



Lecture 5

Eigenvalue Buckling Analysis



Overview • Introduction • Eigenvalue Problem Formulation • ABAQUS Usage • Closely Spaced Eigenvalues • Concluding Remarks • Workshop 5a: Cargo Crane – Critical Load Estimation • Workshop 5b: Eigenvalue Buckling of a Square Tube


L5.2


Introduction



L5.4

Introduction – The stability of structures is a problem that analysts face frequently. • These problems predominantly occur in beam and shell structures. – Such stability studies usually require two types of analyses: • Eigenvalue buckling analysis • Postbuckling or collapse analysis – We focus on eigenvalue buckling analysis, which very often is a required step for the more general collapse or load-displacement response analysis. – Eigenvalue buckling analysis is used to obtain estimates of the critical load at which the response of a structure will bifurcate, assuming that the response prior to bifurcation is essentially linear. • The simplest example is the Euler column, which responds very stiffly to a compressive axial load until a critical load is reached, at which point it bends suddenly and exhibits much lower stiffness.



L5.5

Introduction – Load-displacement response of an Euler column



Introduction – Deformed configurations of an Euler column


L5.6


L5.7

Introduction – The purpose of eigenvalue buckling analysis is to investigate singularities in a linear perturbation of the structure’s stiffness matrix. • The resulting estimates will be of value in design only if the linear perturbation is a realistic reflection of the structure’s response before it buckles. • Therefore, eigenvalue buckling is useful for “stiff” structures (structures that exhibit only small, elastic deformations prior to buckling). – In most cases of stiff structures, even when inelastic response may occur before collapse, eigenvalue buckling analysis provides a useful estimate of the collapse mode shape. – Only in quite restricted cases (linear elastic, stiff response; no imperfection sensitivity) is it the only analysis needed to understand the structure’s collapse limit.



L5.8

Introduction – In many cases the post-buckled response is unstable; the collapse load will then depend strongly on imperfections in the original geometry. • This is known as “imperfection sensitivity.” • In this case the actual collapse load may be significantly lower than the bifurcation load predicted by eigenvalue buckling analysis. – Thus, eigenvalue buckling analysis provides a nonconservative estimate of the structure’s load carrying capacity. – Even if the pre-buckling response is stiff and linear elastic, nonlinear loaddisplacement response analysis (of the imperfect structure) is generally recommended to augment the eigenvalue buckling analysis. • This is essential if the structure is imperfection sensitive.



Eigenvalue Problem Formulation



L5.10

Eigenvalue Problem Formulation – The objective of an eigenvalue buckling analysis is to • find the load level at which the equilibrium becomes unstable or • estimate the maximum load level which the structure can sustain. – The critical load level depends on the structure’s stiffness – The stiffness is dependent on the internal stress and, if the load follows the structure, on the applied load. • It will be assumed that the loading is conservative, so the stiffness matrix is symmetric.



L5.11

Eigenvalue Problem Formulation – First apply a “dead” load, P0. • This defines the stiffness of the base state K0 which includes preload effects (even if NLGEOM is not used). – Now add a “live” load, λ∆P, where λ is the magnitude of the live load being added and ∆P is the pattern of the live load. – As noted earlier, the method works best if the response is linear prior to bifurcation. Thus, as long as the response is stiff and linear elastic, the stress and, hence, the structural stiffness will change proportionally with λ, as Stiffness change is proportional to λ. K 0 + λ∆K , and

∆K = K ∆σ + K ∆P .

Due to incremental loading pattern; made up of two parts: the internal stress and the applied load.



L5.12

Eigenvalue Problem Formulation – We need to find values of λ, which provide singularities in this tangent stiffness; this poses the eigenproblem. • In other words, a loss of stability occurs when the total stiffness matrix is singular:

( K 0 + λ∆K )V = 0.



L5.13

Eigenvalue Problem Formulation – Values λcr, which provide nontrivial solutions to this problem, define the critical buckling load as P0 + λcr ∆P with corresponding buckling mode shapes V . – Buckling mode shapes V are normalized vectors, just as modes of free vibration are, and do not represent actual magnitudes of deformation at the critical load. • They are often the most useful outcome of the eigenvalue analysis since they predict the likely failure mode of the structure. – The mode shapes are also often used to generate perturbations in geometry for collapse analysis. • They are typically scaled to a fraction of a relevant structural dimension (such as a beam cross-section or a shell thickness) before they are used to perturb the geometry.



L5.14

Eigenvalue Problem Formulation – Estimating the maximum load level • Nonlinear pre-buckling makes the method approximate. • The estimate is more accurate if the structure is preloaded to a level close to the pre-buckling load capacity. • Generally alternative solution techniques (e.g., Riks) are required for accurate prediction.



ABAQUS Usage



ABAQUS Usage – ABAQUS will calculate the initial stress and load stiffness matrix corresponding to the live load directly. • The ∗BUCKLE step is a linear perturbation step, and the magnitude of the live load is not important. • The live load is specified in the ∗BUCKLE step. – The ∗BUCKLE step may be preceded by a ∗STATIC step in which the dead load is applied.


L5.16


L5.17

ABAQUS Usage – The buckling mode shapes of symmetric structures are either symmetric or antisymmetric. • For such structures it is more efficient to model only part of the structure and to perform the buckling analysis twice: once with symmetric boundary conditions and once with antisymmetric boundary conditions. – The live load pattern is usually symmetric, so symmetric boundary conditions are needed for the calculation of the perturbation stresses used in the formation of the initial stress stiffness matrix.



ABAQUS Usage – The boundary conditions must be switched to antisymmetric in the ∗BUCKLE step to obtain the antisymmetric modes. • This is done by giving the antisymmetric boundary conditions with LOAD CASE=2 on the ∗BOUNDARY option in the ∗BUCKLE step.


L5.18


L5.19

ABAQUS Usage • Example 1: Antisymmetric buckling of a symmetric structure

Finite element model

Boundary conditions for load case 1

Boundary conditions for load case 2

• B21 elements • Rectangular cross-section (1 in × 1in) • Linear elastic material: E = 30E6 psi

ν=0 Copyright 2004 ABAQUS, Inc.


ABAQUS Usage • Partial input for antisymmetric buckling of a symmetric structure *heading antisymmetric ring buckling eigenvalue estimate : : *nset, nset=left 4 *transform, nset=left 1., 1., 0., -1., 1., 0. *boundary right, 2 right, 6 left, 2 left, 6 *step, name=Step-1 *buckle 3, *boundary, load case = 2, op=new right, 2 right, 6 left, 1 *dsload ring, p, 1. *end step Copyright 2004 ABAQUS, Inc.

L5.20


L5.21

ABAQUS Usage – The dead and live loads can be point loads, distributed loads, or thermal loads; dead loads can also include nonzero prescribed boundary conditions. • If the live loads include uniform motion of a boundary, use multi-point constraints to constrain these nodes to a single point and load that point. – The dead load, P0, and the live load, ∆P, can be entirely different in magnitude and in nature. – Multiple buckling modes and associated critical load values can be obtained in a single eigenvalue buckling step. • Obtaining multiple buckling modes is often useful since many common systems (such as short cylindrical shells) have several closely spaced critical modes.



L5.22

ABAQUS Usage – Negative eigenvalues are sometimes obtained. • These values can indicate that there is a buckling mode corresponding to the load applied in the opposite direction. – For example, a pressure vessel under internal pressure might buckle under external pressure. • However, they can also point to spurious modes if nonlinearities occur before buckling.



L5.23

ABAQUS Usage – The load stiffness can have a significant effect on the critical buckling load. • ABAQUS will use the symmetric form of load stiffness in eigenvalue calculations. – Follower force effects are associated with pressure, hydrostatic pressure, buoyancy effects, centrifugal loading, and Coriolis loading and also with concentrated loads with the FOLLOWER option. – Eigenvalue buckling analysis with concentrated FOLLOWER loads will not yield the correct results since the follower force effects are not taken into account (the load stiffness is generally not symmetric).



L5.24

ABAQUS Usage – If temperature-dependent elastic properties are used, the elastic stiffness will be based on the temperatures prior to the eigenvalue buckling step. • Modifying temperatures in an eigenvalue buckling step will not change the elastic stiffness matrix. – When nonlinear material properties such as hyperelasticity are present in a model, ABAQUS/Standard ignores the nonlinear effects during the eigenvalue buckling analysis. • The material response during the buckling analysis is based on the linear elastic stiffness in the (potentially nonlinear) base state at the end of the previous step. – Inelastic behavior such as plasticity can be used if the eigenvalue buckling step is applied before the stress at any point has reached yield. • ABAQUS will use the elastic stiffness, defined with linear elasticity, in the eigenvalue buckling procedure to calculate ∆K, not the tangent stiffness from the hardening curve. Copyright 2004 ABAQUS, Inc.


L5.25

ABAQUS Usage • Choice of eigenvalue extraction method – In ABAQUS/Standard you have the choice of using either the subspace iteration or the Lanczos method to extract the eigenvalues. – The Lanczos method is generally faster when a large number of eigenmodes are required for a system with many degrees of freedom. • The subspace iteration method may be faster when only a few (less than 20) eigenmodes are needed.



ABAQUS Usage – By default, the subspace iteration method is used when extracting the buckling modes. • To use the Lanczos solver, include the EIGENSOLVER=LANCZOS parameter on the ∗BUCKLE option.


L5.26


L5.27

ABAQUS Usage – When the Lanczos eigensolver is requested, you can also specify the minimum and/or maximum eigenvalues of interest on the data line. • ABAQUS extracts eigenvalues until either the requested number of eigenvalues has been extracted in the given range or all the eigenvalues in the given range have been extracted. – The Lanczos eigensolver has the following restrictions for buckling simulations; it cannot be used with: • A model containing hybrid elements • A model containing distributing coupling elements • A model containing contact pairs or contact elements • A model that has been preloaded above the bifurcation (buckling) load



Closely Spaced Eigenvalues



L5.29

Closely Spaced Eigenvalues – Certain buckling problems may have many buckling modes with very closely spaced critical loads. • The eigenvalue algorithm may converge slowly in such a case. – Cylindrical shells with axial compressive loads are a good example of this case.

Radius = 100 Length = 800 Thickness = 0.25 Young’s modulus = 30 × 106 Poisson’s ratio = 0.3



L5.30

Closely Spaced Eigenvalues • Example 2: Buckling of a thin cylinder – S9R5 elements – Linear elastic material – Lanczos eigensolver – Symmetry (only half the cylinder length is modeled) *heading cylinder buckling : : : *step *buckle, eigensolver=lanczos 5, *cload Midside nodes bot1, 3, 65450.0 Corner nodes bot2, 3, 32725.0 *boundary bottom, 1, 2 top, zsymm *node file u *end step Copyright 2004 ABAQUS, Inc.

bottom

top


L5.31

Closely Spaced Eigenvalues – Critical stress as a function of mode shape (analytical results) Axial modes

Circum. modes

Critical stress

1

4

40718.09

2

5

43291.86

6

9

44283.65

5

8

44292.48

8

10

44662.13

4

7

44711.87

9

11

44751.29

10

11

44867.94

3

6

44874.56

7

10

44909.49

3

7

45608.18

7

9

45718.54

10

12

45792.77

4

8

45827.96

…

…

…



Closely Spaced Eigenvalues – Critical buckling mode of axially compressed cylinder


L5.32


L5.33

Closely Spaced Eigenvalues – Closely spaced eigenvalues are usually an indication that a structure is imperfection sensitive. • The imperfections cause the buckling modes to interact and will trigger collapse at a much lower level than predicted by the eigenvalue buckling analysis. • Hence, the actual buckling mode shape is usually not the same as the lowest buckling mode in the eigenvalue analysis. – Convergence can be improved substantially by applying part of the critical live load as a dead load, loading the structure to just below the buckling load. • This provides a larger separation of the eigenvalues and much improved convergence. • The process is equivalent to a dynamic eigenfrequency extraction with shift.



Closely Spaced Eigenvalues – If you exceed the critical (lowest) buckling load of the structure when applying the dead load, the analysis may terminate prematurely because ABAQUS will not be able to find the lowest buckling loads. • In addition, the Lanczos method will fail in that case.


L5.34


L5.35

Closely Spaced Eigenvalues – Buckling of axially loaded cylinder without imperfections



Closely Spaced Eigenvalues – Buckling of axially loaded cylinder with imperfections


L5.36


L5.37

Closely Spaced Eigenvalues • Example 3: Buckling of a thin cylinder with preload *heading cylinder buckling with preload : : : *step, nlgeom *static *cload bot2, 3, 130900.0 preload bot1, 3, 261800.0 *endstep *step *buckle, eigensolver=lanczos 5, *cload bot2, 3, 32725.0 bot1, 3, 65450.0 *node file u *end step Copyright 2004 ABAQUS, Inc.


L5.38

Closely Spaced Eigenvalues – The analysis with the preload converges much faster. • The analysis without the dead load has 5 converged eigenvalues after 60 iterations. • The analysis with the dead load obtains 5 converged eigenvalues after only 19 iterations. – Buckling of thin-walled cylinders often involves high numbers of waves in both axial and circumferential directions. • For accurate results very refined meshes are needed. – If reduced-integration elements are used, pseudobuckling modes involving extensive hourglassing may be found. • These modes do not affect physical buckling modes and can be suppressed by increasing the hourglass control with the ∗HOURGLASS STIFFNESS option.



Concluding Remarks



L5.40

Concluding Remarks – Eigenvalue buckling analysis yields a reliable estimate for the buckling load only if the assumptions of small geometric changes and linear elastic material response before buckling are realistic for the structure being modeled and if the collapse is not imperfection sensitive. – If in doubt, introduce an imperfection (in the shape of the lowest buckling modes) into the structure and use ∗STEP, NLGEOM with the ∗STATIC, RIKS procedure to obtain the complete pre- and postbuckling history.



L5.41

Concluding Remarks • For more examples of buckling and collapse analysis with ABAQUS see: – ABAQUS Benchmarks Manual: • 1.2.1 Buckling analysis of beams • 1.2.2 Buckling of a ring in a plane under external pressure • 1.2.3 Buckling of a cylindrical shell under uniform axial pressure – ABAQUS Example Problems Manual: • 1.2.2 Laminated composite shells: buckling of a cylindrical panel with a circular hole • 1.2.6 Buckling of an imperfection sensitive cylindrical shell



Workshop 5a: Cargo Crane Buckling Workshop 5b: Square Tube Buckling



Lecture 6

Static Postbuckling and Snap-Through Analysis



Overview • Introduction • ABAQUS Implementation • ABAQUS Usage • Snap-Through Problems • Postbuckling Problems • Introducing Imperfections for Postbuckling Simulations • Postbuckling Examples • Usage Hints • Limitations • Summary • Workshop 6a: Cargo Crane – Riks Analysis • Workshop 6b: Square Tube with Imperfections


L6.2


Introduction



L6.4

Introduction – Eigenvalue buckling analysis is useful for the analysis of “stiff” structures. • The method is not suitable if large geometry changes occur prior to buckling and can provide very misleading results if the structure is imperfection sensitive. – In cases where the eigenvalue buckling procedure is not applicable or its results are questionable, a fully nonlinear transient analysis is required. • A transient analysis can be done dynamically or by addition of viscous forces to the static problem. • The disadvantage of such analyses is that it is hard to understand the characteristics of the structure after the load maximum is reached.



L6.5

Introduction – To avoid any of the effects of the stabilizing forces, we would like to obtain a solution to the static equilibrium equation without adding such forces. – An algorithm is needed in which the applied loads are adapted automatically. • The solution algorithm must solve simultaneously for loads and displacements. – As a consequence another quantity must be selected to measure the progress of the solution. • For this we choose the “arc length,” l, which is the length along the static equilibrium path in load-displacement space. – A form of this method is activated in ABAQUS by adding the RIKS parameter on the ∗STATIC option.



L6.6

Introduction – Static analysis of snap-through and postbuckling problems with the arclength method provides valuable information about the characteristics of structures in the unstable regime. – The method works well if the equilibrium path in the load-displacement space is smooth and does not branch. • Otherwise, convergence and incrementation problems may occur. • Generally, this means that the method should always be applied to imperfect geometries—the “perfect” structure’s initial coordinates should be perturbed to create a suitable imperfection. • This converts a pure bifurcation behavior into a snap-through problem.



ABAQUS Implementation



L6.8

ABAQUS Implementation • Riks method for globally unstable problems – Consider this loaddisplacement curve:

Load P2

P1

Converged solution for increment 1

Displacement

Unstable force-displacement curve



L6.9

ABAQUS Implementation – At the top of the curve the gradient equals zero and the stiffness is singular. This can occur when structures “snap-through,” buckle, or collapse. • The structure’s instability may be the result of geometric or material effects. – In an unstable problem the structure must release energy to remain in equilibrium. In reality, this energy is converted to kinetic energy. – A way of studying a buckling problem is to use displacement control rather than force control; i.e., you prescribe the motion of a particular part of the model and look at the reaction forces to understand the load-displacement behavior. • Even with displacement control the structure may buckle dynamically.



L6.10

ABAQUS Implementation – An alternative is to use the “modified Riks method.” • The basic solution method is still the Newton-Raphson method, so the usual convergence rules apply. • It is the method by which the analysis progresses along the solution path that is changed. – The Riks method solves for both the displacements and the applied loads to find the equilibrium path. • The method can calculate solutions even when the slope of the forcedeflection curve is negative. • The magnitude of the load must be expressed in terms of a load proportionality factor, λ. • The method uses the concept of “arc length” (l) to track the size of the increment and how “far” the analysis has progressed.



L6.11

ABAQUS Implementation • RIKS is an arc-length control procedure – The solution is advanced along the load-deflection curve by solving for the equilibrium position a particular arc-length away from the last position. Load

l ∆l

Displacement Copyright 2004 ABAQUS, Inc.


L6.12

ABAQUS Implementation – In the Riks method we always deal with proportional loading within an analysis step. The load is assumed to consist of: • An initial load vector, P0, which has already been applied at the start of the step and remains constant throughout the step. • A load, λP, where P is a nominal load vector and λ is the “load proportionality factor” that ABAQUS will find as part of the solution. – In the simplest case P0 will be zero and P will be the result of distributing, for example, a uniform pressure of unit magnitude onto the structure. – In general, P is obtained as the difference between the reference load Pref specified in the Riks step and the dead load, P0 :

P = Pref − P0 .



ABAQUS Usage



ABAQUS Usage – The Riks procedure is invoked by including the Riks parameter on the ∗STATIC option. • Since the method is generally used with geometrically nonlinear cases, the NLGEOM parameter is usually included on the ∗STEP option.


L6.14


L6.15

ABAQUS Usage – A typical input sequence for a postbuckling analysis is *STEP, NLGEOM (apply optional dead load) *STATIC… (define the dead load and specify output requests) *END STEP *STEP, NLGEOM, INC=… (postbuckling Riks step) *STATIC, RIKS ∆linit, lperiod, ∆ lmin, ∆ lmax, λend, node, dof, umax (define the reference load and specify output requests) *END STEP



L6.16

ABAQUS Usage – The first two entries on the ∗STATIC, RIKS data line define the initial and estimated total arc lengths associated with the step. *STATIC, RIKS ∆linit, lperiod, ∆ lmin, ∆ lmax, λend, node, dof, umax

∆linit lperiod



L6.17

ABAQUS Usage – The second two entries are optional and form bounds for the arc length increment, ∆l. *STATIC, RIKS ∆linit, lperiod, ∆ lmin, ∆ lmax, λend, node, dof, umax



ABAQUS Usage – The last four optional entries serve as alternate termination criteria. *STATIC, RIKS ∆linit, lperiod, ∆ lmin, ∆ lmax, λend, node, dof, umax

• λend is provided to terminate the step when the load exceeds a certain magnitude.

• node, dof, umax are provided to terminate the step when a particular displacement component exceeds a given value.


L6.18


L6.19

ABAQUS Usage – ABAQUS will not stop exactly at these values but will stop when the values are exceeded. – If none of the above termination criteria is included, ABAQUS will stop when the maximum number of increments is reached or when the solution fails (for example, because of excessive distortion).



L6.20

ABAQUS Usage – Any amplitude references are ignored in the Riks procedure. • All loads are ramped from the initial (dead load) value to the reference value specified. • If the reference load is equal to the dead load, the Riks procedure will fail. • The load magnitudes are available as output. – The status (.sta) file shows clearly that a step uses the Riks procedure. SUMMARY OF JOB INFORMATION: MONITOR NODE: 1 DOF: 2 STEP INC ATT SEVERE EQUIL TOTAL DISCON ITERS ITERS ITERS 1 1 1 0 3 3 1 2 1 0 2 2 1 3 1 0 3 3 1 4 1 0 3 3 1 5 1 0 3 3 1 6 1 0 3 3

TOTAL TIME/ FREQ

STEP TIME/LPF 0.0471 0.0882 0.138 0.184 0.200 0.177

0.04713 0.04110 0.04958 0.04638 0.01590 -0.02278

λ Copyright 2004 ABAQUS, Inc.

INC OF TIME/LPF

∆λ

DOF IF MONITOR RIKS -0.195 -0.397 -0.714 -1.22 -2.00 -2.93

R R R R R R

flag indicating that this is a Riks analysis


Snap-Through Problems



L6.22

Snap-Through Problems – The Riks method works very well for snap-through problems. • Classical snap-through problems are characterized by a smooth loaddisplacement curve and do not exhibit branching (bifurcation). • As a result, the Riks procedure can solve this kind of problem with ease. • Generally, you do not need to take any special precautions to ensure a successful analysis. – An example of a problem with a smooth load-displacement curve (taken from the ABAQUS Example Problems Manual) is the shallow-arch problem shown on the following pages.



L6.23

Snap-Through Problems Example 1: Shallow circular arch under pressure



Snap-Through Problems • History input for shallow circular arch *step, nlgeom loading *static, riks 0.05, 1.0, , 0.2, 0.4 *dsload arch, p, 5000. . . . *end step


L6.24


L6.25

Snap-Through Problems • Load-displacement curve of shallow arch



Postbuckling Problems



L6.27

Postbuckling Problems – The Riks method can also be used to solve postbuckling problems, both with stable and unstable postbuckling behavior. – The exact postbuckling problem cannot be analyzed directly because of the discontinuous response at the point of (bifurcation) buckling. – To analyze the problem, you must turn it into a problem with continuous response instead of bifurcation. • The problem can be converted by introducing an initial imperfection in the model so that there is some response in the buckling mode before the critical load is reached. – If the imperfection is small, the deformation will be quite small (relative to the imperfection) below the critical load.



L6.28

Postbuckling Problems – The response will grow quickly near the critical load, introducing a rapid change in behavior. • Such a rapid transition is difficult to analyze. – If the imperfection is large, the postbuckling response will grow steadily before the critical load is reached. • The transition into postbuckled behavior will be smooth and relatively easy to analyze. – Imperfections are usually introduced as perturbations in the initial geometry of the model. – Imperfections can also be introduced by perturbations in the loads or the boundary conditions. – Moreover, imperfections based on linear buckling modes can be useful for analyzing structures that behave inelastically prior to reaching peak load.



Introducing Imperfections for Postbuckling Simulations



L6.30

Introducing Imperfections for Postbuckling Simulations – Imperfections in otherwise “perfect” models are necessary to develop models that are suitable for use in postbuckling analyses. – Two methods are used to introduce imperfections into a model: 1. Geometric imperfections are the most commonly used method. Perturbations in the model’s initial geometry cause the structure to buckle in the appropriate manner. 2. Loading imperfections may also be used to ensure that the structure buckles in the appropriate manner. Small fictitious “trigger loads” are used to deform the model so that it buckles correctly.



L6.31

Introducing Imperfections for Postbuckling Simulations • Geometric imperfections: – They are typically based on previous eigenvalue buckling analyses. – A few of the buckling modes are used typically to perturb the geometry. • However, the lowest buckling modes are assumed to provide the most critical imperfections, so usually the lower modes are scaled and added to the perfect geometry to create the perturbed mesh.



L6.32

Introducing Imperfections for Postbuckling Simulations – The magnitude of the imperfection should be chosen realistically. • For example, the size of the imperfections may be determined by manufacturing tolerances. • Often the magnitude is chosen as a few percent of a relevant structural dimension such as a beam cross-section or a shell thickness. – In shells the imperfection magnitude is typically chosen to be 1%–100% of the thickness. – Only the coordinates of the nodes are affected; the nodal normals are not modified.



L6.33

Introducing Imperfections for Postbuckling Simulations • Loading imperfections: – The “trigger loads” should perturb the structure in the expected buckling modes. – Typically, these loads are applied as “dead” loads prior to the Riks step so that they have a fixed magnitude. – The magnitude must be sufficiently small so that the trigger loads do not affect the overall postbuckling solution.



L6.34

Introducing Imperfections for Postbuckling Simulations • Introducing geometric imperfections – Use the ∗IMPERFECTION option to introduce geometric imperfections for postbuckling and collapse simulations. – The geometric imperfection can be based on nodal displacements written to the results (.fil) file during a previous simulation. • The FILE parameter is used to identify the name of the results file from the previous simulation. • The STEP parameter must be used to identify the step from the previous analysis containing the results that will define the geometric imperfection. • An imperfection that uses only a subset of the model’s nodes can be created by using the optional NSET parameter to identify the subset.



L6.35

Introducing Imperfections for Postbuckling Simulations – Imperfections can be formed by the superposition of weighted eigenmodes from a previous eigenvalue buckling or frequency extraction analysis. – Any number of eigenmodes can be specified and scaled with this option. – The syntax for this case is: *IMPERFECTION, FILE=file_name, STEP=n [, NSET=name] mode_number, scale_factor

– Eigenmodes are stored such that the largest component of displacement has a magnitude of 1.0. • Therefore, they must be scaled to give an appropriate imperfection.

This option is not currently supported by ABAQUS/CAE. You may use the Keywords Editor to add it to your model, however.



L6.36

Introducing Imperfections for Postbuckling Simulations – Geometric imperfections can also be based on the scaled displacements from a previous static simulation. • Only the displacements from a single increment can be used to form the imperfection. – Use the INC parameter to identify the specific increment containing the results that will define the geometric imperfection. The syntax for this case is *IMPERFECTION, FILE=file_name, STEP=n, INC=m 1, scale_factor

First data line entry must be set to 1 in this case.



L6.37

Introducing Imperfections for Postbuckling Simulations – You can also define geometric imperfections directly with the ∗IMPERFECTION option. • By default, such imperfections are given in the global Cartesian coordinate system. • The SYSTEM parameter may be used if the imperfections are defined in an alternative coordinate system (either cylindrical or spherical). • The data for this format of the ∗IMPERFECTION option can be read from a separate file. The INPUT parameter identifies the additional file containing the imperfection data. – The syntax for this format is: *IMPERFECTION [, SYSTEM=C or S, INPUT=file_name]

node_number, U1, U2, U3

where U1, U2, and U3 are the components of the imperfection that will be added to the node’s initial position.



L6.38

Introducing Imperfections for Postbuckling Simulations – For accurate postbuckling analysis of such structures, it is important that the imperfections be chosen correctly. • The magnitudes of the imperfections should be chosen appropriately. • It is safest to introduce an imperfection of the proper magnitude consisting of several superimposed buckling modes. • The weight of the various modes must be chosen by the user; usually the lowest buckling mode should have the largest weight. • Imperfections consisting of a single buckling mode tend to yield nonconservative results.



L6.39

Introducing Imperfections for Postbuckling Simulations – No default protections are provided to check whether or not the resulting perturbed geometry is reasonable. • It is the user’s responsibility to ensure that the geometry of the model to be analyzed is representative of the problem being considered. • ABAQUS/Viewer can be used to visualize the imperfections to the model. – Likewise, no default protections are provided to check whether or not any of the applied trigger loads are reasonable. • It is the user’s responsibility to choose appropriate magnitudes and locations for such fictitious loads. – Most often, a number of analyses are carried out to investigate the sensitivity of the results to the types of imperfections used in a postbuckling calculation.



L6.40

Introducing Imperfections for Postbuckling Simulations – Certain structures (in particular thin shells) can be very imperfection sensitive. • Imperfection sensitivity means that the load-carrying capacity decreases rapidly with increased imperfection size. • The actual load-carrying capacity of such structures is usually much less than that predicted by eigenvalue buckling analysis. – Often these structures are characterized by closely spaced eigenvalues in an eigenvalue buckling analysis. • The interaction of the buckling modes causes the rapid degradation in load-carrying capacity. • Use all (or many) of the eigenmodes associated with closely spaced eigenvalues to seed the imperfection.



Postbuckling Examples



Postbuckling Examples • Example 2: Rectangular frame with point load at corner – The (lowest) critical load and buckling mode are easily obtained with the eigenvalue buckling procedure.


L6.42


L6.43

Postbuckling Examples – We use the buckling mode to introduce an imperfection with an amplitude of −0.1% of the frame height and analyze the resulting structure with the Riks method.

name of previous analysis scale factor

eigenmode



L6.44

Postbuckling Examples – The load-displacement curve is shown below:

– Since this is a nonsymmetric structure, different behavior is obtained if the sign of the imperfection is reversed. Copyright 2004 ABAQUS, Inc.


L6.45

Postbuckling Examples • Example 3: Buckling of an imperfectionsensitive cylindrical shell – Problem 1.2.6 in the ABAQUS Example Problems Manual. – Simply supported cylinder loaded by uniform, compressive axial load. – Internal pressure also applied (increases imperfection sensitivity of the cylindrical shell). – Very thin shell (t/r = 1/500). – Refined mesh: Full length model accounts for both symmetric and antisymmetric buckling modes.

Perturbed geometry of the cylindrical shell (imperfection factor = 5 × thickness for illustration only; actual imperfection factor used = .5 × thickness).



L6.46

Postbuckling Examples – Solution procedure: 1. Perform linear eigenvalue buckling analysis. 2. Introduce imperfections using different combinations of modes. – Fix imperfection size by prescribing the maximum “out-ofroundness.” 3. Postbuckling analysis using the Riks method. – Repeated eigenvalues: •

The presence of repeated eigenvalues implies there is no preferred direction.

•

The mode shapes associated with repeated eigenvalues are always the same; their phases, however, may vary between analyses (and computer platforms).



L6.47

Postbuckling Examples • As the relative phase between repeated modes changes, the imperfection and therefore the postbuckling response changes. • To overcome these problems, the phase is fixed before the postbuckling analysis is performed. • In this example, the eigenvectors associated with repeated eigenmodes are scaled such that their linear combination generates a maximum displacement of 1 on the X-axis. – A FORTRAN program is run to read the results file from the linear eigenvalue analysis to generate the imperfection: • The scale factors are computed for linear combinations of repeated eigenmodes. • The maximum “out-of-roundness” is enforced.



L6.48

Postbuckling Examples – Results: First 19 eigenvalues of the cylindrical shell. Eigenvalues of the cylindrical shell


Mode number

Eigenvalue

1

11721

2, 3

11722

4, 5

11726

6, 7

11733

8, 9

11744

10, 11

11758

12, 13

11777

14, 15

11802

16, 17

11833

18, 19

11872


L6.49

Postbuckling Examples – The buckling load is normalized with respect to the linear eigenvalue buckling load. The results when different modes are used to seed the imperfection are shown below. Normalized buckling loads Mode used to seed the imperfection

Normalized buckling load

1

0.902

2, 3

0.707

4, 5

0.480

6, 7

0.355

8, 9

0.351

10, 11

0.340

12, 13

0.306

14, 15

0.323

16, 17

0.411

18, 19

0.422

All modes (1–19)

0.352



L6.50

Postbuckling Examples • Load-displacement curve

Load displacement curve when first 19 modes are used to seed the imperfection Copyright 2004 ABAQUS, Inc.


Usage Hints



L6.52

Usage Hints – The Riks procedure works very well for problems exhibiting global snapthrough behavior. – Since the solution may pass unstable points, it is important that the residuals at the beginning of a new increment be small. • The default tolerances in ABAQUS are sufficiently tight in most cases; however, for very unstable postbuckling problems, tighter tolerances may need to be specified with the ∗CONTROLS option—particularly if the prebuckling behavior is nearly linear and very rapid stiffness changes occur near the instability point. – Even with tight controls, the procedure may fail if such a point is approached with large load increments. • Under such circumstances the load and the solution may track back to the starting point, as shown in the following figure.



L6.53

Usage Hints – Backtracking near a sharp transition:



Usage Hints – You can make the problem easier by introducing a larger imperfection into the initial model so that the nonlinearity in the overall response is less severe. – You can avoid the problem by limiting the arc length increment with ∆lmax. • If the problem has already occurred, you can correct it by using the ∗RESTART, READ, END STEP option just before the instability point to make sure that the point is approached with small arc length increments.


L6.54


L6.55

Usage Hints – The analysis of problems involving local instabilities sometimes leads to difficulties. • Such instabilities cause local growth of the solution, which may be insufficiently constrained by the algorithm. • In addition, local instabilities can be “fueled” by release of elastic energy from other parts of the structure, which makes it difficult to control the solution by changing the applied load. – Nevertheless, with careful control of the increment size, it is often possible to complete such analyses successfully.



Limitations



L6.57

Limitations – The Riks postbuckling procedure requires that the equilibrium path be continuous. • Such continuity is not present in instability problems involving loss of contact constraints, as shown below:

Snap-through of shallow, cylindrical roof under a point load applied to A



L6.58

Limitations – Loss of contact occurs as the roof snaps through. • When the contact force is zero, the roof and Point A have separated.



L6.59

Limitations – Problems with discontinuities typically occur when the load on a structure is applied by motion of a rigid surface and the structure buckles under the applied load. • Once the structure buckles away from the constraints, the solution can no longer be controlled by the applied loads and the Riks algorithm no longer has any beneficial effect. – In such cases a successful solution will be obtained only if the regular Newton algorithm is able to bridge the gap in the equilibrium path at this point. • If the jump cannot be made, the analysis may fail or backtrack. • In some cases the contact surface moves back but the structure freezes in a load-free, unstable equilibrium configuration.



Summary



L6.61

Summary – The static Riks procedure in ABAQUS is a useful tool for the analysis of snap-through and postbuckling problems. – Snap-through problems are handled with relative ease. – For postbuckling problems you must ensure that: • Suitable imperfections are introduced. • Sufficiently small load increments are chosen. – Extra tight controls may be required for very unstable postbuckling and localization problems. – For postbuckling problems involving loss of contact, the Riks method will usually not work and inertia or viscous damping forces must be introduced to stabilize the solution. • Such procedures are discussed in Lecture 7.



Workshop 6a: Cargo Crane – Riks Workshop 6b: Square Tube with Imperfections



Lecture 7

Damped Static Postbuckling Analysis



Overview • Motivation • Automatic Stabilization and Dashpots • Postbuckling and Loss of Contact • Example • Summary • Workshop 7a: Cargo Crane – Damped Static Analysis • Workshop 7b: Cargo Crane – Dynamic Analysis


L7.2


Motivation



L7.4

Motivation – To obtain an accurate assessment of the postbuckling behavior of structures, static analysis methods are preferred because they provide insight into the postbuckling characteristics of the structure. – However, it is not always possible to carry out such an analysis: in situations where loss of contact occurs or where the deformation localizes, the static postbuckling method may fail to yield a solution. • In such cases a transient analysis can be done, either dynamically or statically with viscous forces.



L7.5

Motivation – The addition of inertial forces provides a solution to the physical postbuckling behavior. – However, it is not always required or even desired that the actual dynamic solution be obtained. • In many cases the objective of the analysis is not to simulate the actual dynamic response but to obtain the static equilibrium state after buckling. – In some cases, such as in automotive roof crush or side intrusion calculations, elastic buckling is only an initial effect that is followed by extensive bending and plastic deformation.



L7.6

Motivation – In such cases a more effective and less “noisy” solution may be obtained through the addition of suitable “damping” forces in a static analysis. – There are two ways in which damping can be introduced in a static analysis: • Damping can be introduced using automatic viscous damping with the ABAQUS static procedure options. • Alternatively, discrete dashpots can be added to the model. – Element type DASHPOT1 can be used to damp absolute motions. – Element type DASHPOT2 can be used to damp relative motions.



L7.7

Motivation – If damping is used in static analysis, the velocity is assumed to be equal to the displacement increment divided by the time increment. – Assume that the cumulative effect of all damping added to the static model is described by the damping matrix C. – The equilibrium equations can then be written in the form

Cu& + I = C ∆u / ∆t + I = P. – In linearized form this becomes

1    K + ∆t C  cu = P − I − C ∆u / ∆t. – It is clear that the damping matrix becomes more important when the time increment decreases.



Automatic Stabilization and Dashpots



L7.9

Automatic Stabilization and Dashpots – When damping is applied through the automatic stabilization procedure, ABAQUS builds a volume proportional damping matrix:

C = cM1, where

M1 = mass matrix with unit density and c = damping factor. – ABAQUS automatically determines the damping factor, c, based on the following premises: • The model’s response in the first increment of a step to which stabilizing damping is applied is stable. • Under stable circumstances the amount of dissipated energy should be very small.



L7.10

Automatic Stabilization and Dashpots – This is accomplished as follows: • During the first increment of the step, calculations are made of the strain and dissipation energies. • These energies are extrapolated to the time scale of the step, as if the solution were to be scaled linearly in time. • The damping factor, c, is determined in such a way that if the solution were linear, the viscous dissipation energy would be a small fraction of the model’s strain energy at the end of the step. • This small fraction, called the dissipation intensity, a, is controlled by the user. – It has a default value of 2 ×10−4.



L7.11

Automatic Stabilization and Dashpots – Alternatively, the user may specify the damping factor directly. – Since c is related to the model size and material stiffness in nonobvious ways, it may be difficult to choose a proper value. • Initiate a run without explicit declaration of a damping factor. • ABAQUS prints out the value of the damping factor, which can then be used as a guideline for selecting appropriate values.



L7.12

Automatic Stabilization and Dashpots – There are cases where the first increment is either unstable or singular (e.g., due to a rigid body mode). • In such cases it is not possible to obtain a solution in the first increment without damping. • ABAQUS precomputes the damping factor based on a sampling of the average element stiffness. • If the calculated strain energy in the first increment indicates the solution without damping is stable, the damping factor is recalculated as described earlier; otherwise, the initially calculated factor is maintained. – Warning: The damping factor may be stronger than desired; critically review the solution.



L7.13

Automatic Stabilization and Dashpots • ABAQUS usage: Automatic stabilization – Automatic stabilization can be added in the following quasi-static procedures in ABAQUS: *STATIC *VISCO *COUPLED TEMPERATURE-DISPLACEMENT *SOILS, CONSOLIDATION

– It is specified by including the STABILIZE parameter on the procedure option. – In addition, the FACTOR parameter can also be included on the procedure option.



Automatic Stabilization and Dashpots – For example, *STATIC, STABILIZE

or *STATIC, STABILIZE=

dissipated energy fraction

or *STATIC, STABILIZE, FACTOR=

damping factor


L7.14


L7.15

Automatic Stabilization and Dashpots – Volume proportional damping can be activated during any step of an analysis. • The values of the damping coefficient are not carried from one step to the next. • They are deactivated if the STABILIZE parameter is not re-declared and recalculated if this parameter is re-declared.



Automatic Stabilization and Dashpots • Output variables: Automatic stabilization – The total amount of viscous energy dissipated by volume proportional damping is reported separately from other viscous dissipation energies by means of the element output variables ELSD and ESDDEN and the global energy variable ALLSD. • Use the ∗ENERGY OUTPUT or ∗ENERGY PRINT option to request this output. • The reported energy can be limited to a group of elements.


L7.16


L7.17

Automatic Stabilization and Dashpots – The nodal viscous forces and moments are available as nodal output variable VF (VFn and VMn). – The damping factor calculated by ABAQUS is reported in the message (.msg) file.



L7.18

Automatic Stabilization and Dashpots

ELSD ELSDDN ALLSD Not output by default to .odb file!

Element stabilization dissipation energy Element stabilization dissipation energy density Element set or model stabilization dissipation energy

VF

Nodal viscous forces

c

Damping factor (message file)



L7.19

Automatic Stabilization and Dashpots • If you want to know how much you altered a problem by adding stabilization, look at: 1

Energy dissipation due to stabilization • Look at whole model energies.

Here, the total energy dissipated due to stabilization is very small compared to the total energies involved in deformation.

VF



L7.20

Automatic Stabilization and Dashpots 2 Viscous forces during deformation

10000

• The figures at right show the load and viscous forces at the load application point as functions of displacement • VF varies significantly in time; its order-of-magnitude is very small compared to the global load, however. • Can conclude the presence of stabilization has not changed the problem significantly.


1.5


L7.21

Automatic Stabilization and Dashpots • Automatic stabilization usage hints – The automatic calculation of the damping factor, c, is done based on information obtained during the first increment of a step. • Thus, the first increment should be representative of the deformation pattern that follows. • If the character of the deformation changes during the step, split the step to force a reevaluation of damping. – If the first part of the step can be completed without stabilization, it is better to split the step and introduce stabilization in the latter steps. • This ensures that a stable response is the basis for computing the damping factor.



L7.22

Automatic Stabilization and Dashpots • Dashpot usage hints – To select the damping coefficients in the dashpots, the following procedure can be used: • Estimate the magnitude of the displacements that will occur after buckling. • Divide the estimated displacement magnitude by the step time to get an estimate for the velocity that would occur if the response were stable. • Determine typical nodal forces in the model prior to buckling. • Choose the damping coefficients such that, for the estimated velocity, the damping forces will be one to two orders of magnitude less than the static forces.



L7.23

Automatic Stabilization and Dashpots • Dashpot output variables – The total viscous energy dissipated by dashpots is included in the global energy variable ALLVD. – The viscous forces in the dashpots are reported as element variable S11.



L7.24

Automatic Stabilization and Dashpots • Summary – The methods described on the previous pages will have the result that, prior to buckling, the damping has almost no effect on the solution. • However, as soon as instability in the structure develops, the velocities increase rapidly and damping starts to become effective. • For the solution procedure to converge, the time increment will usually decrease as the velocities increase, leading to a controlled postbuckling behavior. – Damping in a static analysis should not be combined with the Riks procedure. • The Riks procedure will calculate the velocities as displacement increments divided by the arc length; hence, these pseudo-velocities will not increase sufficiently for the dashpots to become effective.



L7.25

Automatic Stabilization and Dashpots • Example 1: Damped static postbuckling analysis – As an example of dynamic postbuckling, consider this frame structure. • This structure can also be analyzed with the quasi-static method. – The structure is expected to buckle at a load of about 57,500 lbs.



L7.26

Automatic Stabilization and Dashpots – To investigate the postbuckling behavior, we apply a load of 150,000 lbs. – The load-displacement curve obtained with the Riks quasi-static method and the deformed shape at approximately 250,000 lbs are shown below:

Buckling occurs here

unstable stable



L7.27

Automatic Stabilization and Dashpots – To analyze the problem as a damped static problem, we add DASHPOT1 elements to every single node in degree of freedom 1 and 2. • To calculate a damping value for the dashpots, we estimate typical nodal forces on the order of 10,000 lbs. • Considering that the load is applied over a period of 10 sec and the total deflection is on the order of 100 in, a typical constant velocity to attain the total deformation would be about 10 in/sec. – With these assumptions the damping coefficient corresponding to the velocity would be 1000 lb sec/in. • We choose 1% of this value as the actual damping coefficient. – The partial input for this problem follows; the load-deflection and energydeflection curves are shown on the subsequent pages.



Automatic Stabilization and Dashpots • Damped static postbuckling analysis: partial input *Heading Frame -- damped static postbuckling analysis : *Imperfection, file=framEigen, step=1 1, -0.12 *Boundary ends, 1, 2 *Element, type=dashpot1 : *Dashpot, elset=dashpotx : *Dashpot, elset=dashpoty : *Step, nlgeom, inc=400 *Static 0.1, 10., , 0.25 *Cload corner, 2, -200000. *End step


L7.28


L7.29

Automatic Stabilization and Dashpots • Damped static postbuckling analysis: results

Snap-through

Instability starts here

Load-displacement curve

Energy-displacement curve



L7.30

Automatic Stabilization and Dashpots – As can be seen from the load-displacement curve, the load increases until the instability develops. – When the instability develops, the load remains almost constant while the structure snaps through to a stable state. – The final deformed shape of the frame is in static equilibrium without significant forces in the dashpots and agrees with the solution obtained with the Riks method. – The energy curves show how the strain energy stored in the structure is released in the form of dissipated energy when the snap-through occurs.



L7.31

Automatic Stabilization and Dashpots • Example 2: Stabilized static postbuckling analysis – The same problem is repeated with the dashpots replaced by volume proportional damping. – The problem is run with a dissipation intensity two orders of magnitude smaller than the default. • The default value is too high, because the first increment of the analysis captures essentially axial deformation of the vertical member of the structure. • Later on, the snap-through behavior is dominated by bending of the structure. • Since the bending behavior is much less stiff than the axial behavior, a small fraction of the axial strain energy is still relatively high when compared with the bending strain energy.



Automatic Stabilization and Dashpots • Stabilized static postbuckling analysis: partial input *Heading Frame -- stabilized static postbuckling analysis : : *Imperfection, file=framEigen, step=1 1, -0.12 *Boundary ends, 1, 2 *Step, nlgeom, inc=400 *Static, stabilize=2.e-6 0.1, 10., , 0.25 *Cload corner, 2, -200000. *End step


L7.32


L7.33

Automatic Stabilization and Dashpots • Stabilized static postbuckling analysis: results

Snap-through

Load-displacement curve

Energy-displacement curve



L7.34

Automatic Stabilization and Dashpots – Both the load-displacement curves and the energy curves are very similar to those in the static analysis damped with dashpots. • The amount of damping was somewhat less than in the dashpot case and can be controlled with the dissipation intensity.



Postbuckling and Loss of Contact



L7.36

Postbuckling and Loss of Contact – Often buckling and postbuckling problems are driven by moving contact surfaces, and the structure buckles away from the contact surface. – As discussed in Lecture 6, the Riks method is not able to analyze this kind of problem. – This kind of discontinuity does not present problems for damped static analysis. – At the load level at which contact is lost, the structure deforms without being moved by the boundary conditions, and the inertia and viscous forces ensure that the solution does not diverge.



L7.37

Postbuckling and Loss of Contact • Example 3: Stabilization static snap-through analysis with contact



Postbuckling and Loss of Contact – The contact load and the sum of reaction forces as a function of the prescribed displacement are shown below.


L7.38


Example



L7.40

Example • Local buckling of reinforced plate – Plate with small and large reinforcements – Spring connections to the rest of the structure and symmetry boundary conditions – Linear elastic material – Axial loading

Courtesy of IRCN-France



L7.41

Example – First, localized buckling occurs in the plate sections between the small reinforcements.

– Then, buckling of a line of sections and small reinforcements occurs corresponding to the maximum load carrying capacity. – Total collapse of the plate follows.

global buckling

Contours of localized plate section buckling (displacements normal to structure)

Buckling of a line of sections in the structure



L7.42

Example

Buckling of line of sections (loss of load-carrying capacity) Local plate buckling

Axial force vs. axial displacement


Energy history plots


Summary



L7.44

Summary – Damped static postbuckling analysis is a useful technique to complement classical eigenvalue buckling and static postbuckling analysis with the Riks method. – The primary advantage of this method is the reliability it offers, in particular in conjunction with contact changes. – Like static postbuckling analysis, the method provides an accurate estimate of the critical load of imperfect structures, even if the structures are imperfection sensitive. – Unlike static postbuckling analysis, however, it does not provide detailed insight into the nature of the postbuckling behavior.



L7.45

Summary – The method is often useful for the analysis of crash and crushing problems. • In such problems buckling of the structure away from an indenter may occur in the early phases of analysis, prior to large scale plastic deformation. • In such cases the postbuckling behavior is not the primary interest. – The damped analysis technique regularizes this initial instability and enables the analysis to proceed quickly to the deformation phase that is of primary interest. • The local contact surface damping option is provided specifically for such applications.



Workshop 7a: Cargo Crane – Damped Static Analysis Workshop 7b: Cargo Crane – Dynamic Analysis



Lecture 8

Introduction to Contact in ABAQUS/Standard



L8.2

Overview • Introduction

• Contact Output

• Contact Examples

• Solution of Contact Analyses

• Contact in Finite Element Analysis

• Some Important Contact Issues

• Strict Master/Slave Contact

• Workshop 8a: Hinge Model

• Overview of Defining Two-surface Contact

• Workshop 8b: Clip and Plate Model

• Surface Definition • Adjusting Surfaces • Local Surface Behavior • Relative Sliding of Points in Contact



Introduction



Introduction – When two solid bodies touch, contact stress is transmitted across their common surface. • In some cases only normal stress is transmitted. • If friction is present, a limited amount of shear stress can also be transmitted. • The general objective is to determine contacting areas and stress transmitted. – Contact is a severely discontinuous form of nonlinearity. • The contact constraint is either active or inactive—it is not smoothly varying.


L8.4


Contact Examples



Contact Examples – Hertz contact • Small displacements of the contact surfaces relative to each other. • Contact over a distributed surface area.


L8.6


L8.7

Contact Examples – Deformable to rigid body contact • Typical examples: – Rubber seals – Tire on road – Pipeline on seabed – Forming simulations (rigid die/mold, deformable component).

Example: metal forming simulation

Video Clip



L8.8

Contact Examples – Large-sliding contact between deformable bodies • This is the most general category of contact. • Example: threaded connector.

Contact pressure distribution due to interference resolution



L8.9

Contact Examples – Self-contact SURF1 (rigid)

• Self-contact is contact of a single surface with itself. It is available in two- and threedimensional models in ABAQUS.

SURF2

Contour of minimum principal stress Example: Compression of a rubber gasket (taken from “Self-contact in rubber/foam components: rubber gasket,” Example Problem 1.1.17 in the ABAQUS Example Problems Manual)



Contact in Finite Element Analysis



L8.11

Contact in Finite Element Analysis – Finite elements are based on the concept of “local support”—nodes and elements communicate with their nearest neighbors.

Exploded view of a mesh: center element communicates with its neighbors through its nodes



L8.12

Contact in Finite Element Analysis • Why is it necessary to define contact? – The concept of local support is not sufficient for contact problems. • Points and surfaces on one body may need to recognize points and surfaces on other bodies. – There is currently no logic in ABAQUS/Standard to detect contact unless the user indicates that specified surfaces and/or nodes might come into contact. • The surface of one body cannot penetrate the surface of another body (or itself if it folds).


The example shown here comes from “Submodeling of a stacked sheet metal assembly,” Section 1.1.18 of the ABAQUS Example Problems Manual.


Strict Master/Slave Contact



L8.14

Strict Master/Slave Contact • Contact surfaces must be discretized because the underlying bodies are discretized. • With strict master/slave contact: – Nodes on one surface (the slave surface) contact the discretized segments on the other surface (the master surface).



L8.15

Strict Master/Slave Contact • The strict master/slave formulation used in ABAQUS/Standard has kinematic implications. – Slave nodes cannot penetrate master surface segments. – Nodes on the master surface can penetrate slave surface segments.



L8.16

Strict Master/Slave Contact • Approaches to master/slave contact – Node-to-surface • Contact is enforced between the slave node and the master surface facets local to the slave node • Default method for contact interactions

slave

master These nodes are free to penetrate



L8.17

Strict Master/Slave Contact – Surface-to-surface • Contact is enforced in a weighted sense, between the slave node and a larger number of master surface facets surrounding it. slave

master

More master surface nodes are involved in contact, reducing the likelihood of penetration.

• In effect, contact is smeared over a larger number of facets. – Analogous to converting the slave contact force to a local surface pressure and applying that pressure to the master surface. • Alternative for small sliding contact; default for tie constraints.



L8.18

Strict Master/Slave Contact • Choice of master and slave surfaces – The proper choice of master and slave surfaces is critical. • Slave surfaces allow penetration; master surfaces do not. • With the keywords interface, the slave surface is the first surface named under the *CONTACT PAIR option: *CONTACT PAIR, INTERACTION=EXAMPLE

slave, master

With the GUI interface, the slave and master surfaces are specified explicitly.



L8.19

Strict Master/Slave Contact • Mesh density considerations – Choose slave surfaces to be the more finely meshed surface. – If mesh densities are equal, the slave surface should be the surface with the softer underlying material.

Incorrect Master surface placed on fine mesh⇒ Gross penetration into slave surface

Correct Master surface placed on coarse mesh⇒ Minimal penetration into slave surface



Overview of Defining Two-surface Contact



L8.21

Overview of Defining Two-surface Contact – For even the simplest contact problem the user must decide: • What constitutes each surface. • Which pairs of surfaces will interact. • Which surface is the master, and which is the slave. • Which surface interaction properties are relevant: friction, softened layers, etc. – ABAQUS automatically creates internal contact elements based on these decisions. – These internal elements are almost completely transparent to the user. • The only time a user will typically want to review these elements is when something goes wrong.



L8.22

Overview of Defining Two-surface Contact • Defining a contact interaction in ABAQUS/CAE 1 Create an interaction, and

select the steps in which it will be active.

Create Interaction dialog box



L8.23

Overview of Defining Two-surface Contact 2 Select the application surfaces

from geometric surfaces, element faces, surface sets, or node sets. Surfaces on orphan meshes can be selected by picking one element face and a feature angle. Individual edits make it easy to clean up anomalies.



L8.24

Overview of Defining Two-surface Contact 3 In the Edit Interaction dialog

box, complete the interaction definition (for example, for contact interactions define the friction model).

Create Interaction Property dialog box Copyright 2005 ABAQUS, Inc.

Edit Interaction dialog box


L8.25

Overview of Defining Two-surface Contact 4 Use the Interaction Manager to manage multiple contact

interactions as necessary.

Interaction Manager



Surface Definition



L8.27

Surface Definition • User-specified contact faces: GUI interface Solid bodies – The surface on a solid is defined by selecting the appropriate region of the exterior of the part. – Regions may be selected individually or based on face angles.



Surface Definition • User-specified contact faces: GUI interface (cont'd) Shells and beams The surface on a shell/membrane or beam/truss is defined by choosing the appropriate side of the part.


L8.28


Adjusting Surfaces



L8.30

Adjusting Surfaces – The slave nodes of any contact pair can be “adjusted” automatically so that they are initially in contact with the master surface. • This process is useful when preprocessors do not place nodes in “exact” positions. • ABAQUS modifies coordinates of slave nodes before the analysis starts. • The adjustment does not generate any strain.



L8.31

Adjusting Surfaces – The initial positions of the nodes on the contact surfaces can be adjusted without stress or strain prior to the analysis. • ABAQUS/Standard allows the user to adjust the nodes by specifying either – an absolute distance or – a node set. – Warning: With either method only surface nodes are relocated. • Gross (large) adjustments can severely distort initial element shapes.



L8.32

Adjusting Surfaces

1.0 CONNODE



Local Surface Behavior



Local Surface Behavior – General contact modeling includes contact interactions in directions: • Normal to the master surface • Tangent to the surfaces – Other contact interactions include contact damping.


L8.34


L8.35

Local Surface Behavior • Behavior in the contact normal direction • Hard contact – “Hard” contact is the default local behavior in all contact problems.

Pressure-clearance relationship



L8.36

Local Surface Behavior – Alternatives to hard contact • Contact without separation. • Softened contact (exponential or tabular pressure-clearance relationship)

Contact with separation


“Soft” contact


L8.37

Local Surface Behavior – Behavior in the contact tangential direction • Frictional shear stresses, τ, may develop at the interface between contacting bodies. • If the magnitude reaches a critical value, the bodies will slip; otherwise they will stick. – Friction is a highly nonlinear effect. • Solutions are more difficult to obtain. • Do not use unless physically important.



L8.38

Local Surface Behavior – Four friction models are available in ABAQUS: • Isotropic Coulomb friction (with shear stress cap) • Anisotropic Coulomb friction (with shear stress cap) • Exponential form where µs decays to µk exponentially • User-defined (through user subroutine FRIC or UINTER) – Two friction algorithms are implemented: • Penalty method • Lagrange multiplier method – The most common (and default) combination is isotropic Coulomb friction using the penalty method.



L8.39

Local Surface Behavior – Default Coulomb friction model • The critical frictional stress depends on contact pressure: τcr = µp. • The friction coefficient, µ, can be a function of the relative slip velocity, pressure, temperature,



L8.40

Local Surface Behavior – By default, ABAQUS uses an adaptive penalty method.

τcrit

• It approximates stick with stiff elastic behavior. • Small elastic slip, γcrit, is permitted before τeq = τcrit.

ideal penalty

G


γcrit


L8.41

Local Surface Behavior



Relative Sliding of Points in Contact



L8.43

Relative Sliding of Points in Contact • Two slide distance options: – Finite sliding

Finite sliding is the most general—used by default. Arbitrarily large sliding between surfaces and large rotations are allowed.

– Small-sliding

Small relative sliding between surfaces. Allows large rotations of the surfaces, as long as the surfaces do not move significantly relative to each other. Computationally less expensive than finite sliding.

• While small-sliding is less expensive, take care to use it only in cases where small tangential motions are expected – Non-physical behaviour can result if it is used inappropriately



L8.44

Relative Sliding of Points in Contact

Edit Interaction dialog box Copyright 2005 ABAQUS, Inc.


Contact Output



Contact Output • Contact information is available for all surfaces. – Contact stresses: CSTRESS (contact pressure CPRESS and frictional shear stresses CSHEAR1 and CSHEAR2) – Contact displacements: CDISP (contact opening COPEN, relative tangential motions CSLIP1 and CSLIP2)


L8.46


L8.47

Contact Output • Field output requests

CPRESS, CSHEAR1, and CSHEAR2 COPEN, CSLIP1, and CSLIP2



Contact Output – Solver contact output • Controls output to the message file during the analysis phase. • Gives details of the iteration process. • Use to understand where difficulties are occurring during contact.

Activate in the Edit Diagnostic Print dialog box of the Step module Copyright 2005 ABAQUS, Inc.

L8.48


Solution of Contact Analyses



L8.50

Solution of Contact Analyses • Contact requires the imposition of constraints between the points that are in contact. – Different ways of imposing constraints. – ABAQUS/Standard uses the Lagrange multiplier method. – For each potential contact point the contact condition is described by a single, often nonlinear, inequality constraint:

h(u1 , u 2 , u 3 , ...) ≤ 0, where h is the “penetration” and uN are degrees of freedom.



L8.51

Solution of Contact Analyses • Contact algorithm h≤0 2

determine contact state

1

begin increment open do not apply constraint

2

3

5

point opens; severe discontinuity iteration

h>0

closed apply constraint

perform iteration 5

p<0

4

check for changes in contact

point closes; severe discontinuity iteration

h>0

no changes end increment 8

6

convergence

check equilibrium

7

no convergence



L8.52

Solution of Contact Analyses – The algorithm distinguishes between “severe discontinuity iterations” and “equilibrium iterations” and can be described as follows: 1 Determine current contact state at each point (closed or

open). 2 Impose contact constraints, calculate stiffness. 3 Perform iteration ⇒ pass through the solver once. 4 Contact pressures and clearances consistent with contact

state? If yes, go to 6. If no, go to 5.

– Point was closed; confirm that p > 0. – Point was open; confirm that h < 0.



L8.53

Solution of Contact Analyses 5 Contact state changed: the start of the iteration was

based on the wrong state.

– Flag the point as having an incorrect contact estimate. – Label and count this iteration as an SDI (severe discontinuity iteration). – Reset equilibrium iteration counter to zero. Go back to 1. 6 After all SDIs, check force residuals to determine

equilibrium.

– Label and count this iteration as an equilibrium iteration. 7 If equilibrium is not satisfied, iterate again with the same contact state. Go to 3. 8 If equilibrium is satisfied, the increment ends.



Solution of Contact Analyses • Contact diagnostics example – Reference: Example Problem 1.3.4, Deep drawing of a cylindrical cup


L8.54


L8.55

Solution of Contact Analyses – Visual diagnostics are available in the Visualization module of ABAQUS/CAE.

Step 3, Increment 6: 4 SDIs + 2 equilibrium iterations

Visualization module: Tools Job Diagnostics Copyright 2005 ABAQUS, Inc.


L8.56


Slave nodes that close: h > 0

Toggle on to see the locations in the model where the contact state is changing.



L8.57


Slave nodes that open: p < 0



L8.58


Slave nodes that slip; stick/slip messages cause SDIs only if the Lagrange multiplier method is used.



L8.59


There are no residual checks in this iteration since the contact consistency checks did not pass.



L8.60

Solution of Contact Analyses 3 additional SDIs are required before the contact state is established; once the contact checks pass, the residuals checks are performed.



Some Important Contact Issues



L8.62

Some Important Contact Issues • Contact is an extremely discontinuous form of nonlinearity – During solution of contact problems, ABAQUS has to perform iterations to resolve the correct contact state, ie • which nodes are in contact and what the contact pressures are • which nodes are not in contact – This adds another level of complexity to the solution process • Contact problems in general require more CPU time to solve



L8.63

Some Important Contact Issues • Contact with Friction – Friction is a highly nonlinear effect. • Solutions are more difficult to obtain. • Do not use unless physically important. – Friction is nonconservative ⇒ unsymmetric equation system. • ABAQUS/Standard will automatically use the unsymmetric solver when µ > 0.2 or when contact pressure dependency is detected. • The unsymmetric solver will be used for the entire analysis.



L8.64

Some Important Contact Issues F1

• Rigid body motion – Many mechanical assemblies use contact between bodies to prevent rigid body motions. – This is not effective until the bodies are actually in contact. – If loads are applied to the body, typically a singular system is produced, with unbounded rigid body motion resulting. – Can add stabilization to help in such cases: • Contact pair damping • Automatic viscous damping (whole model)


F2

F1


L8.65

Some Important Contact Issues • Overconstraining the model – A slave node involved in contact is subject to contact constraints. – The user should be careful not to overconstrain a slave surface: • A particular slave surface should only be paired with one master surface (it cannot be slave to two masters). • Do not apply boundary conditions or other constraints to nodes on the slave surface – Overconstraining the model can lead to non-convergence or unreliable results

master surface 1

slave node

master surface 2

Slave node is overconstrained



Workshop 8a: Hinge Model Workshop 8b: Clip and Plate Model



L8.67

Workshop 8a: Hinge Model



Workshop 8b: Clip and Plate Model


L8.68


Lecture 9

Bolted Connection Modeling



Overview • Modeling Bolted Connections • Mesh-Independent Point Fasteners • Beam + Coupling Technique • Modeling Bolts with Solid Elements • Bolt Pre-tension Loads


L9.2


L9.3

Modeling Bolted Connections • Modeling bolted connections usually involves: – Modeling the bolts and their interaction with the bolted components; and – Modeling contact between the bolted components • Contact between the components is achieved through surface-to-surface contact, as usual • Several modeling techniques are available for considering the bolts and their interactions with the other components. – The appropriate choice of modeling technique depends on the desired outcomes of the analysis. For example: – Is it sufficient to have correct load transfer across the joint? – Or are accurate local stress solutions require in and around the bolts? • In this lecture, we aim to give a brief overview of some common modeling techniques Copyright 2004 ABAQUS, Inc.


L9.4

Modeling Bolted Connections

– Rigid or deformable point fasteners (ignores holes in parent components) – Deformable beam fasteners with couplings

Coarse system models Not interested in local detail, just overall load transfer

– Deformable solid fasteners with tie constraints – Deformable solid fasteners with threaded bolt interaction capability (new in v6.6) – Deformable solid fasteners with detailed thread modeling

Detailed component models Interested in accurate local results in vicinity of bolts



Mesh-Independent Point Fasteners



L9.6

Mesh-Independent Point Fasteners • Mesh-independent point fasteners allow you to conveniently define point-topoint connections between surfaces. – They can be located anywhere between surfaces. • They need not be defined at nodal locations. – They can connect multiple layers;

multiple surfaces attachment points

• i.e., the number of connected surfaces is not restricted. – The fastener acts over a specified radius of influence. – The meshes on the surface do not need to match


radius of influence


L9.7

Mesh-Independent Point Fasteners – The fastener capability combines either: • connector elements or • beam multi-point constraints

coupling constraint

with distributing coupling constraints to define a connection. connector element or MPC

– Translation and rotation of the attachment points are related to the translation of nodes on the shell surface.

– Fasteners can model either rigid, elastic, or inelastic connections with failure by using the generality of connector behavior definitions. – Fasteners are not currently supported by ABAQUS/CAE



L9.8

Mesh-Independent Point Fasteners • Example: Rail crush with fasteners

Video Clip

Nodes involved in couplings for mesh-independent fasteners


Fasteners


L9.9

Mesh-Independent Point Fasteners • A major advantage of mesh-independent fasteners is that the necessary elements and couplings are generated automatically by ABAQUS – The user need only define: • The coordinates of a single point to locate each fastener • The properties to be used for the fasteners (eg rigid, deformable, failure, etc.) • This is only a very brief description of mesh-independent fasteners • For more detailed information, see – Section 20.3.4 in the ABAQUS Analysis User’s Manual, “Meshindependent fasteners” – Section 1.2.3 in the ABAQUS Example Problems Manual, “Buckling of a column with spot welds”



Beam + Coupling Technique



L9.11

Beam + Coupling Technique • This is quite a common technique for approximating a bolted connection • Similar to the mesh-independent point fastener technique, but requires more manual work

manually defined coupling constraint

– Manually create beam elements to approximate the bolts – Connect the ends of the beams to the circumference of the hole using coupling constraints (manually defined) – Commonly used in joining components modeled with shell elements, where the holes are included

manually created beam element



Modeling Bolts with Solid Elements



L9.13

Modeling Bolts with Solid Elements • If accurate local stress solution is required in and around the bolt, use a detailed component model

Contact pressure distribution due to interference resolution



Modeling Bolts with Solid Elements • Detailed component models are good for local stress analysis – Can give good accuracy of local stress and contact pressure on threads • However, they are computationally expensive – All components are modeled as deformable bodies – 3D finite-sliding contact with friction – Threads must be meshed quite finely ⇒ large model


L9.14


L9.15

Modeling Bolts with Solid Elements • Coarse system model approach – Only remote stresses in the bolted components are of interest (not detailed local stresses around the bolt) – The bolt and other components are still modeled with solid elements – The bolt thread interaction is approximated by tie constraints – A much coarser mesh can be used for the bolt • The advantages with this technique are – Good for fast system response – Low computational effort – Ease of modeling

These pairs of surfaces are Tied to approximate the meshed threads Copyright 2004 ABAQUS, Inc.


Modeling Bolts with Solid Elements • Tie Constraints – A tie constraint provides a simple way to bond surfaces together permanently. – Surface-based constraint using a master-slave formulation. – The constraint prevents slave nodes from separating or sliding relative to the master surface. – Boundary conditions should not be applied to the nodes on the slave surface of a tie constraint pair; doing so will overconstrain the model at those nodes.


L9.16


L9.17

Modeling Bolts with Solid Elements *TIE,NAME=TubePlateTie, POSITION TOLERANCE=0.01, ADJUST=YES Surface-based constraint. (Can select either predefined surfaces or regions directly in the viewport.) The surface-to-surface method is used by default Only slave nodes within this distance from the master surface are tied to the master surface. Both translational and rotational degrees of freedom can be constrained.

Warnings will be issued in the data (.dat) file for these nodes.

Slave nodes can be moved onto the master surface in the initial configuration without any strain.



L9.18

Modeling Bolts with Solid Elements • Starting in V6.6, ABAQUS provides a new threaded bolt interaction capability • Provides accurate detailed response within a system model framework

Bolt Tension Axial force

– Compromise between meshing and ignoring threads

Radial force

– Mesh-independent surface interaction using bolt-thread specification – Capture 3-D thread interactions • Frictional contact at thread angle (axial and radial) • Model radial spread and load due to axial bolt load • Asymmetric torsion response due to thread helix angle


Bolt

Bolt hole


L9.19

Modeling Bolts with Solid Elements • Supported through ABAQUS/CAE as an extension of surface-to-surface contact • User enters common bolt parameters to define the interaction, such as – Clearance region on slave surface – Bolt direction vector – Half-thread angle – Pitch – Bolt diameter



Modeling Bolts with Solid Elements • Example comparison (Mises stress)


L9.20


L9.21

Modeling Bolts with Solid Elements • Total axial load – differ by 2.3% Axial bolt load versus engaged threads

45 38.7

Axial load in bolt (% of total)

40 35

34.8

30 25 20 Meshed threads New bolt feature

15.6 14.0

15

10.1 9.9

10

8.1

7.7

6.2

6.1

5.1

4.8

5

4.3

4.2

0 1

2

3

4

5

Number of engaged threads



Bolt Pre-tension Loads


6

7


L9.23

Bolt Pre-tension Loads – The pre-tensioning capability can be used to simulate the tightening of fasteners that are used to assemble a structure. – A fastener is identified by means of a pre-tension section, across which a desired load is applied to tighten the fastener.

bolt pre-tension section

gasket A

Example of a fastener



L9.24

Bolt Pre-tension Loads – The pre-tension section is controlled with a “pre-tension node” that has only one degree of freedom and is used to: • apply a load across the pre-tension section; or to • apply a tightening adjustment (displacement) of the pre-tension section, which also results in a preload of the fastener; and to • maintain the tightening adjustment so that the load across the fastener can increase or decrease upon loading of the entire structure. – The load or tightening adjustment acts along the normal to the pre-tension section. – Use concentrated loads to prescribe a pre-tension load at the pre-tension node. – Use boundary conditions to prescribe a pre-tension tightening or to maintain the pre-tension adjustment during further analysis.



L9.25

Bolt Pre-tension Loads – The total force transmitted over the pre-tension section is the sum of the reaction force (identified as RF1) at the pre-tension node, plus any concentrated load (identified as CF1) at that node. • The stress distribution across the pre-tension section can be obtained from the underlying elements. – The tightening of the pre-tension section appears as the U1 displacement of the pre-tension node. – Pre-tension sections can be defined in fasteners modeled with: • Continuum elements • Beam or truss elements



L9.26

Bolt Pre-tension Loads • Fastener modeled with beam or truss elements – If a beam or truss element is used to model the fastener, the pre-tension section is chosen to be inside an element. • The pre-tension direction points from the first node of the element to the last node (following the element connectivity).


n 2 beam or truss element

1 pre-tension node

∗

pre-tension section


L9.27

Bolt Pre-tension Loads – The normal n to the pre-tension section: • Is by default a unit vector oriented from the first node to the last node of the element • Can be given directly by the user • Remains fixed, even for large displacement analysis



L9.28

Bolt Pre-tension Loads • Fastener modeled with continuum elements – If continuum elements are used to model the fastener, the pre-tension section is defined with a surface across the fastener.

n

pre-tension node pre-tension section

elements chosen by user to describe the pre-tension section



L9.29

Bolt Pre-tension Loads – The pre-tension section: • Does not have to be continuous. • May be connected to elements other than continuum elements as long as only continuum elements are used to define the pre-tension section. – The normal n to the pre-tension section: • By default is oriented in the direction of the positive surface normal. • May be given directly by the user. – Hence, the pre-tension section does not have to be orthogonal to the pre-tension direction. • Remains fixed, even for large-displacement applications.



L9.30

Bolt Pre-tension Loads • Usage in ABAQUS/CAE

Create a new bolt load


Select an internal surface for the pretension section

Choose how to specify the pre-tension


L9.31

Bolt Pre-tension Loads • In subsequent steps, you can modify the bolt load – Option to fix the bolt at its current length – This maintains the initial adjustment of the pre-tension section by fixing the degrees of freedom at their current values – This technique enables the load across the pre-tension section to change according to the externally applied loads. – If the initial adjustment of a section is not maintained, the force in the fastener will remain constant.



L9.32

Bolt Pre-tension Loads • Example: Bolted pipe joint – A pre-tension load of 15 kN is applied across the bolt to place the gasket under compression. flange

gasket bolt

Assembly load between bolt, flange, and gasket



Bolt Pre-tension Loads – Contour of stress S22


L9.33

Unioni bullonate con Abaqus

Recommend Documents