An analysis history is defined in ABAQUS by:
dividing the problem history into steps;
specifying an analysis procedure for each step; and
prescribing loads, boundary conditions, and output requests for each step.
A basic concept in ABAQUS is the division of the problem history into steps. A step is any convenient phase of the history—a thermal transient, a creep hold, a dynamic transient, etc. In its simplest form a step can be just a static analysis in ABAQUS/Standard of a load change from one magnitude to another. You can provide a description of each step that will appear in the data (.dat) file; this description is for convenience only.
Step module: Create Step: Description
For each step you choose an analysis procedure. This choice defines the type of analysis to be performed during the step: static stress analysis, dynamic stress analysis, eigenvalue buckling, transient heat transfer analysis, etc. The available analysis procedures are listed below and are described in the sections that follow. Only one procedure is allowed per step. Within ABAQUS/Standard or ABAQUS/Explicit, any combination of available procedures can be used from step to step. However, ABAQUS/Standard and ABAQUS/Explicit procedures cannot be used in the same analysis. See Transferring results between ABAQUS analyses: overview, Section 9.2.1, for information on importing results from one type of analysis to another.
The rest of the step definition consists of load, boundary, and output request specifications (see Applying loads: overview, Section 27.4.1; Boundary conditions, Section 27.3.1; and Output, Section 4.1.1).
|Input File Usage:||The procedure definition option must immediately follow the *STEP option.|
Step module: Create Step: choose the procedure type
There are two kinds of steps in ABAQUS: general analysis steps, which can be used to analyze linear or nonlinear response, and linear perturbation steps, which can be used only to analyze linear problems. General analysis steps can be included in an ABAQUS/Standard or ABAQUS/Explicit analysis; linear perturbation analysis steps are available only in ABAQUS/Standard. In ABAQUS/Standard linear analysis is always considered to be linear perturbation analysis about the state at the time when the linear analysis procedure is introduced. This linear perturbation approach allows general application of linear analysis techniques in cases where the linear response depends on preloading or on the nonlinear response history of the model. See General and linear perturbation procedures, Section 6.1.2, for more details.
In general analysis steps ABAQUS/Standard calculates the solution for a single set of applied loads. This is also the default for linear perturbation steps. However, for static and direct steady-state dynamic linear perturbation steps it is possible to find solutions for multiple load cases. See Multiple load case analysis, Section 6.1.3, for a description of this capability.
The analysis procedure can be changed from step to step in any meaningful way, so you have great flexibility in performing analyses. Since the state of the model (stresses, strains, temperatures, etc.) is updated throughout all general analysis steps, the effects of previous history are always included in the response in each new analysis step. Thus, for example, if natural frequency extraction is performed after a geometrically nonlinear static analysis step, the preload stiffness will be included. Linear perturbation steps have no effect on subsequent general analysis steps.
The most obvious reason for using several steps in an analysis is to change analysis procedure type. However, several steps can also be used as a matter of convenience—for example, to change output requests, contact pairs in ABAQUS/Explicit, boundary conditions, or loading (any information specified as history, or step-dependent, data). Sometimes an analysis may have progressed to a point where the present step definition needs to be modified. ABAQUS provides for this contingency with the restart capability, whereby a step can be terminated prematurely and a new step can be defined for the problem continuation (see Restarting an analysis, Section 9.1.1).
Optional history data (see Defining a model in ABAQUS, Section 1.3.1) prescribing the loading, boundary conditions, output controls, and auxiliary controls will remain in effect for all subsequent general analysis steps, including those that are defined in a restart analysis, until they are modified or reset. ABAQUS will compare all loads and boundary conditions specified in a step with the loads and boundary conditions in effect during the previous step to ensure consistency and continuity. This comparison is expensive if the number of individually specified loads and boundary conditions is very large. Hence, the number of individually specified loads and boundary conditions should be minimized, which can usually be done by using element and node sets instead of individual elements and nodes. For linear perturbation steps only the output controls are continued from one linear perturbation step to the next if there are no intermediate general analysis steps and the output controls are not redefined (see Output, Section 4.1.1).
A large class of stress analysis problems can be solved with ABAQUS. A fundamental division of such problems is into static or dynamic response; dynamic problems are those in which inertia effects are significant.
ABAQUS/Standard offers complete flexibility in making the distinction between static and dynamic response; the same analysis can contain several static and dynamic phases. Thus, a static preload might be applied, and then the linear or nonlinear dynamic response computed (as in the case of vibrations of a component of a rotating machine or the response of a flexible offshore system that is initially moved to an equilibrium position subject to buoyancy and steady current loads and then is excited by wave loading). Similarly, the static solution can be sought after a dynamic event (by following a dynamic analysis step with a step of static loading). See Static stress/displacement analysis, Section 6.2, and Dynamic stress/displacement analysis, Section 6.3, for information on these types of procedures. In addition to static and dynamic stress analysis, ABAQUS/Standard offers the following analysis types:
ABAQUS/Explicit solves dynamic response problems using an explicit direct-integration procedure. See Dynamic stress/displacement analysis, Section 6.3, for more information on the explicit dynamic procedures available in ABAQUS. ABAQUS/Explicit also provides heat transfer and acoustic analysis capabilities: see Heat transfer and thermal-stress analysis, Section 6.5, and Acoustic and shock analysis, Section 6.9, for details.
Results can be transferred between ABAQUS/Standard and ABAQUS/Explicit (Transferring results between ABAQUS analyses: overview, Section 9.2.1).
In addition, the following analysis techniques are provided in ABAQUS:
|Technique||Available in ABAQUS/Standard?||Available in ABAQUS/Explicit?|
|Restarting an analysis, Section 9.1||Yes||Yes|
|Importing and transferring results, Section 9.2||Yes||Yes|
|Substructuring, Section 10.1||Yes||No|
|Submodeling, Section 10.2||Yes||Yes|
|Symmetric model generation, results transfer, and analysis of cyclic symmetry models, Section 10.3||Yes||No|
|Meshed beam cross-sections, Section 10.4||Yes||Yes|
|Inertia relief, Section 11.1||Yes||No|
|Mesh modification or replacement, Section 11.2||Yes||No|
|Geometric imperfections, Section 11.3||Yes||Yes|
|Fracture mechanics, Section 11.4||Yes||No|
|Hydrostatic fluid modeling, Section 11.5||Yes||Yes|
|Surface-based fluid modeling, Section 11.6||No||Yes|
|Mass scaling, Section 11.7||No||Yes|
|Steady-state detection, Section 11.8||No||Yes|
|Parallel execution, Section 11.9||Yes||Yes|
|ALE adaptive meshing, Section 12.2||Yes||Yes|
|Adaptive remeshing, Section 12.3||Yes||No|
|Analysis continuation after mesh replacement, Section 12.4||Yes||No|
|Co-simulation, Section 13.1||Yes||Yes|
|Design sensitivity analysis, Section 14.1||Yes||No|
|Scripting parametric studies, Section 15.1||Yes||Yes|
By default, ABAQUS assumes that external parameters, such as load magnitudes and boundary conditions, are constant (step function) or vary linearly (ramped) over a step, depending on the analysis procedure, as shown in Table 6.1.11. Some exceptions in ABAQUS/Standard are discussed below.
|Procedure||Default amplitude variation|
|Coupled pore fluid diffusion/stress (steady-state)||Ramp|
|Coupled pore fluid diffusion/stress (transient)||Step|
|Coupled thermal-electrical (steady-state)||Ramp|
|Coupled thermal-electrical (transient)||Step|
|Fully coupled thermal-stress in ABAQUS/Standard (steady-state)||Ramp|
|Fully coupled thermal-stress in ABAQUS/Standard (transient)||Step|
|Fully coupled thermal-stress in ABAQUS/Explicit||Step|
|Mass diffusion (steady-state)||Ramp|
|Mass diffusion (transient)||Step|
|Transient modal dynamic||Step|
|Uncoupled heat transfer||Ramp|
|Uncoupled heat transfer (transient)||Step|
No default amplitude variation is defined for a direct cyclic analysis step; for each applied load or boundary condition, the amplitude must be defined explicitly.
For displacement or rotation degrees of freedom prescribed in ABAQUS/Standard using displacement-type boundary conditions or displacement-type connector motions, the default amplitude variation is a ramp function for all procedure types; the default amplitude is a step function for all procedure types when using velocity-type boundary conditions or velocity-type connector motions.
For motions prescribed using a predefined displacement field, the default amplitude variation is a ramp function for all procedure types; the default amplitude is a step function when using a predefined velocity field for all procedures except steady-state transport.
The default amplitude variation is a step function for fluid flux loading in all procedure types.
When a displacement or rotation boundary condition is removed, the corresponding reaction force or moment is reduced to zero according to the amplitude defined for the step. When film or radiation loads are removed, the variation is always a step function.
In ABAQUS/Standard you can change the default amplitude variation for a step (except the removal of film or radiation loads, as noted above).
In both ABAQUS/Standard and ABAQUS/Explicit you can define complicated time variations of loadings, boundary conditions, and predefined fields by referring to an amplitude curve in the prescribed condition definition (see Amplitude curves, Section 27.1.2). User subroutines are also provided for coding general loadings (see User subroutines: overview, Section 13.2.1).
|Input File Usage:||In ABAQUS/Standard use the following option to change the default amplitude variation for a step:|
*STEP, AMPLITUDE=STEP or RAMP
|ABAQUS/CAE Usage:||In ABAQUS/Standard use the following input to change the default amplitude variation for a step:|
Step module: step editor: Other: Default load variation with time: Instantaneous or Ramp linearly over step
Boundary conditions applied during an explicit dynamic response step should use appropriate amplitude references to define the time variation. If boundary conditions are specified for the step without amplitude references, they are applied instantaneously at the beginning of the step. Since ABAQUS/Explicit does not admit jumps in displacement, the value of a nonzero displacement boundary condition that is specified without an amplitude reference will be ignored, and a zero velocity boundary condition will be enforced.
The default amplitude is a step function for transient analysis procedures (fully coupled thermal-stress, coupled thermal-electrical, direct-integration dynamic, uncoupled heat transfer, and mass diffusion). Care should be exercised when the nondefault ramp amplitude variation is specified for transient analysis procedures since unexpected results may occur. For example, if a step of a transient heat transfer analysis uses the ramp amplitude variation and temperature boundary conditions are removed in a subsequent step, the reaction fluxes generated in the previous step will be ramped to zero from their initial values over the duration of the step. Therefore, heat flux will continue to flow through the affected boundary nodes over the entire subsequent step even though the temperature boundary conditions were removed.
Each step in an ABAQUS analysis is divided into multiple increments. In most cases you have two choices for controlling the solution: automatic time incrementation or user-specified fixed time incrementation. Automatic incrementation is recommended for most cases. The methods for selecting automatic or direct incrementation are discussed in the individual procedure sections.
The issues associated with time incrementation in ABAQUS/Standard and ABAQUS/Explicit analyses are quite different, since time increments are generally much smaller in ABAQUS/Explicit.
In nonlinear problems ABAQUS/Standard will increment and iterate as necessary to analyze a step, depending on the severity of the nonlinearity. In transient cases with a physical time scale, you can provide parameters to indicate a level of accuracy in the time integration, and ABAQUS/Standard will choose the time increments to achieve this accuracy. Direct user control is provided because it can sometimes save computational cost in cases where you are familiar with the problem and know a suitable incrementation scheme. Direct control can also occasionally be useful when automatic control has trouble with convergence in nonlinear problems.
You can define the upper limit to the number of increments in an ABAQUS/Standard analysis. In a direct cyclic analysis procedure, this upper limit should be set to the maximum number of increments in a single loading cycle. The default is 100. The analysis will stop if this maximum is exceeded before the complete solution for the step has been obtained. To arrive at a solution, it is often necessary to increase the number of increments allowed by defining a new upper limit.
|Input File Usage:|
Step module: step editor: Incrementation: Maximum number of increments
In nonlinear analyses ABAQUS/Standard uses extrapolation to speed up the solution. Extrapolation refers to the method used to determine the first guess to the incremental solution. The guess is determined by the size of the current time increment and by whether linear, parabolic, or no extrapolation of the previously attained history of each solution variable is chosen. Parabolic extrapolation is not relevant for dynamic or Riks analyses. By default (linear extrapolation), 100% extrapolation (1% for the Riks method) of the previous incremental solution is used at the start of each increment to begin the nonlinear equation solution for the next increment. No extrapolation is used in the first increment of a step.
In some cases extrapolation can cause ABAQUS/Standard to iterate excessively; some common examples are abrupt changes in the load magnitudes or boundary conditions and if unloading occurs as a result of cracking (in concrete models) or buckling. In such cases you should suppress extrapolation.
Parabolic extrapolation uses two previous incremental solutions to obtain the first guess to the current incremental solution. This type of extrapolation is useful in situations when the local variation of the solution with respect to the time scale of the problem is expected to be quadratic, such as the large rotation of structures. If parabolic extrapolation is used in a step, it begins after the second increment of the step: the first increment employs no extrapolation, and the second increment employs linear extrapolation. Consequently, slower convergence rates may occur during the first two increments of the succeeding steps in a multistep analysis.
Step module: step editor: Other: Extrapolation of previous state at start of each increment: Linear, Parabolic, or None
The time increment used in an ABAQUS/Explicit analysis must be smaller than the stability limit of the central-difference operator (see Explicit dynamic analysis, Section 6.3.3); failure to use a small enough time increment will result in an unstable solution. Although the time increments chosen by ABAQUS/Explicit generally satisfy the stability criterion, user control over the size of the time increment is provided to reduce the chance of a solution going unstable. The small increments characteristic of an explicit dynamic analysis product make ABAQUS/Explicit well suited for nonlinear analysis.
ABAQUS/Standard distinguishes between regular, equilibrium iterations (in which the solution varies smoothly) and severe discontinuity iterations (SDIs) in which abrupt changes in stiffness occur. The most common of such severe discontinuities involve open-close changes in contact and stick-slip changes in friction. By default, ABAQUS/Standard will continue to iterate until no severe discontinuities occur and the equilibrium (flux) tolerances are satisfied. Alternatively, you can choose a different approach in which severe discontinuities are converted into force residuals, in which case ABAQUS/Standard will stop iterating when the residual tolerances are satisfied, even if severe discontinuities occur.
Forcing a new iteration whenever a severe discontinuity occurs can sometimes lead to convergence problems, particularly in large problems with many contact points or situations where contact conditions are only weakly determined. Conversion of severe discontinuity iterations is particularly effective in resolving these convergence problems. The conversion involves generating a residual force that gives a good indication of the severity of the discontinuity. When a contact point opens, this is readily accomplished: the (tensile) force is set to zero, resulting in a force residual at the surfaces that were in contact. When a point closes, ABAQUS converts the penetration into a force. For softened contact this can be based on the contact stiffness; for hard contact the penetration is multiplied by the stiffness of the underlying elements, which yields a conservative estimate of the change in force that can be expected due to closing. Similar considerations can be applied to frictional stick-slip behavior and strongly nonlinear softened contact. The usual checks on the magnitude of the residual then determine whether the results can be accepted or not.
|Input File Usage:|
*STEP, CONVERT SDI=YES
SDI conversion can also be activated with the command line variable convert_sdi (see Execution procedure for ABAQUS/Standard and ABAQUS/Explicit, Section 3.2.2) or with the environment variable convert_sdi (see Using the ABAQUS environment settings, Section 3.3.1). The value specified on the *STEP option takes precedence over the value specified on the command line, which in turn takes precedence over the value specified in the environment file.
Step module: step editor: Other: Convert severe discontinuity iterations: On
ABAQUS/Standard generally uses Newton's method to solve nonlinear problems and the stiffness method to solve linear problems. In both cases the stiffness matrix is needed. In some problems—for example, with Coulomb friction—this matrix is not symmetric. ABAQUS/Standard will automatically choose whether a symmetric or unsymmetric matrix storage and solution scheme should be used based on the model and step definition used. In some cases you can override this choice; the rules are explained below.
Usually it is not necessary to specify the matrix storage and solution scheme. The choice is available to improve computational efficiency in those cases where you judge that the default value is not the best choice. In certain cases where the exact tangent stiffness matrix is not symmetric, the extra iterations required by a symmetric approximation to the tangent matrix use less computer time than solving the nonsymmetric tangent matrix at each iteration. Therefore, for example, ABAQUS/Standard invokes the symmetric matrix storage and solution scheme automatically in problems with Coulomb friction where every friction coefficient is less than or equal to 0.2, even though the resulting tangent matrix will have some nonsymmetric terms. However, if any friction coefficient is greater than 0.2, ABAQUS/Standard will use the unsymmetric matrix storage and solution scheme automatically since it may significantly improve the convergence history. This choice of the unsymmetric matrix storage and solution scheme will be made based solely on the model definition. Thus, if you modify the friction definition during the analysis to introduce a friction coefficient greater than 0.2, ABAQUS/Standard will not activate the unsymmetric matrix storage and solution scheme automatically. In cases in which the unsymmetric matrix storage and solution scheme is selected automatically, you must explicitly turn it off if so desired; it is recommended to do so if friction prevents any sliding motions.
|Input File Usage:|
*STEP, UNSYMM=YES or NO
Step module: step editor: Other: Storage: Use solver default or Unsymmetric or Symmetric
Since ABAQUS/Standard provides eigenvalue extraction only for symmetric matrices, steps with eigenfrequency extraction or eigenvalue buckling prediction procedures always use the symmetric matrix storage and solution scheme. You cannot change this setting. In such steps ABAQUS/Standard will symmetrize all contributions to the stiffness matrix.
In all steps except those with eigenfrequency extraction or eigenvalue buckling procedures, ABAQUS/Standard uses the unsymmetric matrix storage and solution scheme when any of the following features are included in the model. You cannot change this setting.
Heat transfer convection/diffusion elements (element types DCCxxx)
General shell sections with unsymmetric section stiffness matrices (Three-dimensional conventional shell element library, Section 23.6.7)
User-defined elements with unsymmetric element matrices (User-defined elements, Section 26.15.1)
User-defined material models with unsymmetric material stiffness matrices (User-defined mechanical material behavior, Section 20.8.1, or User-defined thermal material behavior, Section 20.8.2)
User-defined surface interaction models with unsymmetric interface stiffness matrices (User-defined interfacial constitutive behavior, Section 30.1.6)
The following features all trigger the unsymmetric matrix storage and solution scheme for the step. You cannot change this setting.
Fully coupled thermal-stress analysis, except when a separated solution scheme is specified for the step (Fully coupled thermal-stress analysis, Section 6.5.4)
Coupled thermal-electrical analysis, except when a separated solution scheme is specified for the step (Coupled thermal-electrical analysis, Section 6.6.2)
Coupled pore fluid diffusion/stress analysis with absorption or exsorption behavior (Coupled pore fluid diffusion and stress analysis, Section 6.7.1)
Coupled pore fluid diffusion/stress analysis (steady-state)
Coupled pore fluid diffusion/stress analysis (transient with gravity loading)
Mass diffusion analysis (Mass diffusion analysis, Section 6.8.1)
Radiation viewfactor calculation controls (Cavity radiation, Section 32.1.1)
By default, the unsymmetric matrix storage and solution scheme is used for the complex eigenvalue extraction procedure. You can change this setting.
In all other cases you can control whether a symmetric or a full matrix storage and arithmetic solution is chosen. If you do not specify the matrix storage and solution scheme, ABAQUS/Standard utilizes the value used in the previous general analysis step.
If you do not specify the matrix storage and solution scheme in the first step of an analysis, ABAQUS/Standard will choose the unsymmetric scheme when any of the following are used:
Any ABAQUS/Aqua load type
The concrete damaged plasticity material model
Friction with a friction coefficient greater than 0.2
The default value in the first step is the symmetric scheme for all other cases, except those covered by rules 2 and 3 above. Introducing a friction coefficient greater than 0.2 by modifying the friction definition during the analysis will not cause ABAQUS/Standard to choose the unsymmetric scheme.
For radiative heat transfer surface interactions (Thermal contact properties, Section 30.2.1), certain follower forces (such as concentrated follower forces or moments), three-dimensional finite-sliding analyses, any finite sliding in coupled pore fluid diffusion/stress analyses, and certain material models (particularly nonassociated flow plasticity models and concrete) introduce unsymmetric terms in the model's stiffness matrix. However, ABAQUS/Standard does not automatically use the unsymmetric matrix storage and solution scheme when radiative heat transfer surface interactions are used. Specifying that the unsymmetric scheme should be used can sometimes improve convergence in such cases.
You can choose a double-precision executable (with 64-bit word lengths) for ABAQUS/Explicit on machines with a default, single-precision word length of 32 bits (see Execution procedure for ABAQUS/Standard and ABAQUS/Explicit, Section 3.2.2). Most new computers have 32-bit default word lengths even though they may have 64-bit memory addressing. The single-precision executable typically results in a CPU savings of 20% to 30% compared to the double-precision executable, and single precision provides accurate results in most cases. Exceptions in which single precision tends to be inadequate include analyses that require greater than approximately 300,000 increments, have typical nodal displacement increments less than 106 times the corresponding nodal coordinate values, include hyperelastic materials, or involve multiple revolutions of deformable parts; the double-precision executable is recommended in these cases (for example, see Simulation of propeller rotation, Section 2.3.15 of the ABAQUS Benchmarks Manual). Comparison of solutions obtained with single and double precision will indicate the significance of the precision level. If no significant difference is found between single- and double-precision solutions for a particular model, the single-precision executable will also be adequate after a minor modification to the model.