You can configure general analysis procedures to analyze linear or nonlinear response. You can include general analysis procedures in either Abaqus/Standard or Abaqus/Explicit analyses. For more information, see “General and linear perturbation procedures,” Section 6.1.2 of the Abaqus Analysis User's Manual.
This section provides instructions for using the step editor to configure different types of general analysis procedures. The following topics are covered:
“Configuring a fully coupled, simultaneous heat transfer and stress procedure”
“Configuring a fully coupled, simultaneous heat transfer and electrical procedure”
“Configuring a dynamic fully coupled thermal-stress procedure using explicit integration”
“Configuring an effective stress analysis for fluid-filled porous media”
“Configuring a transient, static, stress/displacement analysis with time-dependent material response”
A static stress procedure is one in which inertia effects are neglected. The analysis can be linear or nonlinear and ignores time-dependent material effects. For more information, see “Static stress analysis,” Section 6.2.2 of the Abaqus Analysis User's Manual.
To create or edit a static, general procedure:
Display the Edit Step dialog box following the procedure outlined in “Creating a step,” Section 14.9.2 (Procedure type: General; Static, General), or “Editing a step,” Section 14.9.3.
On the Basic, Incrementation, and Other tabbed pages, configure settings such as the time period for the step, the maximum number of increments, the increment size, the default load variation with time, and whether to account for geometric nonlinearity as described in the following procedures.
To configure settings on the Basic tabbed page:
In the Edit Step dialog box, display the Basic tabbed page.
In the Description field, enter a short description of the analysis step. Abaqus stores the text that you enter in the output database, and the text is displayed in the state block by the Visualization module.
In the Time period field, enter the time period of the step. For more information, see “Time period” in “Static stress analysis,” Section 6.2.2 of the Abaqus Analysis User's Manual.
Select an Nlgeom option:
Toggle Nlgeom Off to perform a geometrically linear analysis during the current step.
Toggle Nlgeom On to indicate that Abaqus/Standard should account for geometric nonlinearity during the step. Once you have toggled Nlgeom on, it will be active during all subsequent steps in the analysis.
Select an automatic stabilization method if you expect the problem to have local instabilities such as surface wrinkling, material instability, or local buckling. Abaqus/Standard can stabilize this class of problems by applying damping throughout the model. For more information, see “Unstable problems” in “Static stress analysis,” Section 6.2.2 of the Abaqus Analysis User's Manual, and “Automatic stabilization of static problems with a constant damping factor” in “Solving nonlinear problems,” Section 7.1.1 of the Abaqus Analysis User's Manual
Click the arrow to the right of Automatic stabilization, and select a method for defining the damping factor:
Select Specify dissipated energy fraction to allow Abaqus/Standard to calculate the damping factor from a dissipated energy fraction that you provide. Enter a value for the dissipated energy fraction in the adjacent field (the default is 2.0 × 10–4). For more information, see “Calculating the damping factor based on the dissipated energy fraction” in “Solving nonlinear problems,” Section 7.1.1 of the Abaqus Analysis User's Manual.
Select Specify damping factor to enter the damping factor directly. Enter a value for the damping factor in the adjacent field. For more information, see “Directly specifying the damping factor” in “Solving nonlinear problems,” Section 7.1.1 of the Abaqus Analysis User's Manual.
Select Use damping factors from previous general step to use the damping factors at the end of the previous step as the initial factors in the current step's variable damping scheme. These factors override any initial damping factors that are calculated or specified directly in the current step. If there are no damping factors associated with the previous general step (for example, if the previous step does not use any stabilization or the current step is the first step of the analysis), Abaqus uses adaptive stabilization to determine the required damping factors.
When using automatic stabilization, Abaqus can use the same damping factor over the course of a step, or it can vary the damping factor spatially and temporally during a step based on the convergence history and the ratio of the energy dissipated by damping to the total strain energy. For more information, see “Adaptive automatic stabilization scheme” in “Solving nonlinear problems,” Section 7.1.1 of the Abaqus Analysis User's Manual. If you selected Specify dissipated energy fraction, adaptive stabilization is optional and turned on by default. If you selected Specify damping factor, adaptive stabilization is optional and turned off by default. If you selected Use damping factors from previous general step, adaptive stabilization is required.
To use adaptive stabilization, toggle on Use adaptive stabilization with max. ratio of stabilization to strain energy (if necessary), and enter a value in the adjacent field for the allowable accuracy tolerance for the ratio of energy dissipated by damping to total strain energy in each increment. The default value of 0.05 should be suitable in most cases.
Toggle on Include adiabatic heating effects if you are performing an adiabatic stress analysis. This option is relevant only for isotropic metal plasticity materials with a Mises yield surface. For more information, see “Adiabatic analysis,” Section 6.5.5 of the Abaqus Analysis User's Manual.
When you have finished configuring settings for the static, general step, click OK to close the Edit Step dialog box.
To configure settings on the Incrementation tabbed page:
In the Edit Step dialog box, display the Incrementation tabbed page.
(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)
Choose a Type option:
Choose Automatic to allow Abaqus/Standard to choose the size of the time increments based on computational efficiency.
Choose Fixed to specify direct user control of the incrementation. Abaqus/Standard uses an increment size that you specify as the constant increment size throughout the step.
In the Maximum number of increments field, enter the upper limit to the number of increments in the step. The analysis stops if this maximum is exceeded before Abaqus/Standard arrives at the complete solution for the step.
If you selected Automatic in Step 2, enter values for Increment size:
In the Initial field, enter the initial time increment. Abaqus/Standard modifies this value as required throughout the step.
In the Minimum field, enter the minimum time increment allowed. If Abaqus/Standard needs a smaller time increment than this value, it terminates the analysis.
In the Maximum field, enter the maximum time increment allowed.
If you selected Fixed in Step 2, enter a value for the constant time increment in the Increment size field.
When you have finished configuring settings for the static, general step, click OK to close the Edit Step dialog box.
To configure settings on the Other tabbed page:
In the Edit Step dialog box, display the Other tabbed page.
(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)
Choose an Equation Solver Method option:
Choose Direct to use the default direct sparse solver.
Choose Iterative to use the domain decomposition iterative linear equation solver. For more information, see “Iterative linear equation solver,” Section 6.1.5 of the Abaqus Analysis User's Manual.
Choose a Matrix storage option:
Choose Use solver default to allow Abaqus/Standard to decide whether a symmetric or unsymmetric matrix storage and solution scheme is needed.
Choose Unsymmetric to restrict Abaqus/Standard to the unsymmetric storage and solution scheme.
Choose Symmetric to restrict Abaqus/Standard to the symmetric storage and solution scheme.
Choose a Solution technique:
Choose Full Newton to use Newton's method as a numerical technique for solving nonlinear equilibrium equations. For more information, see “Nonlinear solution methods in Abaqus/Standard,” Section 2.2.1 of the Abaqus Theory Manual.
Choose Quasi-Newton to use the quasi-Newton technique for solving nonlinear equilibrium equations. This technique can save substantial computational cost in some cases. Generally it is most successful when the system is large and the stiffness matrix is not changing much from iteration to iteration. You can use this technique only for symmetric systems of equations.
If you choose this technique, enter a value for the Number of iterations allowed before the kernel matrix is reformed. The maximum number of iterations allowed is 25. The default number of iterations is 8.
For more information, see “Quasi-Newton solution technique,” Section 2.2.2 of the Abaqus Theory Manual.
Choose Contact iterations to use contact iterations instead of regular severe discontinuity iterations to speed up computations. Contact iterations are effective for the solution of large, geometrically linear, small-sliding, frictionless static problems with many severe discontinuity iterations.
If you choose this technique, enter the following values:
Adjustment factor for the number of solutions in any iteration. This value is a correction factor on the maximum number of right-hand-side solutions during any contact iteration.
Maximum number of contact iterations. This value specifies the maximum number of contact iterations allowed before new global matrix assemblage and factorization.
Click the arrow to the right of the Convert severe discontinuity iterations field, and select an option for dealing with severe discontinuities during nonlinear analysis:
Select Off to force a new iteration if severe discontinuities occur during an iteration, regardless of the magnitude of the penetration and force errors. This option also changes some time incrementation parameters and uses different criteria to determine whether to do another iteration or to make a new attempt with a smaller increment size.
Select On to use local convergence criteria to determine whether a new iteration is needed. Abaqus/Standard will determine the maximum penetration and estimated force errors associated with severe discontinuities and check whether these errors are within the tolerances. Hence, a solution may converge if the severe discontinuities are small.
Select Propagate from previous step to use the value specified in the previous general analysis step. This value appears in parentheses to the right of the field.
Choose an option for Default load variation with time:
Choose Instantaneous if you want loads to be applied instantaneously at the start of the step and remain constant throughout the step.
Choose Ramp linearly over step if the load magnitude is to vary linearly over the step, from the value at the end of the previous step to the full magnitude of the load.
Click the arrow to the right of the Extrapolation of previous state at start of each increment field, and select a method for determining the first guess to the incremental solution:
Select Linear to indicate that the process is essentially monotonic and Abaqus/Standard should use a 100% linear extrapolation, in time, of the previous incremental solution to begin the nonlinear equation solution for the current increment.
Select Parabolic to indicate that the process should use a quadratic extrapolation, in time, of the previous two incremental solutions to begin the nonlinear equation solution for the current increment.
Select None to suppress any extrapolation.
Toggle on Stop when region region name is fully plastic if “fully plastic” analysis is required with deformation theory plasticity. If you toggle on this option, enter the name of the region being monitored for fully plastic behavior.
The step ends when the solutions at all constitutive calculation points in the element set are fully plastic (defined by the equivalent strain being 10 times the offset yield strain). However, the step can end before this point if either the maximum number of increments that you specified on the Incrementation tabbed page or the time period that you specified on the Basic tabbed page is exceeded.
If you selected Fixed time incrementation on the Incrementation tabbed page, you can toggle on Accept solution after reaching maximum number of iterations. This option directs Abaqus/Standard to accept the solution to an increment after the maximum number of iterations allowed has been completed, even if the equilibrium tolerances are not satisfied. Very small increments and a minimum of two iterations are usually necessary if you use this option.
Warning: This approach is not recommended; you should use it only in special cases when you have a thorough understanding of how to interpret results obtained in this way.
Toggle on Obtain long-term solution with time-domain material properties to obtain the fully relaxed long-term elastic solution with time-domain viscoelasticity or the long-term elastic-plastic solution for two-layer viscoplasticity. This parameter is relevant only for time-domain viscoelastic and two-layer viscoplastic materials.
When you have finished configuring settings for the static, general step, click OK to close the Edit Step dialog box.
Geometrically nonlinear static problems sometimes involve buckling or collapse behavior, where the load-displacement response shows a negative stiffness, and the structure must release strain energy to remain in equilibrium. The modified Riks method allows you to find static equilibrium states during the unstable phase of the response.
You can use this method for cases where the load magnitudes are governed by a single scalar parameter. It is also useful for solving ill-conditioned problems such as limit load problems or almost unstable problems that exhibit softening. For more information, see “Unstable collapse and postbuckling analysis,” Section 6.2.4 of the Abaqus Analysis User's Manual.
To create or edit a static, Riks procedure:
Display the Edit Step dialog box following the procedure outlined in “Creating a step,” Section 14.9.2 (Procedure type: General; Static, Riks), or “Editing a step,” Section 14.9.3.
On the Basic, Incrementation, and Other tabbed pages, configure settings such as stopping criteria, the maximum number of increments, the arc increment length, and whether to account for geometric nonlinearity as described in the following procedures.
To configure settings on the Basic tabbed page:
In the Edit Step dialog box, display the Basic tabbed page.
In the Description field, enter a short description of the analysis step. Abaqus stores the text that you enter in the output database, and the text is displayed in the state block by the Visualization module.
Select an Nlgeom option:
Toggle Nlgeom Off to perform a geometrically linear analysis during the current step.
Toggle Nlgeom On to indicate that Abaqus/Standard should account for geometric nonlinearity during the step. Once you have toggled Nlgeom on, it will be active during all subsequent steps in the analysis.
Toggle on Include adiabatic heating effects if you are performing an adiabatic stress analysis. This option is relevant only for isotropic metal plasticity materials with a Mises yield surface. For more information, see “Adiabatic analysis,” Section 6.5.5 of the Abaqus Analysis User's Manual.
Since the loading magnitude is part of the solution, you need a method to specify when the step is completed. Choose one or both of the following options:
Toggle on Maximum load proportionality factor to enter a maximum value for the load proportionality factor, 
. Abaqus/Standard uses this value to terminate the step when the load exceeds a certain magnitude. For more information, see “Proportional loading” in “Unstable collapse and postbuckling analysis,” Section 6.2.4 of the Abaqus Analysis User's Manual
Toggle on Maximum displacement to enter a maximum displacement value at a specific degree of freedom (DOF). You must also specify the Node Region that Abaqus/Standard will monitor for finishing displacement. If this maximum displacement is exceeded, Abaqus/Standard terminates the step.
To configure settings on the Incrementation tabbed page:
In the Edit Step dialog box, display the Incrementation tabbed page.
(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)
Choose a Type option:
Choose Automatic to allow Abaqus/Standard to choose the size of the arc length increments based on computational efficiency.
Choose Fixed to specify direct user control of the incrementation. Abaqus/Standard uses an arc length increment that you specify as the constant increment size throughout the step. This method is not recommended for a Riks analysis since it prevents Abaqus/Standard from reducing the arc length when a severe nonlinearity is encountered.
In the Maximum number of increments field, enter the upper limit to the number of increments in the step. The analysis stops if this maximum is exceeded before Abaqus/Standard arrives at the complete solution for the step.
If you selected Automatic in Step 2, enter values for Arc length increment:
In the Initial field, enter the initial increment in arc length along the static equilibrium path in scaled load-displacement space, 
.
In the Minimum field, enter the minimum arc length increment, 
. If you enter zero, Abaqus assumes a default value of the smaller of the suggested initial arc length or 10–5 times the total arc length.
In the Maximum field, enter the maximum arc length increment, 
. If this value is not specified, no upper limit is imposed.
In the Estimated total arc length field, enter the total arc length scale factor associated with this step, 
. If this entry is zero or is unspecified, Abaqus/Standard assumes a default value of 
.
If you selected Fixed in Step 2, enter a value for the constant arc length increment in the Arc length increment field.
To configure settings on the Other tabbed page:
In the Edit Step dialog box, display the Other tabbed page.
(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)
Choose a Matrix storage option:
Choose Use solver default to allow Abaqus/Standard to decide whether a symmetric or unsymmetric matrix storage and solution scheme is needed.
Choose Unsymmetric to restrict Abaqus/Standard to the unsymmetric storage and solution scheme.
Choose Symmetric to restrict Abaqus/Standard to the symmetric storage and solution scheme.
Toggle on Apply contact iteration solution technique to use contact iterations instead of regular severe discontinuity iterations to speed up computations. Contact iterations are effective for the solution of large, geometrically linear, small-sliding, frictionless static problems with many severe discontinuity iterations.
If you select this technique, enter the following values:
Adjustment factor for the number of solutions in any iteration. This value is a correction factor on the maximum number of right-hand-side solutions during any contact iteration.
Maximum number of contact iterations. This value specifies the maximum number of contact iterations allowed before new global matrix assemblage and factorization.
Click the arrow to the right of the Convert severe discontinuity iterations field, and select an option for dealing with severe discontinuities during nonlinear analysis:
Select Off to force a new iteration if severe discontinuities occur during an iteration, regardless of the magnitude of the penetration and force errors. This option also changes some time incrementation parameters and uses different criteria to determine whether to do another iteration or to make a new attempt with a smaller increment size.
Select On to use local convergence criteria to determine whether a new iteration is needed. Abaqus/Standard will determine the maximum penetration and estimated force errors associated with severe discontinuities and check whether these errors are within the tolerances. Hence, a solution may converge if the severe discontinuities are small.
Select Propagate from previous step to use the value specified in the previous general analysis step. This value appears in parentheses to the right of the field.
Click the arrow to the right of the Extrapolation of previous state at start of each increment field, and select a method for determining the first guess to the incremental solution:
Select Linear to indicate that the process is essentially monotonic, and Abaqus/Standard should use a 1% linear extrapolation of the previous incremental solution to begin the nonlinear equation solution for the current increment.
Select None to suppress any extrapolation.
Toggle on Stop when region region name is fully plastic if “fully plastic” analysis is required with deformation theory plasticity. If you toggle on this option, enter the name of the region being monitored for fully plastic behavior.
The step ends when the solutions at all constitutive calculation points in the element set are fully plastic (defined by the equivalent strain being 10 times the offset yield strain). However, the step can end before this point if the maximum number of increments that you specified on the Incrementation tabbed page is exceeded.
If you selected Fixed time incrementation on the Incrementation tabbed page, you can toggle on Accept solution after reaching maximum number of iterations. This option directs Abaqus/Standard to accept the solution to an increment after the maximum number of iterations allowed has been completed, even if the equilibrium tolerances are not satisfied. Very small increments and a minimum of two iterations are usually necessary if you use this option.
Warning: This approach is not recommended; you should use it only in special cases when you have a thorough understanding of how to interpret results obtained in this way.
Toggle on Obtain long-term solution with time-domain material properties to obtain the fully relaxed long-term elastic solution with time-domain viscoelasticity or the long-term elastic-plastic solution for two-layer viscoplasticity. This parameter is relevant only for time-domain viscoelastic and two-layer viscoplastic materials.
When you have finished configuring settings for the static, Riks step, click OK to close the Edit Step dialog box.
An explicit, dynamic analysis is computationally efficient for the analysis of large models with relatively short dynamic response times and for the analysis of extremely discontinuous events or processes. This type of analysis allows for the definition of very general contact conditions and uses a consistent, large-deformation theory. For more information, see “Explicit dynamic analysis,” Section 6.3.3 of the Abaqus Analysis User's Manual.
To create or edit a dynamic, explicit procedure:
Display the Edit Step dialog box following the procedure outlined in “Creating a step,” Section 14.9.2 (Procedure type: General; Dynamic, Explicit), or “Editing a step,” Section 14.9.3.
On the Basic, Incrementation, Mass scaling, and Other tabbed pages, configure settings such as the time period for the step, the maximum time increment, the increment size, mass scaling definitions, and bulk viscosity parameters as described in the following procedures.
To configure settings on the Basic tabbed page:
In the Edit Step dialog box, display the Basic tabbed page.
In the Description field, enter a short description of the analysis step. Abaqus stores the text that you enter in the output database, and the text is displayed in the state block by the Visualization module.
In the Time period field, enter the time period of the step.
Select an Nlgeom option:
Toggle Nlgeom Off to perform a geometrically linear analysis during the current step.
Toggle Nlgeom On to indicate that Abaqus/Explicit should account for geometric nonlinearity during the step. Once you have toggled Nlgeom on, it will be active during all subsequent steps in the analysis.
Toggle on Include adiabatic heating effects if you are performing an adiabatic stress analysis. This option is relevant only for metal plasticity. For more information, see “Adiabatic analysis,” Section 6.5.5 of the Abaqus Analysis User's Manual.
To configure settings on the Incrementation tabbed page:
In the Edit Step dialog box, display the Incrementation tabbed page.
(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)
Choose a Type option:
Choose Automatic to allow Abaqus/Explicit to determine the time incrementation automatically. For more information, see “Automatic time incrementation” in “Explicit dynamic analysis,” Section 6.3.3 of the Abaqus Analysis User's Manual.
Choose Fixed to use a fixed time incrementation scheme. The fixed time increment size is determined either by the initial element stability estimate for the step or by a user-specified time increment. For more information, see “Fixed time incrementation” in “Explicit dynamic analysis,” Section 6.3.3 of the Abaqus Analysis User's Manual.
If you selected Automatic time incrementation, perform the following steps:
Choose a Stable increment estimator option:
Choose Global to allow the global estimator to determine the stability limit as the step proceeds. The adaptive, global estimation algorithm determines the maximum frequency of the entire model using the current dilatational wave speed. This algorithm continuously updates the estimate for the maximum frequency. The global estimator will usually allow time increments that exceed the element-by-element values.
Choose Element-by-element to allow Abaqus/Explicit to determine an element-by-element estimate using the current dilatational wave speed in each element.
The element-by-element estimate is conservative; it will give a smaller stable time increment than the true stability limit that is based upon the maximum frequency of the entire model. In general, constraints such as boundary conditions and kinematic contact have the effect of compressing the eigenvalue spectrum, and the element-by-element estimates do not take this into account.
Choose a Max. time increment option:
Choose Unlimited if you do not want to impose an upper limit to time incrementation.
Choose Value to enter a value for the maximum time increment allowed. Enter the value in the field provided.
If you selected Fixed time incrementation, choose an option for determining increment size:
Choose User-defined time increment to specify a time increment size directly. Enter that time increment size in the field provided.
Choose Use element-by-element time increment estimator to use time increments the size of the initial element-by-element stability limit throughout the step. The dilatational wave speed in each element at the beginning of the step is used to compute the fixed time increment size.
If desired, enter a Time scaling factor to adjust the stable time increment computed by Abaqus/Explicit. (This option is unavailable if you have specified a User-defined time increment for the Fixed time incrementation scheme.) For more information, see “Scaling the time increment” in “Explicit dynamic analysis,” Section 6.3.3 of the Abaqus Analysis User's Manual.
To configure settings on the Mass scaling tabbed page:
In the Edit Step dialog box, display the Mass scaling tabbed page. For background information on mass scaling, see “Mass scaling,” Section 11.7.1 of the Abaqus Analysis User's Manual.
(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)
Choose one of the following options for specifying mass scaling:
Choose Use scaled mass and “throughout step” definitions from the previous step if you want mass scaling definitions from the previous step to propagate through the current step. If you choose this option, you can skip the remaining steps in this procedure.
Choose Use scaling definitions below to create one or more new mass scaling definitions for this step. If you choose this option, complete the remaining steps in this procedure.
At the bottom of the Data table, click Create.
An Edit mass scaling dialog box appears.
Specify which type of mass scaling definition you want to create:
Choose Semi-automatic mass scaling to define mass scaling for any type of analysis except bulk metal rolling.
Choose Automatic mass scaling to define mass scaling for a bulk metal rolling analysis. For more information, see “Automatic mass scaling for analysis of bulk metal rolling” in “Mass scaling,” Section 11.7.1 of the Abaqus Analysis User's Manual.
Choose Reinitialize mass to reinitialize masses of elements to their original values. This option allows you to prevent the scaled mass from a previous step from being used in the current step. For more information, see “Reinitializing the mass” in “Mass scaling,” Section 11.7.1 of the Abaqus Analysis User's Manual.
Choose Disable mass scaling thoughout step to disable in this step all variable mass scaling definitions from previous steps. For more information, see “Removing mass scaling definitions” in “Mass scaling,” Section 11.7.1 of the Abaqus Analysis User's Manual.
If you selected Semi-automatic mass scaling, Automatic mass scaling, or Reinitialize mass, indicate the region to which you want the mass scaling definition applied:
Choose Whole model to apply the mass scaling definition to all elements in the model.
Choose Set to apply the mass scaling definition to a particular set of elements. Enter the set name in the field provided.
If you selected Semi-automatic mass scaling, indicate when, during the step, you want Abaqus/Explicit to scale the element masses:
Choose At beginning of step to perform fixed mass scaling only at the beginning of the step. For more information, see “Fixed mass scaling” in “Mass scaling,” Section 11.7.1 of the Abaqus Analysis User's Manual.
Choose Throughout step to scale the mass of elements periodically during the step. For more information, see “Variable mass scaling” in “Mass scaling,” Section 11.7.1 of the Abaqus Analysis User's Manual.
If you selected Semi-automatic mass scaling, indicate how you want Abaqus/Explicit to scale the element masses:
Toggle on Scale by factor to scale the elements once at the beginning of the step by the value you enter in the field provided. For more information, see “Defining a scale factor directly” in “Mass scaling,” Section 11.7.1 of the Abaqus Analysis User's Manual.
Toggle on Scale to target time increment of n to enter a desired element stable time increment in the field provided. Click the arrow to the right of the Scale element mass field, and select how you want Abaqus/Explicit to apply that target time increment:
Select Uniformly to satisfy target to scale the masses of the elements equally so that the smallest element stable time increment of the scaled elements equals the target value.
Select If below minimum target to scale the masses of only the elements whose element stable time increments are less than the target value.
Select Nonuniformly to equal target to scale the masses of all elements so that they all have the same element stable time increment equal to the target value.
If you selected Automatic mass scaling, enter the following values:
In the Feed rate field, enter the estimated average velocity of the workpiece in the rolling direction at steady-state conditions.
In the Extruded element length field, enter the average element length in the rolling direction.
In the Nodes in cross-section field, enter the number of nodes in the cross-section of the workpiece. Increasing this value decreases the amount of mass scaling.
If you selected Semi-automatic mass scaling throughout the step or Automatic mass scaling, specify when, during the step, you want Abaqus/Explicit to perform mass scaling calculations:
Choose Every n increments to specify the frequency, in increments, at which Abaqus/Explicit is to perform mass scaling calculations. Enter the desired frequency in the field provided.
For example, if you enter a value of 5, Abaqus/Explicit scales the mass at the beginning of the step and at increments 5, 10, 15, etc.
Choose At n equal intervals to specify the number of intervals during the step at which Abaqus/Explicit is to perform mass scaling calculations. Enter the desired value in the field provided.
For example, if you enter a value of 2, Abaqus/Explicit scales the mass at the beginning of the step, the increment immediately following the half-way point in the step, and the final increment in the step.
Click OK to close the Edit mass scaling dialog box and return to the Mass scaling tabbed page of the Edit Step dialog box.
The mass scaling definition that you have just created appears in the Data table.
If desired, repeat Steps 3 to 10 to create additional mass scaling definitions.
Once you have created one or more mass scaling definitions, you can edit or delete them if desired. Select a particular mass scaling definition in the Data table, and click Edit or Delete at the bottom of the Data table.
To configure settings on the Other tabbed page:
In the Edit Step dialog box, display the Other tabbed page.
(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)
Enter a value for the Linear bulk viscosity parameter. Linear bulk viscosity is included by default in Abaqus/Explicit.
Enter a value for the Quadratic bulk viscosity parameter. This form of bulk viscosity pressure is found only in solid continuum element and is applied only if the volumetric strain rate is compressive.
For more information, see “Bulk viscosity” in “Explicit dynamic analysis,” Section 6.3.3 of the Abaqus Analysis User's Manual.
When you have finished configuring settings for the dynamic, explicit step, click OK to close the Edit Step dialog box.
You can perform an uncoupled heat transfer analysis to model solid body heat conduction with general, temperature-dependent conductivity, internal energy (including latent heat effects), and general convection and radiation boundary conditions, including cavity radiation. For more information, see “Uncoupled heat transfer analysis,” Section 6.5.2 of the Abaqus Analysis User's Manual.
To create or edit a heat transfer procedure:
Display the Edit Step dialog box following the procedure outlined in “Creating a step,” Section 14.9.2 (Procedure type: General; Heat transfer), or “Editing a step,” Section 14.9.3.
On the Basic, Incrementation, and Other tabbed pages, configure settings such as the time period for the step, the maximum allowable temperature change per increment, and equation solver preferences as described in the following procedures.
To configure settings on the Basic tabbed page:
In the Edit Step dialog box, display the Basic tabbed page.
In the Description field, enter a short description of the analysis step. Abaqus stores the text that you enter in the output database, and the text is displayed in the state block by the Visualization module.
Choose a Response option:
Choose Steady-state to omit the internal energy term (the specific heat term) in the governing heat transfer equation. For more information, see “Steady-state analysis” in “Uncoupled heat transfer analysis,” Section 6.5.2 of the Abaqus Analysis User's Manual.
Choose Transient to perform time integration with the backward Euler method in the pure conduction elements. This method is unconditionally stable for linear problems. For more information, see “Transient analysis” in “Uncoupled heat transfer analysis,” Section 6.5.2 of the Abaqus Analysis User's Manual.
Note: After you have selected a Response option, a message appears informing you that Abaqus/Standard has selected the Default load variation with time option (located on the Other tabbed page) that corresponds to your Response selection. Click Dismiss to close the message dialog box.
In the Time period field, enter the time period of the step.
To configure settings on the Incrementation tabbed page:
In the Edit Step dialog box, display the Incrementation tabbed page.
(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)
Choose a Type option:
Choose Automatic if you want Abaqus/Standard to determine suitable time increment sizes.
Choose Fixed to specify direct user control of the incrementation. Abaqus/Standard uses an increment size that you specify as the constant increment size throughout the step.
In the Maximum number of increments field, enter the upper limit to the number of increments in the step. The analysis stops if this maximum is exceeded before Abaqus/Standard arrives at the complete solution for the step.
If you selected Automatic in Step 2, enter values for Increment size:
In the Initial field, enter the initial time increment. Abaqus/Standard modifies this value as required throughout the step.
In the Minimum field, enter the minimum time increment allowed. If Abaqus/Standard needs a smaller time increment than this value, it terminates the analysis.
In the Maximum field, enter the maximum time increment allowed.
If you selected Fixed in Step 2, enter a value for the constant time increment in the Increment size field.
If you selected Transient analysis on the Basic tabbed page, do the following:
Toggle on End step when temperature change is less than n if you want the analysis to end when the temperature at every temperature degree of freedom changes at a rate that is less than a rate that you specify. If you toggle on this option, enter the desired temperature change rate in the field provided.
If you selected Automatic in Step 2, enter a value for the Max. allowable temperature change per increment. Abaqus/Standard restricts the time step to ensure that this value is not exceeded at any node (except nodes whose temperature degree of freedom is constrained via boundary conditions, MPCs, etc.) during any increment of the step.
If you selected Automatic in Step 2 and you are performing a cavity radiation analysis, enter a value for Max. allowable emissivity change per increment or accept the default of 0.1. If this value is exceeded, Abaqus/Standard cuts back the increment until the maximum change in emissivity is less than the specified value. See “Cavity radiation,” Section 36.1.1 of the Abaqus Analysis User's Manual, for more information.
To configure settings on the Other tabbed page:
In the Edit Step dialog box, display the Other tabbed page.
(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)
Choose an Equation Solver Method option:
Choose Direct to use the default direct sparse solver.
Choose Iterative to use the domain decomposition iterative linear equation solver. For more information, see “Iterative linear equation solver,” Section 6.1.5 of the Abaqus Analysis User's Manual.
Choose a Matrix storage option:
Choose Use solver default to allow Abaqus/Standard to decide whether a symmetric or unsymmetric matrix storage and solution scheme is needed.
Choose Unsymmetric to restrict Abaqus/Standard to the unsymmetric storage and solution scheme.
Choose Symmetric to restrict Abaqus/Standard to the symmetric storage and solution scheme.
Choose a Solution technique option:
Choose Full Newton to use Newton's method as a numerical technique for solving nonlinear equilibrium equations. For more information, see “Nonlinear solution methods in Abaqus/Standard,” Section 2.2.1 of the Abaqus Theory Manual.
Choose Quasi-Newton to use the quasi-Newton technique for solving nonlinear equilibrium equations. This technique can save substantial computational cost in some cases. Generally it is most successful when the system is large and the stiffness matrix is not changing much from iteration to iteration. You can use this technique only for symmetric systems of equations.
If you choose this technique, enter a value for the Number of iterations allowed before the kernel matrix is reformed. The maximum number of iterations allowed is 25. The default number of iterations is 8.
For more information, see “Quasi-Newton solution technique,” Section 2.2.2 of the Abaqus Theory Manual.
Click the arrow to the right of the Convert severe discontinuity iterations field, and select an option for dealing with severe discontinuities during nonlinear analysis:
Select Off to force a new iteration if severe discontinuities occur during an iteration, regardless of the magnitude of the penetration and force errors. This option also changes some time incrementation parameters and uses different criteria to determine whether to do another iteration or to make a new attempt with a smaller increment size.
Select On to use local convergence criteria to determine whether a new iteration is needed. Abaqus/Standard will determine the maximum penetration and estimated force errors associated with severe discontinuities and check whether these errors are within the tolerances. Hence, a solution may converge if the severe discontinuities are small.
Select Propagate from previous step to use the value specified in the previous general analysis step. This value appears in parentheses to the right of the field.
Abaqus/Standard automatically selects the Default load variation with time option that corresponds to your Response selection on the Basic tabbed page. It is recommended that you leave the Default load variation with time selection unchanged.
Click the arrow to the right of the Extrapolation of previous state at start of each increment field, and select a method for determining the first guess to the incremental solution:
Select Linear to indicate that the process is essentially monotonic and Abaqus/Standard should use a 100% linear extrapolation, in time, of the previous incremental solution to begin the nonlinear equation solution for the current increment.
Select Parabolic to indicate that the process should use a quadratic extrapolation, in time, of the previous two incremental solutions to begin the nonlinear equation solution for the current increment.
Select None to suppress any extrapolation.
When you have finished configuring settings for the heat transfer step, click OK to close the Edit Step dialog box.
General linear or nonlinear dynamic analysis in Abaqus/Standard uses implicit time integration to calculate the transient dynamic response of a system. See “Implicit dynamic analysis using direct integration,” Section 6.3.2 of the Abaqus Analysis User's Manual, or “Implicit dynamic analysis,” Section 2.4.1 of the Abaqus Theory Manual, for details on implicit dynamic analysis.
To create or edit a dynamic, implicit procedure:
Display the Edit Step dialog box following the procedure outlined in “Creating a step,” Section 14.9.2 (Procedure type: General; Dynamic, Implicit), or “Editing a step,” Section 14.9.3.
On the Basic, Incrementation, and Other tabbed pages, configure settings such as the time period for the step, increment size, and equation solver preferences as described in the following procedures.
To configure settings on the Basic tabbed page:
In the Edit Step dialog box, display the Basic tabbed page.
In the Description field, enter a short description of the analysis step. Abaqus stores the text that you enter in the output database, and the text is displayed in the state block by the Visualization module.
In the Time period field, enter the time period of the step.
Select an Nlgeom option:
Toggle Nlgeom Off to perform a geometrically linear analysis during the current step.
Toggle Nlgeom On to indicate that Abaqus/Standard should account for geometric nonlinearity during the step. Once you have toggled Nlgeom on, it will be active during all subsequent steps in the analysis.
Toggle on Include adiabatic heating effects if you are performing an adiabatic stress analysis. This option is relevant only for isotropic metal plasticity materials with a Mises yield surface. For more information, see “Adiabatic analysis,” Section 6.5.5 of the Abaqus Analysis User's Manual.
To configure settings on the Incrementation tabbed page:
In the Edit Step dialog box, display the Incrementation tabbed page.
(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)
Choose a Type option:
Choose Automatic to allow Abaqus/Standard to choose the size of the increments based on computational efficiency.
Choose Fixed to specify direct user control of the incrementation. Abaqus/Standard uses an increment size that you specify as the constant increment size throughout the step.
Warning: Fixed incrementation is not generally recommended; it should be used only in special cases when you have a thorough understanding of how to interpret results obtained in this way. Impact events are particularly difficult to solve using fixed time increments.
In the Maximum number of increments field, enter the upper limit to the number of increments in the step. The analysis stops if this maximum is exceeded before Abaqus/Standard arrives at the complete solution for the step.
If you selected Automatic in Step 2, do the following:
Enter values for Increment size:
In the Initial field, enter the initial time increment. Abaqus/Standard modifies this value as required throughout the step.
In the Minimum field, enter the minimum time increment allowed. If Abaqus/Standard needs a smaller time increment than this value, it terminates the analysis.
In the Maximum field, enter the maximum time increment allowed.
In the Half-step residual tolerance field, enter the equilibrium residual error (out-of-balance forces) halfway through a time increment.
This half-step residual check is the basis of the adaptive time incrementation scheme. If the half-step residual is small, it indicates that the accuracy of the solution is high and that the time step can be increased safely; conversely, if the half-step residual is large, the time step used in the solution should be reduced. For more information, see “Automatic time incrementation” in “Implicit dynamic analysis using direct integration,” Section 6.3.2 of the Abaqus Analysis User's Manual.
If you selected Fixed in Step 2, do the following:
Enter a value for the constant time increment in the Increment size field.
If desired, toggle on Suppress half-step residual calculation to reduce the solution cost.
To configure settings on the Other tabbed page:
In the Edit Step dialog box, display the Other tabbed page.
(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)
Choose a Matrix storage option:
Choose Use solver default to allow Abaqus/Standard to decide whether a symmetric or unsymmetric matrix storage and solution scheme is needed.
Choose Unsymmetric to restrict Abaqus/Standard to the unsymmetric storage and solution scheme.
Choose Symmetric to restrict Abaqus/Standard to the symmetric storage and solution scheme.
Choose a Solution technique:
Choose Full Newton to use Newton's method as a numerical technique for solving nonlinear equilibrium equations. For more information, see “Nonlinear solution methods in Abaqus/Standard,” Section 2.2.1 of the Abaqus Theory Manual.
Choose Quasi-Newton to use the quasi-Newton technique for solving nonlinear equilibrium equations. This technique can save substantial computational cost in some cases. Generally it is most successful when the system is large and the stiffness matrix is not changing much from iteration to iteration. You can use this technique only for symmetric systems of equations.
If you choose this technique, enter a value for the Number of iterations allowed before the kernel matrix is reformed. The maximum number of iterations allowed is 25. The default number of iterations is 8.
For more information, see “Quasi-Newton solution technique,” Section 2.2.2 of the Abaqus Theory Manual.
Click the arrow to the right of the Convert severe discontinuity iterations field, and select an option for dealing with severe discontinuities during nonlinear analysis:
Select Off to force a new iteration if severe discontinuities occur during an iteration, regardless of the magnitude of the penetration and force errors. This option also changes some time incrementation parameters and uses different criteria to determine whether to do another iteration or to make a new attempt with a smaller increment size.
Select On to use local convergence criteria to determine whether a new iteration is needed. Abaqus/Standard will determine the maximum penetration and estimated force errors associated with severe discontinuities and check whether these errors are within the tolerances. Hence, a solution may converge if the severe discontinuities are small.
Select Propagate from previous step to use the value specified in the previous general analysis step. This value appears in parentheses to the right of the field.
Choose an option for Default load variation with time:
Choose Instantaneous if you want loads to be applied instantaneously at the start of the step and remain constant throughout the step.
Choose Ramp linearly over step if the load magnitude is to vary linearly over the step, from the value at the end of the previous step to the full magnitude of the load.
Click the arrow to the right of the Extrapolation of previous state at start of each increment field, and select a method for determining the first guess to the incremental solution:
Select Linear to indicate that the process is essentially monotonic and Abaqus/Standard should use a 100% linear extrapolation, in time, of the previous incremental solution to begin the nonlinear equation solution for the current increment.
Select Parabolic to indicate that the process should use a quadratic extrapolation, in time, of the previous two incremental solutions to begin the nonlinear equation solution for the current increment.
Select None to suppress any extrapolation.
In the Numerical damping control parameter field, enter a value for the numerical (artificial) damping control parameter, 
, in the implicit operator. Allowable values are zero (no damping) to –0.333 (maximum damping). The default value is –0.05, which provides slight numerical damping. For more information, see “Artificial damping” in “Implicit dynamic analysis using direct integration,” Section 6.3.2 of the Abaqus Analysis User's Manual.
By default, Abaqus/Standard calculates accelerations at the beginning of a dynamic step. However, you can toggle on Bypass calculations of initial accelerations at the beginning of step if you prefer the following approach:
If the current step is the first dynamic step, Abaqus/Standard assumes that the initial accelerations for the current step are zero.
If the immediately preceding step was also a dynamic step, Abaqus/Standard uses the accelerations from the end of the previous step to continue the new step.
If you selected Fixed time incrementation on the Incrementation tabbed page, you can toggle on Accept solution after reaching maximum number of iterations. This option directs Abaqus/Standard to accept the solution to an increment after the maximum number of iterations allowed has been completed, even if the equilibrium tolerances are not satisfied. Very small increments and a minimum of two iterations are usually necessary if you use this option.
Warning: This approach is not recommended; you should use it only in special cases when you have a thorough understanding of how to interpret results obtained in this way.
When you have finished configuring settings for the step, click OK to close the Edit Step dialog box.
You must configure a fully coupled temperature-displacement analysis when the stress analysis is dependent on the temperature distribution and the temperature distribution depends on the stress solution. For example, metalworking problems may include significant heating due to inelastic deformation of the material which, in turn, changes the material properties. For such cases the thermal and mechanical solutions must be obtained simultaneously rather than sequentially. For more information, see “Fully coupled thermal-stress analysis,” Section 6.5.4 of the Abaqus Analysis User's Manual.
To create or edit a coupled temperature-displacement procedure:
Display the Edit Step dialog box following the procedure outlined in “Creating a step,” Section 14.9.2 (Procedure type: General; Coupled temp-displacement), or “Editing a step,” Section 14.9.3.
On the Basic, Incrementation, and Other tabbed pages, configure settings such as the time period for the step, increment size, and solution technique preferences as described in the following procedures.
To configure settings on the Basic tabbed page:
In the Edit Step dialog box, display the Basic tabbed page.
In the Description field, enter a short description of the analysis step. Abaqus stores the text that you enter in the output database, and the text is displayed in the state block by the Visualization module.
Indicate whether you want Steady-state or Transient response. See the following sections for more information:
Note: After you have selected a Response option, a message appears informing you that Abaqus/Standard has selected the Default load variation with time option (located on the Other tabbed page) that corresponds to your Response selection. Click Dismiss to close the message dialog box.
In the Time period field, enter the time period of the step.
Choose an Nlgeom option:
Toggle Nlgeom Off to perform a geometrically linear analysis during the current step.
Toggle Nlgeom On to indicate that Abaqus/Standard should account for geometric nonlinearity during the step. Once you have toggled Nlgeom on, it will be active during all subsequent steps in the analysis.
Select an automatic stabilization method if you expect the problem to have local instabilities such as surface wrinkling, material instability, or local buckling. Abaqus/Standard can stabilize this class of problems by applying damping throughout the model. For more information, see “Unstable problems” in “Static stress analysis,” Section 6.2.2 of the Abaqus Analysis User's Manual, and “Automatic stabilization of static problems with a constant damping factor” in “Solving nonlinear problems,” Section 7.1.1 of the Abaqus Analysis User's Manual
Click the arrow to the right of Automatic stabilization, and select a method for defining the damping factor:
Select Specify dissipated energy fraction to allow Abaqus/Standard to calculate the damping factor from a dissipated energy fraction that you provide. Enter a value for the dissipated energy fraction in the adjacent field (the default is 2.0 × 10–4). For more information, see “Calculating the damping factor based on the dissipated energy fraction” in “Solving nonlinear problems,” Section 7.1.1 of the Abaqus Analysis User's Manual.
Select Specify damping factor to enter the damping factor directly. Enter a value for the damping factor in the adjacent field. For more information, see “Directly specifying the damping factor” in “Solving nonlinear problems,” Section 7.1.1 of the Abaqus Analysis User's Manual.
Select Use damping factors from previous general step to use the damping factors at the end of the previous step as the initial factors in the current step's variable damping scheme. These factors override any initial damping factors that are calculated or specified directly in the current step. If there are no damping factors associated with the previous general step (for example, if the previous step does not use any stabilization or the current step is the first step of the analysis), Abaqus uses adaptive stabilization to determine the required damping factors.
When using automatic stabilization, Abaqus can use the same damping factor over the course of a step, or it can vary the damping factor spatially and temporally during a step based on the convergence history and the ratio of the energy dissipated by damping to the total strain energy. For more information, see “Adaptive automatic stabilization scheme” in “Solving nonlinear problems,” Section 7.1.1 of the Abaqus Analysis User's Manual. If you selected Specify dissipated energy fraction, adaptive stabilization is optional and turned on by default. If you selected Specify damping factor, adaptive stabilization is optional and turned off by default. If you selected Use damping factors from previous general step, adaptive stabilization is required.
To use adaptive stabilization, toggle on Use adaptive stabilization with max. ratio of stabilization to strain energy (if necessary), and enter a value in the adjacent field for the allowable accuracy tolerance for the ratio of energy dissipated by damping to total strain energy in each increment. The default value of 0.05 should be suitable in most cases.
If desired, toggle on Include creep/swelling/viscoelastic behavior. If you leave this option toggled off, you indicate that there is no creep or viscoelastic response occurring during this step even if creep or viscoelastic material properties have been defined.
To configure settings on the Incrementation tabbed page:
In the Edit Step dialog box, display the Incrementation tabbed page.
(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)
Choose a Type option:
Choose Automatic if you want Abaqus/Standard to determine suitable time increment sizes.
Choose Fixed to specify direct user control of the incrementation. Abaqus/Standard uses an increment size that you specify as the constant increment size throughout the step.
In the Maximum number of increments field, enter the upper limit to the number of increments in the step. The analysis stops if this maximum is exceeded before Abaqus/Standard arrives at the complete solution for the step.
If you selected Automatic in Step 2, enter values for Increment size:
In the Initial field, enter the initial time increment. Abaqus/Standard modifies this value as required throughout the step.
In the Minimum field, enter the minimum time increment allowed. If Abaqus/Standard needs a smaller time increment than this value, it terminates the analysis.
In the Maximum field, enter the maximum time increment allowed.
If you selected Fixed in Step 2, enter a value for the constant time increment in the Increment size field.
If you selected Automatic in Step 2 and if you selected Transient response on the Basic tabbed page, do the following:
Enter a value for the Max. allowable temperature change per increment. Abaqus/Standard restricts the time step to ensure that this value is not exceeded at any node during any increment of the step.
If you toggled on Include creep/swelling/viscoelastic behavior on the Basic tabbed page, toggle on Creep/swelling/viscoelastic strain error tolerance to enter the maximum difference in the creep strain increment calculated from the creep strain rates at the beginning and at the end of the increment. This value controls the accuracy of the creep integration. For more information, see “Automatic incrementation controlled by the creep response” in “Fully coupled thermal-stress analysis,” Section 6.5.4 of the Abaqus Analysis User's Manual.
If you toggled on Include creep/swelling/viscoelastic behavior on the Basic tabbed page, choose a Creep/swelling/viscoelastic integration option:
Choose Explicit/Implicit if you want to allow Abaqus/Standard to invoke the implicit integration scheme. For most coupled thermal-stress analyses, the unconditional stability of the backward difference operator (implicit method) is desirable.
Choose Explicit if you want to restrict Abaqus/Standard to using explicit integration. Explicit integration can be less expensive computationally and simplifies implementation of user-defined creep laws in user subroutine CREEP.
To configure settings on the Other tabbed page:
In the Edit Step dialog box, display the Other tabbed page.
(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)
Choose a Matrix storage option:
Choose Use solver default to allow Abaqus/Standard to decide whether a symmetric or unsymmetric matrix storage and solution scheme is needed.
Choose Unsymmetric to restrict Abaqus/Standard to the unsymmetric storage and solution scheme. (This is the only matrix storage option available if you choose the Full Newton solution technique.)
Choose Symmetric to restrict Abaqus/Standard to the symmetric storage and solution scheme.
Choose a Solution technique:
Choose Full Newton to use Newton's method as a numerical technique for solving nonlinear equilibrium equations. For more information, see “Nonlinear solution methods in Abaqus/Standard,” Section 2.2.1 of the Abaqus Theory Manual.
Choose Separated to specify that linearized equations for the individual fields in the fully coupled procedure are to be decoupled and solved separately for each field. This option provides a less costly solution for an analysis that is fully coupled in the sense that the mechanical and thermal solutions evolve simultaneously, but with a weak coupling between the two solutions. For more information, see “Approximate implementation” in “Fully coupled thermal-stress analysis,” Section 6.5.4 of the Abaqus Analysis User's Manual.
Choose Contact iterations to use contact iterations instead of regular severe discontinuity iterations to speed up computations. Contact iterations are effective for the solution of large, geometrically linear, small-sliding, frictionless static problems with many severe discontinuity iterations.
If you choose this technique, enter the following values:
Adjustment factor for the number of solutions in any iteration. This value is a correction factor on the maximum number of right-hand-side solutions during any contact iteration.
Maximum number of contact iterations. This value specifies the maximum number of contact iterations allowed before new global matrix assemblage and factorization.
Click the arrow to the right of the Convert severe discontinuity iterations field, and select an option for dealing with severe discontinuities during nonlinear analysis:
Select Off to force a new iteration if severe discontinuities occur during an iteration, regardless of the magnitude of the penetration and force errors. This option also changes some time incrementation parameters and uses different criteria to determine whether to do another iteration or to make a new attempt with a smaller increment size.
Select On to use local convergence criteria to determine whether a new iteration is needed. Abaqus/Standard will determine the maximum penetration and estimated force errors associated with severe discontinuities and check whether these errors are within the tolerances. Hence, a solution may converge if the severe discontinuities are small.
Select Propagate from previous step to use the value specified in the previous general analysis step. This value appears in parentheses to the right of the field.
Abaqus/Standard automatically selects the Default load variation with time option that corresponds to your Response selection on the Basic tabbed page. It is recommended that you leave the Default load variation with time selection unchanged.
Click the arrow to the right of the Extrapolation of previous state at start of each increment field, and select a method for determining the first guess to the incremental solution:
Select Linear to indicate that the process is essentially monotonic and Abaqus/Standard should use a 100% linear extrapolation, in time, of the previous incremental solution to begin the nonlinear equation solution for the current increment.
Select Parabolic to indicate that the process should use a quadratic extrapolation, in time, of the previous two incremental solutions to begin the nonlinear equation solution for the current increment.
Select None to suppress any extrapolation.
When you have finished configuring settings for the step, click OK to close the Edit Step dialog box.
Joule heating arises when the energy dissipated by an electrical current flowing through a conductor is converted into thermal energy. Abaqus/Standard provides a fully coupled thermal-electrical procedure for analyzing this type of problem; the coupled thermal-electrical equations are solved simultaneously for both temperature and electrical potential at the nodes. For more information, see “Coupled thermal-electrical analysis,” Section 6.6.2 of the Abaqus Analysis User's Manual.
To create or edit a coupled thermal-electrical procedure:
Display the Edit Step dialog box following the procedure outlined in “Creating a step,” Section 14.9.2 (Procedure type: General; Coupled thermal-electric), or “Editing a step,” Section 14.9.3.
On the Basic, Incrementation, and Other tabbed pages, configure settings such as the time period for the step, increment size, and solution technique preferences as described in the following procedures.
To configure settings on the Basic tabbed page:
In the Edit Step dialog box, display the Basic tabbed page.
In the Description field, enter a short description of the analysis step. Abaqus stores the text that you enter in the output database, and the text is displayed in the state block by the Visualization module.
Choose a Response option:
Choose Steady-state to omit the internal energy term (the specific heat term) in the governing heat transfer equation. Only direct current is considered in the electrical problem, and it is assumed that the system has negligible capacitance. (Electrical transient effects are so rapid that they can be neglected.) For more information, see “Steady-state analysis” in “Coupled thermal-electrical analysis,” Section 6.6.2 of the Abaqus Analysis User's Manual.
Choose Transient to perform time integration with the same backward Euler method used in uncoupled heat transfer analyses. This method is unconditionally stable for linear problems. For more information, see “Transient analysis” in “Coupled thermal-electrical analysis,” Section 6.6.2 of the Abaqus Analysis User's Manual.
Note: After you have selected a Response option, a message appears informing you that Abaqus/Standard has selected the Default load variation with time option (located on the Other tabbed page) that corresponds to your Response selection. Click Dismiss to close the message dialog box.
In the Time period field, enter the time period of the step.
To configure settings on the Incrementation tabbed page:
In the Edit Step dialog box, display the Incrementation tabbed page.
(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)
Choose a Type option:
Choose Automatic if you want Abaqus/Standard to determine suitable time increment sizes.
Choose Fixed to specify direct user control of the incrementation. Abaqus/Standard uses an increment size that you specify as the constant increment size throughout the step.
In the Maximum number of increments field, enter the upper limit to the number of increments in the step. The analysis stops if this maximum is exceeded before Abaqus/Standard arrives at the complete solution for the step.
If you selected Automatic in Step 2, enter values for Increment size:
In the Initial field, enter the initial time increment. Abaqus/Standard modifies this value as required throughout the step.
In the Minimum field, enter the minimum time increment allowed. If Abaqus/Standard needs a smaller time increment than this value, it terminates the analysis.
In the Maximum field, enter the maximum time increment allowed.
If you selected Fixed in Step 2, enter a value for the constant time increment in the Increment size field.
If you selected Transient analysis on the Basic tabbed page, do the following:
Toggle on End step when temperature change is less than n if you want the analysis to end when the temperature at every temperature degree of freedom changes at a rate that is less than a rate that you specify. If you toggle on this option, enter the desired temperature change rate in the field provided.
If you selected Automatic in Step 2, enter a value for the Max. allowable temperature change per increment. Abaqus/Standard restricts the time step to ensure that this value is not exceeded at any node (except nodes with boundary conditions) during any increment of the step.
If you selected Automatic in Step 2 and you are performing a cavity radiation analysis, enter a value for Max. allowable emissivity change per increment, or accept the default of 0.1. If this value is exceeded, Abaqus/Standard cuts back the increment until the maximum change in emissivity is less than the specified value. See “Cavity radiation,” Section 36.1.1 of the Abaqus Analysis User's Manual, for more information.
To configure settings on the Other tabbed page:
In the Edit Step dialog box, display the Other tabbed page.
(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)
Choose a Matrix storage option:
Choose Use solver default to allow Abaqus/Standard to decide whether a symmetric or unsymmetric matrix storage and solution scheme is needed.
Choose Unsymmetric to restrict Abaqus/Standard to the unsymmetric storage and solution scheme. (This is the only matrix storage option available if you choose the Full Newton solution technique.)
Choose Symmetric to restrict Abaqus/Standard to the symmetric storage and solution scheme.
Choose a Solution technique:
Choose Full Newton to use Newton's method as a numerical technique for solving nonlinear equilibrium equations. For more information, see “Nonlinear solution methods in Abaqus/Standard,” Section 2.2.1 of the Abaqus Theory Manual.
Choose Separated to specify that linearized equations for the individual fields in the fully coupled procedure are to be decoupled and solved separately for each field. This option provides a less costly solution for an analysis that is fully coupled in the sense that the electrical and thermal solutions evolve simultaneously, but with a weak coupling between the two solutions. For more information, see “Approximate implementation” in “Coupled thermal-electrical analysis,” Section 6.6.2 of the Abaqus Analysis User's Manual.
Click the arrow to the right of the Convert severe discontinuity iterations field, and select an option for dealing with severe discontinuities during nonlinear analysis:
Select Off to force a new iteration if severe discontinuities occur during an iteration, regardless of the magnitude of the penetration and force errors. This option also changes some time incrementation parameters and uses different criteria to determine whether to do another iteration or to make a new attempt with a smaller increment size.
Select On to use local convergence criteria to determine whether a new iteration is needed. Abaqus/Standard will determine the maximum penetration and estimated force errors associated with severe discontinuities and check whether these errors are within the tolerances. Hence, a solution may converge if the severe discontinuities are small.
Select Propagate from previous step to use the value specified in the previous general analysis step. This value appears in parentheses to the right of the field.
Abaqus/Standard automatically selects the Default load variation with time option that corresponds to your Response selection on the Basic tabbed page. It is recommended that you leave the Default load variation with time selection unchanged.
Click the arrow to the right of the Extrapolation of previous state at start of each increment field, and select a method for determining the first guess to the incremental solution:
Select Linear to indicate that the process is essentially monotonic and Abaqus/Standard should use a 100% linear extrapolation, in time, of the previous incremental solution to begin the nonlinear equation solution for the current increment.
Select Parabolic to indicate that the process should use a quadratic extrapolation, in time, of the previous two incremental solutions to begin the nonlinear equation solution for the current increment.
Select None to suppress any extrapolation.
When you have finished configuring settings for the step, click OK to close the Edit Step dialog box.
You must configure a fully coupled temperature-displacement analysis when the stress analysis is dependent on the temperature distribution and the temperature distribution depends on the stress solution. For such cases the thermal and mechanical solutions must be obtained simultaneously rather than sequentially. In Abaqus/Explicit a fully coupled thermal-stress analysis includes inertia effects and models transient thermal response. For more information, see “Fully coupled thermal-stress analysis in Abaqus/Explicit” in “Fully coupled thermal-stress analysis,” Section 6.5.4 of the Abaqus Analysis User's Manual.
To create or edit a coupled temperature-displacement procedure using explicit integration:
Display the Edit Step dialog box following the procedure outlined in “Creating a step,” Section 14.9.2 (Procedure type: General; Dynamic, Temp-disp, Explicit), or “Editing a step,” Section 14.9.3.
On the Basic, Incrementation, Mass scaling, and Other tabbed pages, configure settings such as the time period for the step, the increment size, mass scaling definitions, and bulk viscosity parameters as described in the following procedures.
To configure settings on the Basic tabbed page:
In the Edit Step dialog box, display the Basic tabbed page.
In the Description field, enter a short description of the analysis step. Abaqus stores the text that you enter in the output database, and the text is displayed in the state block by the Visualization module.
In the Time period field, enter the time period of the step.
Select an Nlgeom option:
Toggle Nlgeom Off to perform a geometrically linear analysis during the current step.
Toggle Nlgeom On to indicate that Abaqus/Explicit should account for geometric nonlinearity during the step. Once you have toggled Nlgeom on, it will be active during all subsequent steps in the analysis.
To configure settings on the Incrementation tabbed page:
In the Edit Step dialog box, display the Incrementation tabbed page.
(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)
Choose a Type option:
Choose Automatic to allow Abaqus/Explicit to determine the time incrementation automatically. For more information, see “Automatic time incrementation” in “Fully coupled thermal-stress analysis,” Section 6.5.4 of the Abaqus Analysis User's Manual.
Choose Fixed to use a fixed time incrementation scheme. The fixed time increment size is determined either by the initial element stability estimate for the step or by a user-specified time increment. For more information, see “Fixed time incrementation” in “Fully coupled thermal-stress analysis,” Section 6.5.4 of the Abaqus Analysis User's Manual.
If you selected Automatic time incrementation, perform the following steps:
Choose a Stable increment estimator option:
Choose Global to allow the global estimator to determine the stability limit as the step proceeds. The adaptive, global estimation algorithm determines the maximum frequency of the entire model using the current dilatational wave speed. This algorithm continuously updates the estimate for the maximum frequency. The global estimator will usually allow time increments that exceed the element-by-element values.
Choose Element-by-element to allow Abaqus/Explicit to determine an element-by-element estimate using the current dilatational wave speed in each element.
The element-by-element estimate is conservative; it will give a smaller stable time increment than the true stability limit that is based upon the maximum frequency of the entire model. In general, constraints such as boundary conditions and kinematic contact have the effect of compressing the eigenvalue spectrum, and the element-by-element estimates do not take this into account.
Choose a Max. time increment option:
Choose Unlimited if you do not want to impose an upper limit to time incrementation.
Choose Value to enter a value for the maximum time increment allowed. Enter the value in the field provided.
If you selected Fixed time incrementation, choose an option for determining increment size:
Choose User-defined time increment to specify a time increment size directly. Enter that time increment size in the field provided.
Choose Use element-by-element time increment estimator to use time increments the size of the initial element-by-element stability limit throughout the step. The dilatational wave speed in each element at the beginning of the step is used to compute the fixed time increment size.
If desired, enter a Time scaling factor to adjust the stable time increment computed by Abaqus/Explicit. (This option is unavailable if you have specified a User-defined time increment for the Fixed time incrementation scheme.) For more information, see “Scaling the time increment” in “Fully coupled thermal-stress analysis,” Section 6.5.4 of the Abaqus Analysis User's Manual.
To configure settings on the Mass scaling tabbed page:
In the Edit Step dialog box, display the Mass scaling tabbed page. For background information on mass scaling, see “Mass scaling,” Section 11.7.1 of the Abaqus Analysis User's Manual.
(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)
Choose one of the following options for specifying mass scaling:
Choose Use scaled mass and “throughout step” definitions from the previous step if you want mass scaling definitions from the previous step to propagate through the current step. If you choose this option, you can skip the remaining steps in this procedure.
Choose Use scaling definitions below to create one or more new mass scaling definitions for this step. If you choose this option, complete the remaining steps in this procedure.
At the bottom of the Data table, click Create.
An Edit mass scaling dialog box appears.
Specify which type of mass scaling definition you want to create:
Choose Semi-automatic mass scaling to define mass scaling for any type of analysis except bulk metal rolling.
Choose Automatic mass scaling to define mass scaling for a bulk metal rolling analysis. For more information, see “Automatic mass scaling for analysis of bulk metal rolling” in “Mass scaling,” Section 11.7.1 of the Abaqus Analysis User's Manual.
Choose Reinitialize mass to reinitialize masses of elements to their original values. This option allows you to prevent the scaled mass from a previous step from being used in the current step. For more information, see “Reinitializing the mass” in “Mass scaling,” Section 11.7.1 of the Abaqus Analysis User's Manual.
Choose Disable mass scaling thoughout step to disable in this step all variable mass scaling definitions from previous steps. For more information, see “Removing mass scaling definitions” in “Mass scaling,” Section 11.7.1 of the Abaqus Analysis User's Manual.
If you selected Semi-automatic mass scaling, Automatic mass scaling, or Reinitialize mass, indicate the region to which you want the mass scaling definition applied:
Choose Whole model to apply the mass scaling definition to all elements in the model.
Choose Set to apply the mass scaling definition to a particular set of elements. Click the arrow to the right of the Set field, and select the set name of interest.
If you selected Semi-automatic mass scaling, indicate when, during the step, you want Abaqus/Explicit to scale the element masses:
Choose At beginning of step to perform fixed mass scaling only at the beginning of the step. For more information, see “Fixed mass scaling” in “Mass scaling,” Section 11.7.1 of the Abaqus Analysis User's Manual.
Choose Throughout step to scale the mass of elements periodically during the step. For more information, see “Variable mass scaling” in “Mass scaling,” Section 11.7.1 of the Abaqus Analysis User's Manual.
If you selected Semi-automatic mass scaling, indicate how you want Abaqus/Explicit to scale the element masses:
Toggle on Scale by factor to scale the elements once at the beginning of the step by the value you enter in the field provided. For more information, see “Defining a scale factor directly” in “Mass scaling,” Section 11.7.1 of the Abaqus Analysis User's Manual.
Toggle on Scale to target time increment of n to enter a desired element stable time increment in the field provided. Click the arrow to the right of the Scale element mass field, and select how you want Abaqus/Explicit to apply that target time increment:
Select Uniformly to satisfy target to scale the masses of the elements equally so that the smallest element stable time increment of the scaled elements equals the target value.
Select If below minimum target to scale the masses of only the elements whose element stable time increments are less than the target value.
Select Nonuniformly to equal target to scale the masses of all elements so that they all have the same element stable time increment equal to the target value.
If you selected Automatic mass scaling, enter the following values:
In the Feed rate field, enter the estimated average velocity of the workpiece in the rolling direction at steady-state conditions.
In the Extruded element length field, enter the average element length in the rolling direction.
In the Nodes in cross-section field, enter the number of nodes in the cross-section of the workpiece. Increasing this value decreases the amount of mass scaling.
If you selected Semi-automatic mass scaling throughout the step or Automatic mass scaling, specify when, during the step, you want Abaqus/Explicit to perform mass scaling calculations:
Choose Every n increments to specify the frequency, in increments, at which Abaqus/Explicit is to perform mass scaling calculations. Enter the desired frequency in the field provided.
For example, if you enter a value of 5, Abaqus/Explicit scales the mass at the beginning of the step and at increments 5, 10, 15, etc.
Choose At n equal intervals to specify the number of intervals during the step at which Abaqus/Explicit is to perform mass scaling calculations. Enter the desired value in the field provided.
For example, if you enter a value of 2, Abaqus/Explicit scales the mass at the beginning of the step, the increment immediately following the half-way point in the step, and the final increment in the step.
Click OK to close the Edit mass scaling dialog box and return to the Mass scaling tabbed page of the Edit Step dialog box.
The mass scaling definition that you have just created appears in the Data table.
If desired, repeat Steps 3 to 10 to create additional mass scaling definitions.
Once you have created one or more mass scaling definitions, you can edit or delete them if desired. Select a particular mass scaling definition in the Data table, and click Edit or Delete at the bottom of the Data table.
To configure settings on the Other tabbed page:
In the Edit Step dialog box, display the Other tabbed page.
(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)
Enter a value for the Linear bulk viscosity parameter. Linear bulk viscosity is included by default in Abaqus/Explicit.
Enter a value for the Quadratic bulk viscosity parameter. This form of bulk viscosity pressure is found only in solid continuum element and is applied only if the volumetric strain rate is compressive.
For more information, see “Bulk viscosity” in “Explicit dynamic analysis,” Section 6.3.3 of the Abaqus Analysis User's Manual.
When you have finished configuring settings for the step, click OK to close the Edit Step dialog box.
A geostatic stress field procedure allows you to verify that the initial geostatic stress field is in equilibrium with applied loads and boundary conditions. It also allows you to iterate, if necessary, to obtain equilibrium. This type of procedure is usually the first step of a geotechnical analysis, followed by a coupled pore fluid diffusion/stress or static analysis procedure. For more information, see “Geostatic stress state,” Section 6.7.2 of the Abaqus Analysis User's Manual.
To create or edit a geostatic stress field procedure:
Display the Edit Step dialog box following the procedure outlined in “Creating a step,” Section 14.9.2 (Procedure type: General; Geostatic), or “Editing a step,” Section 14.9.3.
On the Basic and Other tabbed pages, configure settings such as controls to include nonlinear effects of large displacements and equation solver preferences as described in the following procedures.
To configure settings on the Basic tabbed page:
In the Edit Step dialog box, display the Basic tabbed page.
In the Description field, enter a short description of the analysis step. Abaqus stores the text that you enter in the output database, and the text is displayed in the state block by the Visualization module.
Select an Nlgeom option:
Toggle Nlgeom Off to perform a geometrically linear analysis during the current step.
Toggle Nlgeom On to indicate that Abaqus/Standard should account for geometric nonlinearity during the step. Once you have toggled Nlgeom on, it will be active during all subsequent steps in the analysis.
To configure settings on the Other tabbed page:
In the Edit Step dialog box, display the Other tabbed page.
(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)
Choose a Matrix storage option:
Choose Use solver default to allow Abaqus/Standard to decide whether a symmetric or unsymmetric matrix storage and solution scheme is needed.
Choose Unsymmetric to restrict Abaqus/Standard to the unsymmetric storage and solution scheme.
Choose Symmetric to restrict Abaqus/Standard to the symmetric storage and solution scheme.
Choose a Solution technique:
Choose Full Newton to use Newton's method as a numerical technique for solving nonlinear equilibrium equations. For more information, see “Nonlinear solution methods in Abaqus/Standard,” Section 2.2.1 of the Abaqus Theory Manual.
Choose Quasi-Newton to use the quasi-Newton technique for solving nonlinear equilibrium equations. This technique can save substantial computational cost in some cases. Generally it is most successful when the system is large and the stiffness matrix is not changing much from iteration to iteration. You can use this technique only for symmetric systems of equations.
If you choose this technique, enter a value for the Number of iterations allowed before the kernel matrix is reformed. The maximum number of iterations allowed is 25. The default number of iterations is 8.
For more information, see “Quasi-Newton solution technique,” Section 2.2.2 of the Abaqus Theory Manual.
Choose Contact iterations to use contact iterations instead of regular severe discontinuity iterations to speed up computations. Contact iterations are effective for the solution of large, geometrically linear, small-sliding, frictionless static problems with many severe discontinuity iterations.
If you choose this technique, enter the following values:
Adjustment factor for the number of solutions in any iteration. This value is a correction factor on the maximum number of right-hand-side solutions during any contact iteration.
Maximum number of contact iterations. This value specifies the maximum number of contact iterations allowed before new global matrix assemblage and factorization.
Click the arrow to the right of the Convert severe discontinuity iterations field, and select an option for dealing with severe discontinuities during nonlinear analysis:
Select Off to force a new iteration if severe discontinuities occur during an iteration, regardless of the magnitude of the penetration and force errors. This option also changes some time incrementation parameters and uses different criteria to determine whether to do another iteration or to make a new attempt with a smaller increment size.
Select On to use local convergence criteria to determine whether a new iteration is needed. Abaqus/Standard will determine the maximum penetration and estimated force errors associated with severe discontinuities and check whether these errors are within the tolerances. Hence, a solution may converge if the severe discontinuities are small.
Select Propagate from previous step to use the value specified in the previous general analysis step. This value appears in parentheses to the right of the field.
When you have finished configuring settings for the step, click OK to close the Edit Step dialog box.
A mass diffusion analysis models the transient or steady-state diffusion of one material through another, such as the diffusion of hydrogen through a metal. The governing equations for mass diffusion are an extension of Fick's equations: they allow for nonuniform solubility of the diffusing substance in the base material and for mass diffusion driven by gradients of temperature and pressure. For more information, see “Mass diffusion analysis,” Section 6.8.1 of the Abaqus Analysis User's Manual.
To create or edit a mass diffusion procedure:
Display the Edit Step dialog box following the procedure outlined in “Creating a step,” Section 14.9.2 (Procedure type: General; Mass diffusion), or “Editing a step,” Section 14.9.3.
On the Basic, Incrementation, and Other tabbed pages, configure settings such as steady-state or transient response and automatic or fixed incrementation as described in the following procedures.
To configure settings on the Basic tabbed page:
In the Edit Step dialog box, display the Basic tabbed page.
In the Description field, enter a short description of the analysis step. Abaqus stores the text that you enter in the output database, and the text is displayed in the state block by the Visualization module.
Choose a Response option:
Choose Steady-state to specify that the analysis provide the steady-state solution directly. The rate of change of concentration with respect to time is omitted from the governing diffusion equation in a steady-state analysis. For more information, see “Steady-state analysis” in “Mass diffusion analysis,” Section 6.8.1 of the Abaqus Analysis User's Manual.
Choose Transient to perform time integration with the backward Euler method. This method is unconditionally stable for linear problems. For more information, see “Transient analysis” in “Mass diffusion analysis,” Section 6.8.1 of the Abaqus Analysis User's Manual.
Note: After you have selected a Response option, a message appears informing you that Abaqus/Standard has selected the Default load variation with time option (located on the Other tabbed page) that corresponds to your Response selection. Click Dismiss to close the message dialog box.
In the Time period field, enter the time period of the step.
To configure settings on the Incrementation tabbed page:
In the Edit Step dialog box, display the Incrementation tabbed page.
(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)
Choose a Type option:
Choose Automatic if you want Abaqus/Standard to determine suitable time increment sizes.
Choose Fixed to specify direct user control of the incrementation. Abaqus/Standard uses an increment size that you specify as the constant increment size throughout the step.
In the Maximum number of increments field, enter the upper limit to the number of increments in the step. The analysis stops if this maximum is exceeded before Abaqus/Standard arrives at the complete solution for the step.
If you selected Automatic incrementation in Step 2, enter values for Increment size:
In the Initial field, enter the initial time increment. Abaqus/Standard modifies this value as required throughout the step.
In the Minimum field, enter the minimum time increment allowed. If Abaqus/Standard needs a smaller time increment than this value, it terminates the analysis.
In the Maximum field, enter the maximum time increment allowed.
If you selected Fixed incrementation in Step 2, enter a value for the constant time increment in the Increment size field.
If you selected Automatic incrementation in Step 2 and Transient analysis on the Basic tabbed page, do the following:
Enter a value in the End step when normalized concentration change is less than n field. The analysis will end when all nodal normalized concentrations are changing at a rate that is less than the rate that you enter.
Enter a value in the Max. allowable normalized concentration change field. Abaqus/Standard restricts the time step to ensure that this value is not exceeded at any node (except nodes with boundary conditions) during any increment of the step.
To configure settings on the Other tabbed page:
In the Edit Step dialog box, display the Other tabbed page.
(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)
Accept the selection of the Unsymmetric matrix storage and solution scheme. This scheme is the only Matrix storage option that is valid for mass diffusion analyses. For more information on matrix storage, see “Matrix storage and solution scheme in Abaqus/Standard” in “Procedures: overview,” Section 6.1.1 of the Abaqus Analysis User's Manual.
Click the arrow to the right of the Convert severe discontinuity iterations field, and select an option for dealing with severe discontinuities during nonlinear analysis:
Select Off to force a new iteration if severe discontinuities occur during an iteration, regardless of the magnitude of the penetration and force errors. This option also changes some time incrementation parameters and uses different criteria to determine whether to do another iteration or to make a new attempt with a smaller increment size.
Select On to use local convergence criteria to determine whether a new iteration is needed. Abaqus/Standard will determine the maximum penetration and estimated force errors associated with severe discontinuities and check whether these errors are within the tolerances. Hence, a solution may converge if the severe discontinuities are small.
Select Propagate from previous step to use the value specified in the previous general analysis step. This value appears in parentheses to the right of the field.
Abaqus/Standard automatically selects the Default load variation with time option that corresponds to your Response selection on the Basic tabbed page. It is recommended that you leave the Default load variation with time selection unchanged.
Click the arrow to the right of the Extrapolation of previous state at start of each increment field, and select a method for determining the first guess to the incremental solution:
Select Linear to indicate that the process is essentially monotonic and Abaqus/Standard should use a 100% linear extrapolation, in time, of the previous incremental solution to begin the nonlinear equation solution for the current increment.
Select Parabolic to indicate that the process should use a quadratic extrapolation, in time, of the previous two incremental solutions to begin the nonlinear equation solution for the current increment.
Select None to suppress any extrapolation.
When you have finished configuring settings for the step, click OK to close the Edit Step dialog box.
A coupled pore fluid diffusion/stress analysis allows you to model single phase, partially or fully saturated fluid flow through porous media. For more information, see “Coupled pore fluid diffusion and stress analysis,” Section 6.7.1 of the Abaqus Analysis User's Manual.
To create or edit a coupled pore fluid diffusion/stress procedure:
Display the Edit Step dialog box following the procedure outlined in “Creating a step,” Section 14.9.2 (Procedure type: General; Soils), or “Editing a step,” Section 14.9.3.
On the Basic, Incrementation, and Other tabbed pages, configure settings such as steady-state or transient pore fluid response and automatic or fixed incrementation as described in the following procedures.
To configure settings on the Basic tabbed page:
In the Edit Step dialog box, display the Basic tabbed page.
In the Description field, enter a short description of the analysis step. Abaqus stores the text that you enter in the output database, and the text is displayed in the state block by the Visualization module.
Choose a Pore fluid response option:
Choose Steady-state to specify that there are no transient effects in the wetting liquid continuity equation. The steady-state solution corresponds to constant wetting liquid velocities and constant volume of wetting liquid per unit volume in the continuum. For more information, see “Steady-state analysis” in “Coupled pore fluid diffusion and stress analysis,” Section 6.7.1 of the Abaqus Analysis User's Manual.
Choose Transient consolidation to use the backward difference operator to integrate the continuity equation. This operator provides unconditional stability so that the only concern with respect to time integration is accuracy. For more information, see “Transient analysis” in “Coupled pore fluid diffusion and stress analysis,” Section 6.7.1 of the Abaqus Analysis User's Manual.
Note: After you have selected a Pore fluid response option, a message appears informing you that Abaqus/Standard has selected the Default load variation with time option and the Matrix storage option (both located on the Other tabbed page) that correspond to your Pore fluid response selection. Click Dismiss to close the message dialog box.
In the Time period field, enter the time period of the step.
Select an Nlgeom option:
Toggle Nlgeom Off to perform a geometrically linear analysis during the current step.
Toggle Nlgeom On to indicate that Abaqus/Standard should account for geometric nonlinearity during the step. Once you have toggled Nlgeom on, it will be active during all subsequent steps in the analysis.
Select an automatic stabilization method if you expect the problem to have local instabilities such as surface wrinkling, material instability, or local buckling. Abaqus/Standard can stabilize this class of problems by applying damping throughout the model. For more information, see “Unstable problems” in “Static stress analysis,” Section 6.2.2 of the Abaqus Analysis User's Manual, and “Automatic stabilization of static problems with a constant damping factor” in “Solving nonlinear problems,” Section 7.1.1 of the Abaqus Analysis User's Manual
Click the arrow to the right of Automatic stabilization, and select a method for defining the damping factor:
Select Specify dissipated energy fraction to allow Abaqus/Standard to calculate the damping factor from a dissipated energy fraction that you provide. Enter a value for the dissipated energy fraction in the adjacent field (the default is 2.0 × 10–4). For more information, see “Calculating the damping factor based on the dissipated energy fraction” in “Solving nonlinear problems,” Section 7.1.1 of the Abaqus Analysis User's Manual.
Select Specify damping factor to enter the damping factor directly. Enter a value for the damping factor in the adjacent field. For more information, see “Directly specifying the damping factor” in “Solving nonlinear problems,” Section 7.1.1 of the Abaqus Analysis User's Manual.
Select Use damping factors from previous general step to use the damping factors at the end of the previous step as the initial factors in the current step's variable damping scheme. These factors override any initial damping factors that are calculated or specified directly in the current step. If there are no damping factors associated with the previous general step (for example, if the previous step does not use any stabilization or the current step is the first step of the analysis), Abaqus uses adaptive stabilization to determine the required damping factors.
When using automatic stabilization, Abaqus can use the same damping factor over the course of a step, or it can vary the damping factor spatially and temporally during a step based on the convergence history and the ratio of the energy dissipated by damping to the total strain energy. For more information, see “Adaptive automatic stabilization scheme” in “Solving nonlinear problems,” Section 7.1.1 of the Abaqus Analysis User's Manual. If you selected Specify dissipated energy fraction, adaptive stabilization is optional and turned on by default. If you selected Specify damping factor, adaptive stabilization is optional and turned off by default. If you selected Use damping factors from previous general step, adaptive stabilization is required.
To use adaptive stabilization, toggle on Use adaptive stabilization with max. ratio of stabilization to strain energy (if necessary), and enter a value in the adjacent field for the allowable accuracy tolerance for the ratio of energy dissipated by damping to total strain energy in each increment. The default value of 0.05 should be suitable in most cases.
If desired, toggle on Include creep/swelling/viscoelastic behavior. If you leave this option toggled off, you indicate that there is no creep or viscoelastic response occurring during this step even if creep or viscoelastic material properties have been defined.
To configure settings on the Incrementation tabbed page:
In the Edit Step dialog box, display the Incrementation tabbed page.
(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)
Choose a Type option:
Choose Automatic if you want Abaqus/Standard to determine suitable time increment sizes.
Choose Fixed to specify direct user control of the incrementation. Abaqus/Standard uses an increment size that you specify as the constant increment size throughout the step.
Note: Fixed incrementation is not generally recommended in this case because the time increments in a typical diffusion analysis can increase over several orders of magnitude during the simulation; automatic incrementation is usually a better choice.
In the Maximum number of increments field, enter the upper limit to the number of increments in the step. The analysis stops if this maximum is exceeded before Abaqus/Standard arrives at the complete solution for the step.
If you selected Automatic in Step 2, enter values for Increment size:
In the Initial field, enter the initial time increment. Abaqus/Standard modifies this value as required throughout the step.
In the Minimum field, enter the minimum time increment allowed. If Abaqus/Standard needs a smaller time increment than this value, it terminates the analysis.
In the Maximum field, enter the maximum time increment allowed.
If you selected Fixed in Step 2, enter a value for the constant time increment in the Increment size field.
If you selected the Transient consolidation response on the Basic tabbed page, toggle on End step when pore pressure change rate is less than n to enter a minimum value for the pore pressure change rate. The analysis will end if all pore pressures are changing at a rate that is less than the rate that you enter.
If you selected Automatic in Step 2, do the following:
If you selected the Transient consolidation response on the Basic tabbed page, enter a value for the Max. pore pressure change per increment. Abaqus/Standard restricts the time step to ensure that this value is not exceeded at any node (except nodes with boundary conditions) during any increment of the step.
If you toggled on Include creep/swelling/viscoelastic behavior on the Basic tabbed page, toggle on Creep/swelling/viscoelastic strain error tolerance to enter the maximum difference in the creep strain increment calculated from the creep strain rates at the beginning and at the end of the increment. This value controls the accuracy of the creep integration. For more information, see “Specifying the tolerance for automatic incrementation” in “Rate-dependent plasticity: creep and swelling,” Section 19.2.4 of the Abaqus Analysis User's Manual.
To configure settings on the Other tabbed page:
In the Edit Step dialog box, display the Other tabbed page.
(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)
Choose a Matrix storage option:
Choose Use solver default to allow Abaqus/Standard to decide whether a symmetric or unsymmetric matrix storage and solution scheme is needed.
Choose Unsymmetric to restrict Abaqus/Standard to the unsymmetric storage and solution scheme.
Note: The steady-state coupled equations are strongly unsymmetric; therefore, the unsymmetric matrix solution and storage scheme is selected automatically for steady-state analysis steps (see “Procedures: overview,” Section 6.1.1 of the Abaqus Analysis User's Manual).
Choose Symmetric to restrict Abaqus/Standard to the symmetric storage and solution scheme.
Choose a Solution technique:
Choose Full Newton to use Newton's method as a numerical technique for solving nonlinear equilibrium equations. For more information, see “Nonlinear solution methods in Abaqus/Standard,” Section 2.2.1 of the Abaqus Theory Manual.
Choose Quasi-Newton to use the quasi-Newton technique for solving nonlinear equilibrium equations. This technique can save substantial computational cost in some cases. Generally it is most successful when the system is large and the stiffness matrix is not changing much from iteration to iteration. You can use this technique only for symmetric systems of equations.
If you choose this technique, enter a value for the Number of iterations allowed before the kernel matrix is reformed. The maximum number of iterations allowed is 25. The default number of iterations is 8.
For more information, see “Quasi-Newton solution technique,” Section 2.2.2 of the Abaqus Theory Manual.
Choose Contact iterations to use contact iterations instead of regular severe discontinuity iterations to speed up computations. Contact iterations are effective for the solution of large, geometrically linear, small-sliding, frictionless static problems with many severe discontinuity iterations.
If you choose this technique, enter the following values:
Adjustment factor for the number of solutions in any iteration. This value is a correction factor on the maximum number of right-hand-side solutions during any contact iteration.
Maximum number of contact iterations. This value specifies the maximum number of contact iterations allowed before new global matrix assemblage and factorization.
Click the arrow to the right of the Convert severe discontinuity iterations field, and select an option for dealing with severe discontinuities during nonlinear analysis:
Select Off to force a new iteration if severe discontinuities occur during an iteration, regardless of the magnitude of the penetration and force errors. This option also changes some time incrementation parameters and uses different criteria to determine whether to do another iteration or to make a new attempt with a smaller increment size.
Select On to use local convergence criteria to determine whether a new iteration is needed. Abaqus/Standard will determine the maximum penetration and estimated force errors associated with severe discontinuities and check whether these errors are within the tolerances. Hence, a solution may converge if the severe discontinuities are small.
Select Propagate from previous step to use the value specified in the previous general analysis step. This value appears in parentheses to the right of the field.
Abaqus/Standard automatically selects the Default load variation with time option that corresponds to your Pore fluid response selection on the Basic tabbed page. It is recommended that you leave the Default load variation with time selection unchanged.
Click the arrow to the right of the Extrapolation of previous state at start of each increment field, and select a method for determining the first guess to the incremental solution:
Select Linear to indicate that the process is essentially monotonic and Abaqus/Standard should use a 100% linear extrapolation, in time, of the previous incremental solution to begin the nonlinear equation solution for the current increment.
Select Parabolic to indicate that the process should use a quadratic extrapolation, in time, of the previous two incremental solutions to begin the nonlinear equation solution for the current increment.
Select None to suppress any extrapolation.
When you have finished configuring settings for the step, click OK to close the Edit Step dialog box.
You can use a quasi-static stress analysis to analyze problems with time-dependent material response (creep, swelling, viscoelasticity, and two-layer viscoplasticity). This type of analysis is valid when inertial effects can be neglected. It can be linear or nonlinear. For more information, see “Quasi-static analysis,” Section 6.2.5 of the Abaqus Analysis User's Manual.
To create or edit a quasi-static stress analysis procedure:
Display the Edit Step dialog box following the procedure outlined in “Creating a step,” Section 14.9.2 (Procedure type: General; Visco), or “Editing a step,” Section 14.9.3.
On the Basic, Incrementation, and Other tabbed pages, configure settings such as the time period, automatic or fixed incrementation, and equation solver preferences as described in the following procedures.
To configure settings on the Basic tabbed page:
In the Edit Step dialog box, display the Basic tabbed page.
In the Description field, enter a short description of the analysis step. Abaqus stores the text that you enter in the output database, and the text is displayed in the state block by the Visualization module.
In the Time period field, enter the time period of the step.
Select an Nlgeom option:
Toggle Nlgeom Off to perform a geometrically linear analysis during the current step.
Toggle Nlgeom On to indicate that Abaqus/Standard should account for geometric nonlinearity during the step. Once you have toggled Nlgeom on, it will be active during all subsequent steps in the analysis.
Select an automatic stabilization method if you expect the problem to have local instabilities such as surface wrinkling, material instability, or local buckling. Abaqus/Standard can stabilize this class of problems by applying damping throughout the model. For more information, see “Unstable problems” in “Static stress analysis,” Section 6.2.2 of the Abaqus Analysis User's Manual, and “Automatic stabilization of static problems with a constant damping factor” in “Solving nonlinear problems,” Section 7.1.1 of the Abaqus Analysis User's Manual
Click the arrow to the right of Automatic stabilization, and select a method for defining the damping factor:
Select Specify dissipated energy fraction to allow Abaqus/Standard to calculate the damping factor from a dissipated energy fraction that you provide. Enter a value for the dissipated energy fraction in the adjacent field (the default is 2.0 × 10–4). For more information, see “Calculating the damping factor based on the dissipated energy fraction” in “Solving nonlinear problems,” Section 7.1.1 of the Abaqus Analysis User's Manual.
Select Specify damping factor to enter the damping factor directly. Enter a value for the damping factor in the adjacent field. For more information, see “Directly specifying the damping factor” in “Solving nonlinear problems,” Section 7.1.1 of the Abaqus Analysis User's Manual.
Select Use damping factors from previous general step to use the damping factors at the end of the previous step as the initial factors in the current step's variable damping scheme. These factors override any initial damping factors that are calculated or specified directly in the current step. If there are no damping factors associated with the previous general step (for example, if the previous step does not use any stabilization or the current step is the first step of the analysis), Abaqus uses adaptive stabilization to determine the required damping factors.
When using automatic stabilization, Abaqus can use the same damping factor over the course of a step, or it can vary the damping factor spatially and temporally during a step based on the convergence history and the ratio of the energy dissipated by damping to the total strain energy. For more information, see “Adaptive automatic stabilization scheme” in “Solving nonlinear problems,” Section 7.1.1 of the Abaqus Analysis User's Manual. If you selected Specify dissipated energy fraction, adaptive stabilization is optional and turned on by default. If you selected Specify damping factor, adaptive stabilization is optional and turned off by default. If you selected Use damping factors from previous general step, adaptive stabilization is required.
To use adaptive stabilization, toggle on Use adaptive stabilization with max. ratio of stabilization to strain energy (if necessary), and enter a value in the adjacent field for the allowable accuracy tolerance for the ratio of energy dissipated by damping to total strain energy in each increment. The default value of 0.05 should be suitable in most cases.
To configure settings on the Incrementation tabbed page:
In the Edit Step dialog box, display the Incrementation tabbed page.
(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)
Choose a Type option:
Choose Automatic if you want Abaqus/Standard to select time increments automatically based on the accuracy of the integration. A Creep/swelling/viscoelastic strain error tolerance parameter that you specify limits the maximum inelastic strain rate change allowed over an increment. Automatic incrementation is recommended for almost all cases.
Choose Fixed to specify direct user control of the incrementation. Abaqus/Standard uses an increment size that you specify as the constant increment size throughout the step.
In the Maximum number of increments field, enter the upper limit to the number of increments in the step. The analysis stops if this maximum is exceeded before Abaqus/Standard arrives at the complete solution for the step.
If you selected Automatic in Step 2, do the following:
Enter values for Increment size:
In the Initial field, enter the initial time increment. Abaqus/Standard modifies this value as required throughout the step.
In the Minimum field, enter the minimum time increment allowed. If Abaqus/Standard needs a smaller time increment than this value, it terminates the analysis.
In the Maximum field, enter the maximum time increment allowed.
In the Creep/swelling/viscoelastic strain error tolerance field, enter the maximum difference in the creep strain increment calculated from the creep strain rates at the beginning and at the end of the increment. This value controls the accuracy of the creep integration. For more information, see “Automatic incrementation” in “Quasi-static analysis,” Section 6.2.5 of the Abaqus Analysis User's Manual.
If you selected Fixed in Step 2, enter a value for the constant time increment in the Increment size field.
Choose a Creep/swelling/viscoelastic integration option:
Choose Explicit/Implicit if you want to allow Abaqus/Standard to invoke the implicit integration scheme. For creep at very low stress levels the unconditional stability of the backward difference operator (implicit method) is desirable.
Choose Explicit if you want to restrict Abaqus/Standard to using explicit integration. Explicit integration can be less expensive computationally and simplifies implementation of user-defined creep laws in user subroutine CREEP
To configure settings on the Other tabbed page:
In the Edit Step dialog box, display the Other tabbed page.
(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)
Choose an Equation Solver Method option:
Choose Direct to use the default direct sparse solver.
Choose Iterative to use the domain decomposition iterative linear equation solver. For more information, see “Iterative linear equation solver,” Section 6.1.5 of the Abaqus Analysis User's Manual.
Choose a Matrix storage option:
Choose Use solver default to allow Abaqus/Standard to decide whether a symmetric or unsymmetric matrix storage and solution scheme is needed.
Choose Unsymmetric to restrict Abaqus/Standard to the unsymmetric storage and solution scheme.
Choose Symmetric to restrict Abaqus/Standard to the symmetric storage and solution scheme.
Choose a Solution technique:
Choose Full Newton to use Newton's method as a numerical technique for solving nonlinear equilibrium equations. For more information, see “Nonlinear solution methods in Abaqus/Standard,” Section 2.2.1 of the Abaqus Theory Manual.
Choose Quasi-Newton to use the quasi-Newton technique for solving nonlinear equilibrium equations. This technique can save substantial computational cost in some cases. Generally it is most successful when the system is large and the stiffness matrix is not changing much from iteration to iteration. You can use this technique only for symmetric systems of equations.
If you choose this technique, enter a value for the Number of iterations allowed before the kernel matrix is reformed. The maximum number of iterations allowed is 25. The default number of iterations is 8.
For more information, see “Quasi-Newton solution technique,” Section 2.2.2 of the Abaqus Theory Manual.
Choose Contact iterations to use contact iterations instead of regular severe discontinuity iterations to speed up computations. Contact iterations are effective for the solution of large, geometrically linear, small-sliding, frictionless static problems with many severe discontinuity iterations.
If you choose this technique, enter the following values:
Adjustment factor for the number of solutions in any iteration. This value is a correction factor on the maximum number of right-hand-side solutions during any contact iteration.
Maximum number of contact iterations. This value specifies the maximum number of contact iterations allowed before new global matrix assemblage and factorization.
Click the arrow to the right of the Convert severe discontinuity iterations field, and select an option for dealing with severe discontinuities during nonlinear analysis:
Select Off to force a new iteration if severe discontinuities occur during an iteration, regardless of the magnitude of the penetration and force errors. This option also changes some time incrementation parameters and uses different criteria to determine whether to do another iteration or to make a new attempt with a smaller increment size.
Select On to use local convergence criteria to determine whether a new iteration is needed. Abaqus/Standard will determine the maximum penetration and estimated force errors associated with severe discontinuities and check whether these errors are within the tolerances. Hence, a solution may converge if the severe discontinuities are small.
Select Propagate from previous step to use the value specified in the previous general analysis step. This value appears in parentheses to the right of the field.
Choose an option for Default load variation with time:
Choose Instantaneous if you want loads to be applied instantaneously at the start of the step and remain constant throughout the step.
Choose Ramp linearly over step if the load magnitude is to vary linearly over the step, from the value at the end of the previous step to the full magnitude of the load.
Click the arrow to the right of the Extrapolation of previous state at start of each increment field, and select a method for determining the first guess to the incremental solution:
Select Linear to indicate that the process is essentially monotonic and Abaqus/Standard should use a 100% linear extrapolation, in time, of the previous incremental solution to begin the nonlinear equation solution for the current increment.
Select Parabolic to indicate that the process should use a quadratic extrapolation, in time, of the previous two incremental solutions to begin the nonlinear equation solution for the current increment.
Select None to suppress any extrapolation.
When you have finished configuring settings for the step, click OK to close the Edit Step dialog box.
The anneal procedure is intended to simulate the relaxation of stresses and plastic strains that occurs as metals are heated to high temperatures. Physically, annealing is the process of heating a metal part to a high temperature to allow the microstructure to recrystallize, removing dislocations caused by cold working of the material. During the anneal procedure Abaqus/Explicit sets all appropriate state variables to zero. These variables include stresses, backstresses, plastic strains, and velocities. In the case of metal porous plasticity, the void volume fraction is also set to zero, such that the material becomes fully dense.
There is no time scale in an annealing step; therefore, time does not advance. The annealing process occurs instantaneously. No data are required for the anneal procedure.
For more information, see “Annealing procedure,” Section 6.11.1 of the Abaqus Analysis User's Manual.
To configure an annealing procedure:
Display the Edit Step dialog box following the procedure outlined in “Creating a step,” Section 14.9.2 (Procedure type: General; Anneal), or “Editing a step,” Section 14.9.3.
In the Description field, enter a short description of the analysis step. Abaqus stores the text that you enter in the output database, and the text is displayed in the state block by the Visualization module.
Choose a Post-anneal reference temperature option:
Choose Maintain current to maintain the current temperature at all nodes in the model after the annealing is complete.
Choose Value to specify a final temperature to which all nodes in the model will be set after the annealing is complete. Enter the value in the field provided.
Click OK to close the Edit Step dialog box.