Configuring a fully coupled, simultaneous heat transfer and stress procedure

1. Display the Edit Step dialog box following the procedure outlined in Creating a step (Procedure type: General; Coupled temp-displacement), or Editing a step.

2. 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.

1. In the Edit Step dialog box, display the Basic tabbed page.

2. 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.

3. Indicate whether you want Steady-state or Transient response. See the following sections for more information:

   • Steady-state analysis

   • Transient analysis

   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.

4. In the Time period field, enter the time period of the step.

5. 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.

   For more information, see Linear and nonlinear procedures.

6. 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, and Automatic stabilization of static problems with a constant damping factor.

   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.

   • 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.

   • 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.

7. 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. 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.

8. 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.

1. In the Edit Step dialog box, display the Incrementation tabbed page.

   (For information on displaying the Edit Step dialog box, see Creating a step, or Editing a step.)

2. 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.

3. 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.

4. If you selected Automatic in Step 2, enter values for Increment size:

   1. In the Initial field, enter the initial time increment. Abaqus/Standard modifies this value as required throughout the step.
   2. 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.
   3. In the Maximum field, enter the maximum time increment allowed.

5. If you selected Fixed in Step 2, enter a value for the constant time increment in the Increment size field.

6. If you selected Automatic in Step 2 and if you selected Transient response on the Basic tabbed page, do the following:

   1. 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.
   2. 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.

7. 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.

   For more information, see Automatic incrementation controlled by the creep response.

1. In the Edit Step dialog box, display the Other tabbed page.

   (For information on displaying the Edit Step dialog box, see Creating a step, or Editing a step.)

2. 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.

   For more information on matrix storage, see Matrix storage and solution scheme in Abaqus/Standard.

3. 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.

   • 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.

4. 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.

   For more information on severe discontinuities, see Severe discontinuities in Abaqus/Standard.

5. 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.

6. 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.

   For more information, see Extrapolation of the solution.

When you have finished configuring settings for the step, click OK to close the Edit Step dialog box.