Configuring a heat transfer procedure

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

2. 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.

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. 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.

   • 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.

   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.

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 Transient analysis on the Basic tabbed page, do the following:

   1. 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.
   2. 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.

7. 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 in Abaqus/Standard, for more information.

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 an Equation Solver Method option:

   • Choose Direct to use the default direct sparse solver.

   • Choose Iterative to use the iterative linear equation solver. The iterative solver is typically most useful for blocky structures with millions of degrees of freedom. For more information, see Iterative linear equation solver.

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.

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

4. 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.

   • 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.

5. 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.

6. 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.

7. 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 heat transfer step, click OK to close the Edit Step dialog box.