Configuring a fully coupled, simultaneous heat transfer, electrical, and structural procedure

• Choose Steady-state to omit the internal energy term (the specific heat term) in the governing heat transfer equation. A static displacement solution is assumed. 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.

• Choose Transient to perform a transient analysis. As with the steady-state response, electrical transient effects are neglected and a static displacement solution is assumed. You can control the time incrementation in a transient analysis directly, or Abaqus/Standard can control it automatically. Automatic time incrementation is generally preferred. For more information, see Transient Analysis.

• 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.

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.

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.

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

• 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.

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.

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 (except nodes with boundary conditions) 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.

• 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.

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

• 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.

• 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.

• 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.