About Restart Simulations

A restart analysis lets you develop a complex simulation in multiple stages.

Restart analyses are available only for structural/mechanical simulations (not thermal or thermal-structural). You can restart only from a static step, a frequency step, or an explicit dynamic step.

This page discusses:

See Also
Creating Restart Analysis Cases
Deleting Restart Analysis Data

In large simulations containing many steps, you might want to divide the overall simulation into separate sequential analysis cases. A restart analysis allows you to do the following:

  • Examine the baseline results and confirm that the initial analysis case is performing as expected before continuing with the next analysis case.
  • Add additional steps to the simulation.
  • Modify scenario features and rerun the complete simulation.
  • Save results data from the execution of the initial steps and then create a new analysis starting from any of those completed steps.
  • Create multiple new simulations starting from the same completed analysis case.

Restart Workflow

The overall process for developing a restart simulation is as follows:

  1. Develop your initial (upstream) baseline analysis case containing the preliminary set of steps.
  2. Select one or more static, frequency, or explicit dynamic steps from which you might want to restart the simulation. Define how data is generated in these steps to allow for subsequent restart simulations. For more information, see Defining Static Steps, Defining Frequency Steps, and Defining Explicit Dynamic Steps.

  3. Run the initial analysis case. See Running a Simulation from an App.

    Physics Results Explorer opens, and you can examine the results.

  4. Switch back to Mechanical Scenario Creation.
  5. Create a new restart analysis case, and indicate from which initial analysis case, step, and increment you want to restart.
  6. Continue working in the restart (downstream) analysis case to add steps, restraints, interactions, loads, and output requests.
  7. Run the complete simulation.

    The new set of downstream steps is run after the restart step point.

  8. Create additional restart analysis cases, if required, to simulate different step types and conditions. Each restart analysis creates its own set of results data.
Important: The upstream restart data must be from an analysis case that was run with the same release and functional delivery (FD) of the 3DEXPERIENCE platform as the restart case. If your baseline case was run in an earlier release, you must rerun it to ensure compatible data.

Feature Synchronization

When the downstream analysis case is created, all steps and features up to and including the restart step are cloned in the new analysis. As indicated in the Feature Manager, the cloned steps and features are read-only; you cannot edit, deactivate, or delete them.

If you change simulation features in the upstream analysis case, you must complete one of the following actions to propagate the changes to the feature clones in the downstream analyses:

  • Right-click the downstream (restart) analysis case in the tree, and select Synchronize from the context menu.
  • Run the full simulation (including all analysis cases).
  • Export the simulation to an Abaqus input file. See Exporting Abaqus Files.

Non-Editable Features

The finite element model used in the restart analysis must be the same as the model used in the initial (upstream) analysis. In the restart analysis:

  • You cannot modify or add any geometry, mesh, materials, sections, etc.
  • You cannot modify any steps or step-dependent actions (restraints, interactions, loads, or output requests) in or before the restart step.