About Submodeling Analyses

The submodeling technique lets you study a local part of a model with a refined mesh based on interpolation of the solution from an initial (undeformed), relatively coarse, global model.

This technique is available for structural/mechanical simulations (either an analysis case in a structural analysis or the structural analysis case of a thermal-structural analysis). Only node-based solid-to-solid or shell-to-shell submodeling is available.

This page discusses:

See Also
Creating Submodel Analysis Cases
In Other Guides
Performing a Node-Based Submodeling Analysis

Submodeling is most useful when you need to obtain an accurate, detailed solution in a local region and the detailed modeling of that local region has negligible effect on the overall solution. A submodeling analysis allows you to do the following:

  • Run the simulation for the global model with a relatively coarse mesh.
  • Run the simulation for a local region (the submodel) with a finer mesh and higher-order elements to get an accurate solution of the region.
  • Adjust mesh details and repeat the simulation for the submodel as needed using the same solution from the global model simulation.

Submodeling Workflow

The overall process for performing a submodeling analysis is as follows:

  1. Develop your global model and submodel. The global model could consist of multiple parts while the submodel consists of a subset of those parts.
  2. Define a mesh for the global model, and define a separate mesh for the submodel. See Creating or Editing Finite Element Models.
  3. Create an analysis case, and use the global model mesh as its finite element model. This analysis case is referred to as the global analysis case. See Creating and Duplicating Analysis Cases.
  4. Run a successful, complete simulation of the global analysis case. See Running a Simulation from an App.

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

  5. Switch back to the Mechanical Scenario Creation app.
  6. Create a new analysis case that links to the global analysis case. Use the submodel mesh as the new analysis case's finite element model. This new analysis case is referred to as the submodel analysis case.
  7. Create steps in the submodel analysis case.
  8. In the submodel analysis case, recreate any simulation features from the global model that should also be applied on the submodel.
  9. Create submodel displacements on the boundary of the submodel that connects to the global model. See Applying Submodel Displacements.
  10. Run the simulation of the submodel analysis case.

Feature Creation

When a submodel analysis case is created, the steps or simulation features in its global analysis case are not cloned in the new analysis case. In the submodel analysis case, you must create all steps and simulation features required for the submodeling analysis. If you go back and make simulation feature changes in the global analysis case, those changes are not propagated; you must make changes in the submodel analysis case accordingly.