Prepare the full model for a substructured multibody analysis, as follows:

Perform the generation pass to create the CMS substructure (in the matrix .SUB file) characterizing the dynamic flexibility of the body.

You must decide how many modes to include in the CMS substructure. The number you determine depends on several factors including:

For most analyses, and particularly for rotating bodies, the fixed-interface method (CMSOPT,FIX) is sufficient. For analyses where higher frequencies are of interest (foe example, those involving acoustics or high-speed equipment), the residual-flexible free-interface method (CMSOPT,RFFB) provides more accuracy. For more information, see Supported CMS Methods in the Substructuring Analysis Guide.

For nonrotating bodies, you can apply constraints (D) in the generation pass to the degrees of freedom, but not the master degree of freedom. Set KEYOPT(4) = 1 for these superelements in the use pass; otherwise, your analysis will have convergence problems. For rotating bodies, do not apply constraints in the generation pass because the superelement must have six rigid body modes; you can, however, apply constraints to its master degree of freedom in the use pass.

Loading Considerations

When applying loads, be aware that:

Creating the Superelements

Follow these steps to create the superelements for a substructured multibody analysis:

Repeat the steps above for each flexible body you wish to replace with CMS substructures. Use unique jobnames and substructure names for each flexible body.

Residual-Flexible Free-Interface CMS Method

If you are using the residual-flexible free interface method, use CMSOPT,RFFB,NMODE (rather than CMSOPT,FIX,NMODE) in Step 2.5. You must also define pseudo-constraints (D,,,SUPPORT).

For further information, see The CMS Generation Pass in the Substructuring Analysis Guide.

Replace the flexible bodies with their corresponding CMS substructures.

Repeat the CMSEL,U and SE commands for each flexible body.

Set up the multibody analysis and run it.

To dampen out excessive solution noise, particularly in the velocities and accelerations, you typically use numerical damping. For more information, see Damping.

In Step 4.3, use tabular loads to specify complex load-versus-time histories. By default, loads are simply ramped (or step-applied (KBC)) over the time interval from one load step to the next. Tabular loads, however, allow a general load curve. To use multiple load steps to define the loading, repeat Steps 4.3 and 4.4 for each load configuration.

For more information about setting up and performing a multibody analysis, see Performing a Multibody Analysis.

Using the solutions from the prior step (displacements at the master degrees of freedom at each time point), obtain the displacements and stresses (if desired) for all nodes and elements of the flexible bodies.

Repeat all steps for each substructured body (including clearing the database (/CLEAR)).

Merge all results files (one from the use pass and one from each of the expanded substructures) to create a results file with the full model data. After completing this part of the process, you can perform postprocessing as though you had run the full model in the multibody simulation.

Understanding the example commands in this step:

Postprocess the full model as though you had run a nonsubstructured analysis.

Use the POST1 postprocessor (/POST1) to review the results over the entire model. Use the POST26 postprocessor (/POST26) to obtain time-history listings and plots. For more information, see Reviewing Multibody Analysis Results for specific multibody postprocessing.

Nodal velocity and acceleration nodal results are not available for the substructure interior nodes (non-master degrees of freedom).