# FBD Solver Interfacing

The Free Body Diagram utilities behave differently depending on the solver that you interface with in HyperMesh.

## Abaqus

• Results are supported through the .odb output file.
• Grid point force results are requested with the following output requests:
• *NODE OUTPUT
• RF
• CFD
• *ELEMENT OUTPUT
• NFORC
• Displacement results are requested with the following output request:
• *NODE OUTPUT
• U
• It is recommended practice to output data for only the node/element set(s) of interest. This procedure reduces the size of the solver results file and helps speed up the FBD extractions.
• Abaqus rigid elements, *Rigid bodies, *Coupling constraints, *MPC, *Fastener and *Equations do not export forces and moments. If any of these are attached to the element set of interest, all elements attached to them must be included in the element set to insure the GPF balance is correct. If they are not included, an imbalance will occur. Refer to the Abaqus documentation to determine these elements/bodies. Make sure to check the validity of all GPF results when any of these are present in the model.
• The FBD Export Manager is currently not supported for Abaqus.

## ANSYS

• Results are supported through the .rst output file.
• Grid point force results are requested with the following output requests:
• OUTRES,ALL,ALL
or
• OUTRES,NSOL,ALL
• OUTRES,RSOL,ALL
• Displacement results are requested with the following output requests:
• OUTRES,ALL,ALL
or
• OUTRES,NSOL,ALL
• OUTRES,RSOL,ALL
• The FBD Export Manager is currently not supported for ANSYS.

## Nastran

• Results are supported through the .op2 and .xdb output files.
• Grid point force results are requested with the GPFORCE output request.
• Displacement results are requested with the DISPLACEMENT output request.
• It is recommended practice to output data for only the node set(s) of interest. This procedure reduces the size of the solver results file and helps speed up the FBD extractions. Consider using STRESS=NONE and STRAIN=NONE to further reduce the size of the results file.
• MPC forces and moments are properly extracted for the following MPC constraint types:
• RBE2
• RBE
• RJOINT
• RROD
• RBAR

## OptiStruct

• Results are supported through the .op2 output file.
• Grid point force results are requested with the GPFORCE output request.
• Displacement results are requested with the DISPLACEMENT output request.
• It is recommended practice to output data for only the node set(s) of interest. This procedure reduces the size of the solver results file and helps speed up the FBD extractions. Consider using STRESS=NONE and STRAIN=NONE to further reduce the size of the results file. You may consider using the NOMODEL option on the OUTPUT,OP2 output format request.
• MPC forces and moments are properly extracted for the following MPC constraint types:
• RBE2
• RBE3