If you want the Abaqus Interface for MSC.ADAMS to translate stress or strain to the modal neutral file, you must modify the template in the previous section to prepare an input file for the first Abaqus analysis. You must include an output request for stress or strain in the *FREQUENCY step, as shown in the following example:

********************
*EL FILE, POSITION=NODES, DIRECTIONS=YES
1,
S,
E,
********************

Note the following points about the output request:

• The POSITION=NODES parameter is required.

• The DIRECTIONS=YES parameter is recommended for all models. This parameter is required for models containing shell elements.

• The section point number (1, on the line following *EL FILE, in this example) is required for models containing shell elements. The section point number will be ignored for solid elements. Stress or strain for only a single section point can be translated to the modal neutral file.

• The output variables stress (S), strain (E), or both can be written to the results file.

In addition, you must run a second Abaqus analysis to recover stress or strain in the substructure for the static constraint modes. You can create the input file for the second Abaqus analysis using the procedure described in “Creating the second input file,” Section 3.3.1. Note the following point about the *SUBSTRUCTURE GENERATE step in the first Abaqus analysis:

• If the SORTED=NO parameter is used on the *RETAINED NODAL DOFS option and the same node number (or node set) is listed more than once on the data lines, the second input file must be edited so that the corresponding nodes at the usage level appear the same number of times. For more information, see “Ordering of the substructure nodes on the usage level” in “Using substructures,” Section 10.1.1 of the Abaqus Analysis User's Manual.