If you want the Abaqus Interface for MSC.ADAMS to create a modal neutral file without stress or strain, you can use the following template to prepare an input file for the Abaqus analysis:
*HEADING ... ******************** *STEP *FREQUENCY, EIGENSOLVER=... ... *BOUNDARY ... *ELEMENT MATRIX OUTPUT, MASS=YES, ELSET=... *NODE FILE U, *END STEP ******************** *STEP, UNSYMM=NO *SUBSTRUCTURE GENERATE, TYPE=Z..., RECOVERY MATRIX=YES, MASS MATRIX=YES *RETAINED NODAL DOFS ... *SELECT EIGENMODES ... *SUBSTRUCTURE LOAD CASE, NAME=... *CLOAD ... *SUBSTRUCTURE MATRIX OUTPUT, RECOVERY MATRIX=YES, MASS=YES, STIFFNESS=YES, SLOAD=YES *END STEP ********************
The history section of the input file must contain a *FREQUENCY step to calculate the fixed-interface normal modes, followed by a *SUBSTRUCTURE GENERATE step. The *FREQUENCY step may be preceded by any number of steps to apply a desired preload to the model.
Note the following points about the *FREQUENCY step:
The *FREQUENCY step must apply zero boundary conditions to every degree of freedom that will be retained in the *SUBSTRUCTURE GENERATE step. Other degrees of freedom may be constrained as appropriate.
This step must write element mass matrices and eigenvectors to the results file. For each element the mass at a node is computed by summing all terms in the row of the element mass matrix corresponding to the first degree of freedom at that node. This computation is exact for all elements in the Abaqus element library, but it might not be correct for user elements. In particular, this computation is not correct for user elements representing a substructure.
The UNSYMM=NO parameter on the *STEP option is optional but recommended. Certain preloading histories (for example, contact with high friction coefficients) may create unsymmetric stiffness matrices. The substructure matrix created after such a preloading history will in all cases be symmetric. However, by default, Abaqus will create and write the full substructure matrix to the results file if the stiffness matrix was unsymmetric earlier in the analysis. Using UNSYMM=NO saves computation time and storage space without affecting accuracy.
The *SUBSTRUCTURE GENERATE option must include the parameters RECOVERY MATRIX=YES and MASS MATRIX=YES.
The list of *RETAINED NODAL DOFS must be equal to or a subset of the list of DOFs set to zero in the preceding *FREQUENCY step.
The list of *SELECT EIGENMODES must be equal to or a subset of the eigenmodes computed in the *FREQUENCY step. If the list is a subset, unused eigenmodes must not be written to the results file.
The *SUBSTRUCTURE MATRIX OUTPUT option must write the recovery matrix, stiffness matrix, and mass matrix to the results file.
If the SLOAD=YES parameter is used on the *SUBSTRUCTURE MATRIX OUTPUT option, modal load components corresponding to all internal and external loads acting on the substructure will be translated to modal preloads (block 27) in the modal neutral file.
The *SUBSTRUCTURE LOAD CASE option is optional. If the option is present, *CLOAD data should duplicate the loading defined in an earlier general step to represent the effect of other parts of the model on the substructure. As noted in the preceding paragraph, if SLOAD=YES is used on the *SUBSTRUCTURE MATRIX OUTPUT option, these external loads (along with any internal loads) will be written to the preload data block of the modal neutral file. The NAME used for the load case is immaterial.
The history section of the Abaqus input file may include general steps preceding the required *FREQUENCY and *SUBSTRUCTURE GENERATE steps. Note the following points about these optional general steps:
Displacements written to the results file in these steps will be used to update the nodal coordinates written to the modal neutral file. Displacements for later steps will update those of earlier steps. Therefore, if displacements for a subset of nodes have been written for any step, the final step should write displacements for all nodes of the substructure; otherwise, some nodes will be translated with their original coordinates, and others will be translated with their deformed coordinates.
Loads from these steps may be translated to modal preloads (block 27) in the modal neutral file if SLOAD=YES is used on the *SUBSTRUCTURE MATRIX OUTPUT option. Internal and external loads are treated differently:
Internal loads include distributed loads (such as self-weight) and boundary conditions. These loads are considered to be an intrinsic part of the substructure. All *DLOAD data and the reaction forces due to boundary conditions are treated as internal loads.
The resultant of internal loads may be nonzero. For example, if a gravity load is applied to a structure restrained from rigid body motion, a net force equal to the weight of the body will act on the rest of the MSC.ADAMS model through the retained degrees of freedom.
External loads represent the effect of other parts of the model on the substructure. All *CLOAD options are considered to be external loads. To translate these loads to MSC.ADAMS, the *CLOADs in a general step must be replicated as *SUBSTRUCTURE LOAD CASE data in the *SUBSTRUCTURE GENERATE step.