# Create Output for Third Party Software

How to create output from OptiStruct for third party programs.

The section describes how to create output from OptiStruct for third party programs for Fatigue Analysis (FEMFAT, Design Life, FE-Fatigue, and FE-SAFE), Multibody Dynamic Analysis (AVL EXCITE, SIMPACK, ROMAX, ADAMS, RecurDyn, Ricardo, Virtual Lab, GT-SUITE, and MASTA), and Fluid Structure Interaction Analysis (AcuSolve). Additionally, superelement output for KissSoft and OP2 file output for STRENGTH2000 are available.

## Fatigue Analysis

The .op2 file from OptiStruct can be used directly by Third Party Fatigue Analysis software programs FEMFAT, Design Life, FE-Fatigue, and FE-SAFE.

You need to request the stress output to the .op2 file:
STRESS(OP2) = SET or ALL

The .h3d file can also be used for Design Life and FEMFAT.

## Multibody Dynamic Analysis

### AVL EXCITE

To create the condensed CMS Superelement information for AVL EXCITE, use the CMSMETH CBN Method with ASET or CSET data for the connection DOF. The CBN method with CSET (which is equivalent to CC method or Craig-Chang reduction) can also be used, if that method is preferred.

GPSTRESS is used to specify set of grids for which Grid Point Stresses are calculated for AVL EXCITE.

The PARAM,EXCEXB data controls the output of the AVL EXCITE .exb file directly from OptiStruct. The creation of the _AVL.op2 file can be controlled by PARAM,EXCOP2. The TYPE argument on the parameter data is used to define the type of body to be written out. The choices are SMOT, GMOT, and GMOT. SMOT is for non-rotating bodies like the engine block. GMOT is for rotating bodies such as the crankshaft. These bodies take longer to calculate because they include the inertial invariants. The GMOTR contains a reduced set of inertial invariants. The RECOV argument on the PARAM,EXCEXB controls whether the displacement recovery matrix is written to the main .exb file, a separate recovery only .exb file, both files, or neither.

The creation of the _AVL.op2 file can be controlled by PARAM,EXCOP2.

### Result Recovery for AVL/Excite

There are three ways to recover results using condensed superelements generated for AVL Excite:
1. The condensed H3D superelement is used to recover results in OptiStruct using the INP4 file coming from AVL Excite.
2. The condensed .exb superelement with recovery matrices (or the separate _recover.exb) is used in AVL Excite for recovery. This only supports displacement result recovery.
3. The condensed _AVL.op2 file with recovery matrices is used to recover results in AVL Excite. This supports additional outputs when compared to the recovery directly using .exb file.
The MODEL I/O Options Entry is set to MODEL=ALL by default for AVL Excite condensation runs. If specific entities in the interior of the superelements only are to be selected, the MODEL I/O Options Entry can specify interior grid and element data to be included in the flex body for viewing in EXCITE. The MODEL data format is:
MODEL=Element Set, Grid Set, RIGID/NORIGID

All grids associated with elements in the element set and rigid elements if RIGID is specified are combined with the grids in the Grid Set and output to the flex body. In addition, the keyword PLOTEL can be used for Element Set argument to specify all the grids associated with all of the PLOTEL data in the model.

• Recovery Method 1: H3D Superelement Recovery

Recovery data is only provided for grids that are the intersection of the grids in the specified in the MODEL data and the I/O output request (DISP, GPSTRESS, and so on). The same is true for the MODEL element set and element results (STRESS and STRAIN).

After running AVL EXCITE, a residual run can be made to recover displacement, velocity, acceleration, stress, strain, grip point srtess, strain energy and ERP results for interior grids and elements in the CMS Superelement based on the modal participation results from AVL EXCITE. The results are only calculated for GRID and elements specified by the MODEL data in the CMS Superelement creation run. So, the only output is the intersection of the grids and elements on the MODEL data with the output data sets on the output data specification (DISP, STRESS, GPSTRESS, and so on).
Note: The results data entries should also be specified in the Super Element creation run.
Output in Residual Run (Recovery using H3D SE) Required Output Request in CMS Generation Run
DISP/VELO/ACCE DISP
Stress Stress
Strain Strain
Grid Point Stress (GPSTRESS) Grid Point Stress (GPSTRES)
Strain Energy (ESE) Stress and Strain
ERP DISP
The residual run can be any combination of frequency response and transient analysis subcases. After running AVL EXCITE, a resulting filename.INP4 file is created that contains the modal participation factors for the modes of the CMS Superelement for each loading frequency or transient analysis time step. In the residual run, the CMS Superelement .h3d file and the AVL EXCITE modal results file are specified using the ASSIGN data:
ASSIGN,H3DDMIG,AX,'Crank_split2h_all.h3d'
ASSIGN,EXCINP,10,'Crankshaft_SOL109_time.INP4'
Where the 10 in the ASSIGN,EXCINP data corresponds to the SUBCASE for which the modal participation results will be used. In subcase 10, instead of performing a frequency response or transient response analysis, OptiStruct will just use the modal participation results from AVL EXCITE.
Note: Since the analysis is skipped, it does not matter if the residual run is modal or direct frequency response/transient analysis.
For transient analysis, the number of time steps in the transient analysis residual run must match the number of time steps used in the AVL EXCITE analysis. For frequency response analysis, the number of loading frequencies in the frequency response analysis residual run must match number of loading frequencies used in the AVL EXCITE analysis. Some dummy loading data (TSTEP/FREQ, TLOAD/RLOAD, DAREA, and TABLED data) were required in old version, but they are no longer need as of OptiStruct version 2018. A sample of input data for a transient analysis residual run is shown below.
Note: If the inp4 file comes from AVL Excite v2019 R1 or newer, TSTEP or FREQ are not needed in subcase for recovery run.

You can have multiple .INP4 files in the recovery run, with each EXCINP pointing to a different subcase.

ASSIGN,H3DDMIG,AX,'Crank_split2h_all.h3d'
ASSIGN,EXCINP,10,'Crankshaft_SOL109_time.INP4'
$DISPLACEMENT = ALL STRESS = ALL$
SUBCASE 10
ANALYSIS=DTRAN
TSTEP  = 10133
$BEGIN BULK$
TSTEP,10133,143,2.7778-4
ENDDATA
• Recovery Method 2: .exb Superelement Recovery in AVL/Excite
The .exb file or the _recover.exb file with recovery matrices (generated by specifying MODEL=ALL/<SetID> and DISP=ALL/<SetID>) can be used directly in AVL/Excite to recover displacement results. Other result types are not supported for direct .exb file-based recovery in AVL/Excite.
Output in Residual Run (Recovery using EXB SE) Required Output Request in CMS Generation Run (with PARAM,EXCEXB,YES)
Displacement DISP
• Recovery Method 3: _AVL.op2 Superelement Recovery in AVL/Excite
The _AVL.op2 file with recovery matrices (generated by specifying MODEL=ALL/<SetID>, PARAM,EXCOP2,YES, and any corresponding output request) can be used in AVL/Excite to recover various results, such as displacements, stresses, and so on.
Table 1. Supported Recovery Results using the OP2 file
Output in Residual Run (Recovery using _AVL.OP2 file) Required Output Request in CMS Generation Run (with PARAM,EXCOP2,YES)
DISP/VELO/ACCE DISP
Stress Stress
Strain Strain
Grid Point Stress (GPSTRESS) Grid Point Stress (GPSTRES)
Strain Energy (ESE) Stress and Strain
ERP DISP

### SIMPACK

To create the condensed CMS Superelement information for SIMPACK, you should use the CMSMETH CBN Method with ASET or CSET data for the connection DOF. If CSET connection DOF is used, then the AMSES solver must be specified on the CMSMETH data. The mass, stiffness, structural damping, and viscous damping matrices are output.

The PARAM,SIMPACK data is used to specify what data is written out for SIMPACK. Depending of the setting of PARAM,SIMPACK, the data includes the Superelement Eigenvalue and Eigenvectors, Stiffness, Mass, Structural Damping, and Viscous Damping matrices, as well as the Model Information (grids and elements), Displacement Recovery Information, Rotational Loads, Reduced Loads, and diagonal mass matrix of the full structure. If Stress recovery information is needed, this is controlled by the STRESS output request. See PARAM,SIMPACK for full details.

The MODEL I/O Options Entry can be used to specify interior grid and element data to be included in the Flex Body for viewing in SIMPACK. The MODEL data format is:
MODEL=Element Set, Grid Set, RIGID/NORIGID

All grids associated with elements in the element set and rigid elements if RIGID is specified are combined with the grids in the Grid Set and output as a Flex body. In addition, the Element Set argument can be set to PLOTEL to specify all the grids associated with all of the PLOTEL data in the model.

Recovery output is available for DISP, VELO, ACCE, STRESS, and STRAIN. The results are only calculated for GRID and elements specified by the MODEL data in the CMS Super Element creation run. So, the only output is the intersection of the grids and elements on the MODEL data with the output data sets on the output data specification (DISP, STRESS, and so on).

DISPLACEMENT quantities are only written out if PARAM,SIMPACK is set to 3 or higher. STRESS and STRAIN recovery information is always written out if requested by the output request PARAM,SIMVER is used to specify the version of SIMPACK to be used. The default is 9.0.

Recover SIMPACK Results
ASSIGN,SIMPIMP identifies an external .unv file generated after running a multibody dynamic analysis in SIMPACK. The resulting CMS flexbody modal participation factors in the .unv file can be used by OptiStruct to recover the dynamic displacements, velocities, accelerations, stresses and strains. The format is:
ASSIGN, SIMPINP, Subcase ID, Filename

Subcase ID is used to specify which SUBCASE the modal participation factors should be used for.

For example:
ASSIGN,H3DDMIG,AX,'Crank_split2h_all.h3d'
ASSIGN,SIMPINP,10,'Crankshaft_SOL109_time.unv' 
In SUBCASE 10, instead of performing a frequency response analysis, OptiStruct will just use the modal participation results from SIMPACK.
Note: Since the analysis is skipped, it does not matter if the residual run is modal or direct frequency response analysis.
For frequency response analysis, the number of loading frequencies in the frequency response analysis residual run must match number of loading frequencies used in the SIMPACK analysis. While the frequency response analysis data is ignored, there must still be some dummy loading data (FREQ, RLOAD, DAREA, and TABLED data). A sample of input data for a frequency response analysis residual run is:
ASSIGN,H3DDMIG,AX,'Crank_split2h_all.h3d'
ASSIGN,SIMPINP,10,'Crankshaft_SOL109_time.unv’
$DISPLACEMENT = ALL STRESS = ALL$
SUBCASE 10
FREQ   = 10133
$BEGIN BULK$
GRID,80001,,0.,-62.,0.
\$
DAREA,10202,80001,1,1.0
TABLED1,10301,
,0.0,1.0,0.1,1.0,0.2,1.0,0.3,1.0
,ENDT
FREQ,10133,0.0,1.0,100
ENDDATA

Note: You can have multiple .unv files in the recovery run, with each EXCINP pointing to a different SUBCASE.

### RecurDyn

To create the modal CMS Superelement information for RecurDyn, you must use the CMSMETH CBN Method with ASET data for the connection DOF. If requested by the I/O Options, recovery matrices for DISPLACEMENT, GPSTRESS and GPSTRAIN are output.

The PARAM,RFIOUT,YES data is used to turn on the generation of the .rfi file, which contains the modal superelement that is used by RecurDyn. Stiffness and Mass matrices are always written out. DISPLACEMENT, GPSTRESS, and GPSTRAIN recovery matrices are written out if requested. Only the intersection of the output request and the GRID SET on the MODEL data is written out.

The MODEL data used can specify interior grid and element data to be included in the Flex Body for viewing in RecurDyn. The MODEL data format is:
MODEL=Element Set, Grid Set, RIGID/NORIGID
All grids associated with elements in the element set and rigid elements if RIGID is specified are combined with the grids in the Grid Set and output to the flex body. In addition, the keyword PLOTEL can be used instead of an Element Set ID to specify all the grids associated with all of the PLOTEL data in the model.
Note: This .rfi file can be created only by OptiStruct executables running on 64-bit Windows machines. This file cannot be created while using OptiStruct on Linux or Mac OS X machines.

### ROMAX

To create the condensed CMS Dynamic Superelement information for ROMAX, use PARAM,ROMAX,YES with the CMSMETH CBN Method with ASET data for the connection DOF. The condensed Stiffness, Mass, and Displacement recovery matrices are written out to a binary .op4 file. Only the intersection of the DISPLACEMENT output request and the GRID SET on the MODEL data is written out.

The MODEL data used can specify interior grid and element data to be included in the Flex Body for ROMAX. The MODEL data format is:
MODEL=Element Set, Grid Set, RIGID/NORIGID

All grids associated with elements in the element set and rigid elements if RIGID is specified are combined with the grids in the Grid Set and output to the Flex body. In addition, the keyword PLOTEL can be used instead of an Element Set ID to specify all the grids associated with all of the PLOTEL data in the model.

To create the condensed CMS Static Superelement information for ROMAX, use PARAM,EXTOUT,DMIGPCH with ASET data for the connection DOF. The condensed Stiffness Matrix will be written to the .pch file in DMIG format. This data can be read by any version of ROMAX after release R12.6.2. For the Static Superelement, only the condensed Stiffness matrix is written out.

To create the condensed Flex Body information for ADAMS, use the CMSMETH CC or CB Method.

The MODEL data used can specify interior grid and element data to be included in the Flex Body for viewing in ADAMS. The MODEL data format is:
MODEL = Element Set, Grid Set, RIGID/NORIGID

All grids associated with elements in the element set and rigid elements if RIGID is specified are combined with the grids in the Grid Set and output to ADAMS. In addition, the keyword PLOTEL can be used instead of an Element Set ID to specify all the grids associated with all of the PLOTEL data in the model.

Output request such as Displacement, GPSTRESS and GPSTRAIN are supported in .mnf file.

The OUTPUT command is used to generate the .mnf file for ADAMS. The command is:
OUTPUT = ADAMSMNF

### Ricardo

To create the condensed Flex Body Modes and Full Diagonal Mass Matrix to the .op2 file for Ricardo, use the CMSMETH CBN Method and PARAM,RICARDO,YES.

The MODEL I/O Options Entry can specify interior grid and element data to be included in the Flex Body for Ricardo. The MODEL data format is:
MODEL=Element Set, Grid Set, RIGID/NORIGID

All grids associated with elements in the element set and rigid elements if RIGID is specified are combined with the grids in the Grid Set and output to the flex body. In addition, the keyword PLOTEL can be used for Element Set argument to specify all the grids associated with all of the PLOTEL data in the model.

### GT-SUITE

To create the condensed CMS Super Element Information (Stiffness, Mass, Structural Damping, Viscous Damping, and condensed loads) for GT-SUITE, use the CMSMETH CBN Method with ASET data for the connection DOF.

After running GT-SUITE, a residual run can be made to recover displacement, velocity, acceleration, stress, strain and grid point strain results for interior grids and elements in the CMS Superelement based on the modal participation results from GT-SUITE. The results are only calculated for GRID and elements specified by the MODEL data in the CMS Superelement creation run. So, the only output is the intersection of the grids and elements on the MODEL data with the output data sets on the output data specification (DISP, STRESS, GPSTRESS, and so on). The results data entries should also be specified in the Superelement creation run.

The residual run is transient analysis subcases. After running GT-SUITE, a resulting filename.INP4 file is created that contains the modal participation factors for the modes of the CMS Superelement for each transient analysis time step. In the residual run, the CMS Superelement .h3d file and the GE-SUITE modal results file are specified using the ASSIGN data.
ASSIGN,H3DDMIG,AX,'Crank_split2h_all.h3d'
ASSIGN,EXCINP,10,'Crankshaft_SOL109_time.INP4'
Where, the 10 in the ASSIGN,EXCINP data corresponds to the SUBCASE for which the modal participation results will be used. In subcase 10, instead of performing a transient response analysis, OptiStruct will just use the modal participation results from GT-SUITE. Since the analysis is skipped, it does not matter if the residual run is modal or direct transient analysis.
Note: You can have multiple .INP4 files in the recovery run, with each EXCINP pointing to a different subcase.

### MASTA

To create the condensed CMS Superelement Information (Stiffness, Mass, Structural Damping, Viscous Damping, and condensed loads) for MASTA, use the CMSMETH CBN Method for Dynamic analysis and GUYAN for Static analysis. Interface could be defined with ASET.

Once the analysis in MASTA is completed, either corresponding loading or SPCDs could be applied at the interface dofs on the flexbody for results recovery.

### Virtual Lab

To create the condensed Flex Body Modes and Full Diagonal Mass Matrix to the .op2 file for Virtual Lab, use the CMSMETH CB or CC Methods.

The PARAM,LMSOUT data is to trigger the output of the condensed Flex Body Modes and full Diagonal Mass Matrix to the .op2 file. PARAM,POST is not required. OUTPUT=OP2 is not required.

## Superelement Output

Create the condensed Stiffness Matrix in an ASCII file for KissSoft.

### KissSoft

To create the condensed Stiffness Matrix in an ASCII file for KissSoft, use the CMSMETH method GUYAN and specify PARAM,KISSSOFT,YES.

## Fluid Structure Interaction Analysis

The .op2 file from OptiStruct can be used directly by the AcuSolve CFD code.

Request the eigenvector output to the .op2 file:
DISP(OP2) = ALL
Next, run the Python script from ACUSIM called acuNASTRAN2pev.py:
python acuNastran2Pev.py problem.op2

This creates the nodes.dat, elems.dat, and modeXX.dat files. Be sure to use the latest version of acuNASTRAN2pev.py from ACUSIM.

## General

### STRENGTH2000

To output the required CSTM68 data blocks to the OP2 file for STRENGTH2000, use PARAM,S2K,YES.