|
»Click here to display Table of Contents«
|
Coupling OptiStruct with Third Party Software |
|
|
|
|
|
Coupling OptiStruct with Third Party Software |
|
|
|
|
Creating Output for Third Party Software
The section describes how to create output from OptiStruct for third party programs for Fatigue Analysis (FEMFAT, Design Life, and FE-SAFE), Multi-Body Dynamic Analysis (AVL/EXCITE, SIMPACK, ROMAX, ADAMS, RecurDyn, Ricardo and Virtual Lab), and Fluid Structure Interaction Analysis (AcuSolve). Additionally, superelement output for KissSoft and OP2 file output for STRENGTH2000 are available.
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.
To create the condensed CMS Super Element information for AVL/EXCITE, use the CMSMETH CBN Method with ASET or CSET data for the connection DOF. The CBN method with CSET for 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.
After running AVL/EXCITE, a residual run can be made to recover displacement, velocity, acceleration, stress, and strain results for interior grids and elements in the CMS Super Element based on the modal participation results from AVL/EXCITE. Note that the results are only calculated for GRID and elements specified by the MODEL data in the CMS Super Element creation run. The residual run can be any combination of frequency response and transient analysis SUBCASE’s. After running AVL/EXCITE, a resulting filename.INP4 file is created that contains the modal participation factors for the modes of the CMS Super Element for each loading frequency or transient analysis time step. In the residual run, the CMS Super Element .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 that 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. While the frequency response/transient analysis data is ignored, there must still be some dummy loading data (TLOAD/RLOAD, DAREA, and TABLED data). A sample of input data for a transient analysis residual run is shown below:
ASSIGN,H3DDMIG,AX,'Crank_split2h_all.h3d'
ASSIGN,EXCINP,10,'Crankshaft_SOL109_time.INP4'
$
DISPLACEMENT = ALL
STRESS = ALL
$
SUBCASE 10
DLOAD = 10201
TSTEP = 10133
$
BEGIN BULK
$
GRID,80001,,0.,-62.,0.
$
TLOAD1,10201,10202,,,10301
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
TSTEP,10133,143,2.7778-4
ENDDATA
To create the condensed CMS Super Element information for SIMPACK, you must 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. The SIMPACK values produce the information for SIMPACK.
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 as follows:
ASSIGN, SIMPINP, Subcase ID, Filename
Subcase ID is used to specify which SUBCASE the modal participation factors should be used for.
To create the modal CMS Super Element information for RecurDyn, you must use the CMSMETH CBN Method with ASET data for the connection DOF. If requested, recovery matrices for 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 super element that is used by RecurDyn.
|
To create the condensed CMS Super Element information for ROMAX, use the CMSMETH CBN Method with ASET data for the connection DOF.
Use PARAM,EXTOUT,DMIGPCH to create a PUNCH file containing the Super Element data. This data can be read by any version of ROMAX after release R12.6.2.
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.
GPSTRESS is used to specify set of grids for which Grid Point Stresses are calculated for ADAMS.
The OUTPUT command is used to generate the .mnf file for ADAMS. The command is:
OUTPUT = ADAMSMNF
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.
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.
To create the condensed Stiffness Matrix in an ASCII file for KissSoft, use the CMSMETH GUYAN and specify PARAM,KISSSOFT,YES.
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.
To output required CSTM68 data blocks to the OP2 file for STRENGTH2000, use PARAM,S2K,YES.
