In NX/Nastran v5.0 and later version, in order that the RFI file which is contained CMS Analysis results is generated directly by NX/Nastran, it is necessary to modify or add the DMAP command in the input file for NX/Nastran.
At that time, because the stress/strain shapes cannot be generated in Stress Shape Interface, DMAP commands for the stress/strain shapes must be contained in this file. The outline for DMAP commands for that is as shown below.
|
$--------------------------------------------$ $ EXECUTIVE CONTROL $--------------------------------------------$ SOL 103 TIME 3000 CEND $--------------------------------------------$ $ CASE CONTROL $--------------------------------------------$ TITLE= CMS analysis for RecurDyn $* SUPER = ALL SEALL = ALL $* ECHO = NONE METHOD = 100 $* $* NX Nastran version 5 ~ 6.1: RECURDYNRFI $RECURDYNRFI FLEXBODY=YES,FLEXONLY=YES,OUTGSTRS=YES,OUTGSTRN=YES $* NX Nastran version 6.1 ~: MBDEXPORT RECURDYN MBDEXPORT RECURDYN FLEXBODY=YES,FLEXONLY=YES,OUTGSTRS=YES,OUTGSTRN=YES $* GPSTRAIN=ALL GPSTRESS=ALL $* SET 5 = 1 THRU 100 STRESS=5 STRAIN=5 $* $* OUTPUT(POST) SET 6 = 1 THRU 100 $* Shell element : SURFACE SURFACE 1 SET 6,FIBRE ALL,SYSTEM CORD 0 $* Solid element : VOLUME $VOLUME 1 SET 6,DIRECT,SYSTEM CORD 0 $* $--------------------------------------------$ $ BULK DATA $--------------------------------------------$ BEGIN BULK $-------$-------$-------$------- PARAM AUTOSPC YES PARAM GRDPNT 0 PARAM WTMASS 1.0 PARAM K6ROT 100.0 PARAM BAILOUT -1 PARAM RESVEC YES $ $-------$-------$-------$-------$-------$-------$------- DTI UNITS 1 KG N M S $ $ Extract Normal Mode $-------$-------$-------$-------$-------$-------$-------$-------$------- EIGRL 100 -0.01 10 $ $-------$-------$-------$-------$-------$-------$------- SESET 1 2 THRU 10 SESET 1 12 THRU 110 SESET 1 112 THRU 120 SPOINT 80001 THRU 80010 SEQSET1 1 0 80001 THRU 80010 $ $-------$-------$-------$-------$-------$-------$-------$-------$------- $ GRID/ELEMENT/Material/Property CARDS $-------$-------$-------$-------$-------$-------$-------$-------$------- |
The description of several DMAP Commands in detail is as follows.
|
Command |
Description |
|
SEALL = ALL |
Generates and assembles all super elements |
|
SUPER = ALL |
Assign the subcase to all super elements and loading conditions. |
|
METHOD = 100 |
Select the real eigenvalue extraction parameters. |
|
MBDEXPORT RECURDYN FLEXBODY=YES, FLEXONLY=YES,OUTGSTRS=YES,OUTGSTRN=YES |
Generate RecurDyn RFlex Input (RFI) file. Here, the grid point stress (OUTGSTRS) and the strain (OUTGSTRN) are output to the RFI file. If your version of NX Nastran is 6.1 or later, use this command. Note) If your version of NX Nastran is earlier than 6.1, use this following command. è RECURDYNRFI FLEXBODY=YES,FLEXONLY=YES,OUTGSTRS=YES,OUTGSTRN=YES |
|
GPSTRAIN=ALL |
Output of grid point strain for all SURFACE and VOLUME commands. |
|
GPSTRESS=ALL |
Output of grid point stress for all SURFACE and VOLUME commands. |
|
SET 5 = 1 THRU 100 |
Define a set which contains all of the element’s IDs. |
|
STRESS=5 |
Output of stress for elements defined in Set 5 |
|
STRAIN=5 |
Output of strain for elements defined in Set 5 |
|
OUTPUT(POST) |
Indicates the beginning of surface or volume commands. |
|
SET 6 = 1 THRU 4086 |
Defines Set 6 as the same as Set 5 defined above. |
|
SURFACE 1 SET 6,FIBRE ALL,SYSTEM CORD 0 |
Sets the surface for which strains and stresses are calculated. Here, direct stresses and strains are requested. Note)If solid elements are used in the mesh, the VOLUME command should be used instead, as shown below: è VOLUME 1 SET 6,DIRECT,SYSTEM CORD 0 |
|
DTI UNITS 1 KG N M S |
Defines the units of measurement to be used in FE software. |
|
SESET 1 2 THRU 10 |
Defines interior nodes for the super element of the flexible component. This set should include all the nodes of the flexible body except the interface nodes. |
|
SESET 1 12 THRU 110 | |
|
SESET 1 112 THRU 120 | |
|
SPOINT 80001 THRU 80024 |
Defines Scalar Point. |
|
SEQSET1 1 0 80001 THRU 80024 |
Defines the generalized DOF of the super element |
|
EIGRL 100 -0.01 10 |
Super element modal solution |
To obtain the more accurate stress/strain recovery results for all animation frames after simulating a RFlex model, it is necessary to create a MDF file. If the user want to use the MDF file, refer to How to apply MDF file in NX Nastran because DMAP Commands is different to upper commands.
Note
From the *.rfi file created in NX/Nastran 2019.2 version, CTRIA6 and CQUAD8 elements did not appear on the view. This is a problem that occurred on the NX, and can be solved by adding the command "NASTRAN SYSTEM(700)=1" to the data file.