10.2.3.3. DMAP Command

10.2.3.3.1. DMAP for Modal Analysis (*.op2)

This is the guide for the Modal analysis (Normal mode analysis) in MSC(or NX)/Nastran. It is necessary for you to the appreciate DMAP command in order to run your input file for Nastran. This example file is located in <Install Dir>\Toolkits\Flexible input files\NASTRAN\NASTRAN_normal_OP2.dat.

1. Delete

   • Delete commands related to the super elements

   SEALL = ALL
   SUPER = ALL
   

2. Add or Modify

   • Global Mass and Stiffness Matrix

   COMPILE PHASE1B nolist noref
   Alter ‘call sekmr’$
   OUTPUT2 MGG,KGG//0/12////$
   

   • Stress and Strain Shape

     • The below commands are to create the stress and strain shape data to the OP2 file.

     Note

     If the stress and strain shape is added when you create the RFI file, you should use the Stress/Strain Shape option in Interface Option. (Refer to Interface Options)

   …
   Compile sedrcvr$ nolist
   Alter 'call gpstress'(2,0) $
   OUTPUT2 ogstr1//0/12///$
   CEND
   …
   

   …
   GPSTRESS(PUNCH)=ALL
   GPSTRAIN(PUNCH)=ALL
   …
   

   …
   VECTOR(SORT1,REAL)=ALL
   SPCFORCES(SORT1,REAL)=ALL
   STRESS=ALL
   STRAIN=ALL
   $
   OUTPUT(POST)
   $ Set 6 : write all element ids for
   $      output gpstress and gpstrain (element IDs 1 ~ 50)
   SET 6=1 THRU 50
   $
   $$ Solid element : Use VOLUME instead of SURFACE
   $VOLUME 1 SET 6,DIRECT,SYSTEM CORD 0
   $
   $ Shell type element : Use SURFACE instead of VOLUME
   SURFACE 1 SET 6,FIBRE ALL,SYSTEM CORD 0
   …
   

• The first box is to write the strain shape data in the OP2 file.

• The second box is to write the stress and strain shape in the Punch file and OP2 file

• The third box is the necessary command for GPSTRESS and GPSTRAIN.

Note

When using the OP2 file after this analysis, the DMAP command of

PARAM,POST,-2 should be added. In addition, if there is

PARAM,OGEOM,NO in DMAP commands, it must be deleted.

10.2.3.3.2. DMAP for Modal Analysis (*.pch)

This is the guide for the Modal analysis in MSC (or NX)/NASTRAN. It is necessary for you to the appreciate DMAP command in order to run your input file in MSC (or NX)/ NASTRAN. The below step informs to you how to modify DMAP command. The example file is located in <Install Dir>\Toolkits\Flexible input files\NASTRANNASTRAN_normal.dat.

1. Delete

   • Delete commands related to the super elements

   SEALL = ALL
   

   • Delete unnecessary commands in the case control section.

   ECHO = NONE
   MAXLINES = 999999999
   $ Direct Text Input for Global Case Control Data
   SUBCASE 1
   $ Subcase name : Default
   

   

   Figure 10.62 DMAP command (Delete)

2. Add

   • Input Global mass and stiffness matrix

   COMPILE PHASE18 nolist noref
   Alter ‘call sekmr’$
   

   • Add the following commands in the case control section.

   ECHO = PUNCH
   

   

   Figure 10.63 DMAP command (Add)

10.2.3.3.3. DMAP for CMS Analysis (*.out)

This is the guide for CMS analysis in MSC/NASTRAN. It is necessary for you to appreciate DMAP command in order to run your input file in MSC/NASTRAN. The steps below inform you how to modify DMAP command. The two example files with this DMAP command are included in the folder, <Install Dir>\Toolkits\Flexible input files\NASTRAN\NASTRAN_scm.dat.

1. Output File Name

   • Input a name of output file.

   $============================================$
   $=====     COPYRIGHT (C) 2005            ====$
   $=====     BY FUNCTION BAY INC.          ====$
   $=====     ALL RIGHTS RESERVED           ====$
   $============================================$
   $
   $  DMAP Command for RD/Flex 6.0
   $
   ASSIGN OUTPUT2='Plate_cms.out' STATUS=UNKNOWN UNIT=20
   FORM=UNFORM
   

2. Executive Control

   • Define solution type.

   • Include ALT file, which makes output file written in the form for RecurDyn.

   $--------------------------------------------$
   $  EXECUTIVE CONTROL
   $--------------------------------------------$
   SOL 103
   TIME 3000
   $
   INCLUDE 'RecurDyn_rfi.alt'
   

3. Case Control

   • Define ‘SUPER’ and ‘SEALL’ for Superelemnet

   • Define GPSTRESS and GPSTRAIN for Stress and Strain Shape

   $--------------------------------------------$
   $  CASE CONTROL
   $--------------------------------------------$
   TITLE= CMS analysis for RecurDyn
   SUBTITLE= Plate model
   $
   ECHO = PUNCH
   METHOD=2
   $
   SUPER=1
   SEALL=1
   GPSTRESS(PUNCH)=ALL
   GPSTRAIN(PUNCH)=ALL
   SPC = 1
   METHOD = 1
   $
   VECTOR(SORT1,REAL)=ALL
   SPCFORCES(SORT1,REAL)=ALL
   STRESS=ALL
   STRAIN=ALL
   $
   OUTPUT(POST)
   $ Set 6 : write all element ids for output gpstress and gpstrain (element IDs 1 ~ 50)
   SET 6=1 THRU 100
   $
   $$ Solid element : Use VOLUME instead of SURFACE
   $VOLUME 1 SET 6,DIRECT,SYSTEM CORD 0
   $
   $ Shell type element : Use SURFACE instead of VOLUME
   SURFACE 1 SET 6,FIBRE ALL,SYSTEM CORD 0
   

4. Bulk Data

   • Set Parameters.

   • Specify interior grids except interface nodes.

   • Release some degree of freedoms of interface nodes.

   • Define data needed to perform real eigenvalue analysis with the Lanczos method.

   • Define scalar points.

     • All scalar point identification numbers must be unique with respect to all other structural, scalar points.

     • The number of spoints (Scalar Points) is equal to the sum of normal modes and residual vectors.