1. Workshop 10 procedure to create a flex body with MSC nastran

3. Workshop 10 – Procedure to Create a Flex Body with MSC Nastran
Workshop Objectives
To use an existing FEA model used to perform a modal analysis, capture and reduce the modes of the structure down to a set of boundary nodes (points) that can be transferred to ADAMS. The component modes are captured using the MSC Nastran Component Modal Synthesis (CMS) Technique.
Problem Description
Software Used
MSC Nastran 2012
Adams 2012

4. Workshop 10 – Procedure to Create a Flex Body with MSC Nastran (Cont.)
Suggested Exercise Steps:
Create Flex Bodies Using MSC Nastran.
General Instruction to set up a MSC Nastran input file
Using The Residual Method
Using Superelement Method
Check List
Comparison of major cards between SOL 103 and SOL 103 with ADAMSMNF card
Verify the FLEX_BODY in Adams/View

5. Create Flex Bodies Using MSC Nastran
Go to:
Working directory exercise_dir/mod_09_mnf_nastran
Compare two MSC Nastran input files con_rod_sol103.bdf and con_rod_sol103_for_mnf.bdf
Note the changes required to convert regular SOL103 run for generating mnf file.
SOL103
ADAMSMNF

6. General Instruction to set up a MSC Nastran input file
Using The Residual Method:
Prepare regular finite element model (con_rod_sol103.bdf ) for SOL 103, a normal mode free-free analysis.
Do a MSC Nastran run and check if numbers of eigenvalues (modes) are as per your expectation. Usually it is recommended to include number of modes that covers frequency which is double the frequency of interest. To know the number of modes, first run the model by specifying frequency range in the EIGRL card and then count the number of modes. Use this number of modes in the EIGRL card while preparing deck for the MNF generation.
Use above as base FE model and modify the MSC Nastran deck (.dat or .bdf) to generate MNF file as per below instructions.
[ Optional Step] This step is required only if one is interested in Fatigue analysis: Define the name of op2 file, assign it to the UNIT 20 (fundamental) and specify UNFORM
Example:
$ ADAMS/Durability with MSC.Fatigue requires op2 generation $
ASSIGN OUTPUT2='ex2.out' STATUS=UNKNOWN UNIT=20 FORM=UNFORM

7. General Instruction to set up a MSC Nastran input file (Cont.)
Check if SOL 103 is defined or not (modal analysis and should be FREE-FREE).
Include ADAMSMNF card to instruct MSC Nastran to generate MNF file.
Example:
$ This is required to initiate an MSC Nastran/Adams interface run
$ flexbody=yes is REQUIRED
$ psetid will define face geometry for flexible body display
$ admout=yes also output op2 file for Adams/Durability with MSC.Fatigue
$ outstrs=yes output element stress shapes to op2 file $
ADAMSMNF flexbody=yes, admout=yes, outgstrn=yes, outgstrs=yes, psetid= 1

8. General Instruction to set up a MSC Nastran input file (Cont.)
Define UNITS through DTI statement: it’s fundamental to give ADAMS the UNITS for the Flexible component.
MSC Nastran is a unitsless solver; user has to specify consistent units. Adams understands units via DTI statement. So MSC Nastran units should match the DTI units. One can use WTMASS parameter to convert mass units consistent with the DTI statement.
Example: $
PARAM,WTMASS,1.0
  Find below an explanation of DTI statement:
$ Format:
$ DTI UNITS MASS FORCE LENGTH TIME
$ Example:
DTI UNITS KG N M S

9. General Instruction to set up a MSC Nastran input file (Cont.)
A note of clarification about UNITS and its relation to MSC Nastran's WTMASS parameter:
WTMASS, though necessary to achieve units consistency in MSC Nastran, is ignored in the output for ADAMS. Units data for ADAMS is supplied on the UNITS DTI entry.
For example #1:
In Adams, the user models mass in grams, force in Newtons, length in meters and time in seconds. The WTMASS parameter is set to 0.001, thereby ensuring that MSC Nastran works with the consistent set of kg, N. M and S.
The units reported to Adams should be: "DTI, UNITS, 1, GRAM, N, M, S ."
For example #2:
  In Adams, the user models mass in KG, force in Newtons, length in meters and time in seconds. The WTMASS paramater is set to 0.001, thereby ensuring that MSC Nastran works with the consistent set of Mega-gram, N , M and S.
The units reported to Adams should be: :DTI, UNITS, 1, KG, N, M, S"

10. General Instruction to set up a MSC Nastran input file (Cont.)
Define correctly EIGRL statement, checking the number of Eigenvalues = number of SPOINTs. It is possible to specify more SPOINTs but not less than the number of eigenvalues on the EIGRL card.
$ Select number of modes:
$ Include enough for structure shape and to capture residual flexibility $
$ ========================================================
EIGR LAN

11. General Instruction to set up a MSC Nastran input file (Cont.)
Define a number of SPOINT (Scalar Points) equal to the number of the mode shapes (Eigenvalues) one want to calculate (extract) from the FEM modal analysis. The number of SPOINTs must be equal to or greater than the Eigenvalues number specified in the EIGRL statement (Eigenvalues Lanczos Method).
It’s good rule to number the SPOINTs starting from the last number used as ID for GRID points
For the Residual method approach, define QSET1 statement to include SPOINTs
Example: for 10 normal mode defined on the EIGRL card $
$ SCALAR Point and QSET1 to define DOFs use for component modes
SPOINT,12002,THRU,120027
QSET1,0,12002,THRU,120026

12. General Instruction to set up a MSC Nastran input file (Cont.)
Define nodes on ASET1 statement to promote those as Interface nodes (MASTER nodes). This will add SIX constrained modes for each Interface node.
Example:
ASET1, , 12000, 12001
[Optional Step] Define following PARAM statements
PARAM, AUTOSPC, YES (to fix singularity problems)
PARAM, GDRPNT, 0 (to write global inertial properties in the output f06 file)
PARAM, FIXEDB, -1 (decouple residual structure)
[Optional Step] Define, if necessary, the following PARAM statement:
PARAM, CMSORTHO, NO (disable othogonalization procedure, default = YES)
PARAM, MSGLVL, (enable diagnostic procedure, default = 0)

13. General Instruction to set up a MSC Nastran input file (Cont.)
Notes:
If the user wants to connect the Flexible Body to Ground using SPC cards, the resulting modal shapes contain the constrained information, so in ADAMS the Flexible Body must be connected to the Ground using the same type of Constrain as used in the FEM code. However it is recommend NOT to define any constraint in the FEM model.
If MPC card are present in the FEM model, the first degree of freedom in the MPC sequence is defined to be the dependent degree of freedom, so neither it may be defined as MASTER node, nor it may be assigned to another rigid element (RBAR or RBE2).
If RBE3 element is present in the FEM model, neither the dependent degree of freedom may be defined as MASTER node, nor it may be assigned to another rigid element (RBAR or RBE2). Usually, as workaround, a new node is defined very close the MPC or RBE3 first node and connected to this through a CBEAM element (6 DOFs) with high stiffness in order to model a rigid-like connection.

14. General Instruction to set up a MSC Nastran input file (Cont.)
To get stress and strain modes in the mnf file, you need to specify GPSTRESS, GPSTRAIN card along with OUTPUT (POST) card. The SURFACE card should be use if you have 2D element and VOLUME card should be use if you have 3D element. Both cards can be used if you have combination of elements. Use PLOT option to suppress the output in the .fo6 file.
Example:
$ Generate stress and strain grid shapes $
GPSTRESS (PLOT) = ALL
GPSTRAIN (PLOT) = ALL
$ Define surface for stress and strain grid shapes
$ Use VOLUME entry if you have 3D element
SET 3 = ALL
VOLUME 1 SET 3, PRINCIPAL, DIRECT, SYSTEM CORD 0
$ Use SURFACE entry if you have 2D element
OUTPUT (POST)
SET 9998 = ALL
SURFACE 9998 SET 9998 NORMAL X3

15. General Instruction to set up a MSC Nastran input file (Cont.)
$ Use VOLUME and SURFACE entries if you have 2D and 3D element
SET 3 = ALL
VOLUME 1 SET 3, PRINCIPAL, DIRECT, SYSTEM CORD 0
SET 4 = ALL
SURFACE 2 SET 4, FIBRE ALL, SYSTEM CORD 0, AXIS X1, NORMAL R $
[Optional Step] To reduce the size of mnf file or to share mnf file with third party without letting them know the details of the design, you can use PSETID along with OUTPUT (PLOT) and PLOTEL statement.
Example:
ADAMSMNF flexbody=yes, psetid=7772
OUTPUT(PLOT)
SET 7772 = THRU 10005
$ Define plotel's for set 7772 in output (post) section

16. General Instruction to set up a MSC Nastran input file (Cont.)
PLOTEL,10001,13,109
PLOTEL,10002,12,100
PLOTEL,10003,112,120
PLOTEL,10004,110,22
PLOTEL,10005,10,2 $

17. General Instruction to set up a MSC Nastran input file (Cont.)
Using Superelement Method: [Optional]
Most of the procedure remains identical to residual method except for the QSET1 and ASET1 entries.
For superelement approach, define SEQSET1 entry to include SPOINTs
$ SCALAR Point and SEQSET1 to define DOFs use for component modes $
SPOINT,80001,THRU,80010
SEQSET1,200,0,80001,THRU,80010W
Specify all interface nodes as EXTERNAL to the SUPERELEMENT (which contains ALL internal nodes). It is possible to use two different, equivalent and complementary expressions (we suggest, however, to use either):
SESET, ID super, ID node, ID node, ID node (internal nodes list)
SESET, ID super, ID node, thru, ID node (THRU option) 
//OR//
CSUPEXT, ID super, ID node, ID node, ID node (MASTER nodes list)

18. Check List Starting point is regular SOL 103 run
Check for SOL 103 and Method entry
Include ADAMSMNF card to instruct MSC Nastran to generate MNF file
Define UNITS through DTI statement
Define EIGRL statement
For Residual method approach, define QSET1 statement to include SPOINTs and define nodes on ASET1 statement to promote those as Interface nodes
For superelement approach, define SEQSET1 entry to include SPOINTs and specify all interface nodes as EXTERNAL to the SUPERELEMENT.
Check for GPSTRESS, GPSTRAIN, OUTPUT (POST), VOLUME and SURFACE statement to include stress and strain modes in the mnf file.
Check if you need PSETID, OUTPUT (PLOT) and PLOTEL to reduce size of mnf file or to share it with third party.

19. Comparison of major cards between SOL 103 and SOL 103 with ADAMSMNF card:
SOL 103 – Normal Mode Analysis
SOL 103 with ADAMSMNF card – Normal Mode Analysis
In the Executive Control Section that is above CEND,
- specify the solution sequence
SOL 103
In the Case Control Section, specify
- residual vector
- grid point stress
- grid point strain
- METHOD entry
- specify mandatory Nastran-Adams interface entry.
- specify if stress/strain needs to be in the mnf file
METHOD = #
RESVEC = YES if required
GPSTRAIN
GPSTRESS
METHOD= #
ADAMSMNF
OUTPUT(POST), VOLUME and/or SURFACE
In the BEGIN BULK section,
- preferred but optional PARAM
card entry
Note: WTMASS should be consistent with DTI UNITS card
- to turn on gridpoint weight generator
- mandatory DTI entry
- mandatory EIGRL entry
PARAM POST
PARAM WTMASS
PARAM PRTMAXIM
PARAM,GRDPNT //OR//
AUTOSPC(NOZERO)
EIGRL #
PARAM POST
PARAM WTMASS
PARAM PRTMAXIM
DTI UNITS

20. Comparison of major cards between SOL 103 and SOL 103 with ADAMSMNF card:
SOL 103 – Normal Mode Analysis
SOL 103 with ADAMSMNF card – Normal Mode Analysis
For Superelement approach: specify,
- mandatory EIGRL entry
- to define interior grids as superelement ##
- to define DOFs to use for component modes
SESET,##
SPOINT
SEQSET1,##
Specify mandatory ASET1 entry for static reduction
ASET1
In the subcase, for durability study make sure to add STRESS and STRAIN card
STRESS=ALL
STRAIN=ALL

21. Create Flex Bodies Using MSC Nastran
Go to:
Select Start > All Programs > MSC Software > MSC Nastran
Browse for the input file and click Open
Enter scr=y old=n in the optional keywords field
Click Run a c d b

22. Verify the FLEX_BODY in Adams/View
Launch New Adams/View session:
Change Start in directory if required
Click OK a b

23. Verify the FLEX_BODY in Adams/View (Cont.)
Import Flexible body:
Under the Bodies tab, click Adams/Flex in the Flexible Bodies group
Browse for con_rod_0.mnf file
Uncheck Use Default Damping Ratio and Enter “0” in that field
Click OK c d

24. Verify the FLEX_BODY in Adams/View (Cont.)
Check mode number and mode shape
Right click on the flexible body and select Modify
Check Damping Ratio, it should be set to zero value
Check Mode Number, it should be equal to number of normal modes + 6*interface nodes + 6 residual modes if requested. a c

25. Verify the FLEX_BODY in Adams/View (Cont.)
Check mode number and mode shape:
Check Mode Shape by entering each mode mumbers (For example: Mode 7 and Mode 11) and compare it with mode shape in Patran postprocessor or any other compatible postprocessor. Select the surface to mesh from the GUI.
View Mode shape animation.
Click OK after checking mode shapes and mode number a b c

26. Verify the FLEX_BODY in Adams/View (Cont.)
Do Linear Analysis and compare REAL eigenvalues in fo6 file:
Pull down Settings > Gravity.
In the Gravity settings dialogue box, Uncheck Gravity and click OK
Under the Simulation tab, select Run an Interactive Simulation in the Simulate group.
Click on Find Static Equilibrium icon, this is prerequisite for Linear analysis. Click close button on information window
Click on Compute Linear Modes
Click on Show Table. e d e

27. Verify the FLEX_BODY in Adams/View (Cont.)
Do Linear Analysis and compare REAL eigenvalues in fo6 file:
A table will be displayed in Information Window. Compare it with the REAL eigenvalues in the .fo6 file as shown in the excerpt from fo6 file.
Note that: For 6 rigid body DOF, you should get 6 complex pairs for the eigenvalues. Here, you get 6 real pairs that have split into 12 separate modes (with no imaginary part, one pair "c +/- d" gives you two real roots).
For more information, refer Simcompanion KB article# KB , "Number of eigenvalues/modes vs. number DOF for a model." b a