从nastran到adams产生柔体几种方法.ppt

Chapter 11 MSC.Nastran/MSC.Adams Interface,Table of Contents,Purpose of MSC.Nastran/Adams Flex Interface Features Supported Users Interface Output for MSC.Adams MSC.Adams Units MSC.Nastran/Adams Interface Examples Example 1Component as a superelement Example 2Component as residual structure only Example 3Component Restarting from SOL 106 to SOL 103 Guidelines and Limitations,Purpose of MSC.Nastran/Adams Flex Interface,Incorporates reduced flexible body component dynamics from MSC.Nastran into MSC.Adams Flex For performing system flexible body analysisincluding large rigid body motions Typical Applications: Elasto-kinematic analysis of vehicular suspensions Engine crankshaft-drive train interaction Aircraft landing conditions Satellite panel deployment,Purpose of MSC.Nastran/Adams Flex Interface (cont.),Prior to MSC.Nastran 2004, this type of coupling is a two steps process Generates an output2 file from MSC.Nastran using an dmap alter Converts this output2 file into an MSC.Adams Modal Neutral file (MNF file) using OUT2MNF This file is then readable by MSC.Adams Flex In 2004, you can generate the MNF file directly from MSC.Nastran,Features Supported,The component can be a superelement The exterior points are the attachment points Supports both main bulk and part superelements The component can be residual structure Use ASET/ASETi to define attachment points Supports the use of statsub for prestiffening with small deflection in SOL 103 Supports large displacement with preload Run SOL 106 with preload and save database Restart in SOL 103 using “param,nmloop,x”,Users Interface,Only two new commands/entries are required Case Control command to generate MNF file ADAMSMNF FLEXBODY=YES Bulk Data Entry to specify units used by ADAMS/Flex DTI,UNITS,1,mass_unit,force_unit,length_unit,time_unit e.g., DTI,UNITS,1,KG,N,M,SEC Additional features will be shown in the example sections,Users Interface (cont.),Full ADAMSMNF Case Control command,Most commonly used options,Output for MSC.Adams,The following output are generated for MSC.Adams: Modal stiffness Modal mass Modal load Diagonal matrix of a-set unit boundary displacement Physical mass matrix Stress shape Strain shape,MSC.Adams Units,MSC.Adams is not a unitless code Param,wtmass,x is used in MSC.Nastran to scale weight/mass units, but is ignored in Adams/Flex Correct set of units must be specified on the DTI,UNIT,1, entry Example: If the model are using the following units Mass: grams Force: N Length: meters Time: seconds,MSC.Adams Units (cont.),Example (cont.): The corresponding scale factor on wtmass is .001,but the following DTI entry must be used DTI,UNITS,1,gram,n,m,s A list of acceptable units for MSC.Adams is shown below:,MSC.Nastran/Adams Interface Examples,The simple plate model to the right is used to illustrate 3 separate salient features of the MSC.Nastran/Adams interface. The first example is for a flexible body component as a superelement. The second example is for a flexible body component using residual structure only The third example is to preload the structure in SOL 106 and restart into SOL 103 to genereate the flexible body component,Example 1Component as a superelement,Model the whole structure as a superelement with grid points 1, 11, 111, and 121 as boundary points (exterior points) This is done by the usual SESET entries These boundary points also become attachment points in MSC.Adams Define the SPOINTs and SEQSETs for component modes Define the units for MSC.Adams DTI,UNITS,1,mass_unit,force_unit,length_unit,time_unit,Example 1Component as a superelement (cont.),Request mass invariants for export to MSC.Adams This is done by the param,grdpnt,x The GPWG module will be executed twiceonce for the regular mass matrix for MSC.Nastran and once for the MSC.Adams. The mass matrix is always calculated about the origin of the basic coordinate system for MSC.Adams Request MNF file for MSC.Adams This is done by the “ADAMSMNF flexbody=yes” Case Control callout Use PLOTEL elements to create reduced geometry for MSC.Adams display This is done by the PSETID=x option on the ADAMSMNF Case Control command. The PSETID points to a set ID referenced in the OUTPUT(PLOT) section,Example 1Component as a superelement (cont.),Input File SOL 103 CEND $ TITLE= SIMPLE PLATE MODEL 10 X 10 ELEMENTS $ ADAMSMNF flexbody=yes, psetid=100 $ METHOD=300 $ RESVEC = COMPONENT $ $ Set to define component shapes $ OUTPUT(PLOT) SET 100 = 10001 THRU 10010 $ BEGIN BULK $ $ ADAMS REQUIRES following DTI $ DTI,UNITS,1,KG,N,M,SEC $ $ Turn on gridpoint weight generator $ PARAM,GRDPNT,0 $ EIGR 300 LAN 10 $ SESET,200,2,THRU,10 SESET,200,12,THRU,110 SESET,200,112,THRU,120 $ SPOINT,80001,THRU,80018 SEQSET1,200,0,80001,THRU,80018,$ PLOTEL,10001,1,12 PLOTEL,10002,12,121 PLOTEL,10003,121,111 PLOTEL,10004,111,1 PLOTEL,10006,2,10 PLOTEL,10007,22,110 PLOTEL,10008,120,112 PLOTEL,10009,12,100 $ $ SEELT to put element 1003 and 1004 into SE 200 $ SEELT 200 10003 10004 $ $ Get model data and load data $ include 'model1.dat' $ ENDDATA,Example 1Component as a superelement (cont.),Abridged Output,Example 1Component as a superelement (cont.),Abridged Output (cont.),Example 2Component as residual structure only,Model the whole structure as residual with grid points 1, 11, 111, and 121 as attachment points to MSC.Adams This is done by specifying the boundary grids with the ASET entries Define the SPOINTs and QSETs for component modes Define the units for MSC.Adams DTI,UNITS,1,mass_unit,force_unit,length_unit,time_unit Request mass invariants for export to MSC.Adams This is done by the param,grdpnt,x The GPWG module will be executed twiceonce for the regular mass matrix for MSC.Nastran and once for the MSC.Adams. The mass matrix is always calculated about the origin of the basic coordinate system for MSC.Adams,Example 2Component as residual structure only (cont.),Request MNF file for MSC.Adams This is done by the “ADAMSMNF flexbody=yes” Case Control callout Use PLOTEL elements to create reduced geometry for MSC.Adams display This is done by the PSETID=x option on the ADAMSMNF Case Control command. The PSETID points to a set ID referenced in the OUTPUT(PLOT) section Export grid point stress/strain shapes to the MNF file This is done with the stress, gpstress, strain, and gpstrain command Plot option can be used to reduce the amount of output An OUTPUT(POST) along with the surface definition for the normal gpstress/gpstrain type request,Example 2Component as residual structure only (cont.),$ SOL 103 CEND $ TITLE= without superelement $ ADAMSMNF flexbody=yes, psetid=7772 $ METHOD=300 $ RESVEC = COMPONENT $ STRESS(PLOT)=ALL STRAIN(PLOT)=ALL GPSTRESS(PLOT) = ALL GPSTRAIN(PLOT) = ALL $ OUTPUT(PLOT) SET 7772 = 10001 THRU 10010 $ OUTPUT(POST) SET 9998 = ALL SURFACE 9998 SET 9998 fibre z1 NORMAL X3 $ BEGIN BULK,$ $ ADAMS REQUIRES following DTI $ DTI,UNITS,1,KG,N,M,SEC $ $ Turn on gridpoint weight generator $ PARAM,GRDPNT,0 $ $ Default value - ADAMS must use the above DTI,UNITS $ PARAM,WTMASS,1.0 $ EIGR 300 LAN 10 $ ASET1,123456,1,11,111,121 $ SPOINT,80001,THRU,80018 QSET1,0,80001,THRU,80018 $ PLOTEL,10001,1,12 PLOTEL,10002,12,121 PLOTEL,10003,121,111 PLOTEL,10004,111,1 PLOTEL,10006,2,10 PLOTEL,10007,22,110 PLOTEL,10008,120,112 PLOTEL,10009,12,100 $ include 'model1.dat' $ ENDDATA,Input File,Attachment Points,Example 2Component as residual structure only (cont.),Abridged Output,Example 2Component as residual structure only (cont.),Abridged Output (cont.),Example 3Component Restarting from SOL 106 to SOL 103,Preload the structure in SOL 106 with a distributed tensile loads at the end and restart to calculate modes in SOL 103 This is a two steps process For the SOL 106 cold start run Perform normal SOL 106 runincluding turning on large displacement if desired (param,lgdisp,1) Define the SPOINTs Save the database (scr=no) SPCF(PLOT)=all to form the total reactive preload in SOL 103 For the the SOL 103 restart run Define the QSETs Param,nmloop,x where x is the loopid to restart from,Example 3Component Restarting from SOL 106 to SOL 103 (cont.),For the the SOL 103 restart run (cont.) Define the units for MSC.Adams DTI,UNITS,1,mass_unit,force_unit,length_unit,time_unit Request mass invariants for export to MSC.Adams This is done by the param,grdpnt,x The GPWG module will be executed twiceonce for the regular mass matrix for MSC.Nastran and once for the MSC.Adams. The mass matrix is always calculated about the origin of the basic coordinate system for MSC.Adams Request MNF file for MSC.Adams This is done by the “ADAMSMNF flexbody=yes” Case Control callout Use PLOTEL elements to create reduced geometry for MSC.Adams display This is done by the PSETID=x option on the ADAMSMNF Case Control command. The PSETID points to a set ID referenced in the OUTPUT(PLOT) section,Example 3Component Restarting from SOL 106 to SOL 103 (cont.),$ The data base must be saved for this run therefore SCR=NO required SOL 106 CEND $ TITLE= SIMPLE PLATE MODEL 10 X 10 ELEMENTS $ NLSTRESS = ALL $ SUBCASE 200 LABEL= static stiffining load in plane of plate for preload SPCF(PLOT) = ALL $ Generate forces of constraint SPC = 100 $ LOAD=100 $ NLPARM = 1 $ BEGIN BULK $ PARAM,LGDISP,1 NLPARM,1,4,UPW,YES $ $ Default value - ADAMS must use the DTI,UNITS $ PARAM,WTMASS,1.0,$ $ Add in plate tensioning follower load $ FORCE1 100 111 3000. 1 111 FORCE1 100 112 6000. 2 112 FORCE1 100 113 6000. 3 113 . FORCE1 100 120 6000. 10 120 FORCE1 100 121 3000. 11 121 $ FORCE1 100 1 3000. 111 1 FORCE1 100 2 6000. 112 2 FORCE1 100 3 6000. 113 3 . FORCE1 100 10 6000. 120 10 FORCE1 100 11 3000. 121 11 $ $ $ static support set for preload $ SPC1 100 123 1 SPC1 100 13 11 SPC1 100 3 111 $ $ SPOINT,80001,THRU,80019 $ include 'model1.dat' $ ENDDATA,Cold start run,Example 3Component Restarting from SOL 106 to SOL 103 (cont.),$ $ Get the data base for the nonlinear run $ ASSIGN run1='adams3a.MASTER' restart logical=run1 $ SOL 103 CEND $ TITLE= SIMPLE PLATE MODEL 10 X 10 ELEMENTS $ ADAMSMNF flexbody=yes, psetid=7772 $ METHOD=300 $ RESVEC = COMPONENT $ PARAM,NMLOOP,4 $ SUBCASE 2 LABEL=Sol 106 preload load=100 $ $ Set to define component shapes $ OUTPUT(PLOT) SET 7772 = 10001 THRU 10010 $,$ BEGIN BULK $ DTI,UNITS,1,KG,N,M,SEC $ PARAM,GRDPNT,0 $ $ EIGR 300 LAN 10 $ $ ASET1,123456,1,11,111,121 $ QSET1,0,80001,THRU,80019 $ PLOTEL,10001,1,12 PLOTEL,10002,12,121 PLOTEL,10003,121,111 PLOTEL,10004,111,1 PLOTEL,10006,2,10 PLOTEL,10007,22,110 PLOTEL,10008,120,112 PLOTEL,10009,12,100 $ ENDDATA,Restart modes run,Example 3Component Restarting from SOL 106 to SOL 103 (cont.),Abridged Output for Restart Run,Example 3Component Restarting from SOL 106 to SOL 103 (cont.),Abridged Output for Restart Run (cont.),Guidelines and Limitations,Residual vectors should always be included Specifies enough SPOINT/QSETi to include residual vectors (always overestimate) If MATS1 entry is included in SOL 106, an incremental approach between MSC.Nastran and Adams/Flex should be adopted because of the path dependent load history For restart from SOL 106 to SOL 103 Put the SPOINTs in the SOL 106 cold start run Put the QSETs in the SOL 103 restart run,Guidelines and Limitations (cont.),For static support of preload for residual structure run, use the SUPORT1 entry PLOTELs may be used to define FE mesh detail for MSC.Adams/Flex using the PSETID=set_entry For main bulk data superelement, these elements that lie entirely on the boundary must be sent upstream using the SEELT entry Supports lumped mass only Must use ASET/ASETi, OMIT/OMITi are not supported Does not support p-elements This feature requires a license,