《从nastran到adams的产生柔体几种方法精品课件.pptx》由会员分享，可在线阅读，更多相关《从nastran到adams的产生柔体几种方法精品课件.pptx（28页珍藏版）》请在三一办公上搜索。
1、Table of Contents,Purpose of MSC.Nastran/Adams Flex Interface Features SupportedUsers InterfaceOutput for MSC.AdamsMSC.Adams UnitsMSC.Nastran/Adams Interface ExamplesExample 1Component as a superelementExample 2Component as residual structure onlyExample 3Component Restarting from SOL 106 to SOL 103
2、Guidelines and Limitations,Purpose of MSC.Nastran/Adams Flex Interface,Incorporates reduced flexible body component dynamics from MSC.Nastran into MSC.Adams FlexFor performing system flexible body analysisincluding large rigid body motionsTypical Applications:Elasto-kinematic analysis of vehicular s
3、uspensionsEngine crankshaft-drive train interactionAircraft landing conditionsSatellite panel deployment,Purpose of MSC.Nastran/Adams Flex Interface (cont.),Prior to MSC.Nastran 2004, this type of coupling is a two steps processGenerates an output2 file from MSC.Nastran using an dmap alterConverts t
4、his output2 file into an MSC.Adams Modal Neutral file (MNF file) using OUT2MNF This file is then readable by MSC.Adams FlexIn 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 pointsSupports bot
5、h main bulk and part superelementsThe component can be residual structureUse ASET/ASETi to define attachment pointsSupports the use of statsub for prestiffening with small deflection in SOL 103Supports large displacement with preloadRun SOL 106 with preload and save databaseRestart in SOL 103 using
6、“param,nmloop,x”,Users Interface,Only two new commands/entries are requiredCase Control command to generate MNF fileADAMSMNF FLEXBODY=YESBulk Data Entry to specify units used by ADAMS/FlexDTI,UNITS,1,mass_unit,force_unit,length_unit,time_unite.g.,DTI,UNITS,1,KG,N,M,SECAdditional features will be sho
7、wn 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 stiffnessModal massModal loadDiagonal matrix of a-set unit boundary displacementPhysical mass matrixStress shap
8、eStrain shape,MSC.Adams Units,MSC.Adams is not a unitless codeParam,wtmass,x is used in MSC.Nastran to scale weight/mass units, but is ignored in Adams/FlexCorrect set of units must be specified on the DTI,UNIT,1,. entryExample:If the model are using the following unitsMass:gramsForce:NLength:meters
9、Time:seconds,MSC.Adams Units (cont.),Example (cont.):The corresponding scale factor on wtmass is .001,but the following DTI entry must be usedDTI,UNITS,1,gram,n,m,sA list of acceptable units for MSC.Adams is shown below:,MSC.Nastran/Adams Interface Examples,The simple plate model to the right is use
10、d 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 onlyThe third example is to preload the structure in SOL 106 and restart in
11、to 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 entriesThese boundary points also become attachment points in
12、MSC.AdamsDefine the SPOINTs and SEQSETs for component modesDefine the units for MSC.AdamsDTI,UNITS,1,mass_unit,force_unit,length_unit,time_unit,Example 1Component as a superelement (cont.),Request mass invariants for export to MSC.AdamsThis is done by the param,grdpnt,xThe GPWG module will be execut
13、ed 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.AdamsRequest MNF file for MSC.AdamsThis is done by the “ADAMSMNF flexbody=yes” Case Control calloutUse PLOTEL elements to c
14、reate reduced geometry for MSC.Adams displayThis 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 FileSOL 103CEND$TITLE= SIMPLE PLATE MODEL 10 X 10 ELEMENTS$ADAM
15、SMNF 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$SESET,200,2,THRU,10SESET,200,12,THRU,1
16、10SESET,200,112,THRU,120$SPOINT,80001,THRU,80018SEQSET1,200,0,80001,THRU,80018,$PLOTEL,10001,1,12PLOTEL,10002,12,121PLOTEL,10003,121,111PLOTEL,10004,111,1PLOTEL,10006,2,10PLOTEL,10007,22,110PLOTEL,10008,120,112PLOTEL,10009,12,100$ SEELT to put element 1003 and 1004 into SE 200$SEELT2001000310004$ Ge
17、t 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
18、 121 as attachment points to MSC.AdamsThis is done by specifying the boundary grids with the ASET entriesDefine the SPOINTs and QSETs for component modesDefine the units for MSC.AdamsDTI,UNITS,1,mass_unit,force_unit,length_unit,time_unitRequest mass invariants for export to MSC.AdamsThis is done by
19、the param,grdpnt,xThe 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 fil
20、e for MSC.AdamsThis is done by the “ADAMSMNF flexbody=yes” Case Control calloutUse PLOTEL elements to create reduced geometry for MSC.Adams displayThis 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) sectionExport grid
21、point stress/strain shapes to the MNF fileThis is done with the stress, gpstress, strain, and gpstrain commandPlot option can be used to reduce the amount of outputAn OUTPUT(POST) along with the surface definition for the normal gpstress/gpstrain type request,Example 2Component as residual structure
22、 only (cont.),$SOL 103CEND$TITLE= without superelement $ADAMSMNF flexbody=yes, psetid=7772$METHOD=300$RESVEC = COMPONENT$STRESS(PLOT)=ALLSTRAIN(PLOT)=ALLGPSTRESS(PLOT) = ALLGPSTRAIN(PLOT) = ALL$OUTPUT(PLOT)SET 7772 = 10001 THRU 10010$OUTPUT(POST)SET 9998 = ALLSURFACE 9998 SET 9998 fibre z1 NORMAL X3
23、$BEGIN BULK,$ 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,80018QSET1,0,80001,THRU,80018$PLOTEL,10001,1,12PLOTEL,
24、10002,12,121PLOTEL,10003,121,111PLOTEL,10004,111,1PLOTEL,10006,2,10PLOTEL,10007,22,110PLOTEL,10008,120,112PLOTEL,10009,12,100$include model1.dat$ENDDATA,Input File,Attachment Points,Example 2Component as residual structure only (cont.),Abridged Output,Example 2Component as residual structure only (c
25、ont.),Abridged Output (cont.),Example 3Component Restarting from SOL 106 to SOL 103,Preload the structure in SOL 106 with a distributed tensile loads at the end and restart to calculate modes in SOL 103This is a two steps processFor the SOL 106 cold start run Perform normal SOL 106 runincluding turn
26、ing on large displacement if desired (param,lgdisp,1)Define the SPOINTs Save the database (scr=no)SPCF(PLOT)=all to form the total reactive preload in SOL 103For the the SOL 103 restart runDefine the QSETsParam,nmloop,x where x is the loopid to restart from,Example 3Component Restarting from SOL 106
27、 to SOL 103 (cont.),For the the SOL 103 restart run (cont.)Define the units for MSC.AdamsDTI,UNITS,1,mass_unit,force_unit,length_unit,time_unitRequest mass invariants for export to MSC.AdamsThis is done by the param,grdpnt,xThe GPWG module will be executed twiceonce for the regular mass matrix for M
28、SC.Nastran and once for the MSC.Adams.The mass matrix is always calculated about the origin of the basic coordinate system for MSC.AdamsRequest MNF file for MSC.AdamsThis is done by the “ADAMSMNF flexbody=yes” Case Control calloutUse PLOTEL elements to create reduced geometry for MSC.Adams displayTh
29、is is done by the PSETID=x option on the ADAMSMNF Case Control command.The PSETID points to a set ID referenced in the OUTPUT(PLOT) section,Example 3Component Restarting from SOL 106 to SOL 103 (cont.),$ The data base must be saved for this run therefore SCR=NO requiredSOL 106CEND$TITLE= SIMPLE PLAT
30、E MODEL 10 X 10 ELEMENTS$NLSTRESS = ALL$SUBCASE 200LABEL= static stiffining load in plane of plate for preloadSPCF(PLOT) = ALL $ Generate forces of constraintSPC = 100 $ LOAD=100$NLPARM = 1$BEGIN BULK$PARAM,LGDISP,1NLPARM,1,4,UPW,YES$ Default value - ADAMS must use the DTI,UNITS$PARAM,WTMASS,1.0,$ A
31、dd in plate tensioning follower load$FORCE1 100 111 3000. 1 111FORCE1 100 112 6000. 2 112FORCE1 100 113 6000. 3 113 .FORCE1 100 120 6000. 10 120FORCE1 100 121 3000. 11 121$FORCE1 100 1 3000. 111 1FORCE1 100 2 6000. 112 2FORCE1 100 3 6000. 113 3 .FORCE1 100 10 6000. 120 10FORCE1 100 11 3000. 121 11$
32、static support set for preload$ SPC1 100 123 1SPC1 100 13 11SPC1 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$ASSIGN run1=adams3a.MASTERrestart logical=run1$SOL 103C
33、END$TITLE= SIMPLE PLATE MODEL 10 X 10 ELEMENTS$ADAMSMNF flexbody=yes, psetid=7772$METHOD=300$RESVEC = COMPONENT$PARAM,NMLOOP,4$SUBCASE 2LABEL=Sol 106 preloadload=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 L
34、AN 10$ $ASET1,123456,1,11,111,121$QSET1,0,80001,THRU,80019$PLOTEL,10001,1,12PLOTEL,10002,12,121PLOTEL,10003,121,111PLOTEL,10004,111,1PLOTEL,10006,2,10PLOTEL,10007,22,110PLOTEL,10008,120,112PLOTEL,10009,12,100$ENDDATA,Restart modes run,Example 3Component Restarting from SOL 106 to SOL 103 (cont.),Abr
35、idged 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 includedSpecifies enough SPOINT/QSETi to include residual vectors (always overestimate)If MATS1 entry is inc
36、luded in SOL 106, an incremental approach between MSC.Nastran and Adams/Flex should be adopted because of the path dependent load historyFor restart from SOL 106 to SOL 103Put the SPOINTs in the SOL 106 cold start runPut the QSETs in the SOL 103 restart run,Guidelines and Limitations (cont.),For sta
37、tic 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_entryFor main bulk data superelement, these elements that lie entirely on the boundary must be sent upstream using the SEELT entrySupports lumped mass onlyMust use ASET/ASETi, OMIT/OMITi are not supportedDoes not support p-elementsThis feature requires a license,
