Are there any ANSYS LSDYNA examples showing how to define orthotropic material
properties? The GUI only lists the minor form of the Poisson's ratios and my data
is in terms of the major form.
Yes, please see the ANSYS LSDYNA 9.0 example below (which is also attached to this solution record). You can still enter the Poisson's ratio data in terms of the major form (PRXY, etc.) via the command line (or batch input); it is just that the GUI will only display them in the minor form (NUXY, etc.) after internally converting them, as this is the form requested by LSDYNA. In this example: mp, ex, 1, 2.470E+07 ! Ea = Ex = 2.470E+07 psi mp, ey, 1, 1.200E+06 ! Eb = Ey = 1.200E+06 psi mp, ez, 1, 1.200E+06 ! Ec = Ez = 1.200E+06 psi mp, prxy, 1, 0.2881667 ! PRba = PRxy * (Ey/Ex) = 0.0140000 mp, prxz, 1, 0.2881667 ! PRca = PRxz * (Ez/Ex) = 0.0140000 mp, pryz, 1, 0.1000000 ! PRcb = PRyz * (Ez/Ey) = 0.1000000 !!! mp, nuxy, 1, 0.0140000 ! equivalent minor Poisson's ratios ... !!! mp, nuxz, 1, 0.0140000 !!! mp, nuyz, 1, 0.1000000 Incidentally, there is a bug in the ANSYS LSDYNA 9.0 (and earlier) GUI in that the "CID" value (coordinate system ID) is not written to the dialogue box, so bringing it up after the data is defined (either via the dialogue box or batch input) and then saving it again via the "OK" button will wipe out the "CID" value. Defect 34796 was filed and subsequently corrected in the UP20050523 build of ANSYS LSDYNA 10.0 to resolve this error, which is described in more detail in the input file below. ! = = = = = = = = = = = = = = = = = = = = = = = = = = = = = = = = = = = = = = = = = fini /clear /title, ANSYS LSDYNA 9.0 GUI Test of Orthotropic Materials /psf,pres,norm,2 /plopts,info,1 /view,,1,2,3 /prep7 et,1,SOLID164 r,1 mp, dens, 1, 1.000E04 ! RHO = 1.000E4 lbfsec^2/in^4 (speed up run ...) mp, ex, 1, 2.470E+07 ! Ea = Ex = 2.470E+07 psi mp, ey, 1, 1.200E+06 ! Eb = Ey = 1.200E+06 psi mp, ez, 1, 1.200E+06 ! Ec = Ez = 1.200E+06 psi mp, prxy, 1, 0.2881667 ! PRba = PRxy * (Ey/Ex) = 0.0140000 mp, prxz, 1, 0.2881667 ! PRca = PRxz * (Ez/Ex) = 0.0140000 mp, pryz, 1, 0.1000000 ! PRcb = PRyz * (Ez/Ey) = 0.1000000 !!! mp, nuxy, 1, 0.0140000 ! equivalent minor Poisson's ratios ... !!! mp, nuxz, 1, 0.0140000 !!! mp, nuyz, 1, 0.1000000 mp, gxy, 1, 7.200E+05 ! Gab = Gxy = 7.200E+05 psi mp, gyz, 1, 1.980E+05 ! Gbc = Gyz = 1.980E+05 psi mp, gxz, 1, 7.200E+05 ! Gca = Gzx = Gxz = 7.200E+05 psi edmp,hgls,1,5 ! stiffness form of hourglass control edlcs,add,11,0,1,0,0,0,1,0,0,0 ! fiber direction along Yaxis edmp,ortho,1,11 ! local material coordinate system ... block,,25.0,,1000.0,,100.0 esize,20 vmesh,1 edpart,create eddamp,all,,5.00 ! super heavy damping ... eddamp,1,,1.0e2 eplot fini /solu nsel,s,loc,y,0 cm,nbase,node d,all,ux,0.0,,,,uy,uz esln cm,ebase,elem nsel,s,loc,y,1000 cm,ntip,node esln cm,etip,elem nsel,s,loc,x,0 cm,npress,node esln cm,epress,elem *dim,etime,,3 *dim,epush,,3 etime(1)=0.0,0.001,2.001 epush(1)=0.0,10.0,10.0 edload,add,press,5,epress,etime(1),epush(1) nsel,all esel,all time,2.000 edrst,100 edhtime,1000 edhist,nbase edhist,ebase edhist,ntip edhist,etip edenergy,1,1,1,1 edout,glstat edout,matsum edopt,add,,both edwrite,both,,k mplist ! /eof ! ! If you do the following in the GUI before the SOLVE command: ! ! > Preprocessor > Material Props > Material Models ! > Material Model Number 1 > Linear Orthotropic ! ! You will see that the CID (Coord ID) is missing. Clicking "OK" ! will result in having the CID wiped out, which obviously changes ! the material directions ... ! ! mplist ! see Defect 34796 ... solve save fini /post26 numvar,200 file,,his ntrack=node(0,1000,0) nsol,2,ntrack,u,x,xdisp store,merge prvar,2 /show,png plvar,2 /show,close plvar,2 /eof /wait,3 fini /post1 file,,rst set,last set,prev /edge,,1 /dscale,,1 plnsol,u,sum,2 /wait,2 /user plnsol,u,sum andata,0.5,,0,10,0,1,0,1 . 

