Are there any examples showing how to reorient the element coordinate systems of a
SOLID46 model with the EORIENT command and output the interlaminar shear stresses?
|
Yes, please see the ANSYS 8.1 example below. fini /clear /title, SOLID46 Laminate Orientation Example /view,,1,2,3 /color,pbak,0 /plopts,info,1 /prep7 ! Uni-directional graphite/epoxy data mp, ex, 1, 2.470E+07 ! psi mp, ey, 1, 1.200E+06 ! psi mp, ez, 1, 1.200E+06 ! psi mp, prxy, 1, 0.2881667 ! unitless mp, prxz, 1, 0.2881667 ! unitless mp, pryz, 1, 0.1000000 ! unitless mp, gxy, 1, 7.200E+05 ! psi mp, gyz, 1, 1.980E+05 ! psi mp, gxz, 1, 7.200E+05 ! psi ! Uni-directional E-glass/epoxy data mp, ex, 2, 6.632E+06 ! psi mp, ey, 2, 1.353E+06 ! psi mp, ez, 2, 1.353E+06 ! psi mp, prxy, 2, 0.2870000 ! unitless mp, prxz, 2, 0.2870000 ! unitless mp, pryz, 2, 0.4290000 ! unitless mp, gxy, 2, 4.807E+05 ! psi mp, gyz, 2, 2.826E+05 ! psi mp, gxz, 2, 4.807E+05 ! psi et, 1, SOLID46 keyopt, 1, 1, 0 ! Include extra displacement shapes keyopt, 1, 2, 0 ! Constant thickness layer input keyopt, 1, 3, 4 ! Combination of all output options keyopt, 1, 4, 0 ! No user subroutine to define element x-axis keyopt, 1, 5, 2 ! Both stress and strain results per keyopt(6) keyopt, 1, 6, 5 ! Layer sol w/ fail crit for all layers @ int pts & Tau's keyopt, 1, 8, 1 ! Store data for all layers keyopt, 1, 9, 2 ! Evaluate stresses & strains at layer top, mid, & bottom keyopt, 1, 10, 1 ! Print out material property matrix for first element r, 1 ! Stiff on outside, softer on inside rmodif, 1, 1, 5 ! 5 layers through thickness of element rmodif, 1, 2,0 ! Layer data not symmetric (enter all data) rmodif, 1, 7, 0 ! Mid-plane used as reference plane rmodif, 1, 13, 1, 0.00, 0.10 ! Mat, Theta, and % Thickness for layer 1 rmodif, 1, 16, 2, 45.0, 0.20! Mat, Theta, and % Thickness for layer 2 rmodif, 1, 19, 2, 90.0, 0.30 ! Mat, Theta, and % Thickness for layer 3 rmodif, 1, 22, 2, -45.0, 0.25 ! Mat, Theta, and % Thickness for layer 4 rmodif, 1, 25, 1, 0.00, 0.15 ! Mat, Theta, and % Thickness for layer 5 cyl4, 0.0,0.0, 10.0,0.0, 11.0,90.0, 1.0 ! create quarter cylinder vplot /wait,1 /eshape,1 ! view layers comprising laminate /vscale,,2 ! double size of symbols, like element CS /psymb,esys,1 ! turn on element coordinate system symbols /device,vector,on ! need to view element coordinate systems local,11,1 ! define and activate local cylindrical system esys,11 ! elements to be created will use local CS 11 esize,1.0 vmesh,1 /title, Axial Laminate Orientation eplot /wait,2 eorient,lysl,negx ! recreate SOLID46 elements, as desired /title, Concentric Cylinder Laminate Orientation eplot /wait,2 /device,vect,0 /psymb,esys,0 eplot fini /solu antype,static csys,1 nsel,s,loc,x,10 /psf,pres,norm,2 sf,all,pres,1000.0 csys,0 nsel,s,loc,x,0 nsel,a,loc,y,0 d,all,all,0 nsel,all outres,all,all outpr,all,last solve save fini /post1 set,last /dscale,,1 /edge,,1 esel,s,elem,,10 /graph,full ! RSYS,SOLU requiresfull graphics ! Layer BOTTOM values = Layer TOP values of preceding layer. Obviously, ! to get the top values of the last layer, you need to "add another layer" ! to the ETABLE counter values (NL+1). Therefore, the values shown in the ! last ETABLE output are the top values of the top layer (layer 5 TOP). NL=5 ! element comprised of five layers *do,i,1,NL+1,1 ! for each layer ... get "bottom" values /gopr etable,erase etable,ilsxz,smisc,(2*i)-1 ! interlaminar (transverse) SXZ shear stress etable,ilsyz,smisc,(2*i) ! interlaminar (transverse) SYZ shear stress etable,ilsum,nmisc,(2*i)+5 ! shear stress vector sum etable,ilang,nmisc,(2*i)+6 ! angle of shear stress vector pretab,grp1 *enddo rsys,solu ! needed for output in layer system layer,1 presol,s,comp layer,2 presol,s,comp layer,3 presol,s,comp layer,4 presol,s,comp layer,5 presol,s,comp layer,0 ! element coordinate system presol,s,comp rsys,1 ! Global Y-Z corresponds to Element X-Y layer,1 presol,s,comp layer,2 presol,s,comp layer,3 presol,s,comp layer,4 presol,s,comp layer,5 presol,s,comp layer,0 ! element coordinate system presol,s,comp /eof . |
||
|