/COM,ANSYS MEDIA REL. 182 (07/10/2017) REF. VERIF. MANUAL: REL. 182 /verify,vmr020-t3b-183 /title,vmr020-t3b-183,Angle crack plate embedded in a plate (Uniaxial tension) /com, /com, Problem is taken from NAFEMS Publication /com, "2D Test Cases in Linear Elastic Fracture Mechanics" /com, Test case 3.2, crack angle = 67.5 /com, /com, Reference: Rooke D P and Cartwright D J : Compendium /com, of stress intensity factors, HMSO, London, England (1976) /com, /com, ********************************************************** /com, Stress Intensity Factor Calculation using Interaction /com, Integral Approach /prep7 e=207000 !youngs modulus nu=0.3 !poissons ratio sig=100 !surface load a=25 !crack length pi=3.141593 et,1,plane183,,,2 !plane183 elements, plane strain mp,ex,1,e mp,nuxy,1,nu k,1,,, k,2,50,, k,3,100,, k,4,100,72.069 k,5,73.0969,72.069 k,6,50,62.5 k,7,26.9031,52.933 k,8,,52.933 k,9,,125 k,10,50,125 k,11,50,62.5 k,12,100,125 l,1,2 l,2,6 l,6,7 l,7,8 l,8,1 al,1,2,3,4,5 l,2,3 l,3,4 l,4,5 l,5,6 al,6,7,8,9,2 l,4,12 l,12,10 l,10,11 l,11,5 al,10,11,12,13,8 l,10,9 l,9,8 l,7,11 al,14,15,4,16,12 kscon,5,4,1,8,0.75 !crack tip elements kscon,7,4,1,8,0.75 esize,4 amesh,1 amesh,2 amesh,3 amesh,4 cskp,11,0,7,6,9 cskp,12,0,5,6,3 csys,0 /solu autots,on nsubst,10 outres,all,all nsel,s,loc,y,0 nsel,r,loc,x,0,100 d,all,uy,0 nsel,r,loc,x,100 d,all,ux,0 nsel,all lsel,s,line,,14 lsel,a,line,,11 sfl,all,press,-sig lsel,all nsel,s,loc,y,52.933 nsel,r,loc,x,26.9031 cm,crack1,node ! define the crack tip node component nsel,s,loc,y,72.069 nsel,r,loc,x,73.0969 cm,crack2,node ! define the crack tip node component cint,new,1 cint,type,sifs ! calculate stress intensity factors cint,ctnc,crack1 ! crack ID cint,ncon,6 ! number of countours cint,symm,off ! symmetry off cint,norm,12,2 cint,list allsel,all cint,new,2 cint,type,sifs ! calculate stress intensity factor cint,ctnc,crack2 ! crack ID cint,ncon,6 ! number of countours cint,symm,off ! symmetry off cint,norm,11,2 cint,list allsel,all solve fini /out,scratch /post1 csys,0 rsys,0 prcint,2,,k1 *get,k1_1,cint,2,ctip,node(73.0969,72.069,0),,1,dtype,k1 *get,k1_2,cint,2,ctip,node(73.0969,72.069,0),,2,dtype,k1 *get,k1_3,cint,2,ctip,node(73.0969,72.069,0),,3,dtype,k1 *get,k1_4,cint,2,ctip,node(73.0969,72.069,0),,4,dtype,k1 *get,k1_5,cint,2,ctip,node(73.0969,72.069,0),,5,dtype,k1 *get,k1_6,cint,2,ctip,node(73.0969,72.069,0),,6,dtype,k1 con1 = ((pi*a)**0.5) k1=(k1_2+k1_3+k1_4+k1_5+k1_6)/5 k0=(sig*con1) norm_k1=k1/k0 *stat,norm_k1 prcint,2,,k2 *get,k2_1,cint,2,ctip,node(73.0969,72.069,0),,1,dtype,k2 *get,k2_2,cint,2,ctip,node(73.0969,72.069,0),,2,dtype,k2 *get,k2_3,cint,2,ctip,node(73.0969,72.069,0),,3,dtype,k2 *get,k2_4,cint,2,ctip,node(73.0969,72.069,0),,4,dtype,k2 *get,k2_5,cint,2,ctip,node(73.0969,72.069,0),,5,dtype,k2 *get,k2_6,cint,2,ctip,node(73.0969,72.069,0),,6,dtype,k2 con1 = ((pi*a)**0.5) k2=(k2_2+k2_3+k2_4+k2_5+k2_6)/5 k0=(sig*con1) norm_k2=k2/k0 *stat,norm_k2 /out, *DIM,LABEL,CHAR,2,5 *DIM,VALUE,,2,3 LABEL(1,1) = 'KI', 'KII' *VFILL,VALUE(1,1),DATA,1.03,0.370 *VFILL,VALUE(1,2),DATA,norm_k1,norm_k2 *VFILL,VALUE(1,3),DATA,ABS(norm_k1/1.03 ),ABS(norm_k2/0.370 ) SAVE,TABLE_1 /NOPR /COM /OUT,vmr020-t3b-183,vrt /COM,------------------- vmr020-t3b-183 RESULTS COMPARISON --------------------- /COM, /COM, | TARGET | MECHANICAL APDL | RATIO /COM, RESUME,TABLE_1 /COM,USING STRESS INTENSITY FACTOR CALCULATION *VWRITE,LABEL(1,1),LABEL(1,2),VALUE(1,1),VALUE(1,2),VALUE(1,3) (1X,A4,A4' ',F10.3,' ',F12.3,' ',1F16.3) /COM, /COM, /COM,------------------------------------------------------------------------------- /OUT FINISH *list,vmr020-t3b-183,vrt