Cohesive Zone basic Model

Cohesive zone model is part of Fracture Mechanics. It is used when a crack is present and when a load is applied. For an example I built a simple model in ANSYS. ANSYS has a short description about what is meant to go on in a cohesive zone model, however it's not that good. The main problem is some of the commands can only be done text based i.e. there is no submenu where you input these. I did a simple 2D model, here is the full text input

Show text

! /Com,for a cohesive model
! /Com, directory
/CWD,'J:\ANSYS\SolderModel\cohesive zone'
! /Com, selecte structural from preferences
/NOPR   
/PMETH,OFF,0
KEYW,PR_SET,1   
KEYW,PR_STRUC,1 
KEYW,PR_THERM,0 
KEYW,PR_FLUID,0 
KEYW,PR_ELMAG,0 
KEYW,MAGNOD,0   
KEYW,MAGEDG,0   
KEYW,MAGHFE,0   
KEYW,MAGELC,0   
KEYW,PR_MULTI,0 
KEYW,PR_CFD,0   
/GO 
!*  
!*  
/PREP7  
!*  
! /Com,structural element
ET,1,PLANE42
! /Com,interface element
ET,2,INTER202
! /Com, chip young's modulus and poisson's ratio
MPTEMP,,,,,,,,  
MPTEMP,1,0  
MPDATA,EX,1,,130e9  
MPDATA,PRXY,1,,0.29
! /COM, cohesive zone constants may have some problems with this
TB,CZM, 2,1,,EXPO
! /com,the material number is 2 in this case. You may use other number.
TBDATA,,100e7,0.1,0.1 
! /COM,TBTEMP,100.0 
!*  
! /Com,define keypoints
K,1,0,0,0,  
K,2,6,0,0,  
K,3,0,1.75,0,  
K,4,2,2,0,  
K,5,6,2,0,  
! /Com, define lines
LSTR,       3,       1  
LSTR,       1,       2  
LSTR,       2,       5  
LSTR,       5,       4  
LSTR,       4,       3  
! /Com,define area
FLST,2,5,4  
FITEM,2,1   
FITEM,2,5   
FITEM,2,4   
FITEM,2,3   
FITEM,2,2   
AL,P51X 
! /Com, reflect the area in the x axis
FLST,3,1,5,ORDE,1   
FITEM,3,1   
ARSYM,Y,P51X, , , ,0,0 
! /Com, offset in y direction by 4 
FLST,3,1,5,ORDE,1   
FITEM,3,2   
AGEN, ,P51X, , , ,4, , , ,1
! /Com, merge line and keypoint together
/PNUM,KP,1  
/PNUM,LINE,1
/PNUM,AREA,0
/PNUM,VOLU,0
/PNUM,NODE,0
/PNUM,TABN,0
/PNUM,SVAL,0
/NUMBER,0   
!*  
/PNUM,ELEM,0
/REPLOT 
!*  
NUMMRG,KP, , , ,LOW 
! /Com, assign globally both areas as elements plane42
TYPE,   1   
MAT,       1
REAL,   
ESYS,       0   
SECNUM, 
! /Com,move elements up  
FLST,3,2,5,ORDE,2   
FITEM,3,1   
FITEM,3,-2  
AGEN, ,P51X, , , ,-2, , , ,1
! /Com, mesh and refinenment at specific nodes  
MSHAPE,0,2D 
MSHKEY,0
!*  
FLST,5,2,5,ORDE,2   
FITEM,5,1   
FITEM,5,-2  
CM,_Y,AREA  
ASEL, , , ,P51X 
CM,_Y1,AREA 
CHKMSH,'AREA'   
CMSEL,S,_Y  
!*  
AMESH,_Y1   
!*  
CMDELE,_Y   
CMDELE,_Y1  
CMDELE,_Y2  
!*  
FLST,5,7,1,ORDE,3   
FITEM,5,15  
FITEM,5,18  
FITEM,5,-23 
CM,_Y,NODE  
NSEL, , , ,P51X 
CM,_Y1,NODE 
CMSEL,S,_Y  
CMDELE,_Y   
!*  
!*  
NREFINE,_Y1, , ,1,1,1,1 
CMDELE,_Y1  
!*  
! /Com, cohesive zone mesh
mat,2
czmesh,,,0,y,0 
! /Com, no movement on the bottom left keypoint   
FLST,2,1,3,ORDE,1   
FITEM,2,1   
!*  
/GO 
DK,P51X, ,0.0, ,0,ALL, , , , , ,
! /Com, no movement on the top left keypoint in x direction
FLST,2,1,3,ORDE,1   
FITEM,2,7   
!*  
/GO 
DK,P51X, ,0, ,0,UX, , , , , ,   
! /Com, movement on the top left keypoint in y direction
FLST,2,1,3,ORDE,1   
FITEM,2,7   
!*  
/GO 
DK,P51X, ,0.7, ,0,UY, , , , , ,    
FINISH  
/SOL
/STATUS,SOLU
SOLVE   

One thing I found out is that ANSYS will not show you cracks instead it will show you elements coloured in different colours and you have to use the scale to check to see if it has cracked