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
! /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