Modelling a cohesive zone between two 3D solid elements in ANSYS using the element inter205
Modelling a cohesive zone between two 3D solid elements in ANSYS using the element inter205
(OP)
Hello!
I am analysing the coating delamination in steel plates, using ANSYS. For that, i need to do the modelation of a cohesive zone between the coating layer and the plate. In order to create an interface area composed by cohesive zone elements, i am using the CZMESH.
The macro runs well with certain dimentions of the plate and the layer but, when i change those dimentions, ANSYS gives me the next warning:
"No cohesive elements have been created. Please make sure that your input satisfies the cohesive section definition requirements"
Does anybody knows why i get this warning? Or someone already has received this warning?
Thanks





RE: Modelling a cohesive zone between two 3D solid elements in ANSYS using the element inter205
RE: Modelling a cohesive zone between two 3D solid elements in ANSYS using the element inter205
I am facing this glitch too. Did you cracked the error?
TB, CZM,1,,,CBDD – I used this command to define material properties of the cohesive interface
TBDATA, 1,C1,C2,C3,C4,C5 – To define the interface properties
I merged the nodes (range - 1e-7) at the interface of the two parts and then applied the command – CZMESH,,,1,Z,0
And I am getting this error :
"No cohesive elements have been created. Please make sure that your input satisfies the cohesive section definition requirements"
For a surprise, Just for a try when I used this command: CZMESH,,,1,Y,1
I am getting the cohesive zone elements in Y-plane.Which I dont require.
Can u plz help me in this? P.S.: I have to crack this ASAP
Thanks in advance
RE: Modelling a cohesive zone between two 3D solid elements in ANSYS using the element inter205
CZMESH,,,0,z,1
RE: Modelling a cohesive zone between two 3D solid elements in ANSYS using the element inter205
RE: Modelling a cohesive zone between two 3D solid elements in ANSYS using the element inter205
I was able to model cohesive zone now.
RE: Modelling a cohesive zone between two 3D solid elements in ANSYS using the element inter205
Please help!!!
If i require multiple cohesive zones at different offset in Z plane i.e. at 1mm , 1.5 mm and 2 mm, what shall be the command?
Thanks in advance
RE: Modelling a cohesive zone between two 3D solid elements in ANSYS using the element inter205
you can reissue command
x=number of zones,
1+5 - number constants for tbdata! if they are different
*dim,dist,array,x,6
dist(i,j)=1!creating data for array
*do,i,1,x
RE: Modelling a cohesive zone between two 3D solid elements in ANSYS using the element inter205
P.S. I m in nascent stage of FEA.
RE: Modelling a cohesive zone between two 3D solid elements in ANSYS using the element inter205
So you have x surfaces with czm
Each surface(i) is characterized by following
Distance from the coordinate system in z direction: dist_i
Constants for tbdata command input : C1_i, c2_i etc.
In total 6 parameters for 1 surface and 6*x in total (it can be less if you have similar constants for some surfaces)
These parameters can be placed in the array with dimensions: x,6
*dim, dist_par, array, x, 6
To fill the array with data you can use several options. Two most obvious:
1) just write it down
Dist_par(1,1)=(data that is distance for first surface)
Dist_par(1,2)= (data that corresponds to c1 for first surface)
...
Dist_par(2,1)=(data that is distance for second surface)
...
2) use command *vget(I can be wrong about exact name). And use external file with data to fill your array
1.2) if your data has a dependency for example:
Dist_i=dist+delta*i
You can feel your array directly in do loop
RE: Modelling a cohesive zone between two 3D solid elements in ANSYS using the element inter205
I ENTERED THE COMMAND AFTER TAILORING IT TO THE REQUIREMENTS. i HAVE 5 LAYERS TO MODEL AT A DISTANCE ON 2.562 FROM THE Z PLANE AND SUCCESSIVE OFFSET OF 0.188 MM,THE VALUE OF C1,C2,C3 ARE 61,0.0005 AND 0.0004.
UPON IMPORTING THE FILE FROM HYPERMESH, i ADDED ELEMENT INTER205 IN THE ELEMENT DATABASE.
THEREAFTER I WROTE THIS COMMAND:
*DIM,DIST,ARRAY,5,4
*VFILL,DIST(1,1),RAMP,2.5623,0.188
*VFILL,DIST(1,2),RAMP,61,0
*VFILLM,DIST(1,3),RAMP,0.0005,0
*VFILL,DIST(1,4)RAMP,0,0004,0
*DO,I,1,5
TB,CZM,I,,,,
TBDATA,1,DIST(I,2),DIST(I,3),DIST(I,4)
CZMESH,,,0,Z,DIST(I,1)
*ENDDO
buT I GET THIS ERROR
ELEMENTS TO BE SEPARATED BY COHESIVE ELEMENTS ARE OF MORE THAN ONE STIFFNESS NUMBER (185 AND 205, PERHAPS MORE). THE CZMESH COMMAND IS IGNORED
WHAT SHALL I DO?
RE: Modelling a cohesive zone between two 3D solid elements in ANSYS using the element inter205
here are a few minor corrections to your script
*DIM,DIST,ARRAY,5,4
*VFILL,DIST(1,1),RAMP,2.5623,0.188
*VFILL,DIST(1,2),RAMP,61,0
*VFILL,DIST(1,3),RAMP,0.0005,0
*VFILL,DIST(1,4)RAMP,0.0004,0
*DO,I,1,5
TB,CZM,I,,,CBDD
TBDATA,1,DIST(I,2),DIST(I,3),DIST(I,4)
CZMESH,,,0,Z,DIST(I,1)
*ENDDO
as for the mistake you receive, try your macros on a very simple (geometrically) model, check whether it works.
And be 100% sure that you have nodes at your future separation location. also check whether your inter20x element is consistent with elements you use in your analysis, you can also consider using contact elements and assigning them cohesive behavior.
RE: Modelling a cohesive zone between two 3D solid elements in ANSYS using the element inter205
Can inter 205 be applied to 2D shell element?