Modelling a cohesive zone between two 3D solid elements in ANSYS using the element inter205 3

[Naval123]

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

 

[Stanum]

You should probably provide a part of your apdl macro to receive a more coherent answer. As for me I received such mistake message, when I forgot that inter 20x elements can be applied only to a a bodies that share nodes. So that if you had two bodies with coincident but separate nodes you would receive the message you provided. But I suppose there are probably other reasons why you can receive such message. For example it could occur if there are problems with the location where your interface elements have to be located. You can try to modify the tolerance parameter to handle this, if you are sure that it is the problem source.

 

[chats2808]

Hi Naval123,
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

 

[Stanum]

if you need it in z plane, you can try using cartesian coordinate system:
CZMESH,,,0,z,1

 

[chats2808]

Thanks Stanum, I will try this and get back to you.

 

[chats2808]

Thanks Stanum,
I was able to model cohesive zone now.

 

[chats2808]

One more Doubt Stanum,
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

 

[Stanum]

Do you have nodes at these loacations? If you do, then I suppose
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

tb, czm,i,...​

tbdata,1, dist(i,2), dist(i,3), dist(i,4),dist(i,5), dist(i,6)​

CZMESH,,,0,z,dist(i,1)​

*enddo

 

[chats2808]

Sorry to bother you again, but can u plz explain the code. I mean how is I, and J picked and how to give the distances?

P.S. I m in nascent stage of FEA.

 

[Stanum]

I meant following

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

 

[chats2808]

HI STANUM,
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? :-(

 

[Stanum]

hello chats,

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.

 

[choudhs1]

hello everyone,
Can inter 205 be applied to 2D shell element?