FEM modelling of Cohesive Zone Model in ABAQUS 6.8.3 1

[sartorbjk]

Hello friends,

I am trying to simulate crack propagation with abaqus.
I have a matrix, fiber, and a cohesive section cutting through both of them.
When I run the simulation, I get the following error:

--
Job Job-1: Analysis Input File Processor completed successfully.
Error in job Job-1: Too many attempts made for this increment
Job Job-1: Abaqus/Standard aborted due to errors.
Error in job Job-1: Abaqus/Standard Analysis exited with an error - Please see the message file for possible error messages if the file exists.
Job Job-1 aborted due to errors.
--
Even if I change the maximum number of increments, still same error.

I am also attaching the model for better understanding.
Can anyone please help me to solve my problem?

Best Regards,
Sartor

 

[rstupplebeen]

I checked out your model and here are my observations in no particular order:
1. Turn on nonlinear geometry
2. You do not have any cohesive properties defined
3. I think only 2 contact definitions are required for each side of the matrix
4. Shouldn't you be pulling on the top and bottom? If so you have symmetry that you can exploit.
5. Is your fixed constraint too close to the region of interest?
6. The smaller zones should have a TIE constraint from the matrix to the fiber
7. Is this simulating a chunk of composite potted in epoxy and then bonded to another similar piece?
8. Your current model has RBM which is causing the convergence issues.

I hope this helps.

Rob Stupplebeen

 

[sartorbjk]

Hi
I am quite new in fem. Thank you very much for your help. I checked the geometry again, try to fix the things you told me but still does not work.

1. Done
2. Defined
3. Done
4. Actually, I am just pulling from Left Up and Left Down side to have a stress concentration on the cohesive section
5. I did not understand
6. I used partition feature now so I think now, I do not have to make constraints for the stress transfer.
7. It is a fiber reinforced ceramic
8. I did not understand this, how can I solve it?

Any other suggestions?
Should I create a constraint between cohesive section and my matrix(and also fiber)?


Best Regards,
Sartor

 

[rstupplebeen]

4. Only model on 1 side of the cohesive section
5. The faces on the right are fixed which will cause an infinite stiffness and my gut feel is that there is not sufficient distance for the shear to develop.
6. Agreed
8. In your interaction properties you need to add cohesive behavior. You need something that ties or glues the bond line otherwise you are modeling a part that already has a crack.

I hope this helps.

Rob Stupplebeen

 

[sartorbjk]

Hi Mr. Stupplebeen,
I would really like to thank you for spending time on my problem.

Still I could not solve it Abaqus suggest the same problem.
-
Error in job Job-1: Too many attempts made for this increment
Job Job-1: Abaqus/Standard aborted due to errors.
Error in job Job-1: Abaqus/Standard Analysis exited with an error - Please see the message file for possible error messages if the file exists.
Job Job-1 aborted due to errors.
-
There must be a problem. I think a design or mechanical problem that I could not include in my geometry and model.

I redraw the geometry. Fiber-Matrix is partitioned. I added a frictionless contact btw Matrix-Fiber surface and cohesive section surface. I changed the BC.

5. I think my mechanical knowledge is not enough to understand it right now. or I am just missing something.
8. Do you know how can I define a cohesive behavior? I thought frictionless behavior would be enough.


Best Regards,
Sartor

 

[rstupplebeen]

5. Is this the size of the actual test sample or end product? If not I am guessing you are modeling a crack on a longer piece. If you modeled more of the longer piece I would expect your results to change because your boundary condition is too close to the region of interest.
8. In the Interaction Property dialog: mechanical>cohesive behavior. Now change both interaction from "surface 2 surface" to "node 2 surface"

I would not use a material with damage evolution instead in the interaction property I would add damage there.

Also, your mesh is very coarse and can sometimes lead to issues. I would use a quad>structured mesh for the 3 shapes that are rectangles and either split the 2 remaining ones into rectangles or use quad>free. Try a density of 5 instead.

I hope this helps.

Rob Stupplebeen

 

[kellnerp]

Before you use all the bells and whistles try to run it as a simple static model. That way you can check for insufficient boundary conditions and other problems.

TOP
CSWP, BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[sartorbjk]

Mr. Stupplebeen:
5. In order to make a more realistic geometry, I used now a new geometry with a very very thin cohesive section.
8. Done.
Mesh is now very small.
-
It still says
"Error in job Job-1: Too many attempts made for this increment"

Nlgeom is on.
In the STEP section:
Maximum number of increments is 1000
Increment size,
initial: 0.01, Minimum 1E-005, Maximum:1

Do you think that it can be somehow related to the STEP definition? I mean the increment sizes and so on?
--
Mr. Kellnerp:
Actually, this is a very simplified picture of a complicated geometry. I thought it is the most simple one. but due to poor experience with mechanical stuff and abaqus, I still could not solve my problem.

Best Regards,
Sartor

 

[rstupplebeen]

I would skip explicitly modeling the cohesive section. Use contact with cohesive and damage.

If you are worried that the step size is the problem try
Maximum number of increments is 100000
Increment size,
initial: 0.0001, Minimum 1E-010, Maximum:1
Set it off and come back tomorrow. It is tough to determine what the appropriate step size is without similar simulations to drive the "rule of thumb"

I hope this helps.

Rob Stupplebeen

 

[amubashar]

Hi

I have made some changes to your model and its converging. However, I am not sure how you determined your cohesive zone element material properties. Cohesive zone model is sensitive to model properties and mesh size and convergence difficulties are often encountered.

Aamir

 

[sartorbjk]

Mr. Stupplebeen,
Before changing the step module parameters, I have deleted the interaction between material and cohesive section and put constraints between the surfaces of material and cohesive section (2 surfaces). That way, the simulation is working now.

Results? They are not like what I expected but now it is a good start. Thank you very much for your help.

Mr. Aamir,
Unfortunately I could not open your file. Could you please upload it again so that I can check it?

Best Regards,
Sartor

 

[rstupplebeen]

Aamir
You are probably on a newer version. Uploading the zipped INP file will probably work.

Rob Stupplebeen

 

[sartorbjk]

Mr. Stupplebeen,
Before, we agreed on the 6. point.

Now I again used partition feature to define the cohesive section. So, no need to make any constraints or create/define surfaces/interactions. The simulation also runs this way without so much distorted elements. So I would say this approach is better.

Regards


Best Regards,
Sartor

 

[amubashar]

I have attached a zipped inp file. In regard to pt 6, I would like to add my bit. The two options available for modelling with cohesive zone elements are either using a continuous mesh or use discontinuous meshes and tie the meshes together. Generally cohesive zone elements represent a crack or an interface and require much smaller element size than the other parts of the model. In this case, a discontinuous mesh gives the benefit of using a finer mesh in cohesive zone area and a coarse mesh in the remaining model, thus decreasing the problem size. On the other hand, contact conditions introduce nonlinearity. Thus the selection of approach depends on the model.

 

[sartorbjk]

1) Could you please tell me how I send the input file to the abaqus solver via a/cae?

2) There is a high stress concentration where matrix and fiber meets (near the cohesive elements). So, the crack occurs first here. Since I am interested in the propagation of matrix cracks and their interaction with fiber, I put some stress concentrators to the left side of the matrix, now, everything seems to work correctly.

Best Regards,
Sartor