Cohesive Zone Modeling in ABAQUS - Pull-out test 1

[ISAAC JAMES]

Can anyone please help me with this.

I am getting a message like "Int 1 references a global contact property that contains cohesive behavior option. This option cannot be specified in General Contact (Exp). " I wanted to carry out pull-out test simulation using the Cohesive Zone Model in ABAQUS for a wire embedded in a matrix polymer. Can anyone please help me out with this? I have seen the previous threads regarding this discussion but I am still facing doubts. Please help.

 

[FEA way]

You will need 2 contact properties - one without a cohesive behavior (use it as a global property for general contact) and one with a cohesive behavior (use it as an individual property assignment for the selected surfaces).

 

[ISAAC JAMES]

Could you please let me know how I can do that?I have given tangentil and normal bevior also

 

[FEA way]

You just have to create one more contact property (it can be empty if you want to use the default settings) and select it as global interaction property in general contact definition. Then go to individual property assignments, choose two surfaces and your previous contact property (the one with cohesive behavior) and confirm.

 

[ISAAC JAMES]

Ok Sir. Thanks for the clarificaation. Will check out.

 

[ISAAC JAMES]

I had a doubt while defining constraints. The Cohesive Zone Modeling (CZM) for my simulation involves a wire subjected to a pull-out test. The wire is embedded in a polymer matrix. So, what type of constraint should I use? Should I use the 'Rigid body constraint' or the 'Embedded region constraint'? I am familiar with using the 'Rigid body constraint' but I am not familiar with the other one. Will the 'Rigid body constraint' be enough for my case? Or should I use the 'Embedded region constraint'? By the way, 10mm of the wire is embedded in the polymer matrix while the remaining 10mm is located outside the polymer matrix. If so, how should I proceed?

I also had one more question. Does this type of simulation involve the usage of 'zero thickness cohesive elements' ? If so, how can I implement that?

Basically speaking, it would be really helpful if someone could elaborate on the most essential constraints, contact pairs and interactions that are required for simulations such as these.

Thanks.

 

[ISAAC JAMES]

Can anyone please help me out with this?

 

[ISAAC JAMES]

Please help

 

[FEA way]

If you want to account for cohesive behavior in the interface between the wire and matrix, you don't need any constraints like embedded region or rigid body. You should just model a cavity in the matrix, put the wire inside and either define cohesive contact between them or create a layer of cohesive elements.

 

[ISAAC JAMES]

Oh ok. Thanks a lot, Sir for the help!

 

[ISAAC JAMES]

Lastly, Sir, could you explain me as to how I can obtain the Load vs Displacement graph for my pull-out test? What are the nodes that I need to select for this purpose? How should I edit the history ouput?

It would be a geat help Sir if you could clear this doubt for me.

Thanks.

 

[SWComposites]

depends on what you are going to compare the load-displ output to. if you are going to compare to test data, then you need to determine where displacement is measured during the test, and select nodes at those locations.

 

[FEA way]

You can request history output using predefined node sets or utilize the XY Data from ODB Field Output option. The location of the nodes depends on your case. They should properly represent the deformation of the model.

 

[ISAAC JAMES]

Oh I see. Thank you so much for the help @SWComposites and @FEA way. Thanks a lot.

 

[ISAAC JAMES]

Hi. I was working on this in greater detail. I wanted to use zero thickness cohesive elements between the wire and the matrix. I have defined these zero thicknes cohesive elements at the interface. But, my doubt is, do I need to apply tie constraint at the interface between the cohesive element and the matrix and also between the wire and the cohesive element?

Furthermore, which method is more accurate - using the cohesive contact or the cohesive elements? What are the things that I need to ensure while using cohesive element layer?

 

[ISAAC JAMES]

Could someone kindly help me out with this?

 

[Clara HSU]

Hi, I donot know if you found the solution you are looking for. But indeed the cohesive elements need to be tied to both matrix and wire. or make a single part and make sections and provide material property. But then I think for zero thick elements separate parts work better? this i am not very sure.

If there is also friction involved in the pullout, then contact is a better implementation. If it is with elements, friction will then need to be converted into a traction separation law and applied as a second property to the elements about which I also not know enough of.

Would like to get in touch with you as me myself is also trying to model a fibre pullout.

 

[FEA way]

There are 2 approaches to connect cohesive elements with the rest of the model - via tie constraints or via shared nodes. I described them in some older threads like this one:

https://www.eng-tips.com/viewthread.cfm?qid=468220

but they are also mentioned in the documentation chapter Elements --> Special-Purpose Elements --> Cohesive Elements --> Modeling with Cohesive Elements (paragraph "Connecting Cohesive Elements to Other Components").

Regarding the differences between cohesive elements and cohesive contact, the best summary can be found in the documentation chapter Interactions --> Contact Property Models --> Mechanical Contact Properties --> Contact Cohesive Behavior (paragraph "High-Level Comparison of Cohesive-Element and Cohesive-Contact Approaches").