cohesive elements distortion

[Hossein Mohammadi H]

I am simulating the separation of two different parts which are connected with a thin layer of cohesive elements in a 2D explicit problem. The simulation is conducted successfully without error. But the final results shown in the visualization module seems very weird (see the attached photo-left). I also simulated a similar problem via a static solver and my results do not show this weird distortion anymore (see the attached photo-right). Can anyone help to figure out the problem? Thanks in advance.
Additional information about interactions: in both cases, I used "tie" to connect the cohesive layer to right and left side parts. The interaction between the rigid body that moves downward and right/left parts is a hard contact with penalty friction.

 

[FEA way]

Do you have point mass/inertia assigned to the rigid body’s reference point ? Did you try with general contact ? And what are the other differences between these two analyses ?

 

[Hossein Mohammadi H]

Thank you for your response. I added mass/inertia to the rigid body's RP. But it did not change. The static and explicit models are totally the same. I just defined U2 for rigid body movement in the static simulation while V2 for explicit simulation.
I checked general contact for the explicit solver and the result totally changed (new attached photo). I used the same interaction properties for contacts. Just used General contact instead of Surface-to-surface contact to assign these properties to the surfaces. I do not understand the differences and what was the problem with the previous one. I used surface-to-surface contact in the static solver and it worked.
The other point is that although we do not see the distortion in explicit solver results anymore, the output is not what I expected (sth similar to static output). Do you know what is the problem with it? Your help is greatly appreciated.

 

[FEA way]

Have you tried with prescribed displacement (with amplitude) instead of velocity in Explicit ? Do you use mass scaling ?

 

[Hossein Mohammadi H]

I tried with displacement in Explicit as well. For both contact strategies (General and Surface-to-surface) I get similar results to previous ones.
I mean:
Defining displacement & General contact similar to Defining velocity & General contact
Defining displacement & Surface-to-surface contact similar to Defining velocity & Surface-to-surface contact contact

 

[FEA way]

You should enable element deletion for cohesive elements. But notice that these elements don't resist penetration of the rigid body (only the two connected plates come into contact with it). Thus, the approach that you use may not be correct. Is this analysis based on some research paper ?

 

[Hossein Mohammadi H]

I enabled element deletion in element type for cohesive elements but they do not disappear yet. Do you know what else should I check?
Yes, this analysis is similar to the approach has been used in a research paper. However, I am using my own geometry and material properties. Do you mean the approach of using cohesive elements for the simulation of penetration is not correct or the way I am conducting with it?

 

[FEA way]

Maybe it would be better to use regular elements with damage and deletion in this case. It depends what you want to achieve. Can you share the title of this article ?

 

[Hossein Mohammadi H]

As far as I know, the options we have for the definition of damage in mechanical properties are
Damage for traction separation law
Damage for fiber-reinforced composites
damage for ductile metals
damage for elastomers
As I do not work on metals, composites, and elastomers, I think I should use TSL. Can I use TSL with regular elements?
The paper is "Detailed finite element modelling of deep needle insertions into a soft tissue phantom using acohesive approach" in which cohesive elements with the definition of TSL has been used.

 

[FEA way]

It seems that the problem is caused by the way you implement these cohesive elements in your model. You have to edit coordinates of all nodes in the cohesive layer to make them lie along the interface between parts that are connected with adhesive. Based on the pictures in the article, it seems that its authors did this too. Of course you also have to connect these cohesive elements with regular elements (either via shared or with tie constraints).

 

[Hossein Mohammadi H]

Yes. You are right the problem is probably related to how I defined cohesive elements. But could you please let me know what should I exactly do? How can I edit coordinates of all nodes?
Another important thing is that I used a very thin layer of cohesive layer instead of zero thickness and my simulation is different from the paper in this way as well. Do you think it is a problem too? If yes, how can I create a zero thickness cohesive layer? Thank you very much for your responses.

 

[FEA way]

There are two modeling techniques. In case of 2D model:

a) shared nodes approach:
- start from the part consisting of two objects being connected and finite thickness adhesive layer between them
- mesh the part
- use Edit Mesh —> Node —> Edit —> Coordinates for nodes on both sides of the interface to place them along the same line (toggle off projection to geometry)

b) tie constraints approach:
- create two instances of the objects being connected and position them without the gap
- create an instance of finite thickness adhesive layer, position it properly and define tie constraints (cohesive side should be slave)
- mesh the whole model
- use Edit Mesh —> Node —> Edit —> Coordinates for all nodes of the cohesive layer to make them lie along the interface

 

[Hossein Mohammadi H]

Than you so much.
I tried to apply these approaches for zero thickness cohesive elements. But I have the following problems with them:

approach a) As Abaqus does not allow to create parts from the sketch that intersect itself I created the whole domain as an object and using partitioning I divided it into three partitions (left, thin cohesive layer, and right). I am not sure it was the exact way you said. But it was the only way that I could have the objects in one part. Now the problem is that as in my model there is another body that should insert to this part, I need to define contact with it and cohesive layer left and right borders. But in this way, I can not define such contacts.

approach b) I used this approach and it worked. But I get a more strange output now. The cohesive element seems twisting like before but in a more weird way. Moreover, the result is asymmetric now.
When I do a similar simulation via static solver I get more reasonable results (attached photo, left: explicit, right: static).

 

[FEA way]

For the first approach you can use general contact. It should handle the interaction between this deformable part and rigid tool.