simulation tissue behaviour in kevlar

[jaccio404]

Good morning.
I would need to model the behavior of a component consisting of a kevlar fabric in ansys wb 13. My problem is that I don't know how to model high compression flexibility but at the same time high traction rigidity. I better explain: if you take a kevlar fiber and pull it is very durable, if you compress it along its axis collapses instantly. I have to simulate this, do you have advice?

 

[stefano.garbin]

model the fabric with shell elements.
There is a keyoption, I don't remember which, which introduces the "diaphragm" behavior.
this means that the element has a flexional stiffness practically nothing, resists only to traction.

 

[jaccio404]

Okay, but where can I find her? in the mesh menu?
thanks for the prompt response!

 

[stefano.garbin]

no, for each body (surface) made in kevlar you will have to enter a snippet command.
Let's give you time to inform me, I'll give you an example this afternoon.
Now I don't have ansys in front.

 

[jaccio404]

Thank you.

 

[stefano.garbin]

then, to simulate a fabric you can use a mesh with shell181 (the default wb element for meshare surfaces).
on the body "woven" insert a snippet command and write in:

keyopt,matid,1,1   !opzione membrana
keyopt,matid,3,2   !full integration

Note: Enable all non-linearity (large deflection) and use small time steps. convergence will be a huge problem unfortunately.
if you read This link you will find useful information.
If there are big convergence issues you will see forced to "duplicate" the tissue body, attach it to the other with a bonded contact, assign it a 10-100-time thick smaller and leave it without membrane options.
this is because in any case in reality every fabric expresses a minimum of compression resistance, and this eye helps convergence.
ps: once there was an element made specifically: shell41.

if someone else of expert in this field is reading the invitation to express opinions and experiences in this regard, because the question is only seemingly trivial!

 

[jaccio404]

How did you anticipate there are big convergence problems...with "duplicate" what do you mean? do you refer for example to a layer of 1 mm to simulate as 10 by 1? I have the feeling that I would not be able to solve the following problem anyway: If I have a perfectly linear bar and tickled it with axial compression I don't think she shoves, whether I give her membrane properties is if "duplico" the material as you say. Maybe I'm wrong though!

 

[stefano.garbin]

The bar test that you're putting on is what I quickly did. In fact to make it work you have to put a small pressure on the face so that it slightly curves.
to duplicate I mean this: physically you have a bar (to which you will check the normal thickness, for example 1mm)
in "design modeler" you have to create one of the same perfectly overlapping, then in simulation create a "bonded" contact between the 2 platelets. to the second plate assign a small thickness (e.g. 0.1mm instead of 1mm) but not membrane characteristics.
Forgive me if I explain to you in speed but I'm a little messed up!

 

[jaccio404]

Ahhh, now I understand, thank you. even if so I have to enter a defect in order to make it curve! I try...