Modeling composite by connecting two materials

[simo7]

Hi
I was wondering how to model composite elements using two or more shell elements connected together (which have difrent real conisions or material) - what kind of connections I must use between shell elemensts or nodes to simulate effect of twist in comosites when you put streach force or moment.
Thanks for any clues

 

[Stringmaker]

Why don't you just use an element such as a SHELL 91 or SHELL99? Take a look at these in the documentation. I believe these will be the preferred method of simulating your scenario.

 

[simo7]

Hi
I now that for layer elements we use shell99 or shell91 but I must simulate some separate beween layers (dealmination) so I`m trying model it like a conncted layer. And in place where delamination is I don`t want have this connections. I made it using ,,cp,, command but it doesn`t working because my element don`t have the same properties like element modeled in normal case.
But any way thanks for response.

 

[Stringmaker]

Simo,
I'm not entirely sure that shell elements are supported in a delamination analysis. You may have to use the SOLSH190 element or use 3D quadratic elements with atleast three elements through the thickness to get a response that is provided by shell elements. But anyway, the procedure for this type of analysis would typically be:

1) Build or import the model as you would in any other analysis.

2) When defining element types you will need to specify an appropriate element for the cohesive zone which forms the bond between the two surfaces seperating. You'll end up using INTER202, INTER203, INTER204, or INTER205 for this depending whether you have 2D or 3D linear or quadratic elements. Say you're using SOLSH190 you would use INT205 as it supports 3D linear elements.

3) The next step will be to create a data table using the TB,CZM command to define the material characteristics of the cohesive material that actually forms the bond.

4) Next you'll want to mesh the elements which form the cohesive zone. If you're using V10 the easiest way would be to use the CZMESH command. If you're using an earlier version you'll need to resort to the E or EGEN command in order to mesh the interface elements.

5) During the solution phase you'll want to ensure that the Full Newton method is used to solve. If you're having convergence issues you may need to incorporate contact elements with your interfacing elements.

Good luck,
-Brian

 

[faspin]

Hi,

I had to use the fonction TBCZM, but I don't find how to enter the datas. When I type TBDATA, somes C1..C6 are asked and I don't know with what each one correspond...
If you have an idea..
Thanks