Dear mohammad there some pdf files about abaqus hope it will useful for u .

I recommend getting this reference;

Advanced Simulation of Low Impact on

Fibre Reinforced Laminates by Claudio Lopez, just ggogle the title, it has a good example.

thanks Ali,

I read this paper. it is n't useful to me; because I know about theories but I don't know about using it in Abaqus. If you recommend a step by step tutorial, I would thank you.

I suggest you do the example of an impacting ball in the abaqus documentation to make your hand with it. When it is done, you need to modify the isotropic material used for composite. In abaqus explicit, you can use several methods for element selection/layering.

For composite you will define an elastic with engineering constant and then define damage.

In abaqus explicit you will generally chose shell (S4/S4R) or contiunum shell elements (SC8/SC8R) for which composite layer can be defined. If solid elements are chosen, you will have to define manually every layer direction via partition of the target.

For transverse impact on shell target, cohesive zone elements (for S4R) or cohesive contact (SC8R) needs to be defined between the layups (you must use multiple shell stacked) . Typically 3 or 4 cohesive zone contact are used to stabilize the total strain energy.

You might not find a single tutorial for all the but knowing what you need to use, it is quite easy to evolve with abaqus doc and then adjust your needs.

I hope it helped. Regards

@ Philippe

Thanks it's so useful

could you please define solid element modeling in detail?

Hi Mohammad, as Philippe suggested, it would be convenient to use shell, rather than solid elements for the composite damage under impact. You would be able to use the Hashin / Maximum stress / Maximum strain criteria available from within CAE. Try to look up the "Failure of blunt notched fiber metal laminates" example in the "Example problems" of the Abaqus documentation collection. You are provided with inp files, and CAE scripts to generate the model.

If you do need to go with solid elements though, you probably have to define your own user subroutine for material behaviour, and code whatever failure model you might want to use. The example I mentioned also has a few inp files and CAE scripts for solid element mesh models combined with a UMAT routine.

Thanks Shayam

but could you name an example that combined with a VUMAT routine?

Hi Mohammad, please take a look at the attached subroutine codes. Both describe elastic behaviour using a composite laminate theory approach. If you compare both, you;ll see that there a few differences between UMAT and VUMAT in terms of what variables you have access to, and what you have to update.

If you look at the input file (using UMAT) in the example that I had mentioned, you can see some lines similar to

*MATERIAL, NAME=KINPLAS

*USER MATERIAL, CONSTANTS=4

30.E6, 0.3, 30.E3, 40.E3

*DEPVAR

5

*INITIAL CONDITIONS, TYPE=SOLUTION

These are used to specify the input properties for your user material, and to call the user subroutine code for all elements associated with it. Although the fiber metal laminate example uses a UMAT subroutine, the format for the input lines in the case of a VUMAT are just the same. Only the code itself varies.

I got it!

thanks Shyam

Dear mohammad there some pdf files about abaqus hope it will useful for u .

sir

how to model high velocity impact on composite target could you please help me

@Binil benny Nm

Visit BanuMusaGr.com

There is a tutorial on YouTube,

https://youtu.be/7PrwggZTkWs