Repeated impact in composite plate 2

[Aksil]

thread799-343531
Hello
I have a problem about the simulation of progressive damage in composite plate under repeated (multi-impact) low velocity impact using soubroutine Vumat implimented in Abaqus ,I was developped the soubroutine and i validate with experemental data with different creteria(hashin-puck) in the first drop,but i don't know how i will repeat the impact events ,than if seomone do it preveousely I have one idea,with the use of results of the last impact but when i do the import of odb the simulation dont run,in the message indicate that the model need assign section and materials on the other hand ,i think about another method , creating more than one impactor in the model to achieve successive impacts. Those impactors should be arranged in a queue with an interval, moving downwards together.but the problem that the first impactor when it rebond crash with the second impactor , The interval should be calculated in order to obtain an initial impact velocity ? I will be delighted if someone can explain to me

 

[FEA way]

Import capability is the best option in this case. It supports materials defined via UMAT or VUMAT subroutines. Just make sure that you set it up properly. Detailed instructions can be found in the documentation chapters "About transferring results between Abaqus analyses" and "Transferring results from one Abaqus/Explicit analysis to another".

The second approach could work as well. Penetration between impactors won’t be a problem if they are rigid and you don’t define contact between them or exclude it from general contact definition.

 

[Mustaine3]

Yeah, contact exclusion is an option in general contact. So you you can specify, that the two surfaces do not know each other.

 

[Aksil]

FEA way and Mustaine3 Thanks for your answers ,i will use the second approach ,to model various impactor ,if each impactor i will specify the step ,so multi-steps ? on the other hand how i calculate the interval between impactors ?

 

[FEA way]

Usually in impact analyses we specify initial velocity for the impactor. To do it in this case you would have to place impactors in a line, one behind/above the other. Separate them by such distance that, given the initial velocity, they reach the target at desired moment in time.

 

[Aksil]

FEA way ,thanks ,i do it but the problem between the impactors so for example when the first impactor rebound ,dont permit to the second for impacting the area ,and he toped the second impactor

 

[Aksil]

Mustaine3, where i find contact exclusion , i didn't find it in the interface of Abaqus

 

[FEA way]

Can you attach some pictures showing your model ? It would help us find a solution. With no contact defined between the impactors they should pass through each other with no interference. But maybe in this case it will be better to use import capability.

Contact exclusions can be defined in Contact Domain part of the general contact settings window. Look for "Excluded surface pairs" option and click edit button next to it.

 

[Aksil]

FEA way
now it works well, but without the cohesive elements between the layers. so my last question,in cohesive zone model, i know one method that define properties in the interaction modules but in results we can't see the interface of delamination ,my question how i define the properties in materials and create an interface of delamination for showing it

like the pictures,

 

[FEA way]

This method where you define cohesive zone properties in contact interaction is called surface-based cohesive behavior. This simplified approach to CZM works under the assumption that interface thickness is negligible. If you want to use more detailed method to model connection of finite thickness then you should choose element-based cohesive behavior. Its set up is more complicated though since uou have to create cohesive elements. The details are described in Abaqus documentation (including chapter titled "Modeling with cohesive elements" and the whole section "Adhesive joints and bonded interfaces").