Modeling impact - Impactor velocity 1

[loyal979]

Hey All,

I am modeling an impact simulation of composite materials in ABAQUS explicit. I have two steps on my model, one for impact and then the second one for compression after impact. I have defined the impactor velocity as a predefined field (initial velocity). I could not deactivate this load in the second step since there is no need for the impactor in the second step. What are your suggestions? Thank you!

 

[FEA way]

I suggest using import capability for the purpose of this analysis. To do it first solve only one step (impact) then copy the model and replace this impact step with compression (you can even use Standard for this simulation). To import results from impact analysis to compression one use Predefined field (select initial step) —> Initial state.

 

[loyal979]

Thank you for your reply and suggestion. I like this approach. it would save me some time.

So, Just to clarify, the results of the impact will be imported to the model with the compression setup. is that correct? Or you meant by importing the model along with the impact result from the ODB file?

Do I need to have or use the restart option for my impact analysis in order to use the initial state feature?

 

[FEA way]

When you use import capability, results from the end of the first analysis are used as initial state of the second model. This procedure is automatic. Just use *IMPORT keyword or set it up in CAE and submit the job. Abaqus will find files generated by the impact analysis and use them in compression simulation.

 

[loyal979]

Thank you. I appreciate your help.
The only thing that concerns me is the model stabilization after the impactor leaves the impacted plate. After the impact, the plate will be vibrating (Free vibration) and I am just wondering if I should increase the linear viscosity parameter in the step to damp the plate oscillations after impact and before performing the compression test.

 

[FEA way]

There are several ways to damp vibrations occuring after impact so that the model is stabilized during compression step. Some time ago I listed them here (along with references):

https://www.eng-tips.com/viewthread.cfm?qid=457446

Personally I recommend using viscous pressure approach. This load type is meant for such cases.