Learning Forum

[ablanco953]

Hi everyone!

Im thinking about doing a "Compression After Impact" simulation. This consists of performing a dynamic impact on a specimen and after performing a compression test on the specimen. For this purpose, I have thought of doing two simulations: 1st dynamic and 2nd stactic simulation

My question is how to how to properly transfer the data between these two simulations.

In particular, I need to simulate the impact on a square plate to observe how the material is deformed and damaged, followed by a static compression where both the deformed mesh and the altered material properties in the damaged area are considered.

So far, I have used Explicit Dynamics for the impact analysis and Mechanical for the compression. However, I am having difficulties importing the deformed mesh and the damage/plasticity fields generated in the impact analysis into the compression analysis.

My main questions are:

1. What is the best way to export the deformed mesh and accumulated damage states from the impact analysis in Explicit Dynamics?
2. How can this deformed mesh and altered material properties be imported into the compression analysis in Mechanical so that the damage characteristics are maintained?
3. Has anyone worked with External Data or Data Mapping tools in Workbench for this type of data transfer and could you share your experience?

I welcome any guidance or tutorials you can recommend, as my goal is to maintain continuity between the two simulations and ensure that the impact effects are reflected in the compression phase.

ref: https://www.researchgate.net/figure/Compression-after-impact-CAI-experiments-a-the-new-CAI-fixture-designed-to-avoid_fig2_372666364

[Pedram Samadian]

Hi,

 

Thanks for contacting us. To export the deformed mesh and final material properties from the first simulation and use them as initial conditions for a second simulation in Mechanical, you can follow these steps:

1. Insert a new Mechanical System in the Project Schematic page of Workbench.
2. Connect the Engineering Data cell of the first system to the Engineering Data for the new system.
3. Connect the Solution cell of the first system to the Model cell of the second system.
4. Update the Solution/Results cells in the first system if necessary.

When you open Mechanical in the second system, you should see the deformed shape/mesh ready for further analysis [1]. 

I hope this answer helps.

Thanks,

Pedram

[Chris Quan]

Thanks to Pedram for explaining the procedures of transferring deformed geometry to Static Structural system. 

Since the material model used in Explicit Dynamics system may not be the same as the one used in Static Structural for the same part, it is difficult to transfer the material damage from Explicit Dynamics system to Static Structural system. If there are material failure in Explicit Dynamics analysis, make sure set erosion with material failure to Yes in Erosion Controls under Analysis Settings so the elements that have material failure will not be transferred to Static Structural system.

If residual stress/strain state is also need to be transferred to Static Structural system, you can export them from Explicit Dynamics system and then use External Data system to read the output files before linking the External Data system to Static Structural system to transfer the stress/strain.

 

 

[ablanco953]

Thank you so much for this information, Pedram and Chris!!

I will try your procedures, thank you!

Do you know some tutorial that shows how transfer this type of damage material (or similar) between different simulations?

Cheers.

ablanco