Composite crash test simulation shows ductile failure in RADIOSS v2022.3

Jordi_Aynes45

Hello everybody,

I've been trying to run a basic simulation for an impact attenuator made out of a flax STACK laminate with material card ID MAT25_COMPSH and property with card ID: P17_Stack.

I've tried several different parameters but no matter what I do the simulation animation results in a ductile failure instead of being brittle. At the same time DAM1, DAM2 and DAM3 are always 0 and the plastic strains are also 0, which doesn't make sense to me.

I've tried using Chang, Hashin and Puck failure criterion without any luck. I've also seen in a community post that from v2023 Hoffman, TSAIWH, TSAIHILL and MAX_STRAIN have been added, but when I open Hypermesh 2024 (I don't have the 2023 version, only 2022.3 and 2024) those failure criteria aren't showing.

I leave attached a sample .hm file of a baseline simulation (with a random geometry and laminate) as well as a picture showing the failure mode.

Any help would be more than welcome as I'm not sure what to do from now on,

Thank you so much :))

SampleCHANG.hm

Marina_Lima

Hi,

To see the element failure in your model, I recommend setting a Tau_max on /FAIL/CHANG. This parameter defines the time for the element to be deleted after the failure criteria are met. According to Radioss help, it's best to set this value to 10 times the simulation time step:

https://help.altair.com/hwsolvers/rad/topics/solvers/rad/fail_chang_starter_r.htm?zoom_highlight=%2Ffail%2Fchang

After reviewing your model, I noticed potential issues with the contact. Please consider using the best practice parameters for the interface TYPE 7: Igap= 2; Idel = 2; Iform = 2; Istf = 4.

You mentioned that you're using version 2022. In more recent versions, there is an engine keyword that allows you to view the deleted elements for a specific failure. If possible, I suggest running your model in a more recent version: /H3D/ELEM/FAILURE/ID=FAILID/MODE=ALL

Best regards,
Marina Lima

Jordi_Aynes45

https://community.altair.com/discussion/comment/191943#Comment_191943

Hello Marina,

Thank you so so much for the help, the Tau_max solved my issue which I was trying to solve for weeks.

In terms of the overall simulation would you suggest to use a rigid wall instead of a rigid body for this simulation? Would it be more precise than creating the contact with defined parameters?

Everytime I run the simulation I get the ** RUN KILLED: ENERGY ERROR LIMIT REACHED and there's a huge amount of mass added to some nodes which seem to be normal, do you know how to fix that?

A part from that the simulation is still not showing any DAM1, DAM2 and DAM3 values and regarding " /H3D/ELEM/FAILURE/ID=FAILID/MODE=ALL ", I tried to run the simulation in Hypermesh 2024 and I can't seem to find that Failure parameter, I'll leave a picture attached of what's showing.

Thank you so much for the help, it was really useful and sorry for the amount of questions as it's my first RADIOSS simulation.

Thank you again for everything :)),

Jordi Aynes

Marina_Lima

Hi Jordi,

• In this case, you could face some instability in changing the rigid body for the rigid wall (See comment 1) https://help.altair.com/hwsolvers/rad/topics/solvers/rad/rigid_wall_intro_r.htm?zoom_highlight=%2Frwall
• The energy error you're experiencing might be due to inconsistencies in the material properties or/and the input load. Since the yield and strength stress values are identical, there is no intermediate stage of plastic deformation before rupture. Consequently, if the entire part collapses, the rigid body (input load) will impact the rigid wall, resulting in significant energy generated by the external work
• For the failure output, you have to change the "FAILID" for the ID of your /FAIL/CHANG card. Another output that might help you is Plastic Work, for composites this one of the most useful results: /H3D/SHELL/WPLA/PLY=ALL

Best regards,
Marina Lima