Learning Forum

[livemansleeping]

Hello, I've been attempting to design a simulation for extremely high velocity impacts against a polyethylene surface. The impact surface is, for the time being, simply a simple chunk of material with a young's modulus from relevant data.  I've been getting three different errors when running the simulation depending on the mesh scale I've been using.

[the simulation fails around cycle 2600 without any wrap-up procedure, it just stops]

[The simulation suffers a time-step error] this happens with a coarse mesh scale.

[The simulation suffers an unstructured element error] this happens with a fine mesh scale.

 

Note, when I remove the strain failure mode, and the material behaves solely via stress considerations, acting as a very brittle ceramic, the simulation will run to completion.

One potential solution that I've been informed of, is to modify the stress/strain data for the material failure properties by inputting my own stress/strain data via Isotropic Hardening.

 Is this the correct route, or would you recommend modifying some other aspect of the simulation aspect?

 

[update] I have modified the simulation such that it will erode elements on a minimum timestep of 1e-12 seconds.  This does solve the solution error (up to a 5% completion), however I then suffer an energy error at cycle 27966 seconds, and 6% completion.

The following is a copy of the ANSYS project file I am attempting to use; https://mega.nz/#!0VxT3CbA!_amE0DtO-9ZbmV5u4NARecEiWFgL91QVV9kBNJ9v_PE

[Sandeep Medikonda]

Hi,

Are you trying to use an inbuilt material model or an user-defined material model?

For energy error, please see this post which discussed it in detail.

I want to point out this discussion as well for element erosion. My assumption here is that you are using Material Failure and have also tried time step deletion criteria (which b.t.w is way too low). I would recommend you to try using an inbuilt material from the (explicit dynamics library in Engineering Data) along with the Geometric Strain Limit and see if you are able to observe a converged solution. You can always fine tune from there if it completes.

P.S: Please post such questions in the Structural Mechanics Category, this is the reason you haven't received an answer for this long. Take a moment to review the Guidelines on the Student Community (I will move it this time). Also, please use pictures to explain your problem whenever possible.

Regards,
Sandeep

[livemansleeping]

Thank you for the information, and for moving the post to the 'Structural Mechanics' category, I will keep that in mind for all future posts. I anticipated it was a pre-processing error that I was making initially, but if that's unlikely then this is definitely the correct category.

Yes, I have read that post already, the indication that the energy error increasing slowly is not necessarily a completely failed simulation run.  I would, however, find suspect an energy error that crosses the energy error cutoff when set at a factor of 10 at only 5% of the simulation completion.  The reason why I switched to using material failure on minimum time-step is due to the fact that the simulation failed on a timestep error until I did so.  If the timestep error is what I should be concentrating on, rather than the energy error, then that's something I'd like to know.

My original intention was to use material failure along the materials geometric strain limit, the stress model resulted in brittle failure, while the strain model for material failure resulted in a time-step error.  When the timestep error was sidestepped via material removal on minimum tilmestep, the simulation suffered a very serious energy-error.  

Currently I am using the Polyethylene model from the Explicit Dynamics library in Engineering Data, which I initially was observing under the conditions of a very high velocity (411 m/s) impact.  The impact speed may be what's causing the tilmestep error, which I know will be flawed if the mesh scale is too large for forces to propagate during the tilmestep.  As is, with minimum timestep removal of material, material is removed when the tilmestep value drops to E-12 seconds.

If that is the core problem, what scale of meshing would you recommend for impact velocities ranging from 0.5 km/s to 1 km/s ?

[Sandeep Medikonda]

Hi,

I will try to reach out to you tomorrow via your account manager to help debug.

Thanks,
Sandeep

[wingedr]

Hi,

I'm experiencing similar issues while conducting a high velocity impact. Was this resolved?

Thanks

[livemansleeping]

I partially resolved the issue. The problem for me was my mesh.  A default mesh will form tetrahedrons.  A tetrahedral mesh will result in a failure with divergent solutions as the forces concentrate to points of the tetrahedrons.  So you're forced to either use a very, very, small mesh, or not use tetrahedral meshing at all.  If you can get cubes, 6-sided volumes, as your mesh, the issue is likely to go away.

 

Mess with the shapes of your impact surface and your impactor until you can get cubic meshing in them, that'll cause the strain-failure to occur along stress lines in the cubic mesh.  The best way i found to do it was to use rectangular impact surface and then mesh it layer by layer to get a cubic mesh.  Then the impactor I would simply use a cartesian mesh in order to force a cubic mesh into it.  Not ideal, but it did work quite well for my purposes.