Sheet metal assembly not solving

[lyongoes]

Hi all,

I'm working on a simulation where sheet metal gets formed between a press and a mold. I'm interested in the plastic defomation that remains when the press gets released from the sheet metal. Unfortunately I can't get the simulation to solve properly. I'm working with:

• Nonlinear static analysis.
• Using 2 subcases for the loading and unloading phase.
• Using a nonlinear Elasto-Plastic (Bi-Linear) property for the sheet metal.
• Separation contacts between the different parts.
• 3 solids, including the sheet metal. I've read that shell elements should work better for thin parts like sheet metal, however I can't get the simulation to work at all when using shell elements.
• Symmetry along the x,z plane.

The simulation doesn't seem stable at all and sometimes solves to completion, even when it failed before with exactly the same setup. You can also tell by looking at the results that the sheet metal passes through de press and the mold, eventhough it shouldn't be able to.

I've attached the assembly with the parts below. If someone could be so kind to take a look it would be much appreciated 😁.

I'm using Inventor Professional 2020 with Inventor Nastran Version 2020.0.0.138

Kindest regards,

Lyon Goes

[John_Holtz]

Hi Lyon. Welcome to the Inventor Nastran forum.

There is a lot of things that could be improved in the setup. Here are the things that I suggest.

1. There are two updates to version Inventor Nastran 2020.0. You should update Nastran to version 2020.1 or 2020.2 to have the latest fixes.
2. Starting with a gap between parts in a static analysis is not a good idea. You should move the parts to bring them into contact initially. (The reason the gaps is not a good reason is because it take a load of 0 to move the press as a rigid body, and it is hard to converge on the load when the theoretical solution is 0.)
3. The contact for the model with solids is okay. When using the shell, you should set the master/primary contact face to be on the solid and the slave/secondary contact face to be on the shell. Set the Penetration Type to Unsymmetric Contact since  there is contact on both sides of the plate, and that cannot be handled when using symmetric contact.
4. Eventually you will want to create a finer mesh. The small diameter end of the die only have 3 elements (so 12 elements around the entire perimeter). That is a coarse approximation of the cylindrical surfaces. Likewise, the plate will require a finer mesh to handle the large strain.
5. For the Nonlinear setup, you will need more than 10 increments. Start with 50 increments and set the Intermediate Output to On. (That way, you will have results throughout the entire process to see what is happening.)
6. Is there a reason for the initial temperature in subcase 1 and the applied temperature in subcase 2? Since they are the same temperature, they should not do anything for the analysis.
7. Subcase 2 should have a load to separate the dies. An enforced motion with a vertical motion of 20 to 30 mm should be sufficient. It will fail to converge once the parts separate, but that is okay because the last converged step is the result that you want.
8. I like how you have the constraints "Slider", "Push", and "Bottom fixed" assigned to both subcases. That tells the analysis that the constraints do not change from one subcase to the next. It would be better to do the same thing for the symmetry constraints instead of applying a different "load symmetry" and "unload symmetry" constraint since they are the same setting. The solver may be trying to do something with those constraints when the subcase changes.

Another advantage of using version 2020.2 is having the explicit dynamics analysis type. Explicit dynamics will probably solve this model in 10 minutes. (However, explicit dynamics in version 2020.2 is the Tech Preview version. I do not remember if it has all the features that would be helpful or not, such as shell elements and rigid parts.)

John

[lyongoes]

Hi John,
I greatly appreciate your time and help, thank you. I updated Nastran to 2020.2, and I made sure the parts make contact from the start of the simulation. I also increased the increments to 50 now. With all these changes the simulation runs well and I get good results. However when I use a finer mesh, using a mesh control, the simulation fails to complete the first subcase at around 60%. Why would this be the case?

I would also like to analyse the radius, of the sheet metal, that remains when the sheet metal is released from the press. What would be the best way to analyse this?

I've attached the updated assembly.

Thanks,
Lyon Goes

[lyongoes]

Hi @John_Holtz,
Could you perhaps take another look at my updated assembly? It would be very appreciated.
Thanks!

[John_Holtz · Accepted solution]

Hi @lyongoes 

I made the following changes to the model, and it now runs to 47% in subcase 2 (or a load of 1.47 total). It fails at that load because that is when the press separates from the sheet, so the sheet becomes statically stable. The steps beyond 147% are not needed because nothing changes!

This is the order that I made the changes. It is hard to know if the first changes made any difference in the final solution or not.

1. Removed friction from both contacts. (Friction is harder to converge, so if it does not converge with friction=0, it will not converge with friction. And it did not converge with friction = 0.)
2. I noticed some penetration of the sheet and the part Solid2 (the stationary press). I changed the contact "Penetration Type" from "Symmetric Contact" to "Unsymmetric Contact". (I do not know if this really made any difference or not, but it should reduce the number of contact elements and make the analysis faster.)
3. Added a mesh control to the edge of the part Solid2 where it contacts the sheet.

After getting the results, I noticed the symmetry edge of the sheet is penetrating through the the edge of the stationary part Solid2. This may be related to change #2 above. It would probably be better to keep the bottom contact with symmetry contact. Also, maybe move the sheet 0.5 mm in the +X direction so that the edge of the sheet does not match the edge of the press. (Of course, this violates the symmetry condition in theory, but if the results are better than my run, it will be worth the slight inaccuracy.)

Maybe this would be better to avoid the high stress that I was seeing along the symmetry edge of the shell. Keep the bottom contact as unsymmetric contact. Move the sheet 0.5 mm in the -X direction so that the edge of the sheet extends beyond the press by 0.5 mm.

Full pressing, but deformed shape set to 0.8 so that the shell can be seen more clearly.

I will attach my model in a few minutes.

 = = = = =

I thought that you were going to change the sheet from solid to shell. Are you still planning on doing that? A solid with 1 element through the thickness is not very accurate. There is a Parameter that controls how many "layers" are used in the calculation of the shell. (NLAYERS. The default is 10.)  That would be much more accurate than the solid. However, the contact with the shell will be tricky to setup because you need contact on both sides of the shell. I would set the normal direction of the shell to be facing the bottom stationary press, use symmetric contact for the shell to bottom press contact, and use unsymmetric contact for the shell to top moving press.

Let me know what happens next.

John

[lyongoes]

Hi @john.holtz,

It's been a while. I've been working with your updated assembly and it seemed to work well. I have been able to make various iterations of the model and I'm getting close to my wanted result. However I've seem to ran into another issue where it's once again not being able to solve the simulation. As far as I can tell I've been using exactly the same parameters except for the material of the sheet metal, which I've now changed to the actual material used. I'm sorta lost at the moment.

As for your question if I will be using shell elements. I've tried to use shell elements in a very basic sheet metal press setup, but I haven't been able to get that working in a way I feel I can use in this simlation. That's why I decided to stick with solid elements.

Could you perhaps take another look at my attached assembly?

Thanks,

Lyon Goes

[John_Holtz]

Hi Lyon,

I downloaded your model and did nothing except click the run button. It runs to completion. See the attached animation.

If you are still using version 2020.0 of Nastran, you should update your software to version 2020.2 (the latest update for version 2020.)

John