Bonded Contact Fails when run in non-linear

protontim

I have an enclosure model that has thin walls and has thin front acrylic panel (lens) that is bonded to the enclosure via a silicone gasket. The model runs fine when run as a linear simulation under the native simulator. However, due to the thin plate nature of the model I need to use the CCX non-linear simulator. However, when I choose the CCX simulator I get hundreds of the following warnings, then the simulator tries to run and then quits.

*WARNING in gentiedmpc: no tied MPC
generated for node 1025223
no corresponding master face
found; tolerance: 1.6698005414470245E-005

If I define the bonded contacts as elastic instead of TIE the simulation does not throw any warnings but starts into STEP 1 and then quits. I am running V13 beta with CCX 2.16.

Victor

If you expect all the slave nodes to be bonded to a master face, then that warning means something's wrong - perhaps they're too far apart or not well aligned such as the nodes along an edge overhanging the other panel. For shell elements, bear in mind that the bonded contact is applied to the faces of the expanded elements so their thickness affects it.

Often that warning is harmless though, such as if the slave surface is bigger than the master surface.

Otherwise, I'd try general debugging techniques like removing features or deleting half the model until it works and using lighter or ramped loads.

protontim

Hi Victor, my bonded surfaces are not the same size so, as you say, I think the warnings are not my issue. I am not using shell elements (at least not intentionally). Everything has been meshed from STEP files using Netgen. I can run the the flat plate bonded to the gasket and the opposite side of the gasket fixed - and that works fine. But when I bond the enclosure to the gasket and then fix the back of the enclosure it fails. The problem is that it just bails and does not give me any indication of what might have gone wrong.

Could I be hitting a memory limit? When I run the full model I am at about 550K elements and 1.1M nodes. I started with a half model (symmetry) but that didn't work so I stepped up to the full one to see if my boundary conditions might have been at issue. Neither work, but the half model had more detail so it was not much smaller. Does CCX have a lower max node count than the native simulator?

Victor

Yes, it could be out of memory that can make CCX just silently exit. The default CCX that comes with Mecway can't usually solve very big models, around 300,000 nodes with 16 GB RAM so 1.1 million is a lot. You should be able to do more with the MKL version, and even more if you compile it with MKL and out-of-core. Source code and compiling instructions for that are included with Mecway 13.

Thin plates with tet elements are fairly inefficient. If your geometry allows it, it might be a better idea to make the plate parts from a coarser quad-dominant surface mesh and use shells, or extrude those quads to hexes.

But I would definitely go back to the symmetry model and simplify it because even if it works, the extra time waiting for it to solve and repeating whenever something goes wrong may be much longer than that spent optimizing the model.

protontim

OK. Thanks. I have 64GB of memory, but not sure if that helps CCX or not. I will look at going back to the symmetry model and also see if I can get the MKL version up and running. Probably worth the effort to have a higher capacity non-linear simulator in the future. Thanks again for your help.

protontim

Victor, I built the MKL version of CCX and ran that version on the model with symmetry. It runs much faster and did not fail on memory limit, but it failed to converge - it exceeded the number of cutbacks. I ran the full model (no symmetry) with a simplified mount and it converged OK. So I have at least a base to go from.

As you are well aware MKL runs substantially faster (I am running 8-12 cores) and has a much greater node capacity - though it took a bit more effort that I expected to build the files. Also, I really like the addition of the space mouse control in R13!

Victor

Oh, great.

For the failure to converge, have you tried a linear analysis? That can pick up unexpected rigid body motion that's a common cause of convergence failure.

protontim

Great advice!! Ran the linear simulation and it turns out one of my bonded contacts had gotten "broken" in the process of trying to run down the other issues. That was a big help!

protontim

Well I am not out of the woods yet. When I run the symmetrical model in linear mode with CCX it fails:
*ERROR in e_c3d: nonpositive jacobian determinant in element

When I run it using the MECWAY solver, it solves, but the bonded contacts seem to be spotty at best.

protontim

In the above picture blue is bonded to purple (gasket) which is bonded to orange (Acrylic lens)which overhangs the gasket by a good bit. Looks like it only attaches at a few select points.

Sergio

For that kind of part I would suggest to use hexa elements, and have at least 2 second order element in thikness.

protontim

Hi Sergio, What is the recommended method for generating that kind of mesh? The lens and the gasket are flat parts so they should lend themselves to other meshing methods.

Sergio

Can you share the geomety? Normally what I do is split the faces in the CAD program available, then export the cad to Salome were I mesh with quads, the extude to create the hexas. Another way would be creating the elements in Mecway directly, but can be a little tricky.

Victor

When bonded contact is just hanging on by a few points, it's probably because the master and slave surfaces are the wrong way around. Here, it looks like the blue part has a finer mesh than the purple gasket, so the blue should be the slave. Similarly, the orange lens has a coarser mesh so it should be a master.

Reason is that the bonded contact is between slave nodes projected onto master faces.

JohnM

Your c3d error is likely from elements becoming distorted when they projected onto the adjacent surface. Make sure you are bonded contact pairs are closely mated. If you are using at *TIE command check the tolerance you are using between the surfaces.

For hex mesh, try meshing your step file as a surface only, quad dominant. Select the surface of one side of the plate and identify as a new component. Delete the unused part, then extrude the new component through the thickness to make solid hex elements.

protontim

I made the gasket mesh quite fine and the orange lens mesh a bit finer as well. I also made sure the coarser orange lens was the master. Now the bonds look solid in linear mode. I am currently running in non-linear without the c3d errors. Thank you all for the help.

John, you mentioned the tolerance on the TIE command. I always run 0 (automatic). Are there advantages to changing that setting?

BTW the MKL Pardiso solver is a game changer when it comes to solve times and model sizes with CCX.