Simulations, meshing errors

[mcramblet]

I have 3 tray models that I'm running simulations on. All three ran perfectly fine in the first simulation, no issues at all, meshing was fine. Using those same 3 models, in a different "saved as" file, I'm attempting to run another simulation and keep getting meshing errors. The first of the three models still meshes ok, but the other two refuse to mesh. Settings on all of the simulations has been the same, default settings, including the mesh settings. I'm confused why the same models would mesh fine before and now won't seem to mesh at all. The error says there is intersecting geometry, but there isn't.

This model and simulation worked as expected: https://a360.co/2v36PXG

This same model in a different simulation refuses to mesh for me: https://a360.co/2uZcxd5

Any help would be appreciated.

-Michael

[John_Holtz]

Hi Michael ( @mcramblet )

Keep in mind that the same part in a different model is a different model, so the default mesh is different. In this case, I think the larger volume of the new model results in a larger default mesh size, and that default size is probably too large for the thin-wall geometry of the tray. With a large mesh size, the inside mesh can "poke" through the outside mesh around the corners, and it is the mesh (not the solid geometry) that is being reported as the "intersecting geometry". 

1. Mesh intersects due to the large mesh size. 2. Mesh does not intersect.

I set the mesh size to 0.1 inch, and it was able to generate the mesh. (I did it the easy way and change the mesh size for the entire model. It would be better to use the "Manage > Local Mesh Control" and mesh the tray at that mesh size, and leave the other flat solids at a coarser mesh size.)

Let us know if there is a problem after trying a smaller mesh size.

[mcramblet]

@John_Holtz : Thanks for the info. I'll be getting back to this, shortly, and will let you know if I have any issues.

[mcramblet]

@John_Holtz -

I was using the default mesh settings in Fusion, which was this:

When you used a specific number or size, were you doing so here?:

or some place else?

[John_Holtz]

Hi,

Yes, I used the "Absolute Size" setting.

[mcramblet]

@John_Holtz 

I'm able to get the meshing to work and the simulations to run. I've been leaving the mesh defaults in place and just dropping the mesh value on the tray (locally) until the mesh works without a failure, then apply the same local value to all of the other tray versions. Seems to be fine and I'll remember this for future simulations. Thanks for the response and the help!

[mcramblet]

@John_Holtz -

I've run into some snags. I haven't had any meshing errors and the simulations that I've run have all completed successfully. The results of the simulations, though, aren't matching or aligning to real world examples or what we'd expect, when looking at formed features that should strengthen the models. I've run all sorts of configurations and various loads, but the tray that should be the weakest in reality is showing the strongest in the results. After all sorts of digging around, I've discovered that the tray that should be the weakest is the only one that doesn't have a warning in the Solver data. All of the other models have this is the solver data:

Warning: TET ELEMENT 19575 HAS SINGULAR GEOMETRY
Cause : The specified element is not valid or is highly irregular. The following will result :
- The element stiffness matrix will not be valid.
- The global stiffness matrix may be singular.
- The solution may not be valid.
Action : Check the element connectivity and grid point coordinates.If the element is a bar or beam
with pin flags specified, check that the pin flags are valid.

Some models have one of these warnings, some have multiple.

So it looks as though all of the models that should be "stronger" are not showing accurate results due to these warnings. Shouldn't this issue cause the simulation to fail, rather than lead one to think that, by all outward appearances, the simulation was completed successfully?

I've searched for information regarding this warning, but I'm not coming up with much in regards to how I can fix or remedy these warnings.

This model/simulation completed and doesn't have a warning: https://a360.co/2Pfevz5

This model/simulation completed but has multiple warnings: https://a360.co/2v7JPqm

Any ideas on what I might be able to do to address these warnings that appear to be throwing off the results?

[mcramblet]

Is there anyone else from Autodesk that can jump in on this conversation/issue?

[John_Holtz]

Hi @mcramblet 

I have not had a chance to look at the newer models that you posted, but the original model was a very thin part. It may not be possible to get accurate answers with a solid model and mesh; a shell mesh would be better, but Fusion does not have that capability.

If the solid mesh can give accurate answers, it will require a very fine mesh. That will also help to avoid the singularity warnings that are occurring because of the distorted elements.

I would also suggested turning off the option "Create Curved Mesh Elements" that is located on the Mesh settings dialog ("Manage > Settings > Mesh > Advanced Settings".) The curved elements can create distorted elements when the size of the element is larger than the size of the geometry.

[mcramblet]

@John_Holtz -

I will play around with the settings, as suggested, and see if I can eliminate the warnings.

Thanks.

[John_Holtz]

I think the model and its complex curvatures are forcing the mesh to create some poorly shaped elements.

If the screencast video gets inserted, it shows a few areas where very small features will be forcing very small element edges on some sides of the element. Then based on the element size, the other edges of the elements (extending into the volume) will be large, and this results is a high "long to short" aspect ratio. This is one type of distorted element.

The first face highlighted in the screencast has a narrow, sharp point in one corner. This type of geometry forces a triangle with a sharp corner (small angle between two sides) which is another type of distorted element.

I am not a Fusion modeling expert (really just a novice), so I do not know whether there are tools to eliminate some of the rounds to simplify the geometry, or whether it would be better to create the model from scratch and only build-in the rounds that are fundamental to the design (which may be all of them, but in some cases it is better to get results on a model that approximates the design than it is to get no results on a model that accurately described the shape).

A sample analysis just completed on my computer using a mesh size of 0.05 and turning the "curved elements" off. I am surprised that there were only 2 warnings. There were only 416,000 elements, so going with a slightly finer mesh may eliminate the warnings entirely. (I had suppressed the 3 bodies used to apply loads, so those would add a few more elements to the total analysis, plus the elements used in the contact. But why not split the tray model to apply the loads and constraints instead of adding more bodies and using contact to load and constrain the model?)

Edit. Where oh where did my little screencast video go? (Maybe try this link if the video does not get imbedded.  https://knowledge.autodesk.com/community/screencast/f2112edf-909e-47db-87fd-03bc0306ec24 I may have forgotten to click the "Insert" button to actually insert the video )

Screencast will be displayed here after you click Post.

f2112edf-909e-47db-87fd-03bc0306ec24