Pattern on path distorts solidsurface bug

[meboJ7ER2]

Hello

I am working on a model that has a lot of tiny dimples (0,28 mm) made by tiny spheres that are used to cut into the surface along a path.

I get this weird distortion of the surface. The distortion is not just a rendering bug, i appers also if i export as a STL file.

I have tried the different compute options in the Patters on a path command and the bug is present in all of them, but it doesn't look the same

depending on the compute option used.

I have posted a screenshot.

Any ideas on how to fix this ?

Thanks a lot

Mikkel

[HughesTooling]

How have you made the selection, have you selected a face as the object. Try changing the selection type to feature and select the feature from the timeline.

[meboJ7ER2]

Hi Mark

Thank you for your reply.

Sorry i did not clarify this in my earlier post.

I used the  "feature" when i made the selection of the object to pattern.

Also just tried with the "faces" and i have the same bug.

Thanks

Mikkel

[HughesTooling]

If it fails using feature I think you'll have to export the design as an f3d file and attach here. I guess it's something to do with the surface making the wing as patterning a feature is normally quite reliable. Have you tried the different compute options, identical will probably be your best chance.

This is the example above but the surfaces are only curved in one direction.

[meboJ7ER2]

Hi Mark

Thank you for your reply.

I tried all the different compute options, and the problem is present in all the different options . But it seems to change a little depending on compute option.

I have attached the file.

It is the last two "pattern on path" commands on the timeline of the component called FS Wing.

Thanks a lot for your time

Mikkel

[HughesTooling · Accepted solution]

This is a meshing bug, the underlying surfaces are good. This is what it looks like in Rhino. Not anything you can do in Fusion apart from carry on and hope the display mesher is improved, if you're trying to export as a mesh you'll see the same problem. @jeff_strater can you take a look?

Mark

[meboJ7ER2]

Hi Mark

Thanks a lot for the explanation.

Is it possible to open the f3d file in rhino and then export them as a stl file from rhino ?

Thanks a lot

Mikkel

[HughesTooling · Accepted solution]

You'll need to export as stp to get it into Rhino, from there there's no problem exporting as an stl. You will need to experiment with the mesh setting a bit as there's a big difference in the sizes of the surfaces and details.

Mark

[meboJ7ER2]

Super.

Thanks a lot.

Mikkel

[HughesTooling]

@jeff_strater, @innovatenate did anyone take a look at this?

Thanks Mark

[innovatenate]

Thanks! Spherical surface can be really tricky. I see this type of thing a lot when importing/translating spherical geometry between CAD packages. This is a unique case where you're able to generate it natively in Fusion.

Most of the time if you split up a spherical surface that is doing this you'll resolve the issue. For example you could split the spherical face in half or create a small flattened end on either end of the sphere. However, in this case, my usual bag of tricks doesn't appear work. This is a really stubborn example

I also note if you change the pattern values it makes big difference. For example if you change the spacing to .75 or .875 the results are really different. I'm not sure how critical the dimensions are here but if you can change them and split the face I note that it will work. Also, I've attached a sample file that may help you to work around the issue. I suppressed the instance of the pattern that seems to generate the problem. 

If you're trying to represent rivets, could split a circular face instead of creating a spherical one? That might be another solution here. I suspect performance might be a little better as well with circular faces rather than spherical ones.

I've logged FUS-34369 for development to investigate the issue further. However, hopefully this helps move you forward.