Patch Problems

[Art5]

I am working on another stamping die. The part has some wacky mounting and clearance "holes" in it that must be patched. In the patch workbench, I activate the patch command, click on the boundary, and F360 shows me a preview of the patch. Looks good enough to me for what I need. Hit 'OK', the preview disappears and an error appears, 'Compute Failed'. If F360 is able to show me a preview of the patch, how come it can't create the patch it's showing me? Hasn't it already calculated the creation of the surface to show a preview? In other CAD programs I've used it either won't show a preview of something that is going to error out, or it will give me an error before I try to create the surface. Or crash, of course.

[melisa.kaner]

Hi @Art5 ! 

Could you attach the file so I can have a go?

It could also be an idea to try out different patch types for example the 'Loft Patch'. Could you give that a go and see if that works? It could even help to create some more sketch geometry to help guide the patch.

[TrippyLighting]

Check the curvature of your edges with the Inspect->Curvature Comb.

if you are not familiar with how to interpret these then please attach a screenshot.

[Art5]

We are a prototype shop, all the designs are proprietary, so I'm afraid I cannot provide the file. If you can tell me how to copy a body into a new design, I can isolate the surfaces needed for the patch and stitch them together, then copy just that body into a new design. That I could give you.

[TrippyLighting]

Delete the timeline and then delete the parts you don't need to share.

If you can post this in this thread that would help.

[TrippyLighting]

It would also help if you keep the geometry in the file, either surfaces or sketches, which you uses]d to cut the opening.

[Art5]

[Art5]

I would be happy to do so. How do I copy the body into a new design?

[Art5]

I did not cut the opening, the customer sent me a step file with the finished part. 

[TrippyLighting]

In that case I'd only need the surfaces around the opening. Everything else can be deleted.

[Art5]

I would agree. Is there a way to put those surfaces into a new design? Or do I have to go through and delete everything else?

[Art5]

I made those surfaces into a component and was able to paste this into a new design and save it. How do I attach the file, as in, where do I find it? It doesn't appear to be on my local disk.

[TrippyLighting]

Save the design under a different file name.

Delete the timeline by clicking on the to of the browser and select "do no capture design history"

Change into the Patch (Surface) work space

Select the surfaces to keep in he viewport.

In the tool bar :

Hit the delete key.

Save the file and export it as a .f3d file.

Attach it to your next post.

[Art5]

Here ya go

[TrippyLighting]

The image above with the curvature combs already shows the problem with this geometry. I might be possible to fix this in Fusion 360 but it would take a lot of trial and error.

I've patched this using another application but due to the terrible curvature of the edges the quality of that surface is also rather terrible as shown in the curvature map below. Maybe it is enough for you to proceed, so I've attached the results of that effort as a STEP file

[jeff_strater · Accepted solution]

thanks for the design, @Art5 .  The behavior shown here is a Fusion bug.  The preview and final commit use slightly different logic to determine if the boundary is closed.  In this model (presumably because it was imported from other software), there are some tolerances at a couple of the edges that introduce small apparent gaps in the boundary under the tighter criteria.  I think the preview is correct, so the bug is in the pickier code.  There is a workaround, but it's not beautiful, but it does work:

• create a Base Feature
• do the Boundary Patch in the Base Feature
• exit the Base Feature
• stitch the surface bodies together

and, of course, listen to everything that @TrippyLighting says about surface quality - he knows what he is talking about...

screencast:

Also, this is the same problem discussed here:  modeling-error-can-t-create-patch-toolbody

[Art5]

Thanks a million for your replies and efforts. The surface you created would indeed be good enough as the hole will be cut out of the surface of the part so the patch is somewhat arbitrary, as long as the transitions are fairly smooth. Unfortunately, I can't accept this as a "solution" because having to use another application would defeat the purpose of purchasing F360 in the first place. We're currently running several different applications to take care of our CAD/CAM needs, this is why we're trying F360, since AutoDesk's claims that it can effectively do both.

[Art5 · Accepted solution]

@jeff_strater Solved this one, but once I accepted it as a solution his post vanished?

Anyways, here is a link to the other thread in which he posted a screencast to show the workaround for this bug. This workaround worked for me.

https://forums.autodesk.com/t5/fusion-360-design-validate/modeling-error-can-t-create-patch-toolbody...

[TrippyLighting]

Yes, I have noticed this many times and it is very annoying. I am in process of forward the email to @brianrepp .

[TrippyLighting]

@Art5 I only received the email last night but wanted to try out the workaround. When following the email. Kinke the post did not appear.

Your last post indicates that it actually appeared in the thread. Is that correct ?