Surface Patch Failure. Help!

[huczekdesign]

Any idea why this surface patch won't complete? Seems pretty straightforward to me, but for whatever reason Fusion can't compute it. It's a small offset from my tool body and I'd like to patch it to use as a cutting tool.

Thanks!

 

[TrippyLighting]

Esport your design as a .f3d file and attach it to a post. We can then inspect it and provide feedback.

[huczekdesign]

Sure thing. Here you go. Don't judge my design tree 😂

[jhackney1972]

I did not see a surface to patch but the general shape is the try like cutout so I created a surface of this cutout.  It is Body 16 in the model.  Model is attached.

[TrippyLighting]

It looks to me that the offset surface command you used to create the surface body, somehow creates geometry that resists being patched for no obvious reason. 

Although you've found a workaround (I can easily find another two or three), I'd love to have this behavior explained or even fixed. @Phil.E 

[huczekdesign]

Thanks and I agree.

In the file I uploaded here I was able to create a work around by splitting the surface offset in half and then creating a mid plane patch which I could then I patch the top and knit and mirror, but I would definitely be curious to know why it wouldn't patch the entire top surface as one single piece.

[Phil.E]

There is no surface/patch body to test.

[laughingcreek]

roll the time line back to the point trippy shows in post 5

[Phil.E]

Thanks, I see it now. Logged as FUS-138299.

[SaeedHamza · Accepted solution]

@huczekdesign 

It's not a bug, if you zoom in really close to the region shown in the video, you would notice that the patches are not of the same height

[laughingcreek]

@huczekdesign - the failure of this patch can be traced to this point on the model-

if you zoom in a bit you will see there are 2 vertices nearly on top of each other here-

the edge segment between them is really small. 

In certain cases,  fusion often has trouble with really small things like this.  it's been explained before on the forum as to why but I don't remember the specifics. but basicly - math.  In the same way it has problems with really small angles and near tangency conditions.

this occurred when the surface was offset.  so tracing this back to sketch 7, we see these 2 lines aren't parallel, but rather have a very small angle between them-

so I put a horizontal constraint on it-

which broke the fillet at 5mm, but setting it to 4.9mm allowed the fillet to work.  I didn't investigate this.

so with the sketch fixed and the fillet fixed, the patch applied with out any error.  see attach model.

moral of the story-properly constrain your sketches.

I would get away from relying on using the fixed constraint.

I wouldn't convert a mesh to a brep, but rather use it as a visual reference only and draw everything from scratch.  

[laughingcreek]

another suggestion-

instead of extruding with a taper in  "extrude 4", and then doing all that jazz to rebuild the sides that are suppose to not have a tapper, extrude it straight, and use the draft tool just on the sides you want to have a tapper.  that's what it's there for.  and helps the very real possibility of introducing more errors caused by using such a convoluted process. 

[TrippyLighting]

I don't usually rely on viewport visuals, but you are correct.

The height difference between the two edges is 0.00042016 mm!

Fun fact: That is 238 times smaller than Fusion 360's default stitch tolerance.

So I went back in the timeline - something I should have done more thoroughly - and see inappropriate modeling techniques. Sketches that are not properly dimensioned and constrained, and one bad hack of a workflow to correct the slant created by the extrusion with a draft angle.

Very good catch!

[huczekdesign]

Thanks everyone!

Yes this was very much a "sketch" so to speak throughout haha.Next time I will make sure to properly constrain everything like I normally would. Thanks again for everyone's attention to detail here 🙂