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Stitch adds unwanted features?

23 REPLIES 23
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Message 1 of 24
grahmart
485 Views, 23 Replies

Stitch adds unwanted features?

Stitch is modifying the round shape below where the two pieces should be stitched together.  First pic shows the unstitched correct shape.  Second pic shows the only edges to be stitched highlighted green.  Third pic shows the stitched shape with unwanted added features highlighted in red.  Unstitching everything and stitching everything again causes the same, but slightly smaller, unwanted features to be added.

 

How do i stitch these together without the unwanted features being added?

 

 

Screenshot 2023-09-12 145130.png

Screenshot 2023-09-12 145141.png

Screenshot 2023-09-12 145149.png

   

   

23 REPLIES 23
Message 2 of 24
jhackney1972
in reply to: grahmart

Please attach your model.  If you do not know how to attach your Fusion 360 model follow these easy steps. Open the model in Fusion 360, select the File menu, then Export and save as a F3D or F3Z file to your hard drive. Then use the Attachments section, of a forum post, to attach it.


"If you find my answer solved your question, please select the Accept Solution icon"

John Hackney
Retired

Beyond the Drafting Board


Message 3 of 24
grahmart
in reply to: jhackney1972

Attached, thank you

Message 4 of 24
grahmart
in reply to: jhackney1972

Attached, thank you

Message 5 of 24
jhackney1972
in reply to: grahmart

You had some pretty grubby surfaces around the top of the rounded part going into the upper shape so I replaced them.  I went ahead and turned it into a solid.  You can add any fillets of refinements you desire.  Model attached.

 

By the way, I would recommend you turn on Capture Design History to make your use of Fusion 360 easier and give you a better understanding what is going on.

 

Edit: You may want to play around with the final Loft in the timeline to get different transition effects.

 

Loft Change.jpg


"If you find my answer solved your question, please select the Accept Solution icon"

John Hackney
Retired

Beyond the Drafting Board


Message 6 of 24
grahmart
in reply to: jhackney1972

Thanks for trying however the shape was there for a reason.  The software should be able to stitch these edges without modifying other edges or adding unwanted features.

Message 7 of 24
TrippyLighting
in reply to: grahmart


@grahmart wrote:

Thanks for trying however the shape was there for a reason.  The software should be able to stitch these edges without modifying other edges or adding unwanted features.


Agreed. However, the model geometry is far from ideal and not modeled properly.

That also applies to @jhackney1972's model. He should enable the "Keep tangent edges" option as it creates better geometry.

Peter Doering
Message 8 of 24
TheCADWhisperer
in reply to: grahmart


@grahmart wrote:

Thanks for trying however the shape was there for a reason. 


Examine the Attached...

TheCADWhisperer_0-1694608871585.png

TheCADWhisperer_0-1694608966439.png

 

Message 9 of 24
HughesTooling
in reply to: grahmart

@grahmart Are you going to mill this punch?

 

Won't it end up more like this?

Clipboard01.png

Mark Hughes
Owner, Hughes Tooling
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Message 10 of 24
jeff_strater
in reply to: grahmart

I believe that what you are seeing here are just graphics effects, but I have not been able to prove it.  That is, the geometry may be OK, but the graphics representation has these extra triangles in it (that is one clue, that the apparent glitches are triangle-shaped).  I hope to keep looking into this.  However, the other advice by @HughesTooling , @TheCADWhisperer ,  @TrippyLighting , @jhackney1972 are valuable, as well.  Higher quality surfaces will always result in better outcomes.

 


Jeff Strater
Engineering Director
Message 11 of 24


@jeff_strater wrote:

I believe that what you are seeing here are just graphics effects, but I have not been able to prove it. 


The geometry is flawed.

Message 12 of 24

@jeff_strater @Phil.E

Using the boundary fill feature creates a solid body without any "extra" features.

That could mean something is not quite right with the stitch feature.

I tried lowering the stitch tolerance, but that did not make any difference.

 

Peter Doering
Message 13 of 24
jeff_strater
in reply to: jeff_strater

@TheCADWhisperer is correct.  Looking at the geometry before the stitch, it is already very bad.  It is just a bit of luck that the surfaces don't get drawn differently.  Here is a view of the surface before the stitch in our modeling kernel tool.  The yellow circles indicate a "tolerant vertex".  The size of the circle indicates how big that tolerance is.  That means, the location of that vertex can be anywhere in that circle and still be considered the same surface.

Screenshot 2023-09-14 at 10.27.16 AM.png

 

after the stitch, those vertices still have the same tolerance, but are just drawn in a slightly different place in the sphere of tolerance for that vertex:

 

Screenshot 2023-09-14 at 10.29.35 AM.png

 

So, the surfaces were bad before the stitch, and they are still bad after.

 


Jeff Strater
Engineering Director
Message 14 of 24
grahmart
in reply to: jeff_strater

Thanks for the wisdom guys but bad, flawed doesn't really explain anything.  This is supplied geometry that i am trying to modify.  The yellow circled vertices are unmodified from the supplied CAD and are simply curved surfaces meeting.  What makes it bad? flawed?  How can i make it better?  If it's just bad how did TheCADWhisperer make it work in reply 8?

Message 15 of 24
jeff_strater
in reply to: grahmart

@TheCADWhisperer will have to answer how he did it.  But, my guess is that he deleted and re-created the bad surfaces (no timeline, so it is hard to tell).

 

"The yellow circled vertices are unmodified from the supplied CAD and are simply curved surfaces meeting"

That is the root of the problem.  What format of CAD design was imported here?  Some modelers are very imprecise in their geometry.  Fusion cannot repair bad geometry.  If you didn't have a problem here, you would likely have had a problem later.


Jeff Strater
Engineering Director
Message 16 of 24
grahmart
in reply to: jeff_strater

Step or X_T.  Still don't understand bad or imprecise.   Fusion 360 will highlight and measure these single points as 4.7796mm, 8.0000mm or 3.9756mm apart.   How is this bad or imprecise?

Message 17 of 24
jeff_strater
in reply to: grahmart

I understand your concern.  Unfortunately, Fusion does not expose the body checking capability which exists in the modeling kernel to the user, partly because the errors are of the form:  " CKID_COED_PCU_POS_INCONS (c234 @00000000021D34A8) pcurve location != coedge location", and trying to explain those in terms that would be meaningful to customers would be a challenge.  Measure does not indicate the problems.


Jeff Strater
Engineering Director
Message 18 of 24
grahmart
in reply to: jeff_strater

You're not really giving me anything i can work with here.  What do you suggest i do???  How i can tell bad geometry if anything reporting it as bad is hidden from the user?

Message 19 of 24
jeff_strater
in reply to: grahmart

No dispute with that.  I agree that this is a missing area in Fusion.  We should have body checking.  As to what you should do:  In this case, you should re-design these surfaces.  There are several suggestions in this thread.  In general, I guess the best we can say is:  If you see geometry exhibiting these sorts of bizarre behavior, assume that the geometry might be bad, and think about other ways to model it.  If the bad geometry was created from native Fusion operations, I would say that is a bug (though I do know operations - Boundary Patch, in particular, can sometimes generate not-so-great geometry).  But, especially if you use imported geometry, your radar should be on for bad geometry.


Jeff Strater
Engineering Director
Message 20 of 24
TheCADWhisperer
in reply to: grahmart

@grahmart 

I untrimmed the surfaces back to the generating geometry to figure out how the original designer built the geometry. 
This is not a beginner endeavor. 
I recommend that you:

1. Start over from scratch. 
2. Make sure you have Capture Design History enabled. 
3. Use the imported geometry only as reference. 
4. Ask questions early and often as you proceed. 
5. Attach your *.f3d file here (with history) with each question. 

Edit: The geometry is actually relatively simple if not trying to repair the original ( the GIGO Principle).

 

Edit 2: And get native geometry if you can (I am guessing CREO in this case, but just a guess).

 

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