Welcome to the Onshape forum! Ask questions and join in the discussions about everything Onshape.
First time visiting? Here are some places to start:- Looking for a certain topic? Check out the categories filter or use Search (upper right).
- Need support? Ask a question to our Community Support category.
- Please submit support tickets for bugs but you can request improvements in the Product Feedback category.
- Be respectful, on topic and if you see a problem, Flag it.
If you would like to contact our Community Manager personally, feel free to send a private message or an email.
Yet Another Non-Manifold Body Problem
daniel_crookston
Member Posts: 14 ✭
I have to be honest, when it comes to body related problems, I much prefer the three-body problem over the non-manifold body problem. In fact, I'd even take indigestion in my flimsy mortal body over this non-manifold body I'm facing.
Here's the sketch:
https://cad.onshape.com/documents/f0f23c30820895b85658b7df/w/e607ef7a168213aeb3a0417c/e/c12c3688244b226bbe5d2e83?renderMode=0&uiState=67039e25bdd5e731e0e62b2c
In case it's not rolled back to the proper point, you want "Brace Extrude", it's about halfway down the feature list. Here's some screenshots to save you a click:
The error message is "Brace Extrude did not regenerate properly: Boolean operation would result in non-manifold body." Now, I've read up on what that means and how to fix it, and I found two solutions, neither of which are acceptable:
1. Change the radius of the center circle in my very first sketch to 30mm instead of 31mm. For context, there are 13 features between that sketch and the error. I feel like this should be a huge clue as to the source of the problem but I can't figure out what it means. Like, maybe there's a problem before this extrude that I need to fix? I don't know. (I actually discovered this because the original sketch had a 30mm circle, and it only broke when I changed it to 31mm.)
2. Add an offset distance of 1mm or -1mm. This, plus the big red arc with a big red dot on that final screenshot, makes me think that the problem is in the intersection of the extruded face with that particular edge, or vertie. Vertex? The dot. But how do I fix this? In fact, is it even the problem?
And why does changing the diameter of the circle fix it??
Obviously I could just leave this extrude extending a tiny bit into the model and it will change nothing on the final print. But I don't like doing this: it's a hack and a workaround and more importantly it leaves me ignorant to the real source of the problem. Can someone help me out here please?
Best Answer
-
MDesign
Member Posts: 239 ✭✭✭
ah i see you've set the offset already to compensate.. In Loft 1, Try setting the starting end condition to None.
0
Answers
When I copied your model to inspect it shows no errors
ah i see you've set the offset already to compensate.. In Loft 1, Try setting the starting end condition to None.
That fixed it, but why?
Because when it was set to normal you were forcing the geometry to curve ever so slightly back past that end plane and when that extrusion came init would create an Very tiny area that was too complex and had a zero length to it at some point. That's my non-expert non-technical explanation. I'll post a screenshot that might help explain it. But essentially when you offset the end of the extrusion you were eliminating the need to account for that curvature in that loft surface
Here's the screenshot of the area that is the problem. Onshape kinda points you here when it highlights things that are red during shape creation. the red in this screenshoot is simply showing interferences between two parts.