Non-manifold issue.

[Mongrel_Shark]

Finally got it to work.

I took Normands good one and made a .step. ( I used Normands one because I'm more confident he didn't break stuff early in the tree )
Imported that to a new doc in fc 0.16. Made a new profile in Part Design.
Made a new helix in Part WB. then used Part WB sweep and boolean cut to get the thread.

Took all of 4 min At least now I can 3d print it to check my threads fit, then send it to the prototype lab to get some precision ones made so I can test the part that goes inside.

I would still like to get to the bottom of the fc 0.17 problems I am having. Ideally without further damage to my sanity
Overall I far prefer the 0.17 workflow, when stuffs not breaking for unclear reasons.

[Mongrel_Shark]

Facepalm!

The fc0.16 version is broken too. Its just very fine and took a bit to notice.

what is it with this shape???

Selection_044.png (199.65 KiB) Viewed 810 times

[NormandC]

I'm sorry, I've been looking at your "Broken manifold 0.4" file, and I have no idea why it breaks when mine seems to be fine.

[Mongrel_Shark]

I'm up to broken manifold 0.10 now.

As mentioned before, I'm only saving every 3rd one.

Thats approx 30 ways I have tried to make this shape that didn't work. Over 3-4 days. 6-8 hours a day. I hate to admit defeat, but this one is beating me. 30-nill

For broken manifold 0.10 I thought I would reverse some orders, so little bspt thread first, then the big custom tread. (I say custom to sound fancy, really I just plucked some numbers out of thin air, I really don’t care about this thread, as long as it screws up).

Got the revolve for the basic shape.. Made a helix, shape binder for helix, datum plane on shape binder. Tried a new sketch to avoid needing a tapered hole and to do the thread more properly.
Subtractive sweep broke the file again. tried making the pitch 1um bigger than the profile, just in case it was self intersecting.

Now I'm no expert on dependancy graphs. This is the first time I have used the feature, but this one looks a bit inverted? and forked? Backwards forked even?

Selection_045.png (32.39 KiB) Viewed 804 times

I have attached the file with the sub sweep deleted, so its under the 1mb limit. If anyone can sweep sketch 001 down shape binder I will tip my hat to them.

[NormandC]

Now I'm no expert on dependancy graphs. This is the first time I have used the feature, but this one looks a bit inverted? and forked? Backwards forked even?

It is perfectly fine. It's not forked, because at the top it culminates with a single feature, SubtractivePipe. With a fork there would be two separate branches at the top. Which is now almost impossible to accomplish in 0.17 underneath a Body. It's not inverted either, just that the graph starts from bottom to top.

I tried to change your broken manifold 0.3 settings to be the same as my working file, and yet it didn't fix it. Now I'm wondering if your extremely low tessellation value may be the culprit. Mine is set to 0.1, yours to 0.01. Could you please make this experiment: start with a completely new file, change your global tessellation settings to 0.1, then model your part. But I'll admit it's just a shot in the dark.

[NormandC]

Subtractive sweep broke the file again. tried making the pitch 1um bigger than the profile, just in case it was self intersecting.

I can't make it work either.

I wonder if the problem is with the small arcs that need to be tangent to the face of the hole being cut.

[NormandC]

I redid your file and simplified the sweep profile. The SubtractivePipe works. Check Geometry reports a valid solid.

[Mongrel_Shark]

I redid your file and simplified the sweep profile. The SubtractivePipe works. Check Geometry reports a valid solid.

Was that just a change to the profile vertical distance constraint? tip radius and everything else looks the same as a few I have tried. Loosing track of which version is broken in which way...

I can get one thread to work. either the 19mm or the 1/4 (thats not 1/4 but really half inch, did I mention my brain hurts). That much has been working for most of today at least..

Cant get both to work on the same model.

See if this Google drive link works. I broke your Good Manifold normandc2 file by putting the 19mm thread in.
I also adjusted the revolve so the 1/4 thread had a tapered hole, and ran thread all the way through, because it just looked wrong.
https://drive.google.com/open?id=1aERTz ... ZJECvsYThN

[NormandC]

Was that just a change to the profile vertical distance constraint?

As I wrote I suspected the smaller end arcs were an issue.

I can get one thread to work. either the 19mm or the 1/4 (thats not 1/4 but really half inch, did I mention my brain hurts).

The second thread you added creates a self-intersecting sweep. The height of the thread profile is equal to the helix pitch, 1.5mm. This means an edge of the sweep touches itself after each turn.

Fixing it does not fix your model though.

I started from my own good-manifold-normandc2.fcstd file and I changed it to be on par with your latest file. I copy-pasted Helix001 from your file. Recreated the shapebinder, datum plane, sketch and SubtractivePipe.

Well, mine is all good.

FC017_mongrel_shark_threaded_bushing_01.png (81.35 KiB) Viewed 767 times

good-manifold-normandc3.fcstd (1.8MB)

[NormandC]

I think I found it!

In your file good-manifold-normandc2.1.fcstd (when editing one of my files, it stops being mine; so please remove my nickname or add yours so there is no mix up), both SubtractivePipe have their Refine property set to true; but Revolution is set to false.

This means you have enabled "Automatically refine model after sketch-based operation" in Part Design preferences. I haven't.

So in your file, I changed both features' Refine property to false. Refreshed the model. Used Part CheckGeometry on the Body.

BAM! Problem gone.

I recommend to disable automatic refine when working with threads. In 0.17 you can now set the Refine property to individual features.