Repeatable bug: Joints connect to wrong points after dimension change

[Bjanders]

I'm modeling a lathe quick change tool holder:

Two of the holes for the set screws are mirrored from the other two. I created joints between the four set screws and the holes, and everything is fine. If go back and change the width of the dovetail:

say, from 42 to 44 mm, then the two set screws in the mirrored holes jump to the second hole:

There is now one set screw in the first hole, and three in the second. (I kind of would have better understood if it was 2+2 due to the mirroring. Edit: No, it's because 3 and 4 are copies of 2, so the joint is kind of lost, and the screws don't reposition. Yes, I ensured I am at the end of the edit history.) 

This is fully repeatable. I also tried closing the design and reopening and the error repeats. Surely this must be a bug? This is on an M2 Pro Mac.

Model is attached.

[TrippyLighting]

I can reproduce the behavior and it looks like a bud to me. Tagging @Phil.E ...

[Phil.E]

The bug is in the compute. It has nothing to do with the dimension change, other than the dimension change forces a compute.

Open the design attached, compute all. You'll see the joint features get confused.

Now, delete the mirror feature. Create the 4 holes using 4 hole points, all at once. The mirror, you will find, is the culprit.

Things like this are why I tell my students that mirroring is to be avoided. It's easier to work without mirrored holes in this case, but this is just my opinion. I reserve mirroring to more complex operations where the benefit is only more model geometry (faces/bodies), but never for complex parametric relationships like threads/joints. Give it a try, see if mirroring the holes is actually more work.

Is this file older? Or is it created very recently?

[Bjanders]

Thanks for the tip. I almost always use mirroring when I can, as I find that natural and fast. But then again, I haven't been aware of this anomaly, so I guess I'll avoid it in the future. Disregarding the bug, I think mirroring, even in this simple case, is less work: It's clicking mirror, the two features and the mirror plane, as opposed to setting up a mirror constraint in the sketch (this already is the same amount of work) and then creating the hole features.

Also, if I later choose to change some aspect of the feature, then it would automatically be mirrored. This is even more prominent when the feature is actually mirrored in itself (as opposed to a symmetric hole).  Yes, I know of lot of that can be achieved by parametric design (which is a good practice anyway), but for many things I think mirroring keeps the design simpler and easier to maintain. And that again is, of course, just my personal opinion. 🙂

I created the file the same day I reported the issue, so very recently.

[davebYYPCU]

First I have heard that, “avoid mirror” outside of sketching.

Most regulars in here decry expensive sketching in favour of symmetry and mirrors.

Two way symmetry, we draw 1/4 then two mirrors, strongly recommended.

@Bjanders Surprised you want left handed threads / bolts.

I would insert one and pattern the bolts, then rigid group.

Might help….

[Phil.E]

It's just a personal preference of mine, nothing to do with bugs or even which CAD application I'm using. 25 years of using CAD has created some habits I don't try to change.

Thanks for the info, I'll log a bug report using your model. If you can easily repeat the bug, please let me know. I tried a simple version of your workflow and it was stable, and bug free. So there might be something subtle I'm missing. It helps to provide the file (thanks!) and it also helps to figure out what particular step pushes it into error-territory, if you have time. It may not be required in this case.

(ref: FUS-144759)

[Bjanders]

I just tried to repeat it with a completely new slightly simplified model, and the issue repeats. I didn't yet bother to figure exactly which step is causing it.

What I did:

• Create a rectangular profile with a small rectangular cutout (the dovetail in the original). 
  
  • The cutout width has a symmetry constraint
• Place two dots in the sketch
• Constrain everything
• Extrude the profile
• Create two threaded holes where the dots are (in one operation)
• Mirror the hole feature in the previous step
• Import a screw from McMaster-Carr
• Make a joint between the bottom of the screw and top of the hole. Offset the joint/screw downwards.
• Copy the screw and make a joint in the second hole
• Copy the second screw and make a joint in the third hole
• Copy the second screw and make a joint in the fourth hole
• Edit the width of the cutout in the sketch
• The joint is lost

Attached is my test part. Not much different from the original, but a tad simpler.

[Bjanders]

Where can I find advice like "avoid mirror outside of sketching"? I have many times been wondering what is the best practice of at which step to do mirroring and patterning. My own reasoning has been to do it as late as possible, as I feel that is less work and makes changes easier. For example, if I make a pattern of 10 x 10 in a sketch and then make some feature for that pattern, then I have to repeat that feature 100 times, instead of first making the feature once and then patterning it 10 x 10.

If you look at the design, everything is correctly threaded despite the mirroring. It doesn't mirror the threads, it mirrors the hole feature, which doesn't invert the threading. Why would it?  And the bolts are copies, not mirrored. I appreciate all advice from those with more experience than me, and I'm always looking to improve, but I feel you were a little fast on the trigger. 😉

How would you pattern the spacing of the M8 bolts in the sketch:

Edit: On second thought, please don't reply. This is getting off-topic discussing how to design, instead of discussing the bug. Let's keep this thread reserved for the joint bug so that it doesn't get cluttered with two discussions.

[Phil.E]

I still cannot repeat the bug. Also, if I edit your model, by deleting the second pair of screws, and then copy/paste > joint them into place there is no bug found. At this point I need a video to see what particular click is causing the trouble.

Just curious, have you tried "duplicate with joints"? I know you are interested in efficiency, and it's way more efficient than copy/paste> joint.

[Bjanders]

Here. I join the first screw, then copy, paste #2, join #2, paste #3, join #3, paste #4, join #4. (I messed up a little when recording). At the end I press "Compute all", and the screws jump back.

Joining screws

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Thanks for the tip about duplicate with joints! I was not aware of this at all. I'll have a look at it.

[Phil.E]

Okay, I can repeat the issue now.

FYI, mirroring the threaded holes produces left handed threads.

Workaround: mirror the sketch points, not the hole features.

[Bjanders]

I verified by looking at my model before being a smart ass. They all look right (threaded) to me:

I'm surprised that it changes the properties of the features. Doesn't seem logical to me. What other properties does it invert? 😉 I'll have to admit I was wrong then, but it seems contradictory by looking at the model. 

[Phil.E]

Mirroring creates a mirror of geometry, not a copy. We have requests to avoid mirroring threads, but those are not implemented.

"What other properties does it invert?" Mirroring inverts all face/body geometry.

I go back to my original thoughts: I only mirror things that require a right and left side, not a right and right side. It keeps me out of trouble. Just my opinion. 

[davebYYPCU]

You are asking for LH threads with a mirror command, you are supposed to get them.

Select modelled option for the threads, then activate a section view to compare both types.  Non modelled is a graphic representation, so who knows what you get, but Phil has them labelled as expected.

Copy, paste, joint, offsets, or Pattern first one and Rigid Group, I know what I would do.

I would not expect to see recommendations for sketch mirror over modelling mirror.  Rules are meant to be broken, and as Phil said it a personal preference.  

Might help….

[Phil.E]

I only suggested sketch mirror because points are not left/right handed, so it just works. And the OP wants to use mirror. There are lots of paths 'round the houses' for the desired end result here.

[Bjanders]

But why are all the threads right handed in my screenshot, are they not? They are identical. The two holes are mirrored.

Edit: From another angle. All are clearly right handed:

[Bjanders]

I don't think we'll get anywhere with this discussion, so it is pointless to argue, but my personal opinion is that I find it illogical and strange, that of all these properties it changes one when you mirror the feature. I would not expect a mirror of a feature to change an object property.  And why doesn't it do it my model, if it is supposed to do it?

Yes, I would expect it to mirror geometry (edges and vertices), but I don't think the threading, when you mirror the feature (not the model of the hole) , that the threading would change. If I manually modeled the threading out of a helix, then I would expect the threading to change.

[Phil.E]

There is no argument. There is only the result that Fusion is giving, whether it is what you are expecting or not. At the end of the day, if you are happy with the model, then you are happy.

The threads being not mirrored might be another bug. (ref: FUS-145172) I'm told that manufacture space sees the threads as RH/LH, as well as drawings. The model shows all threads as RH.

If you want to never make a drawing of this part, you'll be fine. The drawing note will call out the mirrored threads, while apparently the model doesn't show the mirrored thread geometry.