Problem deleting sketch constraints

[nbonnett-murphy]

Hello all,

In certain situations, I'm not able to delete coincident constraints in sketches. I've attached a video of a specific example, but this is a general problem that comes up in a variety of contexts on a daily basis. Both the other engineers where I work and I haven't been able to understand why this happens or how to work around it other than by deleting sketch geometry. 

This results in a ton of time consuming model rework. Let me give an example: I open a model from vault that was made in the past. For whatever reason, I need to separate 2 sketch objects to move them apart; say a circle concentric with a construction circle. Both objects have children in dozens of features downstream in the model. After trying to separate the objects for a few minutes, I finally give up and delete one of the objects, then recreate it. Because the deleted object had children, I now need to repair dozens of downstream features. This takes tons of time, and introduces a lot of potential for error. 

Hopefully I'm doing something wrong here and there's a user friendly way do deal with coincident constraints.

Video 1: I make 2 slots, with one end coincident, then try to separate them. I'm able to delete various constraints, but not separate the circles. I thought select other might differentiate between 2 points, but that is incorrect. Aside from my initial question, I'm also confused as to why there are 4 coincident constraints here. The highlighted objects don't differentiate between the first 2 and second 2 constraints.

Video 2: I try the nuclear option, deleting all objects in the sketch other than the 2 coincident arcs. I'm still unable to separate the remaining geometry.

"Display constraints on creation" is on for both videos. "Display coincident constraints in sketch" is off for both, but I repeated the exercise with it turned on and didn't see a difference. It's not clear to me what this option does.

Can someone help me understand how to de-constrain things in sketches? It will save literal hours per week.

I apologize for the wall of text, just trying to be clear because this topic leads to a ton of confusion whenever we discuss it here.

[CCarreiras · Accepted solution]

Hi!

I guess you found a bug, report it!!

[nbonnett-murphy]

Huh, that's a surprise! Is there an official channel for bug reports?

[SBix26]

I doubt that this is a bug, more of a limitation of a faulty design decision. 

When I do the same thing on my system (Inventor 2025) it seems that the center points of the two arcs are not coincident but are in fact the same point, which is not at all helpful.  They should be two distinct points that have a coincident constraint between them.  I recall encountering this a number of times in the past, and it's typically annoying but surmountable.

---

Sam B

Inventor Pro 2025.0.1 | Windows 11 Home 23H2

[johnsonshiue]

Hi! Please share the file here. A quick test to check if this is a bug. Simply copy the sketch and paste it to a new part. Try performing the same edit in the new part. Does it work?

Many thanks!

[nbonnett-murphy]

Hi @johnsonshiue,

I made a new part and did the same test. I then made a second new part, copied the sketch with 2 slots into it, and tried the same operations. I wasn't able to see any difference in any of the 3 cases. I've attached the test part since all 3 are working the same way.

[nbonnett-murphy]

---

It seems that the center points of the two arcs are not coincident but are in fact the same point, which is not at all helpful.

---

You're on to something here, one of our guys had the same thought yesterday afternoon. So maybe not a bug, but a frustrating limitation for sure.

I'm sure I've encountered the same issue with other geometry, but right now I can't find another example. I do find inventor's approach to sketch constraints frustrating in general. But the last resort of mass deleting constraints and restoring them one by one normally gets the job done. At least then I just need to rework one sketch rather than losing references and blowing up the whole tree.

[nbonnett-murphy]

I've done some more testing and managed to find a situation where it works as expected. I've been trying to reproduce it in a new file all morning, but I'm not able to figure out exactly what changes make the difference.

Here are a couple things that are different between the working and non working versions.

1. The 2 slots were made at different times. The horizontal slot was existing from yesterday. I added the vertical slot in the sketch this morning. to have an example for support.

2. The horizontal slot is used in an extrude feature. The vertical one is not.

3. There was a save, close, reboot, and reopen between the horizontal slot and adding the vertical slot in the sketch.

4. Maybe something to do with "display constraints"? Like deleting the correct combination of geometry, constraints, and dimensions simultaneously does it?

[nbonnett-murphy]

Hi Johnson,

I did some more testing and managed to find a way to reproduce both the expected behavior and the "buggy" behavior. A video is attached.

It seems to be draw order related:

It requires three objects. Two slots and a circle. If I draw circle-slot-slot, then delete out geometry, the two arcs are forever merged. If I draw slot-circle-slot, then delete geometry, the two arcs can be separated.

[nbonnett-murphy]

It was in fact a bug. Support has opened this page: https://www.autodesk.com/support/technical/article/caas/sfdcarticles/sfdcarticles/Coincident-constra...

[CCarreiras]

HI!

Well done! This will be fixed in a next update, we hope

It's missing a constraint... I believe someone forget something, since this faulty behaviour only happens between slots. (I tried it in several versions, with the same buggy result).

BTW, If you try the same workflow between a slot  and a circle, it will work well, as expected: an extra constraint appears, and you can delete it to separate the center circle from the slot arc center.