Cannot constrain or dimension reference or fixed geometry

[RRisley]

I've come across this many times now. When in an assembly, I create a sketch. I then try to project geometry and I will sometimes get this error:

"Cannot constrain or dimension reference or fixed geometry."

Any idea why I can't project edges/faces/points of certain parts?

[Anonymous]

Could you post a picture? Is it that you can't pick those edges from those parts or you can pick but the projection fails. Thanks.

shekar

[RRisley]

I can pick the edges, but the projection fails. I will post a picture when it happens again.

[RRisley]

I've attached a screenie of my most recent occurence. I'm trying to project the hole that is highlighted. This hole is hole9 just for reference. So I can't see any reason why I shouldn't be able to project it. I actually just checked and I can't project ANYTHING from the the assembly I am working in (6260-12-03-03).

Any thoughts?

[R.Corriveau]

Just to clarify. The problem you are having is with part projection when editing a part in the context of the assembly.
Not with Assembly sketches. Message was edited by: Rick Corriveau

[RRisley]

Well... I suppose in this instance I am editing a sketch in an assembly that is in an assembly. I don't know if this qualifies as cross-part projection, as the only parts I'm sketching on/projecting are in the assembly that I created the sketch in. I AM able to project from parts outside of the assembly I'm sketching in.

[R.Corriveau]

Ah I see. Assembly in an assembly editing assembly sketches.
Sorry. Looked at your browser pic and thought those were parts.
Never tried this since I don't use assembly sketches.

[RRisley]

We use them mostly for weldments or altering purchased components. But I can get the error in almost any assembly sketch, not just sketching in assemblies while in assemblies. (In case someone other than Rick reads this and wonders, since I realize Rick wasn't questioning that.)

[Anonymous]

Hi RRisley,

On looking into the code this error comes up when trying to create some kind of constraint. We check if all the geometries in the sketch are fixed. If they are then we disallow this constrain creation. I understand this is not helpful.

It is possible we are incorrectly detecting this condition and throwing an error. To verify this, could you please send me the dataset to shekar.subATautodesk.com. Thanks.

shekar

[Chassuer]

I am having the same issue. But it is only on my computer. I can go to other computers and open the same file and it lets me select the edges I need, but when I go back to my computer it says    "Cannot constrain or dimension reference or fixed geometry"

Is there a setting for this or a hot fix?

[kprom]

This bug was fixed in 2009, but has returned in 2013.  It is intermittent, but happens all the time.  It pops up when making a sketch when editing in an assembly.  When you open it seperately it works fine.  This is exteremely frustrating for those of us who edit in assemblies a lot.

[johnsonshiue]

Hi! Do you have an example exhibiting the behavior repeatedly? If yes, could you share it with me (johnson.shiue@autodesk.com)?

Thanks!

[kprom]

It's not a particular part, it just happens intermittentlly.

[DGodwin-XRG]

Old post but still happens consistently for me. At least in Inventor 2020, I'm finding that "Control+Click" while selecting edges allows me to project geometry into the sketch in order to position sketch features, whereas simply selecting the geometry like I should be able to results in this error. It makes an adaptive construction edge in my current settings, which can be cleared and locked manually if that's what you're trying to accomplish.

Hope that helps. Cheers.

[johnsonshiue]

Hi! Do you mind sharing an example that exhibits the behavior? Either the geometry is sick or the source geometry does not have the proper tag. I would like to know which is the case.

Many thanks!

[DGodwin-XRG]

@johnsonshiue 

I've attached a simple Weldment with an included skeleton part file and Frame Generator subassembly which exhibits the behavior. Screenshot with error included in the zip. Note, that I've experienced this bug in the parent assembly as well, but in this attached case I'm finding it only in the frame subassembly "Machining" area. Closing and reopening the assembly maintains the error persistently for me.

The use case is mag-drilling holes in a welded frame, trying to use the frame edges to dimension features to.

Workflow:

At the assembly level (in this case, Frame subassembly level, double-clicking on "Machining" to enter the machining operations.

Insert sketch onto frame member face, select "Project Geometry" command, click on any edge -> error appears.

Retry, but this time Control+Click the geometry and the construction line appears, and is adaptive.

Cheers

Darsey

[johnsonshiue]

Hi Darsey,

Many thanks for sharing the files and the findings! I tried it on Inventor 2020.4 on my machine. I did see the error message when the following option is unchecked.

Tools -> App Options -> Assembly -> Enable associative edge/loop geometry projection during in-place modeling

If it is checked, the error will not come up. Could you confirm?

Thanks again!

[DGodwin-XRG]

@johnsonshiue 

That's correct, if I check the "associative projections in in-place..." box it works, probably explaining why the "control+click" worked as a work-around.

Without that checked, sketching in the assembly environment still makes associative projections as needed, just not in the weldment machining environment. If possible, I'd prefer to leave in-context part editing have non-associative projections by default, which is why I leave those two associative geometry projection options unchecked. Just my preference, I understand everyone's different.

Thanks!