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