Inventor Pro 2013:
Checking the 'adaptive' checkmark on the feature doesn't make the checkmark go away. The sketch doesn't give me a link to break. The 'adaptively used in assembly' option is greyed out. The feature properties doesn't give me any useful options. I've looked through my assemblies, and I don't see any that are actually using it.
What am I missing?
Solved! Go to Solution.
Solved by awatt. Go to Solution.
After Redefining the sketches, I was able to delete the work planes left over from the original assembly part. Then I was able to unshare the sketch, and finally remove the adaptivity.
Hi,
I deleted the sketch having the adaptivity but how to remove the adaptivity from part?
The part is in framework.
Kindly suggest to resolve.
If this issue happens with a hole feature, for example, there is an alternative way to fix it...
(cannot find "Adaptive" checkmark/option here? don't panic...)
First, switch the hole feature to "Linear" Placement:
Then pick any spots, just temporarily. Repeat this for all the features using the same shared Sketch.
Now right-click the Sketch (which is not being used by any features anymore), and you will see the option to remove its adaptivity:
Finally, you can restore your hole feature(s) back to using the points from your sketch:
CAD and PLM admin | My ideas | Inventor-Vault Expert GPT (my AI brain)
@pdessai if you have another issue at the part or assembly level you should post a new topic since this one has a solution.
For the part if there is any Project Geometry from another part it will remain adaptive. You would have to go into the part sketch, delete/break the reference, then you can RMB on the sketch and/or feature to turn off the adaptability.
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Kelly,
Even if you delete EVERYTHING within a sketch, it will be stuck as adaptive in the case I pointed above, until you uncheckmark Adaptivity after making the shared sketch independent of any features.
CAD and PLM admin | My ideas | Inventor-Vault Expert GPT (my AI brain)
This looks to have worked in older versions, but I have the same situation in a newer version and this workaround no longer works.
CAD and PLM admin | My ideas | Inventor-Vault Expert GPT (my AI brain)
This was in 2019.6. We are going to roll out 2023.2. I just checked 3 files. One worked in 23, two still have the same issue. With assembly adaptivity off, the one file worked even without editing the sketch, but it is an extrusion not a hole. The other two are referencing hole centers and they both still don't work with this method. Yes, this is on a different machine as well.
I would love to have a sample to tinker with. If you can attach here an almost empty assembly with just a single part and feature that alone can replicate the issue.
Oh, and you should also try a "Rebuild All".
CAD and PLM admin | My ideas | Inventor-Vault Expert GPT (my AI brain)
Hi John,
On possibility is that the adaptive part has a non-Primary Model State, right? If yes, the adaptive flag will not be available. In general, Adaptivity and non-Primary Model State are like mutually exclusive. Model State table cannot manage cross-part relationship at the moment.
Please share the failed example here. I would like to understand the behavior better.
Many thanks!