adaptive geometry

[alevy]

I design a lot of complexed presses. I project geometry from parts of assemblies to parts of other assemblies. Eventually it stops me and says it failed because the part with the sketch I am projecting geometry to is addpative in amother assembly. I have broken the links, removed all of the adaptive geometry and it still fails. Anyone know how to fix the problem or a good work around?

[tsreagan]

I run into this a lot when creating parts in place.  I am not sure why,  so I now create a blank part, save it, and place it in the assembly, constraining the origins and then ground it.  Then I edit the part in place.

This may or may not be related,  do you create parts within the assembly with the "create" button?

T.S.

[alevy]

I do create parts in the assemblies using the create button. Not sure what the problem is but it creates a lot of problems for me.

[tsreagan]

Try my method above,  it should solve the probelm for now,  untill someone chimes in with a solution.

T.S.

[karthur1]

When you are creating a part in place and you project geometry, it will automatically make it Adaptive (cause that is what it "thinks" you want).

If you dont want it to be adaptive, hold the shift key down when you project it and it will not be adaptive. (but it wont change if the assembly changes either).

Notice when you project and hold down shift, the projected geometry will be black, not purple/pink.

[tsreagan]

karthur1,

Lets say you created a part in place, and it is initially adaptive,  but then you sever the adaptivity later, should this not break the connections to the assebmly?   I even removed adaptivity at the sketch level in these instances.

Yet, I would still get the evil "Geometry is adaptive in another assembly." message when working on these parts.

 just as alevy is reporting.

I don't know if this is a bug or not.

T.S.

[karthur1 · Accepted solution]

After you have the (adaptive) part modeled, all that you have to do to make it non-adaptive is uncheck the adaptivity on the parts context menu from the assembly browser.  To keep that message from coming up, clear this box.

This is not a bug.... it is by design.

This is under Tools>Document Settings, Modeling Tab.

Kirk

 

[tsreagan]

Thanks karthur1

I'm soo happy,  I learned something new 🙂

I did not know that option behaved seperate from the right click adaptivity settings.

It does grey out if you remove adaptivity with a right click on the part/sketch.

and it returns if you re-enable adaptivity with a right click on the part/sketch.

i think its the fact that it is on by default before you create any sketches that threw me off.

Now I can create parts in place agian.

thanks,

T.S.

[alevy]

Thank you, for the help that saves me a lot of time.

[karthur1]

T.S.

Just noticed you said that you constrain the parts to the origin and then ground.  You might already know of this, but there is a tool for that?

On the assembly tab, productivity panel. Pick the part, then this button... bam, done.

If you dont see it, the Assembly Bonus Tools has to be loaded.

http://forums.autodesk.com/t5/Autodesk-Inventor/Inventor-2013-Assembly-Bonus-Tools/m-p/3573748/highl...

[alevy]

I have not used the productivity tools. Thank you for the information, I will try this and see how it works with the assemblies.

[tsreagan]

Yeah,  I need to get in the habit of using that.

T.S.

[alevy]

I am in Inventor 2014 and when I go to the tools document settings and uncheck the adaptive box it no longer fixes the problem. I even tried holding down the shift key and I still get the famous message adaptive in another assembly. This is making my job painful.