Hole tool fails if adaptive reference sketch is deleted & recreated

[gcross]

The hole tool will not let me complete the holes if I delete the cross part references & re-create them again.

Note that I had to change some adaptive hole locations to follow a part that was moved & I couldn't get adaptivity turned on for all components involved (adaptivity grayed out on actual part to change). Not sure why I could turn adaptivity back on. So I opted to just recreate the cross part hole references in the parts hole sketch.

I find I have to now delete the holes completely & start over which causes extra work in IDW & IPN files downstream.

Is this as planned or am I doing something wrong. This used to be easy in 2012.

Gary

[jletcher · Accepted solution]

This is one of the reasons I do not use that feature project geometry. Plus it makes a mess with adaptive assemblies.

If I was you put the hole in then make the feature adaptive using center mate to move the hole in location at the assembly rather than projecting geometry.

[gcross]

Jletcher,



It is difficult to use contraints between the features since I much prefer
the more fool proof way to control the location of the parts in asy using
origin planes. Putting in mate constraints is a little less fool proof.



I still say this didn't happen as much in 2012.



Gary

[jletcher · Accepted solution]

I am not telling you to constrain the part with the holes.

I am telling you to use adaptive feature to move the hole in the part to the location in the assembly.

Your way will fail 99% of the time my way will fail 1%. Projected geometry worked in the early days but now that they changed the way it works it fails 99% of the time. I don't use it any longer because of the fail rate.

Yes you are correct in some manner with using the planes I do it .

And no it does the same thing in 2012. If you delete the projection Inventor thinks of it as a new hole even if you used the same feature and just reconnected it to the new projected geometry.

 put the holes in the part with no dimensions using center point make the feature adaptive save close go into the assembly make part adaptive using mate center pick the adaptive hole (do one at a time) then pick the hole in the assembly and it will move to that location.

This is the best way no fail..

Also the more projected geometry you have the slower your system will be. And I do mean slow. Watch the time when you start constraining things as you and projected geometry.

What you have to know is every time you place a part and start to constrain it Inventor will look at every projected geometry before it snaps into place to make sure it did not move.

If you have one not so bad you add 100 then you will see a slow down like you would not believe. And even if they are in subs you slow down.

Just saying...

I have an assembly over 260,000 parts and I can spin it like it was 1 and I did it back in Inventor 6 with 4 gigs of memory. I could not male a drawing of the whole assembly.

[gcross]

James,

I really appreciate the thorough reply.

I am going to try to avoid the projected geometry from now on when ever possible & avoid the hassles I've been experiencing.

Gary