topic Question about using Frame Generator for Handrails. in Inventor Forum

Question about using Frame Generator for Handrails.

drafter2ZT9Z4 — Thu, 16 May 2024 17:55:11 GMT

Hello, so I've been using frame generator for hand rails for awhile now and I've never had an issue with it until recently. I had to make weep holes so we could galv. the rail but after I go into the frame generated pipe part and make the holes and rebuild the assembly it ends up breaking the notches and other frame design features. Anyone know how to fix this or if there is a plug in that fixes this?

Re: Question about using Frame Generator for Handrails.

drafter2ZT9Z4 — Thu, 16 May 2024 17:56:10 GMT

Here is a sample file, it looks fine at first and I do apply the holes after the notch treatment but when I rebuild all the assembly the holes get moved in the feature browser to before and breaks the notch.

Re: Question about using Frame Generator for Handrails.

kacper.suchomski — Thu, 16 May 2024 18:20:35 GMT

It seems that manual modifications cannot interfere with automatic modeling.

Re: Question about using Frame Generator for Handrails.

BDCollett — Fri, 17 May 2024 23:26:46 GMT

I think, because you have created the cut extrusion after the notch, and referenced the notch edge. When it updates and reorders the features, it breaks the notch.

Delete the notch, create your sketch and constrain the dimensions to the origin points/plane locations. Then notch.

It will mean that in some scenarios the cuts are in the wrong location if you modify your sketch, it will need to be adjusted depending on where the origin or the part is. The notch will work though.

Another option if you want it to all update as you change your sketch is to use Adaptive. Add the cutout locations to the master sketch (102 Profile Sample), edit the Frame Member, create a sketch and then project the cutout from (102 Profile Sample). It will turn on adaptive and you can now cut it out of the part. When you change the original sketch, it will all update and move the cut outs correctly.

If you want features to only be at the assembly level, but still linked to the master. Inventor is really bad with this. You cannot link a sketch, bolted connection (don't bother). You can for whatever reason, create solids or surfaces in the master and then project edges through to an assembly level sketch and then create assembly level cuts or holes.
You can also project work features like points/axis into the assembly level and use those.
It's a bit clunky.