Developing base part for extrusions to drive change in assemblies

[mikek3QMMC]

I'm currently looking into starting a library of our parts and extrusions, and one hurdle I came across was driving updates to models that all access the same part "base".  Here are the paths I've tried and the issues I've come across with each.

1. Derive Sketch -  Pros are I'm able to vary the length of the extrusion as driven by an external spreadsheet, and I can do so across multiple parts referencing the same base sketch.  The biggest issue I've found with this method is changing the sketch will not change the extruded piece correctly.  I would have to go into each individual part and update the extrusion selection to drive the change fully.

2. Derive Part with an exported Parameter - This one had the advantage that I could simply change the base extruded part's sketch, and all changes to the derived part would follow. The biggest Issue I found with this one was I could no longer drive the length (exported) parameter in the derived part. It was all driven from the base part, which meant if we use the extrusion in multiple places in the same assembly, I would need a base part for each instance of a part, which is effectively the same issue I had with solution 1.

3. iPart with a "variable" (blue text) parameter - This one offered the advantage of having varied part lengths that automatically updated the piece if the original iPart was changed in most ways. There were two issues I had with this. The first is every time the part was placed into an assembly, a copy of that part was made as a standalone file. This will quickly clutter the library. The second issue is if the length ever needs to change, a new part needs to be placed, which would mean re-constraining or re-placing the part in every sub assembly and possibly breaking constraints down the line in the subsequent assemblies.

Ideally, some combination of these might be used, but I'm struggling to find a "golden" solution. I want a base part that can be updated effectively only when the die is changed, that can drive this change to any instance of the child in any assembly, as automatically as possible. Those children will have different milling or lengths depending on where in the overall system they're used, and the assemblies would be driven from an overall spreadsheet. Hopefully this is making any sense.  I attached some examples of one of the extrusions as well as an assembly that would vary in height and width (extrusion would vary in length).  It is used as 3 out of the 4 sides in the assembly.  I'd like to update the profile as needed, while still letting the model drive from parameters or a linked spreadsheet.

[kacper.suchomski]

Do you want to create your frame profile?

https://youtu.be/pg6Dci9x0jY

[mikek3QMMC]

I'm still looking into this, but this might be the direction I can take. For now, it's a lot to take in as far as setting everything up. It seems like a hardy solution. How easy is it to share libraries with other users, assuming the library is initially set up on a server?

[Frederick_Law]

It might not be "easy" to update frame profile.

You'll need to test if it'll update old files.

Either way if the profile change too much, you'll lose reference in assembly.

Especially when you add or delete sketch in the profile.

Unless you create planes for constrain.

You can derive part with fixed length, say 1" on both direction.

On the derived part, project the profile on midplane and extrude it to "cover" the 1" part.

Now you have a dimension to drive length.

You can templates for different end cuts.  Holes, cutout etc.

I don't think iPart or Model State will help.

You'll have infinite possible parts which will result in a huge file very fast.

Unless you create (copy) a new one for each project.