topic Re: Design for scaling in Inventor Forum

Design for scaling

Anonymous — Mon, 08 Aug 2016 21:02:27 GMT

I've been designing some models that ultimately end up being cut on a laser cutter and manually assembled. The reason I'm doing this in Inventor is because I can create it all in 3D space (based on the 2D pieces). I create the individual parts, then create an assembly and put them together to form the final product. Once it all works and fits together, I export all the faces individually (as DXF), nest them together onto 8x12" sheets and send to the laser cutter. So far all I've been working with is 3mm[*] material on a laser cutter. So all my pieces in Inventor get extruded by 3mm, all the notches are made specifically for that thickness.

Recently someone asked me if I can scale something to use 1/4" material instead. Well yeah sure, but I don't want to redraw everything for that thickness, although that's certainly one way to do it, but very time consuming. All the pieces will have to be scaled up and re-extruded for that thickness, all the notches and (friction) nodes redone ... a pain to say the least.

I have to believe there is an easier way to do this. Some way to draw the pieces so that if later I want to scale it up or down, I can easily to that for everything and re-export the faces to be cut. So ... is there? Is there some specific way I should be drawing these to facilitate scaling later?

* The material is really 3.18mm, which happens to be perfect for the laser's kerf. I can design at exactly 3mm and things will fit nice and tight.

Re: Design for scaling

JDMather — Mon, 08 Aug 2016 21:08:33 GMT

It sounds like you are doing uniform thickness parts.

Use Sheet Metal (even if it isn't sheet metal).

Then all you have to do is change the Thickness variable.

Re: Design for scaling

Anonymous — Mon, 08 Aug 2016 21:17:12 GMT

But it's not just the thickness that needs changing. The whole part would need to be scaled up, not only in thickness, but also overall dimensions, including the notches where the parts come together.

Re: Design for scaling

Anonymous — Mon, 08 Aug 2016 21:23:57 GMT

For example, this is one of the models that I originally purchased from MakeCNC, made modifications and completely "rebuilt" in Inventor (because their measurements weren't all exact). Each Inventor part gets imported into an assembly to put the whole model together to make sure it all fits, before I export it all for cutting. When asked to scale it, it's not only the thickness that needs scaling ... All of the notches where the pieces join together need to scale up to match the new material thickness, and each part needs to proportionally scale up in dimension as well.

Re: Design for scaling

Binga — Mon, 08 Aug 2016 21:23:43 GMT

And if you use the Direct tool?

Re: Design for scaling

Anonymous — Mon, 08 Aug 2016 21:25:26 GMT

Ok so that would be another possibility ... though also time consuming as some of the models consist of hundreds of parts. The one I'm currently working on is, at the moment, sitting at 250+ parts. I'd have to manually do each one, correct?

Re: Design for scaling

Binga — Mon, 08 Aug 2016 21:27:29 GMT

It is true if you use the direct.
I think there is a way to do it automatically using iLogic. But I don't know how to do it.

Re: Design for scaling

Anonymous — Mon, 08 Aug 2016 21:30:15 GMT

New part -> Manage -> Derive from your model, set desired scale.

Re: Design for scaling

Binga — Mon, 08 Aug 2016 21:40:41 GMT

I achieve it:

Use the Shrinkwrap in the assembly:

Use the option "Maintain each solid as a solid body":

You will get a part with each part as a solid body:

Then use the "Make Component"

Here you can change the scale of all parts:

Re: Design for scaling

Anonymous — Mon, 08 Aug 2016 21:48:54 GMT

Errr, that doesn't work (or I'm missing something). It scales the model correctly, but the individual pieces are no longer what they were. They are now merged. I can no longer select each part to export the face.

Re: Design for scaling

Binga — Mon, 08 Aug 2016 21:52:26 GMT

Set these configurations in the shrinkwrap

Re: Design for scaling

Anonymous — Mon, 08 Aug 2016 21:54:29 GMT

Actually my response was to Jacob, with the creating a new derivative part. i realized I didn't select to keep the solids separate. Once I did that, it worked as expected.

I'll try your method as well Binga and see which one works best.

Re: Design for scaling

Binga — Mon, 08 Aug 2016 21:54:30 GMT

Could you share some "innocent" assembly?

Re: Design for scaling

Binga — Mon, 08 Aug 2016 21:58:57 GMT

The way he made it is simpler.

Re: Design for scaling

Anonymous — Mon, 08 Aug 2016 22:10:21 GMT

I keep finding little gems like these and I have the community to thank for those. I honestly don't know if there is a different, or better solution, but for now, Jacob's solution appears to do the job. I need to try some cut pieces and see how well it comes together, but on the surface it seems to be what I need.

Now I need to figure out how I can export all faces (as DXF) in one fell swoop, rather than having to pick each and every part, one by one, and exporting them. Then figure out if there's a better way to next all the pieces than manually doing so .... ah the joys.

Thanks all!

Re: Design for scaling

Anonymous — Mon, 08 Aug 2016 22:13:42 GMT

For scaling I use derive. If I need to scale and remove certain features or greatly reduce file size for load time etc, I'd use shrinkwrap.

Re: Design for scaling

Anonymous — Mon, 08 Aug 2016 22:16:22 GMT

Right, I can see the advantages of using either of those. In my case, it's a simple case of needing to scale the parts, then re-export for cutting.

Re: Design for scaling

jeremy_wasserstrass — Mon, 08 Aug 2016 23:09:49 GMT

I would draw the model up as a multibody solid and export the parts. Then to scale it you derive the multibody into a new part keeping all the solid bodies separate. This would have the advantage of having only one scaling operation for the whole assembly.

As Jacob said use derive, however I would derive the whole assembly at once, set the scale, relabel the solids, then export the new parts and make the dxf files.

Attached is a 2015 example of the process. One thing the part test1.iam should have been n-part test.iam to make things easier to follow.