Scaling sheet metal parts with rips/holes (to produce flat pattern)

[Anonymous]

Hello forum,

I have been using Inventor to create 3D models of sheet metal animals that we weld to make yard art.  I have an animal that I want to scale down from the original to make a "baby" animal. My 3D model contains 40+ solids with an assortment of holes and rips that enable me to flatten the flanges so they can be cut. All this is fine and I love using Inventor for this purpose.

The problem that I am now having is that I want to scale my part that contains the solids with rips/holes.  I have tried scaling the original in three ways:

1. Using Direct Edit to scale everything

2. Scaling when I create the sheet metal component for the assembly

3. Deriving the part with a scale factor

In doing each of these, I have the problem that the scaled part cannot be flattened. In scenario 1, I see that the rip and hole in the assembly have not been scaled.

Is there a way to do this? I would hate to have to redo all rips/holes after scaling as there are MANY of them.

I am including a zip file containing a simple example with a lofted flange with a rip that I cannot scale successfully to create the flat patterns.

Thanks for your time.

Elaine

[johnsonshiue · Accepted solution]

Hi Elaine,

Direct Edit specifically ignore holes to avoid manufacturing error. What you could do is to derive the part or body as a separate part. Then change scale factory in Derive dialog.

Many thanks!

[Anonymous]

Hello Johnson,

I did try deriving one part only with a scale factor and it didn't seem to work for me.

Are there specific settings/options I must use for the derivation to work so that the holes/rips are included to scale?

Elaine

[JDMather · Accepted solution]

You must also consider the sheet metal Thickness.

When you scale the part are you also scaling the Thickness?

[JDMather · Accepted solution]

[Anonymous]

That did the trick!  I was not scaling the thickness. I can now flatten it.

Thank you both for your help.

Elaine

[JDMather]

Ah, but are you going to make the babies out of thinner material or out of the same thickness material?

[Anonymous]

Well actually, it will be cut from the same thickness material.  I tried deriving with a thinner thickness in my real model and I still could not get it to unfold. Argh!  

I think what I will end up doing is scaling the larger already flattened sheet metal pieces (.dxf).  I would have liked to have done it all in Inventor, but it doesn't seem possible.

I definitely do not want to have to re-rip and re-hole my "mini" model.

Thanks,

Elaine

[johnsonshiue]

Hi! You don't need to remodel the whole thing. In the scaled model, you can simply use the following workflow to get the correct thickness.

Options A:

1) In the source sheet metal part, double-click on a face in one side so all faces are selected, including the tangentially connected ones.

2) Thicken/Offset -> output = surface -> distance = 0.

3) In the derive part, edit Derive feature -> exclude the solid but include the surface.

4) Thicken the scaled surface to desirable thickness.

Option B:

1) Open the derive part.

2) Double-click on a face in one side so all faces are selected.

3) Thicken/Offset -> output = surface -> distance = 0.

4) 3D Model -> Edit -> Delete Face -> Lump selection -> select the solid body.

5) Thicken -> Quilt -> pick the offset surface -> distance = Thickness.

Many thanks!