Creating sheetmetal flatpattern with cutout made in assembly

[Anonymous]

Hi!

I want to create a flat pattern of a sheet metal-part that I've used in an assembly. In this assembly I've made cut-outs in some of the parts (see attached .png). Is it possible to get at flat pattern of the specific parts with the cutouts? I can e-mail a ZIP-file with the assembly (the file was too large too attach).

Glad for any help I can get

Running Inventor professional 2013

[JDMather]

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@Anonymous wrote:
... In this assembly I've made cut-outs

 ... Is it possible to get at flat pattern of the specific parts with the cutouts?

 ...(the file was too large too attach).

Running Inventor professional 2013

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The cut-outs should be at the part level. It appears you have a circular pattern of one part with the cut-outs at the assembly level.  You will need different parts for the ones that are cut (each unique cut).  There are a couple of ways to do this with in-context editing of parts at the assembly level.
I'm going to suggest multi-body solid modeling instead.  But a trick is needed (Derived Component) since Inventor doesn't support multi-body sheet metal parts.

Yes, if done correctly.  In this case, when are the cut-outs made in the actual manufactuing process?  In the flat or in the folded part?  I assume the flat, which means some special considerations will need to be made (to have round in folded with edges perpendicular to flat pattern).

You can dramatically reduce file size by rolling up the EOP.

Open the part file and drag the red End of Part (or End of Folded) to the top of the browser (if a sheet metal part with flat pattern - first delete the flat pattern) hiding all features in the graphics window.  Save the file with the EOP (or EOF) in this rolled up state.  Right click on the file name and select Send to Compressed (zipped) Folder.  Attach the resulting *.zip file(s) here.

[Anonymous]

JDMather,

Yes the cut outs should be made in the flat part. I'm having some trouble following your proposals but I've attached the file.

Thank you for your time

[JDMather]

There are several things done incorrectly and this one will take some time to explain (which I don't have).

If you go to the wing_test.ipt file and create the Flat Pattern

then set to Wireframe view mode, notice that the edges of the flat pattern on not perpendicular to the flat.

I would (almost) never use a Fold feature, this could have more easily have been done with a Contoured Flange, but that still wouldn't result in the correct geometry.

I think you are going to have to do this with a Thickened trimmed surface.

Extrude the surface (in the bent shape) trim and then Thicken.

It would probably be easiest to do in a single part file as surfaces.

Then Derive Component as many times as needed for each unique part.

Thicken/Offset each derived surface part..

I will try to come back to this one later if someone else doesn't jump in and provide the solution.

[Anonymous]

I understand that I may have done this part in a way that's not correct according to you but the flat pattern (without cut-outs for 1" pipes) actually works. I've tried them out in the workshop.

Even so I will try to do them your way so I can get the cut-outs to work. But I'm having a hard time understanding how it should be done (since I'm quite new to inventor and sheetmetal and I'm Swedish so my English isn't that good).

I understand that you don't have the time to explain it to me but I hope someone else will come along and help me out with a "for dummies-explanation". I will try my best until then.

Thank you!

[Anonymous]

So I think I've managed to follow your instructions and made the part with a thickened trimmed surface. But now I'm not really sure how to proceed with the derived components in a single part-file.

[JDMather · Accepted solution]

You are getting closer to solution.

I would Derive Component the Surface Body into as many part files as you have unique trimmed parts.

Add the circle sketch to trim the surface and then Thicken each unique part.

Edit:

After experimenting a bit - it looks like the easiest way would be to pattern the surface body in the part file, trim the needed surfaces then Thicken each as a New Solid and then Manage>Make Components.

[Anonymous]

Thanks JD!

I followed your instructions and now the problem is solved. Thank you so much for your time.

best regards

/Alex