Adding flanges to a cutout on a curved plate

[ENSO-2]

Hello

Hoping somebody can help and are up for a small challenge! 😄

I have a plate that is curved and have a cutout. on the vertical edges of the cutout i need 2 flanges, but i simply just cant get Inventor to draw it.

I tried: 

1. Making the curve with countour flange. Unfold, make a cutout, refold and try using flange feature, nothing happens. 

2.  Making the curve with countour flange. Unfold, make a cutout leaving the material i want to bend up, placing lines and fold flanges, refold = inventor crash

3. (The closest i got) Making the countour flange, unfold, make the cutout, add faces of 5 mm on both sides, add flanges, refold. but then in flat pattern the flanges dont flatten.

 

 
Hope someone can help. Thanks alot ahead! 

[CGBenner]

@ENSO-2 

Hello, and welcome to the forum!  Would it be possible to share your part file here so that others can try to work out how to do this?  Thank you!

[NigelHay]

This is trickier than it seems. I made a flat plate with a cut-out, converted to sheet metal & added the flanges. back to component & used the bend command to curve the plate. 

Prior to the band command, the flat pattern is OK but not after. I guess you could use the flat pattern with the bend supressed & the curved part for the full drawing.

[SBix26]

Dimensions would help, but the key information you omitted is the Inventor version that you're using!

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Sam B

Inventor Pro 2025 | Windows 11 Home 23H2

[SBix26]

This looks like a limitation in Inventor, but one that ought to be remedied as soon as possible!

My workaround is time-consuming and annoying, but here it is (Inventor 2025 version).

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Sam B

Inventor Pro 2025 | Windows 11 Home 23H2

[johnsonshiue · Accepted solution]

Hi! There are multiple ways to create such flanges (see the three solutions in attached file). But none of the approaches are straight forward. The issue here is that the target edges are bend edges. Inventor does not support adding flanges on bend edges or curvy edges.

The first thing  needs to happen is to create linear edge so that the flange can be created. After the linear edge is created, the flange can be created. Please take a look at the 2020 parts in the attached file (a and b require Unfold/Refold; c operates on the bend directly).

Many thanks!

[IgorMir]

Hi,

Here is the part for you to look at. IV2020 format. It is similar to what Johnson has offered but without Unfold/Refold.

Cheers,

Igor.

[chris]

@ENSO-2 The "Unfold" and "Refold" tools are your friend when dealing with something like this. If you start off with a contour flange (curved surface), you almost have to use "unfold", it just makes things so much easier, otherwise you can start off with a flat piece, add all your cuts and flanges and then fold it to your finished curve.

You can also create a solid in the finished shape you want, start your sheet metal part, derive in your solid as a "surface" and then use that surface as a profile selection for your sheet metal, lot of different ways to go about this

[CGBenner]

@ENSO-2 Did the information provided answer your question? If so, please use Accept Solution so that others may find this in the future. Thank you very much!

[ENSO-2 · Accepted solution]

Thanks for the answers everyone. It was really a big help!

@johnsonshiue  solution C, did the job as it enabled me to place the hole off center and have the flatpattern working. 

I attached an image so you can see where the part is being used.
Its an opening for a door and the bend serve as two sides of the frame.