converting a part to sheet metal and unfolding

[DominicGreco]

I have a very simple solid that consists of a lofted solid that was the "hollowed" out via the Shell command

The sketches used to make this lofted solid were two dimensionally similar rectangles. One has radiused corners while the other does not. These rectangles exist on 2 separate planes that are 10" apart. This part (Shroud1.ipt) is supposed to represent a shroud that will be installed between the intake and exhaust of an air filter.

I wanted to convert this to a sheet metal part and then unfold it so I could see what the flat pattern looked like. However, when I attempt to use the "Unfold" command it fails. Similarly, the Flat Pattern command fails as well.

What do I need to do to get this into a flat? I'd rather not redraw this as a sheet metal part. I'm not that familiar with that environment.

[JDMather]

Use Sheet Metal tools to create the part.

Lofted Flange and Rip.

Attached was created in student version - so examine and then delete.

BTW - Shell is almost never the correct tool for sheet metal.

[jletcher]

Well I can't open part done in 2013 I have 2012.

But what you could do is drop an email to SPI for inventor send it to them tell them you are looking into the software and would like a sample unfolded so you can see if the software does what you need.

They did have a upload option on their site not sure if they still do but this software can unfold almost anything.

[JDMather]

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@Anonymous wrote:

I'd rather not redraw this as a sheet metal part. I'm not that familiar with that environment.

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Apparently you are not very familiar with the Loft command either as the mapped points make an ugly part (in my opinion).
I seriously doubt this is what you wanted.

Time to get familiar with sheet metal environment - it is easy.

My part - your part.  Notice the transitions.

There are two different methods using Lofted Flange - Die Formed and Press Brake Formed.  Try both and use the one that will actually be used to manufacture the part.

[DominicGreco]

You are correct, I am not that familiar with the "loft" command in Inventor. I recently switched from Solid Edge to Inventor and just finished the simple tutorial on the Loft Command. Perhaps I should revisit this design.

This part is actually not made from metal. It is knife cut from Neoprene coated Nylon fabric. I just wanted to try to get a flat pattern to see how the flattened part would look.

[JDMather · Accepted solution]

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@Anonymous wrote:

II am not that familiar with the "loft" command in Inventor.

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Did you open my example  attached above to see how to do it with sheet metal?  (doesn't matter that the material isn't metal other than for the bend allowance which you can set to nuetral for your part)

In your example Inventor incorrectly mapped the points for the Loft.

Sometimes it does this.  (usually when the number of points in one profile sketch don't match the number in second sketch  - in this case you need two points in one sketch mapping to one point in second sketch in each corner)

You can take control of the Loft point mapping yourself by turning off Automatic mapping.

[DominicGreco]

Taking your advise I went and made a Sheet Metal part and then used the Lofted Flange command to make the appropriate transition. After that i added  "Rip". Needless to say it worked and gave me the flat pattern I was looking for. Thank you!

[jletcher]

It will look like this unfolded.

[JDMather]

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@Anonymous wrote:

It will look like this unfolded.

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...or this.  Given the material I would use Die Formed in the Contoured Flange.

[jletcher]

Yep that too.....

[Yijiang.Cai]

Hi,

Please see two attached parts for two ideas on the workflow you would like to have. One is using the part loft feature then create flat pattern, the other is using sheet metal lofted flange feature, which should be the most comvenient idea to accomplish this.

These parts are created on R2012.