SHEET METAL HELP - FLAT PATTERN FAILSS TO GENERATE SIMPLE GEOMETRY

[jonathan.victor]

Hi, i have an issue with a simple model, has only 3 bends, with 1 restriction: model need to have different lengths, the smaller one on the top. As you can see below the model is a simple part, but inventor apparently can't create the flat parttern since after a bunch (seriously a lot, including unwrap) of tests of different dimensions and trying different features. I have a sketch below as a reference to my model that can have different dimensions, but a similar geometry. If anyone know anyway to get the flat pattern with the bend lines position, pretty sure that the geometry gods will recognize your wisdom. See below and attached files, currently using the bend part feature, but already used the fold and bend features in tests.

[cadman777]

The reason it won't flatten is b/c it's got doubly curved surfaces.

You may be able to fix that by modeling it differently using advanced sheetmetal modeling techniques.

I don't have time to do it for you, but CAD_Whisper (JD) is the go-to guy for this.

Provided the part thickness is uniform throughout, then you can use a combination of ContourFlange, Flange and ContourRoll. TEDCF also has an excellent tutorial on doing that in their Inventor sheetmetal tutorial. But you have to pay for that.

[jonathan.victor]

I have a similar part in the same way (Flange+contour Roll), then when trying to make a samller length on the top, flat fails, and as your said, i think that @JDMather can help with this, perhaps he appears here in the next days. Thanks for the reply.

[JDMather]

The part is not modeled correctly according to the drawing dimensions - but even if it was you would have to use Unwrap (approximation) rather than sheet metal flat pattern.

[jonathan.victor]

Thanks for the reply, the unwrap works, for aproximation, as you said, but i was looking for flat pattern containg the bend lines, they are the "parameters" we need to send to the factory, and this profile appears very often to produce by our clients, so its not pratical to draw a manual 2D Sketch in the unwraped view, helps, but don't solve.

[gmwi]

You can model this but you have to do the "bend" (under 3D model tab) at the end. This will allow you to do a flat pattern by suppressing the bend. Don't use the "fold" (under sheet metal tab) . Inventor doesn't like stretch style features and you have to work around it. I'm including the '21 ver. so you can see the process. 

[cadman777]

The fabricators I work with call this 'bending the hard way'...

[johnsonshiue]

Hi! To build on top of the solution provided by Mike, it can be done using Model States in 2022. One state has the Bend Part feature computed, which is the folded part to use. The other state has Bend Part feature suppressed, which is the flat pattern to use.

On 2021 or earlier, above approach can also be done via Derive. The downside is the additional file to manage.

Many thanks!

[IgorMir]

iPart approach can be used for this too.

Cheers,

Igor.

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@johnsonshiue wrote:

Hi! To build on top of the solution provided by Mike, it can be done using Model States in 2022. One state has the Bend Part feature computed, which is the folded part to use. The other state has Bend Part feature suppressed, which is the flat pattern to use.

On 2021 or earlier, above approach can also be done via Derive. The downside is the additional file to manage.

Many thanks!

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[IgorMir · Accepted solution]

Here is a iPart in IV2020 format.
It would be nice if the creation of FP could be suppressed in the iPart Author Table. As it is - it just gives you a message that it is failing to create the FP in a bent state. But it is not a show stopper, really,

Cheers,

Igor.

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@IgorMir wrote:

iPart approach can be used for this too.

Cheers,

Igor.

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@johnsonshiue wrote:

Hi! To build on top of the solution provided by Mike, it can be done using Model States in 2022. One state has the Bend Part feature computed, which is the folded part to use. The other state has Bend Part feature suppressed, which is the flat pattern to use.

On 2021 or earlier, above approach can also be done via Derive. The downside is the additional file to manage.

Many thanks!

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