Cant create flat pattern of certain part.

[magn168a]

Hello

I have created this part for a workshop crane, as a part of some reverse engineering. I have no problem in modeling the part and converting it to sheet metal. But when i want to unfold it, nothing happens. The flat pattern is created, but the model remains the same. I seem to have read somewhere, that inventor cant create flat patterns of parts that is "scewed". Does anyone have a solution? So that i can create 2D drawing for manufacturing.

The important parts are the two flanges with mounting holes. The part as it is now, fits the rest of the model perfect.

Is there another way of approching the problem, but with the same result+flat pattern?

[aurel_e]

There are few issues with your model:
1. Is not made using sheet metal features
2. The sheet metal thickness is 0.5mm; your intention appears to be 3mm
3. The thickness is not constant (<3mm in the long section)
4. No bends

See the model attached (Inventor 2026) for indication how to work in this case.

[magn168a]

You are correct. The part was not made with sheet metal features, because i dont know how to do it. I only have the start and end point of where the part needs to be attatched. I dont know how to make the bends in the correct dimensions. And the "scewed" part only makes it more difficult to calculate.

Recreating the part with sheet metal features may be my problem. 

[aurel_e]

Ok, but you need to start learning it if you are expecting to be involved on designing sheet metal.
There are plenty of videos online.
For your part see the video attached.
As you can see, you can play with the sketch dimensions to achieve your "correct dimensions"

[magn168a]

Hi again

The things shown in the video, are already in my toolbox of things i know. My problem is that the two mounting surfaces, are not parallel to each other. Otherwise a contour flange would be an easy solution. There are 10 degrees between the two surfaces. In other words, not parallel to each other.

[kacper.suchomski]

Use Unwrap tool.

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@magn168a wrote:

The things shown in the video, are already in my toolbox of things i know.

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This, however, doesn't exempt you from the need to follow sheet metal design principles.
You claim to know them, but you don't apply them.

[magn168a]

I would use the sheet metal design principles, if they where able to do what i am trying to do. That part attatched is just an representation of what i want to do in sheet metal. Its hard to show the part i want to model in sheet metal, when i cant figure out how to do it 🙂

I will look into Unwrap. I am guessing that using unwrap, wont make me able to add bend lines etc in a 2D drawing? It will just create a flat surface?

[kacper.suchomski]

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@magn168a wrote:

I would use the sheet metal design principles, if they where able to do what i am trying to do. That part attatched is just an representation of what i want to do in sheet metal. Its hard to show the part i want to model in sheet metal, when i cant figure out how to do it 🙂

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The basic rule is that everything that can be done using sheet metal commands should be done using sheet metal commands. Other commands are used only for elements of part that cannot be modeled using sheet metal commands. 

Meanwhile, as @aurel_e pointed out - you used Extrude instead of Face; you did not keep the thickness constant; you did not set the thickness correctly.

Knowing and not applying it is like not knowing, so don't be surprised that other Internet users assume your ignorance.

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@magn168a wrote:

I am guessing that using unwrap, wont make me able to add bend lines etc in a 2D drawing? It will just create a flat surface?

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It all depends on how well you prepare the model.

[SBix26 · Accepted solution]

I managed to create the part so that it produces a flat pattern in Inventor sheet metal.  I created the two end faces (using the Face tool...), then connected them using two 3D splines.  The splines are constrained sufficiently to be pretty close to parallel.  I lofted a surface between them, then thickened it.

I am not able to paste an image into this message (is this a new "feature"?), so it is attached below.

The attached part file is 2024 format.

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Sam B

Inventor Pro 2026.2.1 | Windows 11 Home 25H2

[magn168a]

That is very very cool. And to be honest, way more complex than i can comprehend. I will try to analyse how it is all connected. 

As for now, this is a solution that works, besides it doesnt fit my model when putting it together with the other parts. But i am guessing that this can be resolved by editing measurement 🙂

Thank you very much!

[johnsonshiue]

Hi! There are multiple ways to create the bracket. Here is a solution using Sheet Metal commands. The trick is to find a plane where the connection will be based off. Then create a Face feature as a separate solid body. Use Corner Seam to create the miters. Lastly, use Bend command to join the piece back to the Sheet Metal body.

Many thanks!

[magn168a]

Hi

Thank you very much for your solution. I have looked at the part that you attatched. I am not able to create a flat pattern on the part. Which was my main goal 🙂 For fabrication purpose.

[johnsonshiue]

Hi! Sorry! I forgot to recreate the Flat Pattern. Please delete the FP and recreate it, since it was based on the body before the Bends. Please take a look at the attached part.

Many thanks!