Form Square Tube Using Sheet Metal Techniques

[Roasted By John]

@mike miller Racking My Brain - why you would want to bend weldments - Sheet metal bending is based on "Air Bending" with open profiles, unless it's a two step process, such as hemming etc. Now if you were to just take a square/round tube to the Brake Press and bend it without notching, you would have a different result then what was shown above. That would be almost impossible to calculate properly in a 3D program. It's amazing how far a lot of those molecules need to move in that process.

[mike miller]

@mike miller Racking My Brain - why you would want to bend weldments - Sheet metal bending is based on "Air Bending" with open profiles, unless it's a two step process, such as hemming etc. Now if you were to just take a square/round tube to the Brake Press and bend it without notching, you would have a different result then what was shown above. That would be almost impossible to calculate properly in a 3D program. It's amazing how far a lot of those molecules need to move in that process.

Nooo.......I'm not talking about machine-bending (or rolling) tube, though that would be nice too . I'm talking about this exact scenario where a tube is bent by hand after cutting out the "bird's mouth" notch. IMHO, SWX could build that feature into the weldment tool if they really wanted to. Think about an alternate end condition type instead of just overlap, underlap, and miter.

[Roasted By John]

You should be able to do what you want in sheet metal, if??? you don't completely make a full square profile, leave a gap.

[mike miller]

So I was having some fun this morning......

This is a great example of the Sheet Metal / Combine method. As a side note, I learned that Solidworks doesn't like to fold in two different directions at once, hence the two Fold features at the end of the tree. I was pleasantly surprised that it creates only one flat pattern and seems to work flawlessly in that regard.

[Tim Hoover]

I was able to get your test file to unfold by using "Convert to Sheet Metal", instead of "Base Flange/Tab".

1. Extrude your radius instead of Base Flange.

2. Combine all bodies

3. Convert to Sheet Metal, and select "Keep Body"

4. Combine, selecting sheet metal body first

5. Add fillets to replicate your angle profile.

[xmaniekx]

I was able to get your test file to unfold by using "Convert to Sheet Metal", instead of "Base Flange/Tab".

1. Extrude your radius instead of Base Flange.

2. Combine all bodies

3. Convert to Sheet Metal, and select "Keep Body"

4. Combine, selecting sheet metal body first

5. Add fillets to replicate your angle profile.

Thank you, for more complicated parts which include threads it will require additional operations, but finally it is possible to move on with the project.
I want to keep thread operations because local 3D laser has additional feature of thermal thread drilling.

[Tim Hoover]

Understood. I played around with the test a little more and I was able to get it to flatten if I created a Base-Flange that overlaps the whole weldment.

Obviously this will depend on the geometry that you have in your model, but it might be an option.

[xmaniekx]

Thank you Tim, that is even quicker method.
Right now I am facing my biggest challenge - I have one frame that will be bent in two planes. IF I could get @mike_miller's method to work, it would be simple. Unfortunately - as with previous files - I cannot unbend more than once. Using @Tim Hoover's method I would have to "bend" every corner of angle profile, and then remove them from flatten operation and replace them with straight corners, am I right?

[Tim Hoover]

Not sure if it is any faster, but I did find another option.

1. Flatten the 2 bends to make the frame flat.

2. Make a boss extrude the size of the whole frame.

3. Combine "Common".

4. Convert to Sheet Metal & Keep Body (x2)

5. Combine

[bnemec]

@matt , any chance you would like to move the more recent posts of this secondary conversation to a new thread? The original was sleeping.

I keep seeing the title "Laser cut square tube" and open it then realize it's no longer about laser cut tube.

[xmaniekx]

Thank you Tim Hoover, I have finally finished my technical drawings. Laser technician accepted my files. I hope that it will be weldable after cutting. I really appreciate your help.