Is it possible to unfold a square tube drawing?

[tomHKD9J]

Hello, 

I am working on a seat base that I am building. I have drawn the base and extruded it, hollowed it to represent the material as well as added the appropriate chamfers. I have placed slices where they need to be and am trying to unfold the drawing so I can have the box tubing laser cut. I have tried converting it to sheet metal which it will let me do and then select unfold and it won't let me select the bends. Is there a way to do this? Thanks in advance. File is included.

[TheCADWhisperer]

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@tomHKD9J wrote:

I have drawn the base and extruded it, hollowed it to represent the material as well as added the appropriate chamfers.

I am not at my Fusion machine to check your file.
My guess is that your material is not uniform thickness.

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I would expect to see Fillets rather than Chamfers.

I would expect the Shell to occur after the Fillets (make sure edges are perp to the flat).

[tomHKD9J]

My apologies on the terminology..I did use fillets not chamfer and the material thickness is the same, all of the hallow was done at the same time in one step.

[TheCADWhisperer]

OK, I opened your file and see numerous unresolved issues highlighted in your Timeline.

Surprisingly (or not) I notice that your Sketch1 is not fully defined.

This is going to take some work... ...let me dig deeper.

Oh, and incorrect corners...

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@tomHKD9J wrote:

....and the material thickness is the same, 

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Ahhhhh, material is not uniform thickness???

This can be seen visually, I do not even need to measure...

I think you are going down the wrong road with this anyhow.

Do you have a piece of this material from the shop floor - can you grab a piece and photo the end profile?

[davebYYPCU]

I am not a SM guy, so leave it to the Whisperer - who knows.

I saw this and ... you know the rest

[jhackney1972]

Each tube must be unfolder by itself, you cannot unfold a complete frame that you had showing.  I isolated one Cross Brace and when through the steps to make it a sheet metal body able to unfold it.  Activate the component and start with the added fillet in the timeline.  Model is attached.

[ritste20]

I wouldn't mind seeing how this bend (as modeled) is made in real life.

I agree there is a better approach from the beginning.

Regards,

[TheCADWhisperer]

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@ritste20 wrote:

I wouldn't mind seeing how this bend (as modeled) is made in real life.

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Yep.  Going down the wrong road.

Once I was able to open the file - it became obvious where the OP was intending to go.

[TheCADWhisperer]

@jhackney1972 

I suspect this does not match the true Design Intent.

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@tomHKD9J wrote:

...so I can have the box tubing laser cut.

[TheCADWhisperer]

I've got an idea - I wish I had thought of this at the beginning.

Let's go back to the beginning and let me rephrase my first response.

I'll wager $1,000 that your material thickness is not uniform.

Now, going back in time, would you take that wager without double, triple, quadruple checking your geometry?

🤔

That's the ticket, I finally figured out a way to afford to retire...

[davebYYPCU · Accepted solution]

As far as I got with it, folds back up, but subsequent operations prevent it's unfolding at later stages. (Fillets and cutting...)

Might help....

[tomHKD9J]

Thank you again for your input. Though it is not what I am after it certainly is a good lesson I can use in the future for some other projects I need to get on paper. I apologize for the incorrect terms, I am still very new to this product and designing in a 3D atmosphere. I had very little formal CAD training some 30 years ago on CadKey. Since then I have been drawing with an old copy of Visio so my limitations have always been drawing in 2D. I appreciate your help and the way you present things, it works well for me and I will continue to learn this process. I have had this software for a little over a month and feel I am a quick study with it once I get my thought process wrapped around how to design utilizing this and get into more complex shapes.

[tomHKD9J]

This is what I am after, knowing it can be done answers my main question. Now to figure out how you did it. I can see from the other comments that I used the shell tool at the wrong point in the timeline and now understand what they mean by varying material thickness. I will go back and work it over some more and see if I can get the final results I am after. Thank you again for your response. I am hoping someone will chime in and explain what it is that you did exactly to accomplish that. I see you used a flat piece to create the bend then folded it and later added the rest of the tubing. Mr Hackney does an excellent job with his voice over and brief tutorial.

[davebYYPCU]

Short story, 

make the outside wall of the frame, I used surface Extrude and Thicken.

convert that to SM body, and Unfold it.

Go to solid area to work on it.

I sketched the mitres by measuring the original body.

The trick is using the K factor dimension for the base of the vee.

Made the other 3 walls as thin wall Extrude new body, cut the mitres and notches, joined the SM body to the frame cut pieces with Combine join, then

Refolded all into place.

I tried adding fillets and any new refold would not work, for me, but.....

you only need to step left of the Refold icon in the timeline to see the steps taken.

Might help....