Flat Pattern for Round Bar: How?

[Anonymous]

Hello

I'm sure there is a solution somewhere but I haven't been able to find it.

I work in Inventor 2016.

I have a multibody ipt containing 122 solids. I derived those solids into parts where the parts were needed. Then I transformed some of those parts to sheet metal and created flat patterns so I can use them for my IDWs.

One of the said parts is a very simple handle made of a round bar of metal with two bends in it. In my multibody part I swept a profile around a path by using sweep and it gave me the folded model I needed. But for the life of me I have no idea how to make a flat pattern for that part.

Do bare in mind, I am aware that it isn't possible to flatten a sweep in sheet metal. That's not the issue. I'm just wondering how to model a round bar with two bends in order to get to have a flat pattern that can be placed in an IDW. I did look at a tutorial about achieving this via normal ipt bend part, iPart creation and feature suppression. Visually that helps. But it still does not produce a real flat pattern where I can point to the bend lines like with normal sheet metal parts.

Please do not ask me for a file :). The part itself is not important. I am just wondering how to make the flat pattern.

I also thought about using tubes and pipes, but I am actually not sure if it is possible to pick round bars. (as in, not hollow). I tried defining a path and a contour in sheet metal but the contour sweep tool does not pick up a closed contour.

I mean, yes, I do realize it is called SHEET metal and a round bar is not a sheet and all that, but still... HOW do you get a real flat pattern for a bent bar? It bugs me 😛

Many thanks for your help.

BR,
Kami

[AdamAG99T · Accepted solution]

The best workaround I can think of for this would be to copy the sketch used to sweep the bar and use a contour flange with it to produce a sheet metal piece with the same dimensions as the bar. You will need to adjust your sheet metal style and bend compensations to match how the bar behaves when bent more accurately. Once you do this you can just take the flat pattern of the sheet metal piece and use that to get the bend dimensions. 

[SBix26 · Accepted solution]

Here's one workaround (Inventor 2016 format).  This involves modeling the rod as a square bar (Thickness x Thickness + .001"), then adding Thickness / 2 ul fillets to all four corners.  It will flatten, but it does have that minuscule flat on two sides which will show in drawing views.

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Sam B
Inventor Pro 2020.0.1 | Windows 7 SP1
LinkedIn

[Anonymous]

Hello

and thank you both for your replies..

@ Adam

I didn't have to copy the sketch, I just linked parameters and drew it in a new separate sheet metal part file. (This handle is part of a project I am setting up for our blacksmith apprentices and I want to make sure that, should anyone need to modify some dimensions, this handle will be altered automatically along with everything else).

But I set sheet metal thickness to be equal to my rod diameter and I set the height of the contour flange to be the same value, so I have a square bar that looks just like my handle and I can use it to create a flat pattern. For the normal bent part, I will simply use the model I made initially to properly display all roundings and such like. My IDW will thusly pull the isometric and projection views from one file and the flat pattern from another ipt file.

So this works. Thank you for the idea. I think I was thinking somewhere along these lines yesterday when I made the post but I think I was a wee bit too tired to take it all the way. 🙂

@ SBix26

I first tried your solution without the + .001 thingy because I didn't realize why you put it there. And it naturally didn't work because the fillet on the edges disabled my flat pattern. But as soon as I put in the + .001" as 0.010 mm, it worked like you mentioned.

As for the imperfection you mentioned in your post, it isn't visible on the IDW. I think that's because both bends in my rod were coplanar and I selected to set the contour flange height as thickness + 0.01 mm. Might be wrong about this. Either way, it worked.

So thank you too for a solution. 🙂

BR,

Kami

[QUI_JohnG]

I'm attempting to do this, but my bends are on two perpendicular planes (image1) i.e. bending on the thickness of a sheet metal part.

Tried combinations of folding and unfolding but the default flat pattern output is always a U-shape (image2) which makes sense considering the logic of how sheet metal behaves; but my stock material is intended to be 1" round bar. I think my solution will be to have THREE files to communicate all the information to the fabricator via an intermediate flat pattern.

I feel like this should have been obvious to me from the start, so I'm posting to save somebody else some time. (Unless there is a three-dimensional-flat-pattern-calculator hidden somewhere in the software, please let me know, it'll save me tens of minutes)