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"Rolled" Sheet metal part

13 REPLIES 13
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Message 1 of 14
mshannon2003
955 Views, 13 Replies

"Rolled" Sheet metal part

I'm a novice Inventor 2012 user trying to draw some sheet metal parts for use in our plant.  I've been able to create most of the parts I need except for one.  I have a triangular-shaped piece of sheet metal that needs to be rolled so that it has a specific radius.  This part will in turn be attached perpendicular to another piece of sheet metal with the same radius.  I've messed about with the contour flange, but that only seems to work with open sketches.  Can anyone please help with this one?  I've been reading similar needs on this forum for the last couple days, but cannot find anything that I can get to work.  I've included an attachment to help the explanation.

 

Thanks in advance!

13 REPLIES 13
Message 2 of 14
CCarreiras
in reply to: mshannon2003

Hi!

 

I can't help, because i don't understand what you need to achieve, post a drawing, or something that help us to understand.

 

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Regards.
CCarreiras
Message 3 of 14
CCarreiras
in reply to: mshannon2003

HI!

 

Is this what you need?

 

Did you find this reply helpful ? If so, use the  Mark Solutions!  Accept as Solution or Give Kudos!Kudos - Thank you!

 

Clipboard02.jpg



Regards.
CCarreiras
Message 4 of 14
mrattray
in reply to: mshannon2003

I thought I understood the issue, until I looked at your attachment. Can you post something that shows what you want it to look like?
Mike (not Matt) Rattray

Message 5 of 14
mshannon2003
in reply to: CCarreiras

CarlosC.  That appears to be it.  Can you explain how you created the drawing?  I know the radius of mine needs to be 17.50625 (calculated).  The triangular piece is 12.5 inches long by 2.75 inches tall and the arc has a 48 inch radius.

 

Thanks,

 

MichaelS

Message 6 of 14
CCarreiras
in reply to: mshannon2003

Hi!

 

Let's go...

 

First draw a arc with the radius=17.50625 and lenght:12.5. Full constrain the sketch with constrains and dimensions.1.png

 

 

 

Apply "Contour flange" With 2.75in

 

2.png

 

 

 Be aware about the side of the thickness grow...



Regards.
CCarreiras
Message 7 of 14
CCarreiras
in reply to: mshannon2003

Unfold the part, select one plane in the edge and one curvature face:3.png

 

now the part is flat, cut the square too achieve the triangle: make a sketch in the flat face and use "Cut" tool to create your triangle:

 

4.png



Regards.
CCarreiras
Message 8 of 14
CCarreiras
in reply to: mshannon2003

Now it's flatten and cuted, lets refold the part:

 

In browser, hover the cursor above Unfold, right mouse button and select "Refold"

 

5.png

 

And that's it!!! easy ;)!!!

 

6.png

 

 

Good luck!!!

 

Did you find this reply helpful ? If so, use the  Mark Solutions!  Accept as Solution or Give Kudos!Kudos - Thank you!

 



Regards.
CCarreiras
Message 9 of 14
mshannon2003
in reply to: CCarreiras

Exactly what I needed, CarlosC!  Let me say that your method was a lot easier than anything I had thought to try in the last couple days!  One last thing...I've tried to create a drawing file of this part.  I would like to show it unfolded where I can dimension it flat for the person making the part as well as folded.  When inserting the "Base" part there is a Sheet Metal View option where the default is set to "Folded Model".  There is also an option for "Flat Pattern" that is greyed out.  Am I doing something wrong where it is hiding that option?

 

MichaelS

Message 10 of 14
CCarreiras
in reply to: mshannon2003

Hi!

 

You have to perform a flat pattern in 3D before you document it in the drawing.:

 

Open again the 3D Part and perform the flat pattern, save and go again to the drawing, now the flat pattern isn't grey out.

 

 



Regards.
CCarreiras
Message 11 of 14
mshannon2003
in reply to: CCarreiras

Got it!  I was confusing the unfold and flatten pattern commands.  Works great and I can even add the flattened and original curved parts into the same drawing.  Thanks for all the help with this one!

 

 

Message 12 of 14
mshannon2003
in reply to: CCarreiras

CarlosC. I'm new to the forum. Can I accept the whole thread as a solution as I think it all goes together? Please let me know as I consider my questions resolved at this point.
Message 13 of 14
CCarreiras
in reply to: mshannon2003

Hi!

 

You can have only one "accept as solution", so if some post solve your problem you can accept it as solution, maybe chose the first of the tutorial post.

 

Kudos, you can post where you learn something good, it's up to you.

 



Regards.
CCarreiras
Message 14 of 14
mrattray
in reply to: CCarreiras

You can mark as many replies as you would like as the solution.
Mike (not Matt) Rattray

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