help with sheet metal traffic cone. 1

[Dingo0z]

I draw the profile of a traffic cone & then revolve it 359 degrees. I then try to "insert bends" to convert it to sheet metal. I keep getting error messages when it tries to insert bends saying "no bends found". I've tried selecting not just the profile edge, but every edge possible & I keep getting errors. I have attached the file I'm working with.

Any help would be greatly appreciated.
Thank you for your time,
-Dan

 

[CorBlimeyLimey]

That is beyond the capability of the SW SM function.

You will have to create the cone and flange as two separate bodies, or as separate parts.

An alternative is to create a segmented (multi-facetted) cone, the flange being created by an edge flange at each segment.

 

[Dingo0z]

Thanks for the reply.
I really wasn't expecting that limitation!
So is it possible to make the cone a part & the flange a part, then mate the two together to form one flat pattern?
Also, I'm interested in your alternative but don't fully understand the process. is is possible for you to attach an example?

-Dan

 

[ctopher]

Lots of Google info.
Check out YouTube:

http://www.youtube.com/watch?v=o-aDmAYekIo

Chris
SolidWorks 10 SP4.0
ctopher's home
SolidWorks Legion

 

[CorBlimeyLimey]

Here's an image of what I was suggesting.

 

[Dingo0z]

@ctopher,
None of those cones have flanges, thats the difficulty here. Please let me know if you come across one that does.
Thanks.


@CorBlimeyLimey,
I drew two polygons & lofted them, then added an edge flange to one of the "facets". It worked great!, but the flat pattern wont unsupress. This would be very handy if the flat pattern worked. Please see example attached.
Thanks again for your help.
-Dan

 

[CorBlimeyLimey]

Edit the Edge-Flange1 feature
Change the bend angle to be flat to the ground (in this case approx 76°)
Change the Flange Position setting to Outside bend

The Flatten tool should then work.

 

[Dingo0z]

@ CorBlimeyLImey,

Got it. Thanks for all your'e help!

 

[ShaggyPE]

You can do the cone with lofted bends and circular profiles. As the others mentioned, the flange will need to be a separate part.

-Dustin
Professional Engineer
Pretty good with SolidWorks

 

[rollupswx]

Autodesk Inventor - Contour Roll.

 

[ctopher]

Dingo0z,
I know it didn't have the flange, but it's a start to learn the cone then add the flange.

Chris
SolidWorks 10 SP4.0
ctopher's home
SolidWorks Legion

 

[gwubs]

I think that this is not a true sheet metal part in the sense of developement and forming, but rather a stamped shape which involves material deformation in plane with the material.

 

[KirbyWan]

DingoOz,

Remember that the sheet metal tools are intended for bending flat metal with simple curvature, that is a linear bend, or curvature along only one direction. Complex contour where the metal is curved in two directions can never be flattened without deforming the metal and is beyond the capabilites of the sheet metal tools. As an example take a couple pieces of paper and tape them together as a traffic cone shape and try and then take scissors and cut the part to become a flat pattern. You can either cut the base off, or almost completely off leaving only a tab and slit the cone up the side or you can use CBL's trick of making radial cuts toward the cone. He gave his cone flattened sides because a true cone would require many small strips, i.e. approching infinity. By the way the first method I mentioned where you leave the base connected to the cone by a tab would not work because the material for the cone would lay on top of the material for the flange which means it could not be made from a single piece of material.

I always like to think about a flat pattern in paper. Can I really cut it so it lays flat? Think about the cuts that would be needed for a sphere to lay flat. Something like the world maps with curved triangular tabs running toward the poles, only since we are working with software that requires mathematical precision the number of curved triangular tabs would be many. This is positive complex curvature. Negative complex curature would look something like a saddle and zero complex curvature is what is really simple curvature which only bends in one direction and can be flattend without deforming the material.

-Kirby

-Kirby

Kirby Wilkerson

Remember, first define the problem, then solve it.

 

[Dingo0z]

Thanks again for the replies.
I understand now that you cannot bend a curved edge to add a flange without material deformation. So I have changed my design a little bit. What is actually being made here is a "killing cone" for poultry. The large end of the cone accepts the body and retains it while only the head protrudes from the narrow opening at the bottom. This allows easy access for decapitation without the chicken "running around with it's head cut off". It is a tried and true tool but scarcley found and difficult to nail down the exact dimensions for the breed of poultry a farmer raises. The only reason there needs to be a flange on the end of the cone is to provide a reinforced "hem" to hang it from. The photos attached to this reply illustrate what I'm trying to accomplish. Please take a look at the photos & let me know if its possible in SW. The curved edge doesn't need to be bent, but I do need to be able to add material to it as shown.
Thank you for your time,
-Dan