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Problem Converting Cone To Sheet Metal Part
6

Problem Converting Cone To Sheet Metal Part

Problem Converting Cone To Sheet Metal Part

(OP)
I create a circle and extrude with draft. I shell the cone. I create a rectangle and cut-extrude so that the cone is now split. I select insert bends from the sheet metal tool bar but I am not able to select the edge where I split the cone for the fixed face or edge in the insert bends dialog box. What am I doing wrong?

RE: Problem Converting Cone To Sheet Metal Part

Create the part using a lofted bend. Create an arc on the top plane. Offset a plane the desired distance and create another arc. Both arcs should be in separate sketches. Create the loft.

Jeff Mirisola, CSWP
http://designsmarter.typepad.com/jeffs_blog
Dell M90, Core2 Duo
4GB RAM
Nvidia 3500M

RE: Problem Converting Cone To Sheet Metal Part

Even if you were able to select a face, you would not end up with a sheet metal part which could be flattened. Flattening the conical shape would involve plastic deformation (thinning and stretching) of the material ... and that's something SW is only just beginning to handle.

To create the cone, you will need to use the Lofted Bend function. Check the Help file.

cheers

RE: Problem Converting Cone To Sheet Metal Part

(OP)
Thanks to everyone for their help.

RE: Problem Converting Cone To Sheet Metal Part

3
Respectfully, CorBlimeyLimey is wrong.  A cone is a Gaussian surface and can be flattened without deformation.  Grab a sheet of paper and see for yourself.

I just tried and was able to flatten a cone in SW.  Make the cone in a non-sheetmetal part as a revolve.  Then convert to sheetmetal using "Insert --> Sheet Metal --> Bends"  Cone can not be 360° revolve.

I prefer not to use lofted bends as I do not trust the flattening algorithm.

batHonesty may be the best policy, but insanity is a better defense.bat
http://www.EsoxRepublic.com-SolidWorks API VB programming help

RE: Problem Converting Cone To Sheet Metal Part

I stand corrected. Thank you TheTick. My memory must be going ... I've done that many times.

I was using the draft method per the OP and SW would not allow conversion to an SM part.

cheers

RE: Problem Converting Cone To Sheet Metal Part

(OP)
Can I take it that you don't need bend lines when you flatten the cone made with the revolve feature?

RE: Problem Converting Cone To Sheet Metal Part

Depends how you are going to produce the actual part ... by multiple bumps in a brake press (bend lines needed) or by rolling through tapered rolls (bend lines not needed).

cheers

RE: Problem Converting Cone To Sheet Metal Part

(OP)
Using a brake. How do I add the bend lines?

RE: Problem Converting Cone To Sheet Metal Part

They should already be there. Make sure you have sketches turned on under 'View'.

Jeff Mirisola, CSWP
http://designsmarter.typepad.com/jeffs_blog
Dell M90, Core2 Duo
4GB RAM
Nvidia 3500M

RE: Problem Converting Cone To Sheet Metal Part

A flat pattern from a revolve will only show the one central bend line with a total degree callout.

To create others for the brake, you can;
1) Sketch them manually in the flat pattern view ... evenly spaced radial lines from the converged centre every X°.
2) Create Sketch Bends on a flat sheet in the model.
3) Create the model using multi-faceted profiles in a loft, and then converting to SM.

cheers

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