Problem Converting Cone To Sheet Metal Part 6

• Oct 9, 2007

1
• #2

JMirisola

Mechanical

Sep 28, 2006

2,357

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

 

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• Oct 9, 2007

1
• #3

CorBlimeyLimey

Mechanical

Nov 5, 2003

15,292

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.

 

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• Oct 9, 2007

1
• #4

ctopher

Mechanical

Jan 9, 2003

17,506

thread559-193827

http://www.sheetmetaldesign.com/Cad-SolidWorks/index.htm

Chris
SolidWorks 07 4.0/PDMWorks 07
AutoCAD 06
ctopher's home (updated 10-07-07)
ctopher's blog

 

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• Oct 10, 2007

• Thread starter
• #5

neiljones898

Automotive

Oct 1, 2007

15

Thanks to everyone for their help.

 

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• Oct 10, 2007

3
• #6

TheTick

Mechanical

Mar 5, 2003

10,194

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.

Honesty may be the best policy, but insanity is a better defense.

http://www.EsoxRepublic.com

-SolidWorks API VB programming help

 

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• Oct 10, 2007

• #7

CorBlimeyLimey

Mechanical

Nov 5, 2003

15,292

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.

 

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• Oct 10, 2007

• Thread starter
• #8

neiljones898

Automotive

Oct 1, 2007

15

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

 

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• Oct 10, 2007

• #9

CorBlimeyLimey

Mechanical

Nov 5, 2003

15,292

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).

 

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• Oct 10, 2007

• Thread starter
• #10

neiljones898

Automotive

Oct 1, 2007

15

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

 

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• Oct 10, 2007

• #11

JMirisola

Mechanical

Sep 28, 2006

2,357

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

 

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• Oct 10, 2007

• #12

CorBlimeyLimey

Mechanical

Nov 5, 2003

15,292

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.

 

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