correct flat pattern 5

[Ripper2009]

Hello all,

Please find attached a sheetmetal part which I cannot get to provide a correct flat pattern. I have a feeling this is just another limitation of the sheet metal functionality in SolidWorks. If this is.... is there any way this file can be turned into development to get them to make this work. I have done parts like this in Solid Edge and the flat pattern works.

Thanks in advance!!

http://www.savefile.com/files/1049836

Thanks,

Rip


SolidWorks 2007
SP 4.0

 

[MDGroup]

Ripper,
It is my undestanding that SW can't flatten a smooth curve. It just doesn't know where to bend it. In reality you are rolling the part and therefore creating an infinite number of bends.

One possible option for creating the flat pattern is to replace the arc with several straight line segments. The more segments you use, the closer it will approximate the true curve of the part. Then SW will be able to flatten the part and create a bend at each of those segments. Obviously it isn't exactly the continuous arc that you are looking for.

One note of caution. SW will add/subtract material at each bend depending on the bend radius, mat'l thickness, etc. You should check that the length of the flat pattern is consistent with the length of the bent part. If you add a large number of bends, it may add up to a lot.

Hope this helps.

 

[msjames1]

It looks like the problem is the value you used for the bend allowance. My company uses a k-factor instead of bend allowance/deduction. When I used a k-factor for your part instead of a bend allowance, SW produced a flat pattern.

 

[SBaugh]

I assume there is a reason for you using Bend allowance, but check your help on the equation.

If I change that to K-factor and then rollback above the hole wizard feature, then add an "unfold" command (SM command) and then the piece is flat. From there I redefine your hole. Then "fold" it back up it looks fine.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"

faq731-376

 

[SBaugh]

Sorry I mis-understood what you were doing. I thought you need to fold the item down to get the hole in... but I agree the problem is in your Bend Allowance... Look at the help as it indicates how the SW will work when you use "X" option when bending SM.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"

faq731-376

 

[TheTick]

I got it to unfold, but I had to reconstruct it.

Make the model by first making a regular extrude feature, including bends. Then convert it to sheet metal using "Insert --> Sheet metal --> Bends".

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

http://www.EsoxRepublic.com

-SolidWorks API VB programming help

 

[SBaugh]

Why use Bends?

If you are going to remake it just make a line of the profile and use Base-flange. But of course that is how he did it and I think that is the best practice... its just a matter of the allowance he used.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"

faq731-376

 

[Ripper2009]

The man said....Yow...ZAA!!!

Thanks to all for the great advice.

Ripster

Thanks,

Rip


SolidWorks 2007
SP 4.0

 

[Ripper2009]

...the man said...Yow...ZAA!!!

Thanks to all for all the great advice.
later,

Ripster

Thanks,

Rip


SolidWorks 2007
SP 4.0

 

[Heckler]

When I design sheet metal parts I start with the end in mind. What I mean by this is I look at how complex the finished part with end up. Then I decide if using sheet metal specific features will make this a better part or if starting as a solid then converting. I think the best practice is understanding the sheet metal process and what method will work in the grand scheme of things (file size, & part/feature health)

Heckler
Sr. Mechanical Engineer
SWx 2007 SP 4.0 & Pro/E 2001
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_`\(,_
(_)/ (_)

This post contains no political overtones or undertones for that matter and in no way represents the poster's political agenda.