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solid to sheet metal

solid to sheet metal

solid to sheet metal

(OP)
I'd like to design a part as a solid, and then seperate EACH face into sheet metal.  For easier visualization, I'll tell ya it's gonna be a motorcycle swingarm.  

I'm a bit familar with SW sheetmetal, but am getting stuck here.  I don't really have and "traditional" bends, jogs, hems, etc. etc.  I'm just going to cut (laser) each face as a seperate "part", lightly form, and then weld together all joints/edges together.  Basic hollowform construction.  Not even sure if I should be even designing in sw sheetmetal, or just an assembly!  Although I do have to flatten all curved panels to get them laser'd.  

oh, I think it will be somewhat easier because I'm planning no compound bends, just "calculatable" curves that you can rolled.  No hammering or english wheel on this one. :D

thx ahead of time, you all are always incredibly helpful.

RE: solid to sheet metal

Why not just create each part as a separate & individual piece/part from the begining?

cheers
Helpful SW websites  FAQ559-520
How to get answers to your SW questions  FAQ559-1091

RE: solid to sheet metal

crizzo,

I've done exactly what you are describing.  It's pretty easy.

1) Create solid "master" part in the shape of the completed weldment
2) Create "slave" parts by using insert->part in a new model and selecting your "master"
3) Shell your slave parts, removing the faces you don't want
4) Convert your slave parts to sheetmetal
5) Reassemble your slave parts in a new assembly to check.  Face offsets inserted before the shell can help quickly tailor the fits.

-b

RE: solid to sheet metal

(OP)
bvanhiel,

If I follow you correctly, I'll use my master part (the finished weldment) in each component part as a template of sorts.

So if I have 10 faces, I'll have 10 seperate .sldprt's, with the master in each one but shelled differently.

thanks

RE: solid to sheet metal

crizzo,

Correct.  Once you've created "slave1.sldprt" with the master and shell, you can copy it to "slave2...", etc and then just edit which faces you are removing in the shell.

-b

RE: solid to sheet metal

I was going to suggest the exact same method as bvanhiel.

Also, it seems like they added multibody functionality to the sheet metal capabilities in SolidWorks a release or two ago.  I've never tried it, and I could be completely wrong, but it might be worth looking into.

RE: solid to sheet metal

It doesn't sound like you need SW sheetmetal to do what you want.  With no bends, there's no advantage to using SW sheetmetal.  Parts can be laser cut from plain SW, IGE, parasolid, etc.

You can "convert" a part to sheet metal at almost any point in the design, as long as the part is uniform thickness and has no compound or lofted bends.  SW sheetmetal will even recognize and convert square corners to bends.

I could be the world's greatest underachiever, if I could just learn to apply myself.
http://www.EsoxRepublic.com-SolidWorks API VB programming help

RE: solid to sheet metal

TheTick,

I think some of his faces have one-directional curvature and need to be flattened.  Otherwise you could do it as a multibody.

-b

RE: solid to sheet metal

(OP)
Yes there are some curved faces that need to be flattened.  Thanks for the link to those nice examples.

It's funny there are so many nifty sheet metal tools and features, which one tends to associate with true "sheet metal" .025-.125 thicknesses and ideology.  However alot of the heavier fabrication industry uses similar principals and features in combination with welding and forming to create features.  aka shipbuilding, truck frames, containers, etc. etc.

Sure it can be done in SW (like you all have just helped me figure out), but not quite as simple as "jog, bend, rip, etc."

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