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Weldment to Seperate Parts

Weldment to Seperate Parts

Weldment to Seperate Parts

(OP)
Isn't there a way to take a weldment (.sldprt) that consists of 5 bodies and make it an assembly (.sldasm) consisting of 5 components each with their respective properties that can be modified?  I tried to do this but the new individual parts features only list "save body" and has no features in the FM.

I want to design this weldment at the part level and then save each body out for manufacturing and creating an assembly.

Thanks,
BB

RE: Weldment to Seperate Parts

(OP)
Sorry, forgot the following:

SW2009, SP 4.1

RE: Weldment to Seperate Parts

Insert\Save bodies - there is an option at the bottom to create and assembly. You have to select your bodies of course before it will save as an assembly.

Regards,

Scott Baugh, CSWP pc2
www.scottjbaugh.com

Quote:

"If it's not broke, Don't fix it!"
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RE: Weldment to Seperate Parts

(OP)
Hi Scott,
I did try that before posting the question.  The problem is that the individual parts then show an external reference and the FM only shows one feature "saved-body" with an icon like a body split down the middle with a leg at opposite ends (no sketches, no extrudes, no cuts, etc.)

Thanks

RE: Weldment to Seperate Parts

BodyBagger,

Have you tried adding the features to the weldment members and then using the Relative View function to create the manufacturing views? It might simplify things for you.

RE: Weldment to Seperate Parts

Using 2008, I learned the hard way that this option does not work well! The one thing I noticed is that, make all of your parts individual structural members and don't use patterns. Patterned components don't appear in the assembly. I don't think Solidworks has realized this problem.

RE: Weldment to Seperate Parts

Can you use the weldment as the master and save each individual body as a separate part?  Then you can create your assembly from there.  You will have to be careful about your references and how you modify things, but other than saving the whole thing as dumb solid I don't see a way around this.

Dan

www.eltronresearch.com
Dan's Blog

RE: Weldment to Seperate Parts

(OP)
Hi all,
I am sure the way CBL mentioned would be better, however this is how they do things here.  They need each part of the weldment to have its own drawing, even if it is a tube just cut to length.  I thought the simplest way would be to do it as a weldment part file and then somehow save each body out as a unique part item.  However, the saved part files can not be modified as the FM does not list any features.  The references are easily broken, no problem there.  Seems like a simple thing to do, but.....

RE: Weldment to Seperate Parts

Why not make configurations and hide the bodies per each drawing sheet. You have a single part with multiple configs and you can still make changes easy.

That seems like a much easier way than anything mentioned above.

Scott Baugh, CSWP pc2
www.scottjbaugh.com

Quote:

"If it's not broke, Don't fix it!"
FAQ731-376: Eng-Tips.com Forum Policies

RE: Weldment to Seperate Parts

(OP)
Hi Scott,
I am not sure how that will flow with PDM Enterprise and the Data Card for each config.  I will look into it, thanks.

BB

RE: Weldment to Seperate Parts

I am not seeing a real problem here.

1.  Create the weldment file.
2.  Save bodies as separate parts
3.  Do your drawings of the separate part files.
4.  If you need to make a change, go back to your original weldment file and make the change.  The changes will automatically propagate to the individual files.
5.  Update your drawing to include any new dimensions.

-Dustin
Professional Engineer
Certified SolidWorks Professional
Certified COSMOSWorks Designer Specialist
Certified SolidWorks Advanced Sheet Metal Specialist
 

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