Copy Body to another Part... 2

[TateJ]

Is it possible in 2006 to copy a BODY from one MULTI-BODY PART to another?
...would come in handy often enough for me.

The bestI can do is COPY/PASTE the SKETCH & recreate the BODY.

Windows XP / Logitech "Premium" Optical mouse
SolidWorks 2006 SP4.1 / SpaceBall 5000
Lava Lamp
www.Tate3d.com​

 

[SBaugh]

No a body cannot be copied from one to another... You might try split part, but that can get you into trouble if you ever change the names or if the references ever got lost.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376

 

[mmurphy50]

When we need to do this we use the "Insert-Features-Save Bodies" command. This will maintain a link to the original file. If you don't want that link you could alway export a parasolid an imoprt that to its own file.

 

[Theophilus]

Try Insert > Features > Save Bodies. You can export solid bodies to a file. Then Insert > Part to bring the part into your part file as another body.

If you need surfaces, you can copy them within the context of an assembly.

Jeff Mowry

http://www.industrialdesignhaus.com

Reason trumps all. And awe trumps reason.

 

[CorBlimeyLimey]

You could try creating a Library Feature of the features that form the body, but you may have to merge the body first.

​

Helpful SW websites faq559-520​

How to find answers ... faq559-1091​

SW2006-SP5 Basic ... No PDM​

 

[J-C]

Open the part you want to copy the body to.

Use "Insert/Part" to insert the first multibody part into the currently open part file.

It brings in all solid bodies but you can create a "delete body" feature to get rid of the others.
--------

This keeps it linked paramtrically to the original so that changes update. If you just want a dumb solid body with no link back to the original, save the part in parasolid format, then open the other part file and theres an option either in the "insert menu" or "features" that allow you to import a file.


Jason

UG NX2.02.2 on Win2000 SP3
SolidWorks 2006 SP4.0 on WinXP SP2

 

[TateJ]

These are all good ideas - I will file for future use.

Thanks...

Windows XP / Logitech "Premium" Optical mouse
SolidWorks 2006 SP4.1 / SpaceBall 5000
Lava Lamp
www.Tate3d.com​

 

[CorBlimeyLimey]

I didn't know about the Insert > Features > Save Bodies function. Handy to know.

mmurphy50 ... FYI, you don't need to export a parasolid to break association ... just RMB on the Stock Multi-Body feature and select List External Refs, then select Break All.

​

Helpful SW websites faq559-520​

How to find answers ... faq559-1091​

SW2006-SP5 Basic ... No PDM​

 

[mmurphy50]

CBL,

I do know about breaking External Refs. I find it eaiser that if someone sees the Imported body there is no question.

 

[J-C]

I don't like the break reference option cause it still seems to leave the link in there.....it just never updates again. I'm thinking that Solidworks Explorer (Pack & Go) etc...will still show the link.

Need a way in Solidworks to extract a dumb solid. Assemblies can do it with the 'Save as part" function.


Jason

UG NX2.02.2 on Win2000 SP3
SolidWorks 2006 SP4.0 on WinXP SP2

 

[rfus]

Jason,

Its called save as parasolid if you don't like the old broken ref.

RFUS

 

[J-C]

I believe I suggested that earlier in the thread as the prefered way I like to do this.

I would just like to see a way to extract and import without going through the translation. Maybe a way to "dumbify" a model and get rid of the tree. UG has a command to do this called "Remove Parameters" which allows you to select any body to delete its history and jsut leave a dumb solid. Just a few less steps.

Jason

UG NX2.02.2 on Win2000 SP3
SolidWorks 2006 SP4.0 on WinXP SP2