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Forums > COE Forums > CATIA V5
Subject: Part body symmetry problem

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Author Messages
jkalish

17 Sep 2008 07:01 AM

I am working in version 16 which does not allow symmetry of parts except the first part body. So what I have done is symmetry the part bodies in the part document about a plane. Problem is the draft views; it will show both sides. One thought I have is to deactivate all the mirrors (called mirror in part) throughout the specs tree but this is time consuming. Is there a way to do this via a formula, macro, etc.? Or does anyone know of a better way to handle symmetry in version 16? I know this is fixed in version 17 and beyond.

Thanks for you help

Jon
God bless America!
SKWOK

17 Sep 2008 07:19 AM
Jon,

Are you talking about the assembly symmetry function? I think that was upgraded in R17, but I haven't really used it. If you want to symmetry a single part, the best way I know of is to use CCP links.

1. Open the existing part and a new blank part.
2. Copy body from existing part
3. Window over to new part
4. With nothing selected go to Edit ==> Paste Special ==> As Result With Link
5. Apply Mirror Command (any plane will do, just be consistent)
6. Repeat 2-5 with all bodies as necessary.

This will create a new part document (that you can give a unique filename/part number to) that is a resultant of the original, and then mirrored. This is a one-way link that goes from parent (original) to child (new mirrored version). If both documents are open, the child will automatically see the update and turn red and wait for the Update All icon to be clicked. If you only open the child, you will need to right click on the "Solids" and go to the object menu and select "Load" in order to synchronize any possible changes. Alternatively you can use the desk "Load" command as well.
Steven Kwok
PLM Solutions Consultant
CATIA V5 Instructor
TechniGraphics Inc.
CATIA V5 R16/17/18/19
CATVBA
VB 6.0
Visual Basic .NET 2003/2005
jkalish

20 Sep 2008 12:24 PM

Steven,

Thanks for your response, sorry I took so long to reply, I was working on another project. However, your advice worked very well, thanks a lot.

Jon
God bless America!
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