creating a symmetry 1

[alkemixt]

hi,

How can i create a symmetry of a part that has 100 part bodies, and I don't want to creat a symmetry of 100 part bodies..is there a way to create a symmetry of the CatPart without creating symmetries of individual part bodies in a part? perhaps in an assembly?
except, the symmetry function in the assembly work bench only allows you to create symmetry of the first part body.

thanks in advance.

 

[Akesson]

Add all 100 part bodies into one new (using boolean operations) and create the symmetry on your new body.

 

[flangewiper]

You could open a New Product, insert the Part into the Product and then use the Create CATPart from Product command which is in the Tools drop down menu in Assembly Design. This also give the option to merge all Bodies into one single body.

 

[DBezaire]

alkemixt - I am assuming these part bodies are in 1 CATPart file. These are some of the reasons to work in an assembly structure, but that doesn't help you now. What Akesson suggests will work until the solids make contact with each other. You could create an new Geometric set, turn datum on, extract with point continuity and pick a face on each partbody. Create a new Geometric set and mirror the results. If you change a solid the mirror should change as well.

Regards,
Derek

 

[DBezaire]

What licensing is required for Assembly -- Insert -- Symmetry? I run with MD2, HD2, YYZ/CCV/MTD lincensing.
I can follow the example in the manual with respect to the rotation and translation of the door/wheel assembly. If I try to use the symmetry option I get the error of
Door.1 Symmetric product not created or initialized
Pane.1 Symmetric product not created or initialized
I find it hard to believe that big bad Catia cannot handle a -1 to geometry!

Derek

 

[catiajim]

An MD2 should be sufficient.

One thing to look for in Tools --> Options --> Infrastructur --> Part Infrastructure, is the option "Only create links to Published Elements". This option will result in a failure of the Assembly Symmetry, as CATIA is trying to create linked copies of each of your parts, but the solids probably are not published. You can either publish your solids, or turn this option off, and it should work.

 

[DBezaire]

Jim - as always, you are the superstar. I do publish my elements, why the keep link option in the symmetry menu did not register. I will never know.
Thanks again

Regards,
Derek

 

[catiajim]

I just spoke from the voice of experience. I fought that one for a week - normally I use VPM, and the Assembly Symmetry doesn't work there at all.