Splitting a part solid

[skashyap]

Hi All,

Is there any way to split one solid part into different pieces with known references?

If there is no inbuilt functionality, any workaround will be helpful.

Thanks,

Srikanth

[rrich-2]

Copy part to another name.  Cut away the part you do not want. 

or

Make a family table.  Add a cut to get rid of half of the part.  Put that feature in the table and turn it on or off.  Make a second cut to get rid of the other side and put that feature in the table.

[skashyap]

Thanks alot Ron,

I had another concern, What if user selects the references dynamically to cut the part?

Through family table it might be difficult to handle if references are not fixed I suppose.

[rrich-2]

In the family table the two cuts you would use could both use the edges of a curve that is an earlier feature.  Then one of the cuts you flip the arrow outside, and the other inside.  This way they are both tied to the same geometry.  Name the curve Splitline or something like that, you could lock the dimensions of the curve so that no one could easily change it.

[BenLoosli]

Creo does not support multiple solid bodies in the same part file, so you are limited on how you can do what you want.

[sjuraj]

If you need split it only for appearance reasons this is very nice trick https://www.youtube.com/watch?v=WKQs5ODeP70

If you need 2 separate bodies you will have to do it in assembly mode with 2 parts. You can modify parts in assembly and get references from other models.

[cgorni · Accepted solution]

To close this community thread on Splitting a part solid

Summary of the exchanges and list of solutions proposed:

• Copy part to another name.  Cut away the part you do not want in both parts.
• Make a Family Table and control the visibility of 2 cuts, splitting the geometry, by adding them into columns. Switch on/off the features in different instances.
• Use Quilts to divide the model:
  • Copy the solid surfaces and use the Trim, Warp and Solidify commands to get different entities or patches to select, as highlighted in article CS20578 or in this video.
• In Creo Parametric 7.0 and later this operation can be performed directly using the Multibody capabilities, like the Split Body one