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"PartBody" and "Body"

Bert

New member
Hi. I have worked with Catia V5 since this January and I currently have been on my first project since this October.

I have a question I got from my customer today about a specification tree in general. I was asked what are the differences between a "PartBody" and a "Body." But I couldn't really answer well about it, except that a "PartBody" is unable to be deleted or added while a "Body" is able to.

Could anyone out here teach me that, or tell me if there has been any question & answers already done here in this forum?

Thank you,

Bert Tsunezawa
 
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MrCATIA

Super Moderator
I couldn't find any explanation in the Help files on this Bert, so I'll give you my best attempt at explaining the difference.

Basically, a PartBody and a Body are the same. It's where the solid-geometry based definition of the part is found.

However, there are some differences:

  1. Every CATPart file must contain a single PartBody, and it cannot be deleted, and there can never be more than one PartBody.
  2. Downstream applications (analysis, NC, etc) require the PartBody for their source geometry.
  3. The PartBody must be the first operand in a Boolean operation. (A Body can be removed from a PartBody, but a PartBody cannot be removed from a Body).
  4. Every CATPart file is created with a PartBody; users must add a Body (which can also be deleted).
  5. A Body has polarity (+ or -), which affects Boolean operations
  6. A Body can be converted into the PartBody, which causes the old PartBody to become a Body.

CATIA V5 was intended to be used where each CATPart file contained the definition (feature-based, solid geometry) of a single part which was geometrically defined in the PartBody. However, often CATPart files contain multi-body definitions of several parts (assemblies).
 
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Bert

New member
Thank you!

Thank you MrCATIA for a great reply. It was very clear to get to know about it :)

Bert
 

felixthecat

New member
hi mr. catia,

It makes sense that there is a difference between a main partbody and other bodies. My problem is to generate an ordinary body. All the objects I create from sketches are part of the partbody. When I try to perform a boolean operation it says it is not possible. I cannot select single bodies. :confused:
 

MrCATIA

Super Moderator
We use boolean operations alot where I work, so I'm not sure what is causing your problem, Felix.

What release are you using? Do you have Hybrid Design enabled?

Could you attach a screen image of your CATIA model, including a good image of the tree.
 

AFROUZ.E

New member
A Body has polarity (+ or -), which affects Boolean operations
What is the definition of a plus body or minus body?
And, is there any difference between assembling a - body to partbody and removing a + body from partbody? Well, I don't know exactly why there are the boolean operation assemble and remove.

Thanks in advance.
 

MrCATIA

Super Moderator
After reading those old posts, I'd like to add to my previous definition:

2a. The PartBody is the primary body in the part file. All other Bodies are secondary bodies.
 

MrCATIA

Super Moderator
What is the definition of a plus body or minus body?
And, is there any difference between assembling a - body to partbody and removing a + body from partbody? Well, I don't know exactly why there are the boolean operation assemble and remove.

Thanks in advance.
All Bodies have polarity; they can be a positive body (+) or a negative body (-).

The polarity is determined by the first feature in the Body. + Bodies will have a Pad or Shaft or Rib as the first feature (these features add mass to the part). - Bodies will have a Pocket or Groove or Slot as the first feature (these features remove mass from to the part).

When combining Bodies with Boolean Operations, the polarity is ignored when a Boolean Add or a Boolean Remove is used.

But when a Boolean Assemble operation is used, it looks at the polarity of the Body to determine if the Body is Added (+) or Removed (-).

As you observed, Assembling a - Body will result in the same shape as Removing the body.

Likewise, Assembling a + Body will result in the same shape as Adding a body.

This gives CATIA V5 users more flexibility and robustness. I suspect it might also allow for converting other Boolean-based solids models into CATIA V5 from other CAD systems.
 

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