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BodyPart and Geometrical Set

Monstrobolaxa

New member
I was given a set of files, CATPart and CATProducts.

Opening each part they don't have BodyPart only Geometrical Set.

First what is the difference?

Second question is: how do I work on these and change them? (as I'd like to alter a few things).

Third does anyone have a link for a tutorial that might help me out a bit?

All my previous work has been with BodyPart...so I'm kind of lost!

Thank you.
 

MrCATIA

Super Moderator
PartBodies contain the solid definition of a part.

Geometric Sets contain the wireframe and surface geometry - the construction geometry that is used to help define the solid

Sounds like you may have some files that were converted with IGES; IGES data typically ends up as surfaces in CATIA V5.

You might be able to create a solid in the PartBody from the surfaces:

1. Take a close look at the part file and make sure you have a complete model with all the surfaces.

2. In the GSD workbench, use the Join command to connect all the surfaces together into a single envelope of the part. You might have to adjust the gap tolerance to do this.

3. Back in the Part Design workbench, use CLOSESURFACE to convert the Join into a solid.

4. Hide the Geometric Set to see only the solid in the PartBody

The solid will not have any history, but you will be able to work with it. And hopefully make the changes you want.
 
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Monstrobolaxa

New member
Doing step 3 an error message shows up:
"The current In Work object isn't in a Body"

Can you help me out?
Thank you once again!
 

spinner962

New member
"Define In Work Object"

Hi!
I´ll try to help you: If you try to right-click on your current body and choose "Define In Work Object"
Does that help you to do what you wanted?

Regards, Fredrik
 

MrCATIA

Super Moderator
Doing step 3 an error message shows up:
"The current In Work object isn't in a Body"

Can you help me out?
Thank you once again!
That's just a little warning message, and it shouldn't stop you from continuing on.

Fredrik provided the tip to avoid the message.
 

Monstrobolaxa

New member
Hello!
And thanks for the help a few months ago!
It's been a while...and only now I've come back to the geometric parts...to bodypart conversion!
I am still having problems with the 3rd step...
I've tried the "Define in Work Object" and then doing the closing...but still not working!
I get this message:

"...Close operator: an opening in the selected body cannot be closed by planar face. Check all body opening for planarity"

Any ideas?
 

MrCATIA

Super Moderator
Usually the problem encountered in step #3 is the Join is not closed due to gaps or overlaps in adjacent surfaces. This is often caused by data inaccuracies, and can easily be fixed by increasing the maximum allowable gap in the Join.

The message "... cannot be closed by planar face..." means that one or more faces are missing or not included in the Join. CATIA is trying to close the Join, but the opening is not planar. Look closely at the surfaces in the Geometric Set. Maybe a surface was not included in the Join? Or, you might have to add a surface yourself - Use the Fill command, and select all the curves that are the boundaries of the missing surface. And add this new surface to the Join.

It would be very helpful to see a picture of the data, especially with the error message.
 

MrCATIA

Super Moderator
Thanks for the picture. It helps better understand what you are doing.

For this type of part, quite often the surfaces have gaps or overlaps in the adjacent edges. This will prevent the Join from being used to make a solid.

A couple things to help troubleshoot the Join:

1. selecting the Join should highlight all the surfaces

2. use the Boundary Curve tool and select the Join. Any surface edges that contain gaps or overlaps will be displayed in green. This will show you where you have to fix the surface geometry.

3. try increasing the allowable gap distance in the Join. Often a wider distance is all you need.

4. sometimes you might have to delete a surface and create a new one. Use a Fill surface and select all the adjacent surface edges
 

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