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Boolean operations ADD/ASSEMBLE and polarity

Kult2015

New member
Hello there!

I am puzzled with Boolean operations, I need some advice to figure out how it works! As far as I know, the difference between ASSEMBLE and ADD is that the ASSEMBLE respects the “nature” of a sign and the ADD operation should ignore polarity.

So, here is what I do. I created a new PART file (Part Body is added automatically and by default is positive), created a new PAD (a simple rectangle). Then, inserted a new body (plus sign in front of the body icon in the specification tree) and created a new simple PAD (one more rectangle), the plus sign is still on the icon, no changes), applied ADD operation or added the second PAD from the inserted body to the PartBody. Okay, here we go, I have one solid! Good, it is fine, that is what I expected!

Then, if I try to create a negative part such as a POCKET, what will happen?

I created a new PART file (Part Body is added automatically and by default is positive), created a new PAD (a simple rectangle). Then, inserted a new body (plus sign in front of the body icon in the specification tree) and created a new simple POCKET (one more rectangle, IT IS A NEGATIVE SOLID), THE PLUS SIGN IS CHANGED TO MINUS ON THE ICON), applied ADD operation or added the second NEGATIVE POCKET from the inserted body to the PartBody (I cannot do vase verse) …… and the POCKET is subtracted from the PART BODY? What is wrong? ADD operations is supposed to ignore polarity, as far as I know! ASSEMBLE operation respects polarity, not ADD. What I have just described should be okay for the ASSEMBLE operation, not the ADD operation.

Please help to figure it out? What is wrong? Did I miss something, should I configure CATIA in another way?

Thank you!
 

MrCATIA

Super Moderator
Nothing is wrong - everything is working as it should. The reason the ADD and ASSEMBLE operations are behaving as they are is answered in your second sentence: "the ADD operation should ignore the polarity." The ADD looks only at the shape (or mass), and then it adds that shape. It doesn't matter if its a positive Pad or a negative Pocket - ADD only considers the shape of the body and it ignores the polarity.

If you make the negative body the work object, you will see the shape that is being added.

If you change both ADDS to REMOVES, you will get the same result with the positive and negative bodies.

boolean add.jpg
 

MrCATIA

Super Moderator
I recreated a simple part showing the boolean operation results with + and - bodies:

The upper row shows the results of ADDing different polarity bodies (+ on left and - on right), and the middle row shows REMOVEing similar bodies.

The bottom row shows the results of ASSEMBLE operations, where the polarity determines if the body is added or subtracted

BOOLEAN 1.JPG
 
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MrCATIA

Super Moderator
Using this simple part, we can look closer at the results of working with "+" and "-" bodies:

Adding a pad to a "+" body gives us this: boolean 2a.JPG

but adding a pad to a "-" body gives us something different (even though we used Pads on both): boolean 2b.JPG
Features in negative ("-") bodies are reversed in polarity; Pads, Shafts, etc. are subtracted, while Pockets, Grooves, etc are added.

And we can see the end results of adding these pads to all 6 of our boolean bodies:
BOOLEAN 3.JPG

Conclusion: Boolean Operations and multi-body part files are normally not required. But if used, the "+" and "-" bodies should be used carefully!
 
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Kult2015

New member
Thank you for your reply!

Well, still I cannot get it … when I read CATIA v5 manual, everything looks quite obvious and logic but if I try to do these operations in CATIA v5 I rarely get what I expected to get …. I am not a fan of Boolean operations but I am planning of taking CATIA v5 Certification Exams, and Boolean Operations are a part of the exam, and that is why I need to figure out how to use them and be able to predict what will happen if this or that operation/command is used, etc. No possibility to have a try at the exam …

Does anybody know where I can get a step by step guide how to use the operations, not just a general CATIA v5 manual?

Could you please make a video or more detailed screenshots?

Thank you!
 

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