Boolean Operation Real Usage in CATIA?

[waqahmad]

Hi All,

This is my first message on this forum. I am an expert user of Pro/Engineer But recently we have shifted ourselves from Pro/E to CATIA V5R16. So I am very kind of new to CATIA V5.

I have a question which I will be obliged if some of you could answer. What exactly is the purpose of Boolean Operation in CATIA V5. As I dont see it helps much in making shapes which are not possible to make through parametric modeling. There is one valid point about Boolean Features that its fast in regeneration/update. Besides this point can someone elaborate me on their real usage. There are many shapes that can be modeled with or without Boolean Operation so my question would be when to use Boolean Operation and when not to? OR is it just an old obsolete tool which DS is keeping it along just to leverage the old users of CATIA??

I will really appreaciate anyone's remarks on the above mentioned issue.

Regards

waqahmad

 

[DBezaire]

Wagahmad - you could parametric model everything if you want, the boolean features allow you to share the same solid for many purposes. We use a significant amount of boolean operations in our assemblies. If I add a component(A) to the mold, generally it requires material to be removed from another component(B). Inside component A there is a removal solid that is linked copy to the primary solid of Component A. This removal solid has a boolean remove operation performed to Component B. If I change any portion of the primary solid in Component A - the removal solid updates which intern updates Component B. Alternatively I could parametric model everything, update the primary solid of Component A, then lets not forget to update the removal of material from component B.

Regards,
Derek

 

[jackk]

Wagahmad - I used to agree with you that Boolean Operations were no longer necessary, but I've changed my opinion.

Compared to CATIA V4 (where every feature had to be booleaned into the solid), V5 booleans are no longer neccessary.

But, like Derek said, the ability to organize the part model into multiple partbodies is valuable, and booleans can then be used to "assemble" the partbodies.

Where I work, we design many molded parts and we use a core/cavity method. A big block of material goes into the first partbody; the cavity side is boolean removed; and the core side is boolean removed. Machining operations are in another partbody that is also boolean removed.

I also like to use individual partbodies when I do patterns of features using the 'current solid' option. Again these bodies are boolean assembled into the higher level partbody.

 

[Hora]

Waqahmad,

Imagine this particular situation: In Pro sometimes you cannot create a readius into a small cavity because there is not enough material. To solve the problem, you will make a colosed surface, round edges and then you cut the solid with this surface.

Same thing cam be done in CATIA but using solids in diffrent bodies.

-Hora

 

[abeschneider]

Booleans are also useful in reducing rebuild times for complex parts like a screw or spring with detailed helix, or for large patterned features (ie: many holes on a user pattern, etc).

If you create the pattern on a separate body, then boolean it into the main body, it helps cut down on the rebuild time, I think. (See the catia online help docs on this one...)

 

[solid7]

You can't appreciate the value of booleans, until you actually NEED them.

Classic example - operations that require shell, draft, and fillet, all in one part.

I had a casting that needed to be made with molded pockets in the "legs", which were joined to a cylindrical part. The best way to make them was to make the "legs" first, in their own part body, shell them, and then join them before putting radii on the whole thing.

In this case, due to the logic of creating the objects, it was not possible, in any even, to create the part without booleans.

If you do enough of this, for a long enough time, you will certainly find a need for Booleans.

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