Boolean Operations

[Akesson]

Hi,

I have a few questions about Boolean operations and Hybrid Design.

When I read forums like this I often see that users are recommended not to use Boolean Operations like “Remove” instead of features like “Hole” etc. Which advantages and disadvantages have these to different methodologies and when to use them?

What are the differences between the Boolean Operations “Assemble” and “Add”?

What are the advantages and disadvantages with “Hybrid Design” (mixing features from both Part Design and GSD in the same Body) and suggested methodology how to use it?

/Akesson

 

[catiajim]

1) Boolean operations. Features like Hole have more intelligence built into them than a simple cylinder that has been removed does. It will be easier to automate, and if your part is being NC Programmed at a later phase, the NC tools will automatically pick up Holes as Drill operations, where as a removed cylinder has to be manually selected.

In general, boolean operations are not necessary in V5. The only really bad thing about them is that they are extra steps. It is easier to simply create a pocket than it is to insert a new body, create a pad, and perform a remove. There are many times, however, that they are necessary - for example when your removed shape contains multiple primitives. In that case, go ahead and use them. Just don't use them to perform single operations like subtracting a single cylinder.

2) Assemble and Add appear to be the same thing initially. However, as you work with CATIA, you will discover that in anything except the first Part Body, you can create a Negative Primative as the first operation. If you do this and use Assemble, you will remove material from your solid. If you use Add, CATIA will ignore the polarity of the primatives and force the shape to add material. While this is generally not of much use for single parts when working alone, if you are working collaboratively on the same part, or if you are creating PowerCopies and UserFeatures, it can be extremely powerful.

3) I have yet to run into anyone that is using Hybrid Design. It may have some powerful use somewhere, but for most CATIA users, it just messes them up.

 

[solid7]

In general, boolean operations are not necessary in V5.

I would respectfully disagree on this point. While boolean operations are not standard V5 logic, there are certain operations that are not possible without them. (yes, in V5)

Admittedly, I don't like boolean, and Parametric modeling is so much nicer. However, booleans are still here, because they occupy a very important place - a gap which has not yet been filled with any other method.

I know that you said "in general"; however, I think that might be from only one design perspective. I use Booleans everyday, (although in VERY limited numbers, and only where I can't do it any other way) so to me, it's also a "general" issue. I hope that you can understand what I'm trying to say in all of this.




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[Akesson]

Thanks!

I'm interested in different methodologies for modeling. It's interesting to know how others do. For en example, we have a customer that uses Boolean operations for solid modeling of injection molded plastic parts. They create inside and outside of the part in different bodies.

I myself use Booleans to structure the tree when creating for an example a mirrored part.

Part
-PartBody
--Assemble
---Body
----Solid
----Symmetry

Hope the discussion will continue....

/Akesson

 

[solid7]

Internal threads, where the lenght changes, and the bottom depth is determined by a plane. This is one of my most frequent uses of Boolean.

I use the Boolean here to make the thread definition, that gets used OVER and OVER again, but with slight modifications.

First, I use the helix function to lay out my angle and pitch, then use that same helix as a center curve to create the thread revolute. Inside the thread revolute, there is a diameter that may or may not continue past the thread. (equivalent to the minor dia. of the thread, since the revolute cannot self-intersect) The depth of the thread/hole is determined by a plane with history, based off of the XY plane, which performs a split operation. I can change the position of the thread (in Z axis) and the depth of the bore, simply by changing parameters, before or after removing the whole body. And, I can use this as a "drop-in" solution for other models.

Booleans, in my experience, still come in most handy where you have very complex shell and draft operations, such as is the case with die cast, or injection molded parts. Creating bosses that are attached to a shelled part can be very cumbesome WITH Booleans, but almost impossible without them.

I generally use Boolean in this case to separate bosses from shelled walls. First, I create a body with bosses, and lay them out. Many times, I have to create a draft angle on the outside of the boss first, and then after using the Boolean to attach the bosses to the shelled wall, I have to apply ANOTHER draft on the inside - as a shelled wall means that you have a different pulling direction on the inside of the part, than you do on the outside of the part.

One thing is abundantly clear, however - Catia V5 abolutely, positively, cannot dump the Boolean operations. They do not have sufficient logic in place to eliminate them. The above examples are only a glimpse of available scenarios.




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[belvedere64]

I use all positive space:
Core/Cavity for injection mold.
Casting/Machining for forging.
Many of my stampings end up with pads removed.
It is easy to reuse features.

I did not realize CNC can detect pocket for programming. I am a firm believer in capturing downstream requirements early.

As I automate more, I see I'll have more need for negative space.

Thanks for the comments!

K. C.

 

[catiajim]

Absolutely, Booleans are necessary many times. But I see way too many times where a V5 user (who is a former V4 user) uses Booleans to remove a cylinder from a pad - when they should have used the hole feature.

As Solid7 and others have pointed out, when you are manipulating complex shapes that are not easily represented as single primitives, then booleans should be used. But when dealing with simple primitives, use the features, not booleans.

 

[Akesson]

As an old ProE user I'm not used to use Booleans but I understand that in some cases they are useful and my only interest is to build the models in the best possible way.

I totally agree with catiajim that many former V4 users use Booleans a lot when they shouldn't and many suggested methodologies in V5 that I've seen on different companies are V4 methodology that are translated in to V5 methodology. In many of these cases the methodology isn't made/adapted for V5 and not using its full potential.

I use Booleans to create multibody parts (parts where every body present one detail in a structure) for layout purpose. I build these standard parts to be used in big layout assemblies. I use this methodology because Catia has difficulties to handle large assemblies.

/Akesson