Boolean operations

What are boolean operations?

Boolean operations in Catia are just like boolean operation that you may have studied in mathematics or a subject called sets. It's not exactly the same and somewhat different and is more suited for modeling. In Catia, this is known as multibody concept. For that matter in most softwares, this is referred to as multi-body concept.

Common sets operations taught in school 

In Catia, boolean operation are applied between two bodies. So, unless you have two different bodies, you cannot apply the boolean operations. Boolean operations are available under Insert > Boolean operations. You can also apply boolean operations using the respective toolbar.

By default, all the solid models are created in the Part Body, which can be seen in the specification tree. However, you can add other bodies using Insert > Body. This will create another body in the specification tree. As you used the Part body for creating geometry, you can utilize the newly added body for creating geometry too. The body in which you wish to add solid geometry, you can do so by selecting it, using right click and Define in work object, this will send the operations that you do in that particular body

Concept of Polarity

The concept of polarity is worth understanding before we understand boolean operations. The operations that add material like pad, shaft etc. are of positive polarity, while the ones which remove material are of negative polarity.

Some of the features and their polarity

A thing to keep in mind is that in case of Part body, a negative polarity operation i.e. an operation that removes material like Pocket, Groove, Remove Multi-section solid etc. cannot be the first operation. However, in case of a Body, you can even have negative operation as your first operation and it will be visible in space. Boolean operations simply provide us a way of interacting with polarities of the solids we create. We will see ahead how different operations work with the polarities that we have.

Another thing worth keeping in mind is that the first operation 

What is the use of Boolean operation?

Boolean operations helps in many ways. It significantly helps in managing overall modelling data based on requirements such that you can place and group similar modeling data using part bodies. An advantage that these bodies present is that they can be straightaway copied into other files. These can be effectively utilised for visualizing stock material required for machining. 

It also helps in modeling and visualising negative spaces i.e. material that may be need to removed in a final product but needed to be visualised in positive. Consider that if you need to model HVAC pathways in a building, it would be a much difficult task if you use a single body to model the geometry or model it using pocket in the main part body. So, even though the passageways in case of HVACs, water jacket or cylinders in case of IC engines are negative spaces, they can be modeled and visualised using another body since these bodies can have a negative operation as first operation, and finally a boolean operation may be applied to extract the useful geometry. 

Also, boolean operations are best utilised to create core and cavity from modeled plastic parts which can be utilised for creating tooling.

What are the different Boolean operation that can be applied in Catia?   

Different boolean operations will yield results also depending upon the kind of geometry that is present in the part bodies. Let us see how they work using practical examples. Boolean operations that can be applied in Catia are the following. 

Assemble operation

• Assemble - Assemble will subtract material / combine material depending on the operations that are applied in the body i.e they are sensitive to the operations that are applied in the bodies. Below you can see the assemble operation applied to separate bodies (purple and yellow) where both operations were of positive polarity, hence both got combined and the result can be seen below. You should try this with features such that positive polarity is in part body, and negative in body.

Assemble operation applied

• Add - This will add the bodies regardless of the operations. So even if you have operation like pocket in body i.e. a negative operation, it will be added to the main Part body. Assuming that you have the same features as above, apply the add operation and see the result you get. Also try this with negative polarity. Both will yield the same result.

• Remove - This will remove one body from the other regardless of the polarity of the operations present in the body, so the result will be a subtracted body from main body. So in essence it behaves the same as Add boolean operation i.e. it does not take into account the polarity of the body, and simply subtracts the body from another.

• Intersect - Intersect will compute the intersection between two bodies. Above two bodies in different colours when applied intersect will yield the following result. 

Intersection applied between two bodies

• Union trim - This operation will unite the bodies and it can be simultaneously used to remove / keep any faces independently that we desire. For example, if you see below, all other protrusions were kept will only one was removed using union trim.

Union trim applied - with one face of protrusion selected for removal

• Remove lump - Remove lump proves useful in cases when stray bodies are left after application of boolean operations. This may be used to remove independent lying features that do not belong to any main body or features that are not required, so if there is basically a leftover result of any of the other boolean operations applied before, those can be removed using remove lump. If you see below, at the centre there's a cylindrical leftover lump which is not connected to the main body and is not desired, this can be removed using the remove lump boolean operation.

Remove lump can be applied to centre cylindrical portion