assemble vs add

Add (and Remove) ignore the feature type and performs the boolean to add (or remove) the two solids.

Assemble recognizes the feature type. It adds the volume of pads, shafts and other "positive" solid features; and it removes the volume of pockets, grooves, holes and other "negative" solid features.

Hey forfun.
I dont know about you but jackks reply really didnt help my understanding.
jackk.
I still cant pick the difference between a solid with 'add' and the same solid using 'assemble'.
Sounds like double talk to me.
What is the physical difference, advantages, disadvantages of one against the other?
Can you please give an example?
I have had users ask me the difference but I have to say I dont know.
Dave

If you add a second body to your part, the first operation can actually be a negative body (i.e. Hole, Pocket, etc).

If you perform an Add of this body, it forces the polarity to be positive, and treats the final shape of the body as a lump of material to be added to your first Body.

If you perform a Subtract of this body, it forces the polarity to be negitive, and treats the final shape of the body as a lump of material to be removed from your first Body.

If you perform a Assemble of this body, it uses whatever polarity that the body contains. If it's is negative, it subtracts. If it's positive, it adds.

Normally, this isn't something you would use day in and day out. It is extremely powerful, however, when using any of the Design Automation tools such as PowerCopies, User Defined Features, Templates, Knowledgeware, etc.

Notice on the gear icon the polarity (+/-).

Catiajim, I'm interested in your "extremely powerful" statement, how do you mean this is so powerful that you don't use add/remove instead??

Kadego - did CATIAJim's explanation help you?

For a quick lesson: make two partbodies, with a pad in the first partbody and a pocket in the second. Now do an Add, Subtract and Assemble and see if you can tell the difference. Would a picture help?

If your blob was Assembled to the main body of the part, then you can use KWE Rules, or even Parameters to change the polarity of a feature. You can also do this with tabulated parts driven by a Design Table.

For example, you could have a pair of identical parts, whose only difference is whether or now they have a hole or a pin (for alignment or for idiot-proofing). If your Power Copy or UDF contained both the Positive and the Negative bodies with one active and the other in-active, you can tie their "Activity" to a parameter. Then you simply switch the Parameter from True to False, and the bodies switch their activity. The end user doesn't need to do anything to the geometry.