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B-Reps for sketches, good or evil?

ACCLR8N

New member
I'm having a disagreement over our company's global design manual. The statement is "Avoid selection of B-Reps in part design". I disagree with this. Most of my sketches, sketch constraints and pad/pocket limits are faces from previous features. I do discourage edges and vertexes. I can't imagine setting up planes for every sketch or limit. What are your opinions?

I'd also like to hear some people chime in on "hole" vs. "pocket". I prefer a single sketch (on a work plane) to blast multiple holes in one pocket operation. My German counterparts again frown on this practice. My view is the simplist tree, the faster easier to modify. FYI: Metal stampings and injection molded parts in CATIA V5 R18.
 

Kevin De Smet

New member
This is always a bit of an issue, and in my opinion, it's the software that's the problem. Why should we be forced to keep referencing our sketches and planes?

It would be cool if the software automatically put a constraint on the underlying sketch of the face or edge you would click, when possible. But I'm just ranting. I do like being able to even constrain to faces, I wish SolidWorks could do that, because I love that.

Yeah, the hole feature sucks. Sorry for the bluntness, but I too would be itching to use a pocket instead. Hmm... are you sure you can't use multiple points for hole center in one hole feature? I think so to, but somehow that still seems all backwards and so 1999!
 

ACCLR8N

New member
It appears I have been trumped with the presentation of the German OEM CAD methodology guideline. Audi, BMW, Daimler, Porche and VW have an agreement on what is best.
 

MrCATIA

Super Moderator
I'm having a disagreement over our company's global design manual. The statement is "Avoid selection of B-Reps in part design". I disagree with this. Most of my sketches, sketch constraints and pad/pocket limits are faces from previous features. I do discourage edges and vertexes. I can't imagine setting up planes for every sketch or limit. What are your opinions?
We have a similar "rule" where I work. The reason is that the face might change in the future (replaced when a pocket is added, or the edge is filleted, etc.) which replaces the old face with a new one, and makes your constraint go "bad."

In my opinion, it is better to constrain to a known feature (such as a plane, or another sketch) instead of a face. Although sometimes you have little choice and have to constrain to the face.

I would say constraining to a face is not good, but I wouldn't call it "evil"
 

MrCATIA

Super Moderator
I'd also like to hear some people chime in on "hole" vs. "pocket". I prefer a single sketch (on a work plane) to blast multiple holes in one pocket operation. My German counterparts again frown on this practice. My view is the simplist tree, the faster easier to modify. FYI: Metal stampings and injection molded parts in CATIA V5 R18.
I'm in favor of using Holes instead of Pockets. Holes can be specified as threaded, counterbored, end-type, etc. as part of the Hole definition. Plus they show-up on the drawing with the correct thread symbology. Multiple holes can be "blasted" by using the User-Defined Pattern.

I'm not in favor of defining all the holes as several circles in a single sketch, expecially when the holes are different sizes.
 

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