Drafted surface in Catia V5R14SP2 2

[Darrude]

Dear All,

I wonder if anyone can help me. I'm trying to produce a surface model of a plastic component with draft. I want to extract a closed profile with 5 degrees draft. The only way I can think to do this, is to do a surface extract, then close to a solid and then draft the solid. Then I have to extract the faces of the solid to bring back into my surface model!

There must be a better way (IE, exract a surface with draft (like in V4). Maybe I need an additional package to do this, we only have Generative shape desgin.

Many Thanks in Advance,

Darren

 

[solid7]

I have to tell you that after having done MANY, MANY, MANY parts like you are describing, I can't believe that you would ever want to do it any other way, EXCEPT by the solid method.

Yes, I think you can do it if you have the mold maker package, but the advantage of doing the closed volume, is that you clean up your surfaces as you go. So many times, the surfaces for parts like you are describing, are pure junk, because they are either done by translation, or they are done quick and dirty.

I make my living from cleaning up such parts, and getting them ready for manufacture. In my opinion, take the time, fix the part, and find out what tolerance you can close the part to. Why, you ask? Because if you have ANY problems later on, with your draft operations, (drafts are still a difficult and sticky operation) you will be able to narrow them down that much easier.

I can't tell you how many times that I've gotten almost done with a part, putting on the last draft angle, and the I find that it won't go - just because of some little gap or overlap in a surface, or a vertex left over from funky filleting, or some other bizarre little annoyance, keeps what is otherwise, a perfect model, from reaching an acceptable close tolerance. And yes, there is a direct correlation between close tolerances, and the ability to do certain operations. (filleting and drafting specifically)

 

[jackk]

Darren...

I'm not sure how sculptured your part is, but I'd suggest you define shape with a surface first and then make a solid from it later.

Use a SWEPT surface to define the draft.
profile type = line
subtype = with reference surface
guide 1 = your profile
reference surface = plane of your profile
angle = 85 (or 95)
length 1 = a little longer than the draft length
spine = default (your profile)

then trim the SWEPT surface to desired length

 

[Darrude]

Jackk,

Thank you for this reply (our help desk couldn't answer this querey). There is another option in subtype which is draft with direction. This has given me exactly what I wanted.

Solid7, thanks for your reply but the part is a bit to scultuped to turn into a solid so early (it has componded surfaces on both the "A" and "B" side, the component is a plastic handle that is cored out with Gas injection, every surface is componded and a head impact requirment meana a minimum rad size on all edges of 3mm).

Thanks to both of you for replying.

Darren

 

[jackk]

The nice thing about CATIA is there is always more than one way to do something

Glad to help