Rework V5 models

[jeffmill]

Hi All
Boy I wonder how much this posting will attract.
I have used V4 and V5 Catia for about one year and find the contrast remarkable. V4 would appear to be very easy to modify "old" models in, V5 seems to be very good at producing new models. Now when I attempt to modify documents in either version things could not be more different. V4 could not give a monkey (in the round) about dependencies between solids and 3D geometry but in V5, boy you had better wear a tin hat. Just how many dialog boxes are displayed telling you of various dependencies that require fixing? - does anyone remember the game "pick up sticks" you can't alter one thing without affecting something else.

Anyone have anything to addd?

My training in V4 & V5 Is IBM

 

[haribabuAus]

I do have the same feeling. Too much muck-around ;
I think at the first place proper stict procedures needs to be followed in V5 than in V4 ;

 

[jackk]

How long have you been using V5?

I had the same opinion for maybe 2 days after I finished my training, but once I starting using V5 in production, I changed my opinion: V5 is much easier to modify parts than V4.

One technique I use when making heavy modifications, is to start at the top of the part body tree, and right click on the first feature to be changed and DEFINE WORK OBJECT. Change that feature and then do a local update. If you get error messages - read them and fix them. If you can do a local update OK, change the next feature as the underlined work object and change it and local update it. Changing the part from the top of the tree down, helps me get through all my changes and minimizes the error messages.

A V5 modeling technique that helps: Create an open body of REFERENCE MASTER GEOMETRY containing datum planes, center points or centerlines, and other important geometry. Then when you model the partbody, use the master geometry to define everything. ie; contrain sketches to master geometry, or extrude pads to reference planes, etc. When it comes time to make changes, just edit the master geometry and the part should "magically morph" to the new design.

Haribabuaus is right: procedures need to be established and followed.

 

[roseda]

Solid Modelling: Do most of you use Boolean operations as per V4?

I ask, because V5 seems like it is designed to work without using these operations. My trees generally end up looking like this (for a machined from solid part)

Body xxx
Pad (for machining blank)
Remove Longitudinal Bores
Body xxx
Add
Body xxx
Groove
Add
Body xxx
Hole
Mirror
Remove Other Holes
Body xxx
Add
Body xxx
Hole
Hole
Add
Body xxx
Hole
Rectangular Pattern

etc.....

In V4 the tree for this would be a lot simpler. Is this the way most of you model (is there another way?)

 

[bsurfN99]

I agree with many of the other posts with the exeption of that V5 is any easier to modify than V4. You can modify many features within V4 just a easily as in V5. Something to consider within both enviroments is your modeling integrity. My experiences have pointed me towards using the boolean operations on larger files, mainly because you can manage the degree at which operations fail. I look at booleans as groupings of geometry, and in doing so I have been able to minimize failures to lets say 10 items vs. the 60+ you could face with fillets being referenced to drafts that have been deactivated.

A bigger challege I've run into is the difference in modeling tolerance, V4 being .01 and V5 being .001. Tangent surfaces in V4 are whacked in V5.

Good luck with the developement of your V5 methodology.

 

[jackk]

I agree with Bsurf!

Limit booleans to only when you must use them, and do use them to group design features of larger, more complex parts.

50% of the lines in Roseda's example are unnessary.

 

[roseda]

jackk, please can you spell out how you would create the same tree.

 

[jackk]

I'd do something like this, Roseda:

Body xxx
Pad
Groove
Pocket (sketch contains hole circle and mirrored circle)
Hole
Hole
Hole
Rectangular Pattern (of just the last hole)

My guess is simiplier trees result in faster processing, and easier understanding for the next person who works on this part.