"Best Practice" Modeling
"Best Practice" Modeling
(OP)
I am currently trying to develop a stratergy for training & guiding users on "best paractice" CAD modelling in UG.
To beter understand this I want to find out if there are any low level (CPU time & memory usage) advantages to keeping the number of features in the model tree to a minimum.
An example of this is to create an Extrude with a taper as part of the extrude feature and also maybe unite it as part of the extrude as well. This would result in 1 feature in the tree (an extrude). The other method would be to extrude the profile.
Apply taper to the relevant faces and then unite the object to an existing solid.
This would result in 3 features (extrude,taper,unite).
I have my own opinions on this but I'm interested in other peoples opinions to the pros and cons to both approaches.
To beter understand this I want to find out if there are any low level (CPU time & memory usage) advantages to keeping the number of features in the model tree to a minimum.
An example of this is to create an Extrude with a taper as part of the extrude feature and also maybe unite it as part of the extrude as well. This would result in 1 feature in the tree (an extrude). The other method would be to extrude the profile.
Apply taper to the relevant faces and then unite the object to an existing solid.
This would result in 3 features (extrude,taper,unite).
I have my own opinions on this but I'm interested in other peoples opinions to the pros and cons to both approaches.
Mark Benson
CAD Support Engineer





RE: "Best Practice" Modeling
I do not like to create and unite (or create and subtract, etc) a feature in the same operation because it is very difficult, sometimes impossible, to edit the feature without recreating it. Regardless of any cost in memory, I would much rather have the two operations separate.
RE: "Best Practice" Modeling
I absolutely agree with EWH... the diffences in cpu/mem usage is neglible to the user with a modern machine and the advantages far outweight the disadvantages. I believe modeling (in general) should be done with an eye towards easing the re-interations during the design cycle as well as future edits after the drawing has been created.
I'd even go a step further and suggest that when subtracting (or anyother type of boolean) the user clicks the option to "maintain the tool solid". This allows very easy editing of the tool solid without having reset your current feature or suppressing the subtraction (or whatever).
Personally, I'd also prefer that fully constrained sketches be utilized versus explicite curves for generating extrusions or revolves. I do however recognize that there's a 'right' way and a 'wrong' way to utilize sketcher....
Hope part of this helps...
SS
RE: "Best Practice" Modeling
RE: "Best Practice" Modeling
Also, name them features in the tree. Nothing worse than extude01, extrude02, etc...
--
Bill
RE: "Best Practice" Modeling
Matt Freeman,
Design Engineer,
UK
RE: "Best Practice" Modeling
I agree completely with not creating the Booleans on the fly.
RE: "Best Practice" Modeling
RE: "Best Practice" Modeling
Adding the taper and boolean features on the initial operation is a no-no. Sure you can do it, but the downstream user will have trouble updating that, most likely will have to re-create it. Than you will have to re-associate the dimensions, if a drawing is there, to those features. It just doesn't maintain the associativity throughout the model to drawing.
RE: "Best Practice" Modeling
SS
RE: "Best Practice" Modeling
I guess that depends on who you ask, I personally have never needed it.
RE: "Best Practice" Modeling
I never create booleans on the fly either. Learned that the hard way and also with my experience with GM (Working there and working at suppliers) you just don't do it.
RE: "Best Practice" Modeling
RE: "Best Practice" Modeling
There are radio boxes in the middle of the dialoge box for 'maintain tool' and 'maintain target'. Just make sure you check the box before hitting the 'ok' button. You will then have your boolean feature (add/sub of the tool to the solid) as well as the original tool solid to work with.
SS
Regards,
SS
CAD should pay for itself, shouldn't it?
RE: "Best Practice" Modeling
Those radio boxes don't exist when you create them 'on the fly' (ie during the extrude/revolve operation); at least not on NX2 (unsure on later versions).