"Best Practice" Modeling 1

[MSPBenson]

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.


Mark Benson
CAD Support Engineer

 

[ewh]

(I responded to this question on the BBS, but will again for those that don't have access.)
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.

 

[Shadowspawn]

MSPBenson,
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

 

[ewh]

I am also in the habit of creating tool solids as Shadowspawn mentioned. Yes, it does increase the feature count, but it makes editing much more simple. Instead of having to go thru the tree to find out which subtraction you need to suppress to edit the subtracted body, you instead turn on the layer of the tool solid and edit that. Viola, the model is updated.

 

[wmalan]

In my modeling class I took years back at Cypress, they recommended creating as many solids as you can before doing the booleans. They also said to save filleting and corner radii for last. When extruding solids from curves or sketches, don't create the corner radii with the curves, do it with the filleting or corner radius features for better control later.
Also, name them features in the tree. Nothing worse than extude01, extrude02, etc...

--
Bill

 

[mhf23]

Totally agree with everything written here. I've never had to work in UG on a system where this sort of resource husbandry was an issue. Having a compact model may sound elegant, but you can get in a terrible mess later when you come back to alter things. Also, it makes it harder for other people to understand your work when they come to edit it at a later date.

Matt Freeman,
Design Engineer,
UK

 

[claireandmabel]

These thoughts are great! I, too, am looking for insights on "best practices" in NX modeling. My organization subscribes to the "chunky solid" methodology but I have seen some elegant sheet modeling lately. What type of modeling approach are others in the NX modeling world taking?

I agree completely with not creating the Booleans on the fly.

 

[ewh]

Wether to use "chunky" or sheet modeling depends much on the type of part you are creating. It is much easier to create a solid cube than to create 6 sheet bodies and sew them together. Working with aircraft lofts, I use both methods, but I tend to use sheet modeling the most.

 

[jackley]

It doesn't matter if you apply the taper/boolean operations in the initial operation, it still creates seperate ID #'s per actual operation. So either the tree grows or the internal tree grows. Just easier to not do operations on the fly.

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.

 

[Shadowspawn]

Creating the booleans 'on the fly' is fine, and often needed for describing the necessary shape, but one needs to make sure that they are saving or maintaining the 'tool' solid.

SS

 

[cowski]

I know of no way to create booleans 'on the fly' AND maintain the tool solid.

often needed for describing the necessary shape

I guess that depends on who you ask, I personally have never needed it.

 

[jackley]

I have never kept any of my tool solids, unless I am going to use them in another model. We have uncompressed and compressed parts. The customer wants the compressed models so I will retain the tool solid if it's going to be used later on. Otherwise I never do keep them.

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.

 

[ewh]

I never used to keep the tool solids until I was forced to by a customer where I was a contractor. It really opened my eyes as to how much easier it makes it to edit the model.

 

[Shadowspawn]

cowski,
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?

 

[cowski]

SS,
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).