When assigning a parameter to a dimension, I have two options:
A. Rename the dimension. For example, if I have dimension p1, change its name to, say, "rod_length" and maybe edit its value (50mm).
B. Define a new expression named "rod_length" with a length value of 50mm, then assign it to dimension p1.
Is one approach consider better than the other? Approach A seems easier, but B may be a little cleaner and can be done ahead of time. I'm working on a model in which I'll need to define several dozen parameters and wondering which way to go. Thanks!
In most cases it does not make much difference. But there is one case you might want to consider. If you rename the expression and you delete the feature (and it is not referenced elsewhere) then your expression is deleted as well. When you create an expression first and reference it, then the dimension is retained.
When you type "A=10" into the extrude limit then NX will create an expression A=0 and have the extrude reference it as p456=A. so you can do this on the fly.
Last tip: Use capitals for user expressions, it makes them easier to find/sort when looking at the complete list.
There's one big difference between A and B.
When you create an user expression NX will show this exppressions in the Part Navigator and you can edit this expressions with double klick.
I would create user expressions for all key parameters. The other parameters you can rename.
As @DickBaardse mentioned, Creating expressions on the fly is easier rather than creating the dimensions and assigning the expressions.
One suggestion could be if there is need to create considerable number of expressions (say 50). Use of Export/Import option will be helpful. Define some expressions with different unit (Length,Angle,Area etc) as per your requirement.
Export expressions to the file, it will export with .exp format which can be edited using text editor. Open the file with notepad and observe the format of expressions. Add the desired expressions using proper format (You can use excel in efficient way from which you can copy paste to text file)
Save and close the text file. Import it again to the NX.
My personal preference is to create the expression, say Thk=.10, and then apply "Thk" as I need it, ie p5=Thk. This allows me to use the value for "Thk" in multiple places, and I don't have to worry about being dependant on the original. I can change any expression that uses "Thk", without affeting the others.
I think it boils down to how you use the expressions, and how things tend to change in your work enviornment.
Thanks for the feedback on this.
The fact that if I rename a dimension (option A) and then happen to delete that dimension (or the part it's referenced to) later on (thereby deleting the expression) is good reason not to do it that way.
So it definitely safest to keep the expressions independent, and that's what I'll do.
Just realized NX will keep the expression from a deleted feature if it's being used elsewhere (very nice). So option A is not as hazardous as I originally thought, and seeing meaningful names for the dimensions is nice in some situations. Also I didn't realize user defined expressions (option B) are displayed in the part navigator (also very nice). So I'll probably use both.