Dimensions Versus Parameters(SolidWorks) 1

[LosGriegos]

Way back when...
I was always told to use smart dimensions instead of feature parameters. I never was told why.
My guess is that the parameters "lock" a feature to a certain value, and not be adjustable. Or could it be, having the ability to "name" a dimension?

Any ideas?

Regards,
Mon

 

[ShaggyPE]

you lost me... I think you are using terminology that is not the typical SolidWorks terminology.

-Dustin
Professional Engineer
Pretty good with SolidWorks

 

[Updraft]

Mon,

If you mean "Is it better to use geometric constraints or dimensions to completely define a sketch?" the answer is that depends on the design intent. There are times when a feature/sketch element should be constrained to some other element so they move together - if that is the most elegent form of the design intent. There are other times when it makes more sense to use an independent dimension to define an element.

- - -Updraft

 

[TheTick]

It's even better to know what you need without being told.

 

[handleman]

"Parameters" (as they are labeled in the Property Manager page for sketch entities) are not useful. They should be eliminated from the software. They move entities to a certain location, but do nothing to make them "stay" there. Parameters do not continue to control entity position. If model changes cause some sketch geometry to move, there is no way to predict what will happen to under-defined entities that you have just put where you want using Parameters. Dimensions and relations define entity location based on your design intent.

This is 2D CAD thinking vs. parametric modeling thinking. With 2D CAD, you draw lines and put them places, then you add dimensions to communicate information about where you drew the lines. With parametric modeling, you use relations and dimensions to control where entities go.

-handleman, CSWP (The new, easy test)

 

[LosGriegos]

Thx handleman, I guess I knew it was something like that.

Mon

 

[fcsuper]

I don't think they should be elimentated at all. They are useful when you do want to place something in a particular way. Design can be locked down at a later time with other methods. Design intent is not always known when one starts creating parts. In my mind, the assumption that design intent is completely understood at the start of the modelling process is more of Pro/E thinking vs. SolidWorks thinking.

Also, it is not necessary to completely define every entity within a sketch, though this is an unpopular view among CAD admins and CAD managers. The reason is that sometimes there is no value in fully defining every entity within a sketch. Sketches only need to be defined to the degree necessary to capture the design intent. Often, this does mean the sketch is fully defined, but there are plenty of instances where it's just a waste of time and computer resources to fully define a sketch.



Matt Lorono
Lorono's SolidWorks Resources & SolidWorks Legion

http://groups.yahoo.com/group/solidworks & http://twitter.com/fcsuper