can a sketch dimension drive a "feature dimension"

Lets say one makes a rectangle sketch and gives the rectangle length the
dimension d1@Sketch1. now using this sketch one has created a boss/base
extrusion feature with a height which is irrelevant to this topic. after
rebuilding one uses the quick dimension to give the height of the extrusion
the name RD1@Annotations. now the question is this:
Is it possible by equation to control the derived dimension RD1@Annotation
by formulating some equation like : RD1@Annotations = 0.1 * d1@Sketch1 ?
As it appears for now in SW2005 SP2 in the equation manager the dimension is
solved correctly. but in solidworks itself the change is unnoticeable and
solidworks maintains the original height of extrusion to RD1@Annotations
together with the red sum symbol and not the one which is evaluated by the
weird isn't it? or did I misunderstood completely the equation concept in
Gil Alsberg
Reply to
Gil Alsberg
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RD1@Annotations is a reference dimension. It is driven by the geometry and cannot drive the geometry. If you double-click on the extrusion, you should see a blue dimension appear. This is the dimension that drives the extrusion height, and it will have the value you assigned when yo ucreated the extrusion. You can drive that with an equation.
The equation editor probably should not have allowed you to try to drive a reference dimension with an equation. But that's not something an experienced user would normally try to do. How long have you been using SW?
Reply to
Dale Dunn
Thanks Dale, I have an experience of two years in modelling in solidworks although most of my time is spent with surfacing work on Rhino. As you mentioned the term "reference dimension" - I would like to ask you: what is the purpose of such a dimension, besides being visible all of the time when the part which contains it, is on the active viewport in solidworks?
Reply to
Gil Alsberg
Sometimes they are useful for hte other end of an equation, or even just showing a measurement all the time instead of having to use the measuretool over and over. The vast majority of the time that I use them, they are linked to a custom property so that the finished material size can appear in the BOM.
Reply to
Dale Dunn
Just my 2-cents added to this is that I would say 90% of the time, when most users insert reference dimensions, they are on the actual drawings, not so much in the models' sketch(s). There are a lot of times where SW will just not display the dim on the print where you want it or more correctly, you may want to show an overall length (for example) on a part/assembly and SW doesn't have that dimension to insert, as it would normally over-define the part. These are driven dimensions and will not allow you to change the model from the drawing (which I don't do very often as I hate having to cross my fingers that it doesn't blow out a whole assembly drawing after it's rebuilding for 5 minutes) ;)
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