Controlling the diameter of a cylinder using a parameter

[IanEdwards]

I have a very simple cylindrical part. I want to control the diameter of this using a parameter called "DV_DIA" Whilst this should be straight forward, I am getting a little confused! At first I thought that the dimension controlling this diameter was "d7" therefore I entered d7=DV_DIA, but in the sketch view this dimension has the name "sd0" so should I enter sd0=DV_DIA? Is there two dimensions controlling one diameter?
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[RussDavidson]

Are you writing the relation at the sketch level or the part level? The same dimension has a different name depending upon where you are using it. If you write the relation while in the sketch, use the sd0. If not, use the d7. It's rare (at least for us) to write relations at the sketch level.

[IanEdwards]

I am writing the relation at the part level. So yes, initially I used d7=DV_DIA.... the only way to then modify my diameter was to revise the parameter accordingly, perfect. But I was supprised however that the dimension in the sketcher was modifyable. Maybe I could enter a relation in the section sd0=d7?

[RussDavidson]

It should use the part relation for that dimension once you exit the sketch and regenerate the part even though you modify it in sketcher. I doubt it would let you use that section relation, seems circular, but I guess it could be interesting to see what it does.

[DavidButz]

Ian, Russ is right in his last post. When you are in the isolated environment of the Sketch it isn't at that moment looking at the part level relations to see if there is a conflict. The main reason folks need to use the sd numbers in relations is to be able to have the dimensions vary along the development trajectory of a Variable Section Sweep. Another use is to make dependencies within a Sketch, so that changes to one Sketcher dimension can drive others, e.g. sd7=sd5/3. David