Edit the sketch, Select the sketch from part navigator > RMB > Edit Parameters.
You can select a dimension from GUI or from a list of expressions that are displayed in the 'Sketch Parameters' dialog. Use slider to vary the dimension value. You can also click on the slider and use mouse wheel to see the changes to the dimension in GUI.
I have a sketch line of the length p32=p10*0.67. This dimension appears in the Sketch Parameters list, but can't be adjusted with the slider. Then I create an expression myFactor=0.67 and make p32=p10*myFactor. But I find that the expression myFactor does not belong to the sketch and would not apprear in the Sketch Parameters list.
Is there any workaround to add the expression myFactor to the sketch? Thanks!
While the sketch is active, you can still access your user expressions with Tools-Expressions, or in the User Expressions folder in the Part Navigator.
Something you need to keep in mind is that all expressions have units. When you give an expresssion in a sketch like A*B, one variable has the units of length and the other is dimensionless. Using Expressions, you have full control over the units.
As far as I know, there is no slider on Expressions. And if you think about it, the entire part might have to be resolved for every motion of the slider.
Expressions that are defined using the expression editor can be used in the sketch on the right hand side of p# expressions. As already mentioned by @MarkLawry , slider in the 'Edit Parameters' on such expressions will not work. These expressions will be visible under the 'User Expressions' folder in the part navigator.
On the other hand, if you define the expressions while in the sketch edit mode, they will be listed in the 'Edit Parameters' dialog and can be varied with the slider. If you look in the expression editor then source of such dimensions will be sketch. Note that they will not be listed in the part navigator under 'User Expressions' folder.