When I am drawing things (Assembly) in SolidWorks, on some parts which I work on, I can select the edge of a circle and then measure the dimension to a line, like shown below:

Measuring Edge of Circle

But the problem is that on some others I simply can't. It won't allow me to select the Edge of a cirlce when I hold down the SHIFT key. If I "insist" and drag the measurement to an edge, it jumps to the other end, like shown below:

Opposite Edge selected

I think I'm doing everything right: Doubleclick Sketch to edit it, select a line, then hold SHIFT and then try selecting the edge of a circle. I already searched on the internet around, but no one had really a solution for it. The closest I came was this.

Why does it work on some projects and on some others it don't?

Any help is greatly appreciated.

EDIT: I'm using SolidWork 2016 Premium x64 (SP 0.0)

  • $\begingroup$ I can't quite recall, I now use NX, but does Solidworks have selection filters? $\endgroup$
    – Petrichor
    Feb 8, 2018 at 11:37
  • $\begingroup$ @Petrichor Yes, it seems so (help.solidworks.com/2014/english/solidworks/sldworks/…) $\endgroup$
    – Fusseldieb
    Feb 8, 2018 at 11:40
  • $\begingroup$ @Petrichor Even using filters, it won't let me select the edge and if I use SHIFT, the selection disappears completely. $\endgroup$
    – Fusseldieb
    Feb 8, 2018 at 11:50

1 Answer 1


You can achieve this simply and quickly by adding a point to the circumference of your circle. I like this method because it's easy to see exactly where the dimension is going to, and it's robust in the case where the line become non-horizontal etc.

point on circle demo

You can achieve this more 'officially' by using the 'minimum' arc condition in the 'leader' tab of the dimension properties. I don't like this method, because relying on manually altering dimension properties doesn't sit well in my personal workflow. You may prefer it, though.

dimension options demo

A more pertinent point, however, is that it's not good practice to dimension a part like this, since that's not how it will be manufactured. If possible, the dimensions in your sketches should match with those that would be desirable on the 2D manufacturing drawing.

  • $\begingroup$ Thanks. Works just fine - finally. I personally prefer the second option, as the first seems like a little 'hack', but one last question: is that it's not good practice to dimension a part like this What do you mean with that? I didn't quite get it. $\endgroup$
    – Fusseldieb
    Feb 9, 2018 at 11:39
  • $\begingroup$ Imagine you are manufacturing a plate with a hole in it, on a milling machine. The position of the cutter is measured to the centre. Reading an engineering drawing that is dimensioned to the edge of the hole means that the operator has to add the radius of the cutting tool to calculate where the hole actually needs to be drilled. That in itself doesn't sound too bad, but, once you add in tolerances, then it becomes really annoying. If it's 0.95+/-0.1 to the edge of the hole, but the drill itself has a tolerance of +/-0.1 on the diameter of hole that it produces... See where this is going? $\endgroup$ Feb 9, 2018 at 11:56
  • $\begingroup$ Oh okay, thanks for the tip. As I only print out these pieces using a 3D printer, this doesn't represent a problem, and even if this piece would go for milling, those strange measurement formats won't "leave the digital format", as I would create a drawing in SW, inserting new measurements, measuring the center of the holes and stuff and finally print them out on paper. $\endgroup$
    – Fusseldieb
    Feb 9, 2018 at 12:35
  • 2
    $\begingroup$ In SW you can mark sketch dimensions to be automatically inserted into drawings when you get to the 2D manufacturing drawing stage, saving a whole lot of time! If you're going to get something made, It's worth setting out your sketches with that in mind during modelling. That said, for a quick 3D print, just do whatever feels best to you - remember "best practice" is a guideline, not a law! $\endgroup$ Feb 9, 2018 at 14:01

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