Concentric circle dimensions

[tct]

In Sketcher, is there a way of constraining the radii/diameter of two concentric circles relative to each other?
Basically something similar to the bottom right annotations illustrated here:

[openBrain]

There are basically 2 simple ways.
The first is to use expressions.
The second is to place 1 point on each circle, constrain them to be horizontally (vertically) aligned with the common center, then fix the horizontal (vertical) distance between them.

[chrisb]

Add construction lines and equality constraints:

[MisterMaker]

I ended here after searching if this was really how I should do it.
Freecad is the only CAD software that I know off that cannot place a dimension between to circles.
I don't think this is on purpose.
Should I make a feature request for this?

[jmaustpc]

Freecad is the only CAD software that I know off that cannot place a dimension between to circles.

three ways were just mentioned, by the way we are talking about constraints not dimensions, two different things.

[papyblaise]

or you place a point on each circle tangent to the circles and to an axis line and you measure the space from point to point
I will thus have faith in my life to use the point tool

[watsug]

three ways were just mentioned, by the way we are talking about constraints not dimensions, two different things.

Isn't op talking about dimensional constraints? The distance between the circles lines, dimensioning the difference of radius.

[jmaustpc]

three ways were just mentioned, by the way we are talking about constraints not dimensions, two different things.

Isn't op talking about dimensional constraints? The distance between the circles lines, dimensioning the difference of radius.

there is often a lot of confusion between constraints and dimensions, they are different things.

dimensioning the difference of radius.

no, this topic is about constraining a radius with a constraint, one specific set of constraints are described as dimensional constraints but not all and even those are still constraints that constrain geometry.

To put it simply, a dimension object/tool in FreeCAD reads a value from something, the constraint forces something to have a value or do something else of a non-numerical value, like tangent etc. Depending on context a dimension could be an aspect of an item e.g. a line length could described as its dimension, but something else creates or forces that dimension (a property, a constraint, etc.).

[jmaustpc]

point on each circle tangent to the circles

that is not right, you can not apply a tangent between a point and the circle edge in sketcher. You would use "point on object" constraint.

Every way has advantages and disadvantages.

Point requires you to add a distance constraint between each point, if the circles radii increase by the same amount as the OP asked then a construction poly line is better like Chris said, because you can just add a set of "equals" constraints.

Also tangent has a relatively high computational cost, better to use something else if possible. Same with point on object, better to use only use "point on object" for the points or poly line nodes to the circles and only one of them to the axis, the rest of the points or line segments can then just be constrained with a "Horizontal" constraint.

of course an Expression applied to their radii has a lot of flexibility, as the Expression can read a value from anywhere and even apply maths to it.

[papyblaise]

that is not right, you can not apply a tangent between a point and the circle edge in sketcher. You would use "point on object" constraint.

What is your remark
I place the point on the circle, then I made this point tangent to the OX axis, and the proof by the image is correct