Dimension by midpoint between a sketch and the edge of its part

3D Design Volume Model
1

Hello everyone,

 

I would like to know how to dimension a sketch by the midpoint of an edited part in an assembly.

I know that by right-clicking on my line I managed to access the midpoint, only after selecting the midpoint I can no longer select the edge of my piece (Unable to select).

And conversely, when I select the edge of my piece, I no longer have access to the right-click menu to select the midpoint.

Is there a solution other than putting a dot or making a construction line on the edge of my part, to be able to make a dimension between sketch elements.

Or, is it possible to make a midpoint dimension between the sketch and the part, and what is the way to do this?

Hoping I have been clear enough.

Thanks in advance

2

Hello

Don't get tired, create a shot going through the midpoint of your sketch  piece and in the constrained assembly with this plane.
 

may the force be with you.

 

2 Likes
3

Hello

An image of your problem would be more telling, but I'll draw a construction line through the midpoint and then I could place the dimension.

3 Likes
4

Hello

Which version of Solidworks?

I do the following with sld 2015

Quotation

Right-click on the line to be constrained by the middle

choose "Select midpoint"

Click on an edge in the room

Position the dimension

the opposite does not work

4 Likes
5

you need to create a line passing through your axis in a perpendicular plane and coincident with this said axis

and you dimension this line at the point of intersection line/axis at the circumference of your circle

see attached

@+ 

1 Like
6

Hello

@yoan.pacquelet's answer is correct, so if you can't do it, is the "Do not create external references to the template" option unchecked? (he had to uncheck it).

Kind regards

PS: the other solutions offered are also correct but require the creation of additional entities.

1 Like
7

At the time for me, the " Select midpoint " appears at the end of the drop-down menu for a dimension, unlike a normal selection where it appears at the beginning. Adding an entity is not useful.

Tricky !

Check what @jmsavoyat says, it's definitely the cause.

8

Hello

Note that on the 2012 version, in edit mode in an assembly, after selecting the midpoint of the sketch line, the edge of the part you want to dimension (with this midpoint) does not go into protrusion when you hover the mouse over it, but it is selected anyway if you click on it . 

1 Like
9

Hello

There is also the solution of placing a coordinate system on the edge, the simple CLI on  the stop and then coordinate system automatically places it in the middle.