How do a dimension the true (diagonal) distance between two points on a drawing?

dave_franchino

Hey folks,

I am truly stumped on how to get Onshape to dimension the true diagonal distance between two holes on a drawing. No matter what I've tried the dimension keeps snapping between the orthogonal horizontal and vertical. How can I get Onshape to show me the diagonal true distance between these holes?

Thanks!!!

StephenG

I know 2 workarounds...

1. Use "Maximum or minimum dimension (m)" and select the circle centers.


2. Create sketch that contains a construction line between the 2 points of interest, then use "Show/Hide sketches" to make the sketch visible in the view. Then you can use the normal "Dimension (D)" function, select the line to create a diagonal dimension along its length.

   

glen_dewsbury

2 point linear dimension will behave as you were expecting or pick the holes with basic dim tool not the center point.
Odd behaver to give only vert & horizontal when using basic dimension tool between points.

Hans_Leirvik_1

Create a plane that goes through the two points.
Select the plane and press keyboard N to view it from top.
Then create a Named View.

In a drawing create a View showing the part/assembly and select the Named view.

Now you can dimension the two diagonal holes in the drawing.

Yann_Roth_91

https://forum.onshape.com/discussion/comment/81586#Comment_81586

It's not in my case, the 2 point linear dimension also only allows to have horizontal or vertical dimensions. Feels like a bug to me.

I managed but I had to initially place the dimension very far, it was weird to find where the switch happened.

Oliver_Couch

https://forum.onshape.com/discussion/comment/107400#Comment_107400

I ran into this as well and submitted a support ticket. Apparently a change for drawings is in the works to make the drawing dimension tool behaviour match the sketch dimension tool behaviour.

Onshape appears to draw vertical and horizontal bounding boxes where it sets the dimension to be horizontal or vertical, respectively. It also maintains the current dimension type until the cursor goes outside the connecting lines. Once you go outside the connecting lines, it switches style based on the region the cursor is in:

So, to draw a diagonal/aligned dimension you need to first move your cursor quite far away to get outside the horizontal or vertical regions, particularly if the points you're dimensioni g between are far apart on your drawing. Then you can move you cursor back to where you want the dimension to be and place it.

Once a dimension is placed it remains horizontal, or vertical, or aligned, no matter where you drag the text value.