Positioning on the face of a surface with snaps

[gtz01]

Suppose that I have an extruded object I want to make a sketch on.

Object

• gtz01
• Apr 8, 2021

Something common I might do is create a sketch to cut a hole on either side, or at the midpoint of the object. So, using the measuring tool I can take the lengths of the sides of this object and figure out where the midpoint is, offsetting it from the origin using construction lines.

Forced Midpoint

• gtz01
• Apr 8, 2021

But this seems like "reaching around your head to touch your nose". It would be far easier if I could snap a construction line to the midpoint of the surface in question and then project a construction line from that point. Additionally, this would make finding the midpoint of shapes that are not linear far easier.

Is there a way to do this that doesnt involve this way?

 

[HaroldL]

Start your sketch then select either the face or the edge then use Project to Sketch to create Reference geometry. You can then sketch from the circle to the Mid point of the edge reference line.

 

[OTE_TheMissile]

I'll often do something similar to what Harold suggested. In my case, if I wanted the circle to always be at the geometric center of the feature, the first thing I'd do in the Sketch is draw a reference line diagonally across the part, then Coincident constrain the endpoints to either of the parallel edges. That will cause the edges themselves to appear as reference lines with their own endpoints, so I'll Coincident constrain the endpoints of the diagonal line I drew with those so they stay exactly at the corners of the part.

Then I draw a circle on the midpoint of my diagonal line and I'm done.



I've also done it in the other direction where if the circle in the center of the part is more critical than the body of the part, (i.e., if the part is symmetrical in both directions) I'll start by centering the rectangular Sketch around the origin, then draw the circle Sketch directly on the origin.

 

[Oldbelt]

Keep it simple

 

[idslk]

Hello @gtz01 ,

have you taken a look to the reference videos? This one will show you one solution (of a lot) for your question...
Btw. you can put images from the snipping tool directly into your posts without using the gallery...

Regards
Stefan

 

[OTE_TheMissile]

Or if you REALLY want to look clever...

 

[DV410]

I make a habit of always trying to draw things centered on the origin for this reason and also in that it often makes assembly constraints easier.

Drawing the box, use the drop-down to choose the "Rectangle by Center"
Click the origin, size the box and then add a horizontal or verticle constraint.
Extrude, but choose by Type = Midplane

This puts the box centered on the origin.
Then, add a sketch on the face and the origin is in the center ready for a circle to be snapped to.

I feel that this is fewer clicks than drawing diagonals and can aid in further processing later.