SKETCH GEOMTRY ON PRINTS

[chris14]

The vast majority of our parts have a taper on one end (Morse Taper).  The taper is defined by an angle and a certain diameter at a certain distance from the end of the part.  The taper extends well past this gage point in both directions.

Our QC manager, who also lords over the prints, wants there to be a dimension for the taper diameter at the gage point.  I can sketch a line at the gage point no problem and dimension the line.  The problem is he wants me to remove the line, but keep the dimension.

The QC manager has been using white out on the prints to remove the line.  He then scans this print and puts it in the drawing folder.

Is there any way I can hide the sketch line and retain the dimension???

Inventor 2024

Thanks,

Chris

[ampster40]

one possibility is you can enable Tangent Edges in that view in order to be able to place a dimension there but even if that works I suspect in reality that should be a reference dimension only.

[jeremy_wasserstrass]

Could you make a sketch on the correct plane on the part and create 2 work points at the gage line, then in your drawing view include those work points to dimension from?

[kacper.suchomski · Accepted solution]

Hi

If the sketch is made in the drawing environment, you can edit the sketch after creating the dimension, point to the line, and select Sketch only.

[chris14]

That did the trick.  Thanks!

[b.mccarthy]

@chris14 

There is another option I have used:

• In the model, create a work plane (Test Plane below) where the taper is defined:

• In the drawing view, RMB on the Test Plane and select "Include"

• The plane will appear on the drawing. Add your dimension:

• RMB on the projected plane and uncheck "Visibility":

• The line will no longer be visible, but the dimension persists:

• Updates to the model are reflected:

Thx.