MINIMUM DIMENSION ON DRAWINGS

[dbolden]

I need to define the distance between two edges.  They are both round.  I want the minimum distance and not the center to center.  How do I do this both in the measure tool and also in my drawing.  See below:

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[StephenW]

In the measure tool, by default it will go to center-center on radii. Unclick the "USE AS CENTER" in the dialog box.

In the drawing, in your example, I would create a dimension select the 2 radii and select tangent for both in the menu manager. It's sensitive to where you pick the radius, so don't pick to close to an endpoint.

Other methods for the drawing are to use intersect when creating the dimension (pick your radius and the centerline you have shown for each point) or to create the feature using a construction point and dimension it in the model and then just show the dimension.

[dbolden]

This is an assembly.  I tried to create a dimension in the model using the tangent and then vertical options but it still places a .376 dimension to the larger dimension.  I should be getting .002.  It snaps to the tangent further up on the top radii.

When I try to dimension within the drawing it doesn't let me choose (2) entities.  Even when I hold the control key when I click the second line it wipes out the first.

When I try to do this as construction geometry it doesn't let me exit the sketch because there is no real geometry.

[dbolden]

[StephenW · Accepted solution]

Use the intersect option and the ctrl key when in dimension creation.

Since it is an assembly, adding it to a sketch isn't really an option unless you are willing to add real curve geometry. Although at .002, no one would see it.  There also may be accuracy issues if the part is large and the feature is really really small.

Are you sure you are picking the right radius for the tangent dimension image, it shouldn't go to another radius, I've seen to jump to unexpected spots but never to the completely wrong radius.

[dbolden]

As I suspected I wasn't doing the intersect command correctly.  I didn't pick the second set of points.  I picked the first radii and the center line, but not the second radii and centerline.  I was holding the control key but not completing the selection set.

Thanks once again for your assistance.  I can always count on you to have a prompt answer

[StephenW]

Anytime...but don't confuse prompt with correct!!!