I am trying to dimension a bean shaped part that has two different radii. One is set from the center point, while the other is set .225 inches away from the center point. My problem is that the bean shape is extruded, drafted at 5 degrees, and rounded at a radius of 0.016. When the rounded radii are suppressed, the bean radii are correct and snap to the correct points, but when the bean is rounded the bean radii are off by 0.001. Is there a way to get the true radii values while the bean is rounded?
The values of R. 0.237 and R. 364 are the correct values I am trying to achieve.
I don't support you can upload the part file without violating and intellectual property or export rules?
The edge that you have without the round is not there when rounded as there is no "Edge" geometry there to dimension to. Because of the draft, when the round is applied the edge moves slightly down the drafted face therefore the dimension you see when it is rounded is the correct radius.
In your draft, you're likely dimensioning to tangent edges instead of the actual radii. A tedius solution would be to project an outline sketch onto a plane above the feature before adding the corner radii and drafts. You can then show and dimension to the sketch on your drawing. A section view might be a bit easier.
It would sure be nice if Seimens could develop a view option to overcome this. The software can calculate a tangency, why not a theo. sharp corner.
I would create a section and dimension to the intersection as shown in Ken's sketch.
It would be much clearer that way.
Other option would be to create a Simplified part rep with rounding removed. You can then place a view of the Simplified version in your Draft as well.