I have a drawing that has a section through a radius. When I dimension in section view, it has an 'L' prefix that I can't remove, it is not in Dim prefix dialog. When I put 'R' in dim prefix dialog, it appears before the 'L'. Same radius in non-sectioned view dimensions as expected. I have another radius that has to be dimensioned in section view and it is doing same thing.
Radius is on an imported body. I deleted original radius in sychronous and readded with no change to 'L'.
What am I missing?
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Check the placement of the section cutting plane. It is probably off-centre by a poofteenth. If it does not pass exactly through the centreline then the section radii will be splines (curves) instead of circles and you won't be able to apply a radius dimension. Instead, the L-prefix will appear. So something is off in your geometry. Maybe a "live" rule somewhere is subtly playing havoc. Note also the 5.3 dimension does not have a diameter prefix either.
Chrisstandring's reply led me to find cause of 'L' prefix in my case.
Attached picture view with cutting plane. The part was an imported solid body that had been done in Pro-E. In left view, the top and bottom R. 4.0 radii were not on the same centerline as the 3 hole features in part. Very small offset that was not apparent, 0.002mm (0.00008"). The cutting plane was snapped to the R. 4.0 radii and thus did not cut through the centerline of the hole features or the R. 0.2 radius that was giving the 'L' dimension prefix. I replaced cutting plane using the 2 smaller holes as positioning points for cutting plane and the radius now dimensions as intended.
I will corect model to fix alingment issue, so future use of model do not cause issue.
Thank You !
It would be useful if you could adjust the precision required before that happens. .002mm might be significant to some but not at all to others. And what is the required precision now? Is it 4 places? 8? 12? Infinity and beyond?
I seem to recall reading somewhere that geometry created in ProE sometimes has issues with accuracy and that can become apparent when exported to other CAD platforms. As it has done in this particular case. Nobody would deliberately make the outer radii 0.002 mm off-centre from the holes in the model unless there was some special reason -- and looking at that piece -- probably highly unlikely to be the case. Making the CAD modelling precision lower would be sure to cause all kinds of mayhem.
My intent wasn't to say make the modeling precision lower but to make the sectioning tool more able to round off so if it sees the .00008" offset it makes the section a true radius instead of a spline.
Just suggesting a possibility. Especially given that there are, as you suggest, known innaccuracies in translation. So either fix the model translation or allow the drafting to adjust per user parameters.
My personal opinion is that having the sectioning tool bahave the way it does provides an excellent flag for alerting the user that something might be amiss with the geometry. So I say keep the accuracy setting (or rounding) for sectioning just the way it is. That way you can catch the error early before it comes back later on to really bite you in the arse!