Select general dimension, select the first line, select the a second line, RMB, "Intersection", select a line that forms the intersection you want to dimension from.
Thanks for the response. I have been trying that method, but it keeps selecting the center of the arc (40")and not the intersection point of the line and the arc. What I have is basically two parallel horizontal lines and two large circular arcs for vertical segments. The top and bottom lines are offset laterally about 50% of length to form a sort of parallelogram shape with the arcs. Each of the corners / intersections are filleted with various radii (3/8" to 1"). I get the same problem trying to select both bottom or both top corners to get an overall horizontal dim to the intersections. Any suggestions? I can dimension to the centers of the arcs, but my fabricators (this is glass) need the intersections for laying out the shapes.
The problem may be the radii. Because you have an arc that is tangent to the radii, I'm not sure it will recognize the apparent intersections. I'll give this a try and see if I can make it work. I would ask you to just post the file but I am using IV8 and I can't read a ver10 file.
Alright try this, when you draw the part, do not trim the ends off of the arcs. Put the fillets in without trimming. Then dimension the part, but add in dimensions to the intersections as reference dims. Then in the idw you can retrieve those reference dims. You can change them to regular dimensions if you want in the idw but I would dimension it as you would normally and then leave the other ones on as reference for the fab shop.
Thanks for the help. I had been doing two things wrong. One was I made my fillets in sketch mode rather than applying them to the extruded model body. Secondly I was not dimensioning the sketch so I had nothing to retrieve. Again, thanks for the help and time spent.
It is always a bad idea to leave a sketch unconstrained. It WILL come back to bite you on the hindquarters, garaunteed. I make it a point to constrain my sketches to the origin point and then I build my model the way I would manufacture the part. It works well for me, and anyone that comes back to work on my part can usually figureout why and how I built something.
