I was trying to do the part of modelmania 2006 (photo 1) and I was using revolve cut instead of sweep cut.
Solidworks gives a rebuild error "sketch is open, self-intersecting, or intersect the centerline."
Can someone tell me what this error means?
1) "sketch is open"- the sketch is definitely not open, that's for sure.
2) "self-intersecting"- is it the arc profile and the vertical line? it doesn't look like that. (photo-2)
3)" intersect the centerline"- wth does this means- it can definitely be used when making semisphere revolve cut or other situation. (photo 3 shows the centerline intersect/coincident with the revolve cut profile near the red mark.)
Also if I use that profile shown in photo 3, Revolve cut works just fine. Can someone tell me why the revolve profile in photo 3 works but not the one in photo 2?
I am expecting an explanation for avoiding future mistake. Thank you
The profile can not meet the centerline at just a single point (or at multiple single points; 2 in your case). The resulting tool body that it creates for the cut would have zero thickness geometry at the two points where it meets the centerline. The profile in your 3rd image works because the extra lines at the end connecting to the centerline remove that zero thickness condition. It is always good practice to "overbuild" your cutting goemetry anyway; just like in both of your profile examples, you have made the line defining the outside of the revolve much higher than the part height itself, it is good practice to do that on the sides too. Here is a help topic that explains zero thickness:
http://help.solidworks.com/2019/english/solidworks/sldworks/hide_non_manifold.htm
By the way, I do hope that you figured out that the revolve cut will not make the correct geometry as compared to a sweep for this model. AS shown in the image below, the geometry is correct at the R32 end but at the R20 end, the top radius will be R20 with a revolve, not R32 and then at the transition from the large arc to the small arc in the revolve profile, it is an even smaller radius and that edge is perpendicular/normal to the bottom edge of the model, not normal to the top curved surface of the part as the drawing specifies.
-Jim