I have a project that requires numerous planar patterns to be projected onto various angled faces of the model. Unless I'm reading the help file wrong, the projected curve function only works with cylindrical (or maybe curved) faces and not flat ones. I have tried projecting a sketch onto a sketch (empty sketch on the target face open) and sketch to a face. Neither will give me full projection of all entities. The entities are either lines or arcs. Am I missing something here or is this something for another app or an add-in?
Think of projected curve this way - sketch onto sketch - it creates a curve in space that would be identical to the edge you would get at the intersection of an extruded boss from sketch 1 and an extruded cut from sketch 2
Sketch onto face - it would generate a curve identical to the edge you would get if you extruded a boss up to a surface.
If you are not getting the full curve, there can be several issues - are all the sketches single contours, or do you have multiple strings of edges with some gaps between them? A projected curve has to be a single string (I've used this as a workaround in the last couple of days to get around issues with certain intersection curves and 3D sketches that can't be used as loft edge, guide curves, etc because of little gaps due to round off errors. I make the projected curve, then convert that into a 3 sketch - its the same curve, but guaranteed to be continuous!)
There can also be -intermittent- problems if the sketches intersect in space (I.e one is on the top plane, one is on the front, and they are both centered on the origin) In this case, moving one off to the side will remedy the situation. Its not always necessary, but its useful to know you have a fallback position.
OK maybe I am missing something. You are creating a composite curve of a projected curve. Unless it is a set of projected curves on that face, then I could see the reason for doing that. Other wise it seems like a double step. Ed's work around using the 3D sketch "convert entities" is a nice way to go. For some reason SW will not allow you to project more than one profile in a sketch at a time. (annoying) Matt's answer, if I understand it correctly, is another way if it is a feature that you can pattern after you create the first one.
I guess my question would be is this a path that the robot will follow? or it is being used for something else?
Ummm... that shouldn't be a problem at all if the two lines are a) in the same sketch and b)share an endpoint (the lines are merged together into a single contour). I learned a neat trick on this newsgroup a while back about evaluating sketch contours (wish I could give credit by name - sorry) - RMB a sketch segment and choose 'select chain' from the context sensitive menu. If your whole sketch lights up, then it is valid for a projected curve. If only part of it lights up, then you have a discontinuity.
I then extruded a surface, using
This is EXACTLY what a projected curve should give you, minus all the extra steps - you would get the 'intersect curve', without having to extrude the surface and manually create an intersect curve, if I understand you correctly. Odd that it doesn't work - I'd pass it by your VAR to root out bugs.
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