I have a pretty straighforward setup which i want to se to create a lofted surface in SW 06. I have three planes, 2 with profiles and one with a guide curve. The guide curve is a spline,and it has coincident relations to both profiles on each end. Profile one is drawn on the “right” plane, and profile 2 is drawn on a plane that is directly parallel to the “right” plane. The guide curve is drawn on the front plane, which is by default perpendicular to the right plane. However, when I try to create the lofted surface, I get an error massage saying "guide curve no. 1 is invalid. It does not intersect with section no. 1. I don’t understand why this happens because this is how i normally loft surfaces, and like I mentioned before, the guide curve is coincident to the profiles. Any idea how I can fix this?
coincident doesn’t mean it is pierced. you should click on the spline points individually and delete all their relations. then click on one end again hold cntrl down and pick the first curve. relation box comes up then check pierce.same with second. now loft.
in solidworks when picking guidecurves make sure you pick them on the same alignment. then you can go back and edit tangents with guides provided. tangency is an important factor in lofts. use the mesh by right clicking to see it better once the loft is completed.
thanks ufo. I’m still having a bit of trouble. In followed your directions, but I was only able to pierce one point. When I tried to pierce the remaining endpoint to its respective profile, the only relations that I could assign were concentric, coincident, and fix. I tried lofting with with pierced end and one coincident, but it didn’t work. Any suggesions?
Can’t give you specifics, but you’ll find a load of info in these downloadable ppt presentations.
UFO is right, you must have the endpoints of that spline pierced to the profiles. if you can’t pierce to one of the profiles, then that profile does not intersect the sketchplane of your guidecurve.
Be sure the endpoints nearest to the front plane are coincident to your Front plane (guide curve sketch plane) for both profiles.
if you fix your point it wont move, so it wont pierce either! as i mentioned earlier get rid of all your relations first and make sure your profiles or sections are intersecting the front plane and are fully defined. to check if a section is intersecting the front plane you can use the grid “on” or “shaded plane” option for better visibility.
it’s best to use construction geometry and try to make a habit of it. i know it takes time to set it up but it’s the professional way to do design.
thanks so much guys!! Great advice…