I am having problem with my sweep, My trajectory profile path is on the surface and the othe other one is trajectory but it doesn't work
please help me
and which version of Inventor???
Only going to annoy people if they spend time creating an example for you to say you're on a previous version and can't open it.
looking at the dwf I dont think sweep is the answer (and I'm wondering how it will mould).
personally would use surfaces as each "tooth" looks like a extrusion (presumably with a taper to be moulded) but instead of being a distance it's "to" a surface revolved around the body.
1) revolve body
2) revolve curved top of tooth as a surface
3) create a sketch on the base and extrude a tooth to the surface
4) create the hole on the inside
5) pattern extrusion and hole
You can try create a Loft feature starting in your sketch15 and end in a point (points also available to create Loft features) and then by giving the centerline to better control the loft shape.
I'm on 2011 so can't open your ipt and edit it.
here's a quick bodge that kinda resembles the dwf. Tbh, with more time I'd redo it and probably come up with something cleaner (especially for the tangent of the top surface to the draw-angle of the extrusion).
1) revolve the body
2) revolve a surface for the top of the tooth
3) extrude a surface for the exterior of the tooth
4) create "inside" surfaces of the above
5) sculpt a solid tooth
6) sculpt away the inside of the tooth
8) pattern sculpts and fillets
quick and dirty but might give you some ideas how to do it on your model.
(still have no idea how you would expect this part to be moulded/made though).
To achieve your sweep roll up the EOP below sketch 15
create intersection point(working point) with construction plane 15 and radius on sketch 15
after edit the sketch 16 and apply coincident constraint on end line and projected working point
try to built your loft with parallel condition and that's it
after use sculpt feature.
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