Hello guys,
I tried multiple profile sweep and loft in solidworks( image attached) but to no avail. Kindly tell me how to do this. Sorry for asking such a stupid thing. I use solidworks 2010.
Thnx
can you provide a 3d sketch of what you are trying to achieve, I can’t determine what the end result you want is from the above image. or email me your SW part and i will see what i can do for you.
looks like a circular path - why not just revolve?
Ditto. Revolve/Sweep the circular shape then you could cut away the rectangular sides at the top. Lofting never produces results you can count on accurately.
actually if you revolve you won’t get what you have drawn.
You have the sketch planes oriented vertically rather than normal to the path. this might be part of the problem you’ve got going on.
Also usually when i’m sweeping a path i won’t use a centerline; For example if I’m sweeping a circle i’ll sweep from a quad point.
Well, what I can tell is that your profiles aren’t normal to the ends of the curve, that’s a bad thing. Make a plane normal to the start of the curve and sketch your circle. You may need to make your path slightly larger or the start might undershoot. Use a surface sweep. Then use each blue plane in turn with a Surface Trim to cut the model back. Then use planar surface to cap the ends, and use knit with the option “try to form solid” to arrive to your desired shape.
You can do it with a solid sweep and some clever extruded cuts too, if you wish.
Thnx everyone. This is what I am trying to achieve(image attached). There is no multiple profile sweep in SW2010 and I want the end profile(N0 2) to be vertical(currently it is horizontal). Tried loft(2 circular profile and a U guide curve) but it says self intersecting.
Got to be the easiest and quickest way. IMO.
What sort of cross-section and path shape are you trying to achieve? If you want to have a circular cross section and a circular path, the start and end profiles each need to be an irregular oval.
If you really wanted to make the feature with the way you have drawn it out, here is a way your could do it:
- revolve a surface to make the whole part as ring
- create intersection curves in sketches on your two base planes and one on the center plane at the bottom – this will create your two spline oval and a circle for the bottom (circle might not be needed, but it does not hurt)
3)create two guide curves in a sketch that represent your ID and your OD - create a boundary surface (which can act as a multi-profile sweep) by selecting your one oval, then the bottom circle, then a second oval for your profiles in Direction #1. Use the ID and OD sketch lines as guide curves in Direction #2
- Create a fill surface on each of the open ovals
- Select your three surface bodies and knit them together. Select the “Try to form solid” box to make a solid part
That said, the easier way is definitely the revolve+ cut.
Thnank You guys.
Wods: This is a Loft with a center line not a sweep… also change the 2nd profile so that it reflects the end shape or just cut it off after the loft is done.