I have a 3d wire frame which gives the geometry of a pipe that I want to create.I tried using the convert entities tool and make a surface out of it to thicken it and make a pipe but for some reasons my sketch was not converted .I have also attached the file in this post.
The way I did it was to use the wireframe as a skeleton to base planes and sketches upon, and then use the sketches to create a swept boss/base for the pipe.
The end of the sweep didn't match up exactly with the curves and sketch on that end of the pipe, so I overshot it and added one of my favorite tricks, using a surface and 'replace face' to get it just right.
I didn't bother with the wall thickness, you can 'shell' it, or edit the profile of the sweep to get that to your liking.
AttachmentsPipe Bend.SLDPRT, 630 KB
Making two assumptions, this is another way:
The assumptions are:
- The ends are meant to be circular
- Each cross section is the same diameter
1- Use Composite Curve to create three curves to represent the curve of the pipe. These should be spaced about equally around the circumference
2- Create a reference plane on each end through the three points formed by the ends of the composite curves
3- Sketch circles on the new planes. Relate the diameter of the circle to pierce each of the composite curves
4- Loft from circle to circle using the composite curves as guides.
If the pipe diameter varies, additional planes and circles can be made for each segment.
If the outside of the pipe is supposed to be smooth additional steps can be taken to convert each composite curve into a 2D or 3D sketch, then the Fit Spline tool can be used to make the multi-segment curve into a smooth spline.
Ultimately it depends on how accurately you need to follow this wire-frame, and what the end result need to look like.