3 Replies Latest reply on May 26, 2012 3:44 AM by irmeli rehbein

    pipe, not sweep

    irmeli rehbein

      we all know, sometimes if you want to add a very shallow or steep chamfer (one direction is much bigger than the other) the feature does not work.

       

      pipe_1.JPG

       

      pipe_2.JPG

       

       

      now in other programs you have a pipe command where you select any 2d or 3d sketch and input the radius of the pipe.

      in solidworks i have to use the sweep command - so i have to create another sketch (circle) and extrude it along the 3d sketch.

      pipe_3.JPG

       

       

       

      with this swept surface i can trim away. bottom surfaces trimmed by big sweep.

       

      pipe_4.JPG

       

       

      i can use different radii for the trims. small radius for the top trim.

      pipe_5.JPG

       

      and from there i can loft these edges with compound curves.

      pipe_6.JPG

       

       

      the problem is - the swept surface is not a very clean surface. now of course i can't have a equal or bigger radius for the profile, than the minimal radius of the path curve.

       

      but even when i chose a smaller one, the swept surface is wrinkly (due to surface tensions) and results in a nasty trim. i checked all options of the swept surface like minimum twist etc..it often results in a bad surface when the radius is a bit big.

       

      --> so i wish we had a pipe command that gives me a clean surface or solid from a single 2d or 3d sketch.

       

       

      so here is a cumbersome way (on another part)

       

      again, i want a very shallow chamfer, going 1mm down and 3mm outside

      chamfer_1.JPG

       

      chamfer_2.JPG

       

       

      so from the top edge i use a ruled surface going inside the hole tangent to the surface. then another ruled surface going down, perpendicular to the first ruled surface. then again perpendicular to the second another ruled surface - big enough to penetrate the extruded hole. this way i now have a clean ruled surface with wich i can trim.

      chamfer_3.JPG

       

       

      trimmed away surface with ruled surface

      chamfer_4.JPG

       

       

      for the top surface, an offset curve from the original curve that create the hole is fine. i trim with that offset curve.

      chamfer_5.JPG

       

      now i can loft or patch the surface and filet it.

      chamfer_6.JPG

       

       

      i know there are many other ways to do this, i just wish we had a pipe command.

       

       

      EDIT:

       

      here you can see the chamfer feature fails, because in one direction the distance is too big (3mm)

       

      ch_feature_1.JPG

       

       

      with 2.5mm it works - looking at the resulting outer boundary of the chamfer the minimal radius at the 'waist' of the 8-shaped cut is big enough, it should even allow a 4mm chamfer in that direction - but it does not..hence the work around

       

      ch_feature_2.JPG