5 Replies Latest reply on Sep 25, 2009 12:46 PM by 1-4EQZK9

    90 degree loft problem

    Allen Miotke Jr

      I'm sort of new to solidworks...

       

      I'm trying to create a part in SW09 and I'm having trouble getting the loft feature to do exactly what I want.  I would really like to create this part without the split line through the middle but I am only able to create 2 seperate lofts instead of the 1 feature performing what I really desire.  The part isn't prfectly symmetrical, which also made it a little harder.  Perhaps there would be a better feature option to use in place of a loft?  Somebody help me, please!

       

      -Allen

        • Re: 90 degree loft problem

          Allen,

           

          Take a look at attached.  Although you can do it this way, if I were doing this part (depending on what it is - my guess a furniture piece given that your units are fractional), I wouldn't be happy with the surface transistions off of the corners. I would take a different approach to control those corners and how they flow into the middle of the surface. Perhaps someone else in the Forum community might want to take a crack at it to get the corners looking better.

           

          Regards

           

          Mark

          • Re: 90 degree loft problem
            Christopher Thompson

            Allen,

             

            Mark gave you a good example of the techniques required to model this part. From your original model, it appears you where trying to make a solid. Attached is this model completed as a solid using Mark's uploaded model as a template. I changed the conditions on the fill surface in the corners from tangent to curvature. Not sure if this can easily be improved upon, although I would be interested in seeing someone else's attempt to improve this model.

             

            To complete the solid, additonal surfaces need to be added, knitted, then solidified using the thicken command and selecting make solid. As I could not use the planar surface on an open sketch, I used the fill surface to close the openings in the model. The delete body (extruded surfaces) removes the construction surfaces from the model tree which are no longer required for creating additional features.

             

            Stationary-Block.JPG

             

            Regards,

             

            Chris Thompson

            www.appianwaytech.com

            • Re: 90 degree loft problem
              Kieran Choy

              Allen, the main problem with your lofts are that the end profiles have multiple sketch segments (lines, arcs) and the middle profile only has a single smooth semi-elliptical arc. In this part I've converted the end profiles to Fit Splines to get a smooth transition around the fillets - if you wanted more control over the way the fillets transition like Mark suggested then you could split the elliptical profile into an equal number of segments with the Split Sketch Entity tool.

               

              I've kept the part solid for the most part - and by adjusting the tangency weighting of the end conditions I've matched your side profile reasonably closely. If you want them to match more closely you can use two loft features like I have suppressed (loft1 and 2) to get more control over the tangency weighting of the center profile. Using tangency weighting instead of guide cruves makes for a better model.

               

              If the accuracy of the part isn't ultra crucial, you can ignore everything after the loft3 feature - here I've just cleaned up that bottom corner like Christopher and Mark.

              • Re: 90 degree loft problem
                Kieran Choy
                And here's how I'd do it with surfaces. Interestingly, the main surface worked better as a Loft than as a Boundary surface - Mark, does the Boundary Surface feature join profiles based on sketch segments? This is something you can control with loft but isn't available (as far as I could tell) in the Boundary Feature.