5 Replies Latest reply on Jul 10, 2012 8:17 PM by Andrew B

    Creating fillets between two curved bodies

    Andrew B

      I'm trying to model an impeller stage.  My work thusfar is attached as Impeller_Hub.sldprt.  I have an example which I am trying to replicate the general features of, attached as Example_Impeller.sldprt.  The main stumbling point is making the fillets around the impeller blades as they attach to the hub.  Specifically, I'm running to errors like "Laminar edges cannot be filleted", which as far as I can tell means that I need to knit the surface first, but then I run into errors trying to do that.  And so on.  I used the blade edges as guide curves when creating the hub, so I would think they would be coincident, but I'm not sure why I'm unable to create a fillet.

       

      I suspect that the problems I'm running into are the result of poor design choices made earlier in the model.  For example, I wasn't able to make a solid loft for the hub initially; I had to create a lofted surface and then a solid loft with merge bodies unchecked.  This is my first foray into using SolidWorks, so I'm sure I'm making some pretty obvious mistakes, but any advice anyone has would be greatly appreciated.

       

      Also looming in the near future are the fillets that would be attached to the shell.  In the example file, this appears to be done by creating a thin solid body parallel to the outer edge of the blade and filleting from that to a surface that is coincident to the surfaces of the blade itself.  Is that... feasible? 

       

      Thank you for reading!

        • Re: Creating fillets between two curved bodies
          Jason Swackhamer

          Andrew-

           

          Yes, the major problem is the loft. I tried some quick cheats and couldn't get them to work. To do this right, I think you need to replace the inner and outer faces of the  blades with revolved surfaces. This usually works better when you are trying to combine a revolved pattern of bodies.

           

          The problem is that you are starting with the 3d curves and a revolved shape works from a 2d sketch, so it gets pretty complicated. I reworked the part of the model before you lofts to modify it along these lines. Hope you can follow the changes and the logic behind them in the attached file.

           

          -Jason S.

            • Re: Creating fillets between two curved bodies
              Andrew B

              Jason,

               

              The 3d curves are design constraints, so I can't change the data points themselves, though if I can represent them another way, that would work too.  Unfortunately, I am unable to open your modifications, as I'm limited to SolidWorks 2010.  My apologies about not stating that earlier.  How did you modify things? 

               

              I tried making the loft as one piece (converted the 3d curve data to cylindrical coordinates and maked guide curves along the +/- x and y axes), but fillets with the blade edges didn't work there either.  So I wonder if the problem isn't the loft itself and is instead trying to do this kind of thing with predefined 3d curves.  Any ideas?

               

              Thanks for your help so far.

                • Re: Creating fillets between two curved bodies
                  Jason Swackhamer

                  Andrew-

                   

                  Ouch...I started to describe how I thought you might fix your model, but decided it would be easier just to send it back with the modifications. Oh well...

                   

                  Basically you need to get away from the loft and use a revolved body. I made the 2d revolve profile by using points at 10mm increments along the edge if your blade.

                   

                  Anyway, not at work now, but if I have time tomorrow, I'll send some jpegs of the sketches and feature tree. 

                   

                  -Jason S. 

                  • Re: Creating fillets between two curved bodies
                    Jason Swackhamer

                    Andrew-

                     

                    Plan B:

                     

                    You can get this to work with your loft. In both sketches 1 and 2, eliminate both the coincident relationships and set the center of the circle coincident to the origin. Leave the diameter dimensions. The sketch geometry should be black.

                     

                    Proceed past your circular patterns, and add a "move face feature" to the inside of each fin as shown (I used 1mm, but the distance is not important):

                     

                     

                    Capture1.JPG

                    Then combine the bodies:

                     

                    Capture2.JPG

                     

                    Cut the extra material off the bottom of the part, and now you can fillet:

                     

                    Capture3.JPG

                    -Jason S.