6 Replies Latest reply on Apr 8, 2009 12:42 PM by Mark Matthews

    ProE convert needs help!

    Brian Kurn
      I've had SolidWorks about 2 weeks and I love it - with some exceptions. I'm sure you guys can remedy that situation.

      I'm trying to create an editable model of a 4-valve exhaust port that will be used for CNC machining. I have surfaces of a hand-ported head that I've imported and copied using 2 boundary surfaces. I tried using lofts but I was unable to achieve smooth surfaces. Here's what I did:

      1. Imported surface
      2. Built centerline curves through ports using 3D sketch
      3. Created points along those curves and created planes normal to curve
      4. Used Intersection Curve command to create chains for reference
      (The imported surfaces were made up of many small patches and the intersection curves wound up with multiple points per chain - not always the same number of points per chain)
      5. Used Fit Spline command to create splines that I can use for loft or boundary
      6. Created both boundary surfaces, trimmed overlapping surfaces and knitted together

      What I wound up with is a surface that desperately needs a more uniform divider between the ports! The surface looks terrible and the divider has some unwanted curvature.

      How can I fix this? Better yet, How can I model this geometry more efficiently in SWx 2009? How would you SolidWorks Jedis do this? In the future I'll be creating the surfaces from scratch.

      Thanks for the help! I am a big believer in forums and this one is a very impressive community. You'll see me here often!
        • ProE convert needs help!
          Mark Matthews
          First off i would not use so many sections for the Boundary surfaces, try to use as few as possible. Don't use intersection curves directly, just use them as guides and create your sections from scratch; you'll end up with more control and less complex splines. Are those two round looking flanges at the top really round? If they are then start with those sections that are truly round as revolves. Are these surfaces mirrors of each other? If so build one side and mirror it. Don't just try to intersect the two legs of the ports together as you will get an unpredictable intersection; instead trim them away from each other and create more new surfaces between them to join them.

          You can use loft to do this one leg at a time; have you tried the "centerline" option using the 3-D curve as the centerline?

          Did you make this originally in Pro-E? Are you a proficient surface creator in Pro or are you new to surfacing? If this wasn't made in Pro originally, what program was used and why not use the originial data for machining?
            • ProE convert needs help!
              Brian Kurn
              I have a few years under my belt surfacing in ProE but I wouldn't say I was proficient. I worked with many people in my last job who I relied on heavily to show me the ropes in ProE. Most all my experience has been modeling 2-Valve NASCAR port geometries.

              The imported surface was created by reverse engineering a hand-ported exhaust port by a Scanning/Reverse Engineering vendor. The point cloud was manipulated in Geomagic.

              I created several planes because I wanted the SolidWorks surface to follow the imported surfaces very closely. I also wanted to have better control over the cross-sectional area throughout the ports for future models. The client (friend) came to me because he wanted to clean up the ports a little bit. They were ported by hand and the surfaces leave much to be desired. Since this will be mass produced he wants the finished product to be more aesthetically pleasing. I've never done a 4-valve head before. He knows that. I took the job as a favor to him and to learn SolidWorks.

              This geometry is not symmmetrical but the intake ports are. I will use your advice. Thank you for the guidance!
              • ProE convert needs help!
                Brian Kurn
                How would you reccomend creating the sections on each plane? In ProE I used 4 conic arcs. I'd create a vertical and horizontal axis and connect the 4 conic arcs between them. I'd then dimension the points connecting the arcs and then adjust the arcs' own dimensions (the arcs would also share a common axis when constrained tangent to one another) for full control to match nearly any geometry. SolidWorks 2009 has no conic arc function that I am aware of.

                I realize that by using splines I can copy nearly any shape very accurately (probably more accurately than conic arcs) but for me, the strength of the conic arc lies in its ability to be easily dimensioned. I can make an exact duplicate of a section just by dimensioning the two sections identically. Using splines I'd have to fiddle with them, drag, push, pull and even then it would probably never be an exact match.

                Got any suggestions?
              • ProE convert needs help!
                Charles Culp
                I don't have time to go into great detail, but you can set the curvatures on the spline points equal to each other, or give them tangent lines (create construction geometry, and make the spline tangent to the line, or dimension the tangency directly). You can also dimension the strength of the tangency. It is not easy, nor should you dimension every single point.

                You can also create reference geometry, where you create a surface that doesn't go into the final part, but you can use the edge of that surface as your control for the edge of the real surface.
                • ProE convert needs help!
                  Mark Matthews
                  Yes, conics would be nice to have; but as Charles says, you can use two point splines and fully dimension them, though you may find your sketches becoming over-constrained. They may not be geometrically over-constrained, but the solver SW uses chokes on me all the time when I'm making curvature constraints.