5 Replies Latest reply on Jul 12, 2009 3:29 PM by Dwight Livingston

    Pattern on a conical helix

      Guru's

      I am designing a finned tubing for a conic spiral heat exchanger. Creating the tubing was the easy part. I can't figure out how to pattern a "washer shaped" extrusion (representing the fins) about the helex. I tried using the "by curve", but the protrusion stays parallel to the sketching plane of the fin and I need it to be radial. My sketching plane is radial.

      Does anybody know how to do this?
        • Pattern on a conical helix
          Charles Culp
          In the Curve Driven Pattern:

          Select Alignment method:
          -Tangent to curve

          Face normal:
          (select the conical face)

          If the conical face isn't actually continuous, breaks apart, or is oddly shaped, you can make a dummy object (just make sure it is a separate surface or body), and use that as the "face normal".
          • Pattern on a conical helix
            Charles Culp
            No problem. Create a conical shape using the circle you created to make the helix. You can probably just extrude it with the appropriate amount of draft. Make sure to click the checkmark for "merge" so that it is OFF. That way it will create a solid body that does NOT merge with your helix shape; it will be two separate solid bodies. Then you can select the exterior of that face as your normal face. Then, in the curve driven pattern, make sure it does not merge all the bodies together. After you complete the pattern, you can then hide that body.
              • Pattern on a conical helix
                Finally got it to work. However I could not find in the curve pattern where to "not merge all the bodies together". Instead, I used a surface instead of a solid for the cone. Also you have to pick the normal face before the feature to extrude.

                Thanks for your help Charles!
                  • Pattern on a conical helix
                    Dwight Livingston
                    Greg

                    I believe Charles was saying to uncheck "merge" when you extrude the first instance, before you make a pattern feature. That way you make a separate solid body. It is sometimes easier to pattern a solid body rather than an extrude feature. Once you have made a pattern of solid bodies, you can use a "combine" feature to make it all one solid body.