15 Replies Latest reply on Mar 26, 2008 5:08 PM by Geno Phipps

    Converting surfaces to solid bodies

    Geno Phipps
      I am new to the software--not sure this is the right thread to post in--sorry if it isn't.

      I am working on a pump design and the part was drawn with mostly solids or solid bodies, that is sketches that were extruded. I was not able to draw all of it with solids however and had to also use surfaces. The areas that needed to be created with surfaces mostly deal with a helix shaped water path--picture one of those big spiral slides on a playground =)

      Anyway the part is all drawn now in the sense that all the surfaces are there I believe. Because this is a molded part and I need a finished thickness of .0625" I used the thicken command whre I could, and trim surface also. I ended up with a very muddled design tree that is nowhere near "best practices" but I do have my part =)

      The problem is I can't seem to convert the entire thing into a single solid body so I can add my fillets and draft. Is there a way to do this? I tried knit surface but it will not work in all locations.

      One of the issues I seem to have is that any circle or arc I draw is made up (at least the visual representation of it in the work area) of multiple line segments. Where another circle or arc meets these the surfaces of the line segments do not always lign up. The stated diameter/radius is the same but the line segments are rotated.

      You can download the file herehere (you will get a good laugh after the eye roll) if that helps.

      Thanks!



        • Converting surfaces to solid bodies
          Robert Hoyt
          I wish I could look at your model, but I'm still in '07. I've been doing a lot of pump modeling lately too, and one thing I've found helpful is to start with a model of the "water" inside the pump, and then shell with the "shell outward" command. Sounds like you're far enough down the path with your current part that to switch over to this paradigm would be a complete do-over, though....
          • Converting surfaces to solid bodies
            Charles Culp
            Geno,

            unfortunately, I can't spend the time to go through your model to find the details that don't work, but here are a couple suggestions:

            1. Instead of doing just the helical part as a thickend surface, and then trying to "clean it up" with solids, I suggest doing the "cleanup" work on the surface itself. You are running into at least two potential situations where there are areas with zero thickness. I suggest filling in areas with filled surfaces and boundary surfaces, and then thickening the whole thing as a last step.

            2. For any solid bodies to combine (Insert>Features>Combine), they cannot have an area of zero thickness, or where two corners meet opposite each other. The easiest way around this (although it may end up in longer rebuild times), is to just have the parts extend well into each other.

            Hope it helps, at least enough.
            • Converting surfaces to solid bodies
              Geno Phipps
              I tried it as a solid volume and then cutting material away but I hit the same snag. Then I did just the water surface and tried thickening outward--it runs for quite a while (say 2 minutes) then says the geometry could not be created.

              It is very frustrating because I know it is my 2D CAD way of thinking that is the issue, not really the software. I have redrawn the part 4 times 4 different ways and just sttall out at the helix/spiral.

              Maybe the 5th times the charm =). Thanks all for the suggestions.
              • Converting surfaces to solid bodies
                Geno Phipps
                Dwight, Again, that is a big help, thanks. Not sure how I will tie it in to the 45 degree inner beveled portion yet, but that should not be a huge deal.

                It looks like the extrudes 28 and 29 use a different end condition. 28 is up to body and 29 is up to face--is that on purpose? Also, I am not clear on what purpose sketch 61 serves...is that just some of my garbage left over? So does Solidworks just ignore when one extrude overlaps or extends into another and just sees the whole outer "skin" only as the solid? I think I had that part wrong in my head because of using the surface tools.

                I have been drawing on that for a solid WEEK! Thanks again.
                  • Converting surfaces to solid bodies
                    Dwight Livingston

                    Geno Phipps wrote:

                     

                    It looks like the extrudes 28 and 29 use a different end condition. 28 is up to body and 29 is up to face--is that on purpose?

                    SW wouldn't extrude the whole loop up to the whole spirol, so I did it in two steps. For some reason, the second extrude woudln't go to the body, so I tried the surface and that worked.

                    Also, I am not clear on what purpose sketch 61 serves...is that just some of my garbage left over?

                    Yes, just left-over garbage.

                    So does Solidworks just ignore when one extrude overlaps or extends into another and just sees the whole outer "skin" only as the solid?

                    Very much yes. Overlapping extrudes combine to a single solid. Very powerful. Complex surfaces may not fit perfectly and will be hard to combind surface to surface, while an overlap may prevent those problems.

                  • Converting surfaces to solid bodies
                    Geno Phipps
                    I am trying to do the rest now (the center). Not having a lot of luck but I am pretty slow at this still. I tried building out the rest of the shape first (continuing as you did) then using the shell feature but as before, it just won't do that. Now I am going to try to carve it out from the top down and see how that goes. If that doesn't work I will try doing the center as a separate shell maybe. I think the problem is really that the top of the ramp has a different profile then the bottom...which is why I started messing with the surface tools in the first place.

                    If I am still stuck tomorrow I will ask for another pointer.

                    I appreciate you sharing your knowledge.

                    • Converting surfaces to solid bodies
                      Geno Phipps
                      Yeah, I only added the fillets to be sure I could--having finally gotten one solid body part thanks to you =)

                      I also didn't get that after each extrude etc that it really is one body. This morning I tried it with one step and of course it worked. I guess at my age it sometimes takes longer to "un learn" old things then to actually learn something new.

                      The odd split was the small cheat I mentioned. The method you showed me with hollowing out the outer shape (shell tool) will not shell the part if I do the complete part then shell, so I don't know any other way that doesn't get me back to using the surface tools.

                      The part is being cast in acrylic and they insist it will do fine. Not my area so I follow their instructions. If I were paying for the tooling different story.

                      Thank you again for taking the time to help with this.
                      • Converting surfaces to solid bodies
                        Geno Phipps
                        Whoops...Just noticed the this question has been answered check box!