9 Replies Latest reply on Oct 17, 2006 10:01 PM by

    Drawing an Oval/Extrude on curved shape

      Shelling probably isn't the easiest way to make a multi-thickness curvey thing.

      In the attached, I created a separate body to represent the fluid chamber. I then used feature combine to subtract the fluid from the bottle. Note the trick of lofting to a point.

      Don't you just love cadjocky talk?

      Gerald Davis CSWP
      SW07 SP1.1 Office Professional
      2GB / Opteron 175 / FX3400 / ASUS A8N32-SLI
      http://www.cosug.com Colorado SolidWorks User Group
        • Drawing an Oval/Extrude on curved shape
          Hi,

          Can you walk me through shelling out a bottle
          into different wall thicknesses.
          I am getting lost with the help menu.

          Thanks,

          Julian
          • Drawing an Oval/Extrude on curved shape
            How can I show liquid in a clear bottle that has thick glass walls?

            Thanks

            Julian
            • Drawing an Oval/Extrude on curved shape
              > While in sketch mode, Tools>Sketch Entities>Ellipse
              Tools>Offset

              The ellipse is always dimmed when I am in 3D sketch or 3D sketch on a plane,
              I need to make a bottle cap that's oval at the bottom and round at the top, which means I need 2 different planes.

              Thanks for the help.
              • Drawing an Oval/Extrude on curved shape
                thanks,

                Julian
                • Drawing an Oval/Extrude on curved shape
                  on 2006 17 19:01 julian berard wrote:
                  > 1. Does any one know the easiest way to draw an oval in SW?
                  If by "oval' you mean ellipse, then the easiest way is to use the ellipse tool. While in sketch mode, Tools>Sketch Entities>Ellipse

                  If you're looking for a slot, then sketch a construction line that represents the distance between centers, then use the offset tool (Tools>Sketch Tools>Offset Entities...) and select Bi-directional with Cap Ends as Arcs.

                  > 2. How can I make a hole on the curved side of a cylinder?
                  Use the Hole Wizard.

                  > Thanks
                  You're welcome.

                  Gerald Davis CSWP
                  SW06 SP5.0 Office Professional
                  2GB / Opteron 175 / FX3400 / ASUS A8N32-SLI
                  http://www.cosug.com Colorado SolidWorks User Group
                  • Drawing an Oval/Extrude on curved shape
                    1. Does any one know the easiest way to draw an oval in SW?

                    2. How can I make a hole on the curved side of a cylinder?

                    Thanks
                    • Drawing an Oval/Extrude on curved shape
                      I'm not clear on why you're using a 3d sketch.

                      I used a pair planes separated by the height of the bottle cap.
                      On one plane I sketched an ellipse, on the other a circle.
                      I then extruded a loft between the sketches.

                      From there, you could add other details and shell the part to hollow it out.

                      Gerald Davis CSWP
                      SW06 SP5.0 Office Professional
                      2GB / Opteron 175 / FX3400 / ASUS A8N32-SLI
                      http://www.cosug.com Colorado SolidWorks User Group
                      • Drawing an Oval/Extrude on curved shape
                        Please see the attached drawing, I am trying to use Lofted boss/bass to cover
                        the surface all around this bottle shape but it won't let me select the top ellipse shape.

                        After this I want to create the thickness of the glass, the shape inside the bottle.

                        Thanks for the advice.
                        • Drawing an Oval/Extrude on curved shape
                          That's a lovely shape that you're designing. The problem was with the sketches that you were trying to use to generate the loft (too much stuff per sketch).

                          To get the loft to work, I created a plane that corresponds to your 3d sketch plane. On my new plane, I converted your round sketch to a new separate sketch. Using the front plane, I created 2 sketches that converted your 3d sketch curves into separate guide curves.

                          I then made a loft from the round to the ellipse using my guide curves.

                          Next step was to check the feature for minimum radius of curvature (Tools>Check)since I wanted to shell the bottle to hollow it out. The answer was 1mm, so I shelled the bottle with a .9mm wall thickness (very thin!). I did this just as an example of a simple shell operation. If you want variable thicknesses, read the help on shell. You might also consider modeling the interior volume that you want and subtract it (see Insert>Features>Combine in the help system).

                          I set the material to glass for show and tell.

                          Gerald Davis CSWP
                          SW06 SP5.0 Office Professional
                          2GB / Opteron 175 / FX3400 / ASUS A8N32-SLI
                          http://www.cosug.com Colorado SolidWorks User Group