4 Replies Latest reply on Feb 18, 2013 4:38 PM by Adam Snow

    how to make facetings forms?

    Miguel Ramirez

      ho averyone.

       

      how to make a blow pet bottle with this amazing faceting in solidworks?

       

      example

       

      http://grabcad.com/library/mineral-bottle--1

       

      i thonk is fantastic job

        • Re: how to make facetings forms?
          Jerry Steiger

          Miguel,

           

          I would be inclined to try making a 3D Sketch with all of the facet edges, then build Planar Surfaces, Knit them all together, and Thicken.

           

          Jerry S.

          • Re: how to make facetings forms?
            John Burrill

            Miguel, that bottle was probably made using a surface imported from 3DS Max or Maya.

            Those programs have mesh based entities that can be modified with noise to produce that random-faceted look.  Usually, those surfaces are saved as 3DS or OBJ files.  If you have the ScanTo3D plug-in, you can import those files into Solidworks and then use replace face to substitute a smooth cylindrical face with them.

            • Re: how to make facetings forms?
              Adam Snow

              The original question is "How to make a similar shape in SolidWorks". Unfortunately the answer is “not very easily”. If doing it in SolidWorks, I think the best results could be had with a 3D sketch. You’d draw in all of the facets and then “fill” in the wireframe with the Planar Surface, Fill, Loft, or Boundary Surface tools.

              How long would it take to create? I’d say at least an hour or two of 3D sketching. How long would it take to modify later when the tool maker asks for something that can be molded… Well, maybe a bit longer.

              I cheated to form my bottle by using the “Triangle Reduction” tool in the Materialise Magics software.

              1. Sketch the bottle in SolidWorks. Here I just traced over the original image (that is slightly tilted) with lines, arcs and splines.
              2. Revolve the SolidWorks sketch into a solid body.
              3. Split the body into a top and bottom.
              4. Export the bottom as an STL file and open in Materialise Magics.
              5. You might be able to skip Magics at this point by experimenting with the STL export settings from SolidWorks. Exporting a file at a very low resolution may actually give a similar result, and you could just open the STL file again in SolidWorks to see the results.
              6. Two notes on taking STL files into SolidWorks:
              7. There is a limit to the number of faces that SolidWorks will allow to open. Since the goal is a faceted model, this limit should not be reached in this example.
              8. SolidWorks by default will open a STL file in Graphic mode, meaning it is just an image. So make sure you set the option to open STL files as a Solid Body.
              9. In Magics, run the Triangle Reduction tool until you get something nice and faceted.
              10. Export from Magics as an STL or 3D DXF file. I choose the DXF option since STL into SolidWorks can be messy. Plus, I had never tried the DXF option before.
              11. Import the file into SolidWorks. Here you can see that lots (82) of surfaces were created, but none were stitched together. Import Diagnostics would not run either, so…
              12. Knit the surfaces together. I did it in three steps here (yellow, purple and green) because things were slowing down when selecting lots of surfaces to knit at once.
              13. Knit, Fill and finally turn the imported surfaces into a solid body.
              14. Insert – Part and bring the upper body into the now faceted lower body. Using the Move/Copy command, you’ll be able to “mate” them back together.

              Eight Steps.jpg