Tutorial – Faceted (Low-Poly) Shapes in Solidworks

Faceted Pocket AllAnother design and another excuse to share some of my modelling process using Solidworks. This can be applied to far more complex forms to achieve that faceted or ‘low-poly‘ effect with as much dimensional control as you like. Of course there are a million ways to skin a cat (or model a Solidworks part) and this is just the best process I could think of for accuracy on this particular design I’m working on. Feel free to leave a comment about your own methods or tips, I’m no expert!

Step 1 Give yourself some orthogonal views of the overall shape you want to achieve. This includes the triangles that will be used for the facets. For this one I just used a front and top view.

Step 2 Create a 3D sketch and connect all your vertices. Of course you can move things around if you like, but connecting back to those first sketches you set up really helps control the 3D sketch, which are notorious for having a mind of their own.

Step 3 Create another new 3D sketch, and convert just 3 lines from the previous 3D sketch that forms a triangle. Exit the sketch and use the Filled Surface tool to create a flat 2D surface.

Step 4 Repeat until you have enough flat surfaces to define your shape. Always be on the lookout for a pattern in your design – any opportunity to use the Linear Pattern or Mirror tools will really save time, so in this example I’ve only had to model 3 surfaces which I can later reflect to generate the larger design. Then Knit the surfaces together. The coming steps are where there are a number of ways to proceed, including use of the Offset Surfaces tool or Thicken. However these always result in messy, uncontrolled edges, so I’m not a fan. Instead I have setup another 3D sketch, and drawn some lines back in the z-axis from the vertices of the knitted surface – this will determine the thickness of the part.

Step 5 Repeat steps 3 and 4 to create another surface that sits perfectly behind (or in front of) the first.

Step 6 On the front plane (or whichever plane is the primary view) convert the lines of the outside perimeter of the surfaces you’ve created. These can then be extruded into a large block – just make sure you continue beyond the surfaces you’ve created.

Step 7 Use the Surface Cut tool for both knitted surfaces, making sure you cut away the block in the right direction. You want to be left with a solid only between the 2 surfaces. In the feature tree you can then right-click on the knitted surfaces and hide them, leaving only the solid material on screen.

Step 8 The hard work’s over, now use the Mirror or Linear Pattern tools to expand your design. You can also add any other details (in this case some cut-outs) before using these pattern features.

As I said there are many ways to achieve this aesthetic, and many other programs that you can achieve faceted objects far quicker. But if like me you’re wanting specific control of the facets and dimensions (rather than simply taking a shape and reducing the poly count), this might be useful. Please leave a comment with any questions, or like the post so I know it’s been useful for you. Happy cadding (if that’s a word)!

– Posted by James Novak

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One thought on “Tutorial – Faceted (Low-Poly) Shapes in Solidworks

  1. Pingback: Simple Facets in CAD | edditive blog

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