In this step, I will show you the designing part of Fusion 360. There are pictures of each step to help you orientate.

Images are in chronological order

Creating new component and drawing up a base sketch

  • First, I created a new component and named it «Base».
  • Next, created a new sketch on the XY plane. Selected 2-point Rectangle and used origin as the starting point. Both dimensions should be 100mm. This is the approximate stock size.
  • Then I selected tool «Offset» and clicked on the rectangle, (As seen on the image). Typed 1mm (or -1mm if sides are switched so that the new rectangle faces inward). Selected the rectangle and changed it to «Construction».

    Now design will have a 98×98 actual size. Why? By taking 1mm from each side,I will have a nicer finished surface.

  • I used «Offset» tool again and offset 1st rectangle by 9mm. This is the width of the side. It’s a reference for the Voronoi pattern.
  • Using «Circle» tool and placing a 5,5mm circle between 2 and 3 rectangle in the middle (Dimension it from the second rectangle in the middle for 4mm) Dimension it from the side by 12mm. (See the image for help)
  • I repeated the process for all other 4 corners.


  • Using Extrude tool, I picked the whole sketch(including circles)and extruded it for 8m,

Getting the Voronoi Generator.

With Autodesk’s App Store, you can quickly search for any plugin and install it in minutes

  • Navigate to , select Fusion 360, and type «Voronoi generator», You should find a generator made by Autodesk. Select win64 version(if you use win), download and install.
  • Restart Fusion.

Using the Voronoi generator

  1. First, I hid the body I just created(So that only the sketch is visible).
  2. The plugin should be located under «Create» tab at the bottom. A box opens up where you can select the sketch or profile. Select the innermost rectangle and click on «use profile size«.
  3. The width and height should be exactly 82mm, add 3-4mm to both (The pattern has a «buffer» between border and cells). Click Voronoi editor.
  4. Another tab opens where we can generate the pattern.
  5. Cell style should be «curved«(as we can’t machine straight edges, but you can use it for laser cutting!),
  6. In the cell count slider, you can see the pattern changing depending on the number of cells, I suggest using between 20-30 cells as too much generates small cells which are impossible to machine (I’ve tried).
  7. Click publish. The sketch pattern should appear next to the sketch.
  8. Navigate to Top plane for a better visual, select the whole sketch and drag it into inner rectangle. Place it approximately in the middle (if you don’t see the sketch, double click on the sketch and edit it).


  1. Finally, I unhid the body, selected each cell, and extruded through(see image for help). Now that the base is finished (adding holes comes later), ill continue the work on the sides.
  2. Again, I created a sketch on top of the body. Used a rectangle tool to outline the part and offset it by 8mm(Width!). Added 2 small rectangles in the corner (each 4mm). I repeated this for each corner. (See the image for reference)
  3. The first side should be extruded for about 48mm without selecting squares (Don’t forget to select «Create new Component»!). I did the same for the other side but this time I selected both squares on each side, so the side is longer.

Now we have 1 base plate with 4 sides of which 2 are 98mm long and other two 90mm

By this point, we are half the way designing the box

Placing Voronoi pattern on each side

Instead of placing 4 unique patterns on each side, which would take a lot of time, I simply created just 2 and extend them to the other two.

To help me orientate I used «project» Tool(P key). Picked the inner face of the side I wanted to place a pattern on then. (see the image for more help). This is important as placing the pattern can be tricky

Important! To avoid any problems you should activate the component on which the pattern is placed.

I repeated the process by selecting the same face and used Voronoi generator. (in the Voronoi editor we repeat as before (20-30 cells))

A pattern appeares next to the model. I just drag it into our projected sketch and finished it. Again In the extruded box, I selected individual cells but this time I put direction as «Two Sides». Drag both sides to «cut through«(See image)

Tip! If Extrude command doesn’t cut through both components but just one, go back and in the Extrude box and in the «objects to cut» select both bodies/components.

After finishing one side, I repeated the same process for the other side. But this time I edited the projected sketch and offset it additionally by 4mm on each vertical side. (See image). Then I placed Voronoi pattern and extruded the same as before.

Now our box is almost complete. The only thing that is missing is the holes for screws.

By this point you can also 3D print the box, just use combine tool to merge all the components together for a better printing experience(i printed each separately to accurately see the design).

I flipped the part and used «Holes» tool. Using 1st sketch(Where I created 5,5mm holes), I placed each hole. The hole is around size 3mm and depth 12mm (m3 hex screw!). In the hole type, I used «Counterbore» and made the «hat» of the screw 5mm in diameter and 3mm in length (See the image)

Tip! Check the box Modeled. This will model our threads as we need them for our 3D print.

But wait, after analyzing the design I realized that the screws intersect with our pattern, so if I were to machine in this state, the screws would be visible, which would make the box look ugly. In order to fix this, I used «Analysis» tool(which cuts through the model unveiling the problem),

I selected the side and drag it until I saw the screws. Found the right Voronoi sketch and using Arc and Spline tool shortened up the pattern, so the screw will have a solid body to thread in (See image for help).

Great! Our box is finished! Now onto 3D printing!

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