Introduction: Labyrinth Puzzle Box
Like many other people, I came across this puzzle box on Thingiverse by SneakyPoo (https://www.thingiverse.com/thing:201097) and after printing it out and playing with it I was struck with how much fun it was, and wanted to see how to make one from scratch.
Instructable-er adena2 has an excellent instructable ( http://media.nbcmontana.com/Labyrinth-Puzzle-Box/) which shows a similar process. The main difference between that instructable and this one, is that rather than having the maze hidden inside the cap, this one has the maze on the outside of the inner core. The method used to create the maze is a little different as well, so between these two instructables you should get a clear idea how to go about making one of these fun puzzles.
- Fusion 360
- 3D Printer
Step 1: Create and Flatten a Cylinder in Fusion 360 - Part 1
- In a new design in Fusion 360, create a new sketch on the XY plane. Using the circle tool, create a circle with the diameter sized to the inside of the cylinder. In this case I want the inner diameter to be 25 mm
- In order to unfold our cylinder, we will need to have a small cut in the geometry. Draw a line that intersects the circle, and then create an offset of that line at a distance of 1 mm
- Using the trim tool, trim the small piece of the circle between the two lines. You can also turn the two lines into construction lines, just to make them easier to distinguish
- Click finish sketch, and click the Sheet Metal tab in Fusion 360
Step 2: Create and Flatten a Cylinder in Fusion 360 - Part 2
- Select the Flange tool from the Create menu and click and drag on the circle path to start to create a cylinder. Enter the height that you want for the maze, and click OK to create.
- Note that in the Flange dialog, the default sheet metal material that is selected is Steel (mm), the first one in the library. Now that you have the height of the cylinder set, we will adjust the wall thickness to what we want
- In the Modify menu, select Sheet Metal Rules, which will open the dialog for the material. Hover over the material name and you will see a small edit icon (pencil) appear. Click on it to edit the material specs.
- In the Edit dialog that appears, change the value of the thickness to whatever you want for your wall thickness. In this case I will make it 4mm thick, which will allow me to have a groove in the surface as deep as 3mm.
- Make sure to do this at the start, as the thickness is added to the exterior diameter, which is where we are going to make the labyrinth so we want this dimension to stay fixed.
Step 3: Create and Flatten a Cylinder in Fusion 360 - Part 3
- In order to unfold the cylinder, Fusion 360 needs a flat surface to reference, so we will add one to one side of the split we made in the cylinder
- Zoom into the edge of the split and select Extrude from the Create menu.
- Click on the face and create an extrusion that is 0.5 mm wide. This will create the flat reference plane. Make sure that Join is selected in the Operations dialog
- Click Unfold in the Modify menu and in the dialog make sure that All Bends is checked, and then click the outside surface of the small extrusion we just made
- Click OK and this will unfold the cylinder into a plane, with the exterior of the cylinder facing out
Step 4: Create and Flatten a Cylinder in Fusion 360 - Part 4
- Before we get to drawing out the maze, we need to close that small remaining 0.5 mm gap in the cylinder to make it 3D printable
- Click Refold Faces in the sheet metal menu to return the sheet metal object to a cylinder. Note it's important to click the Refold Faces button rather than do an undo command, because we want to have the unfold and refold steps captured in the timeline for the next step
- There are a couple of ways to fill this gap, the way we will use is to create a loft from one surface to the other. Switch the top tab from Sheet Metal to Solid, and select Loft from the Create menu
- Select the two opposite faces and make sure that Join is selected in the Operations menu. Click OK and the cylinder should be complete
- If you try and do an Unfold at this point, you will get an error, but since we have our earlier Unfold command captured in the timeline, simply move the timeline marker to just after the unfold command and you will see the cylinder open up again. We are ready to add our maze!
Step 5: Create the Maze
- Create a sketch on top of the exterior side of the flattened cylinder and this is where we will create the maze
- If you like, you can edit the grid settings to help make things line up and by turning on the snap to grid. note that in this case I want to use a groove that is 3 mm deep, and has a 45 degree angle on the sites. This means the width of the path at the surface needs to be 6 mm so I set that to the grid size to make it easier.
- Create the 'right' path that will allow you to unlock the cylinder. Starting at the top edge create your path using a series of lines.
- I've also included a small horizontal length at the bottom which will help lock the box together I'm keeping the last path 6 mm from the bottom of the cylinder to account for the fact that the pin will be below the top edge of the cap
- At this point you can go ahead and add all the false paths, or even a second 'right' path if you wanted to have that option.
- Remember that we added a 0.5 mm flat plane to allow us to unroll the cylinder, so make sure that any lines that cross the edges are extended so they go right to that edge
Step 6: Create the Grooves in the Cylinder
- To create the grooves in the cylinder face, we are going to use a simple extrude command, and using an angle in the cut will give us a triangular profile for the groove. The reason I want a triangle shaped groove is that you will get the cleanest 3D print with 45 degree overhangs without having to use any supports
- Since our groove will be 6 mm wide and 3 mm deep, we will create the extrusion profile by offsetting the paths by 2.9 mm each side of each path and then joining the ends. Note that the reason we are using 2.9 and not 3 mm for the offset, is that in the case where two paths are right next to each other, there needs to be a tiny amount of material between them otherwise the area will be combined together.
- Using the offset tool, select a path and create two offsets at + 2.9 mm and - 2.9 mm. Once the paths are created, to make things a little clearer I change the style of the original line in the middle to construction
- Using this basic technique work your way around the paths until they are all offset. Note you may have to do some trimming / extending lines to get everything right. Don't forget to close the paths anywhere they touch the outside of the plane, or where a path ends
- You should end up with one or more fully connected paths you can use to extrude into the cylinder surface
- To create the grooves, use the Extrude command. Extrude a distance of -3 mm, and in the Taper Angle field use a value of -44.0 degrees (normally we'd use -45 degrees, but since we made the paths slightly narrower, you need a steeper angle to avoid any errors)
- To check if everything is working correctly, in the design timeline, roll the marker right to the end and you should see the grooves wrap around the cylinder
Step 7: Extending the Grooves Across the Edges
- There is at least one spot where you will have to cut away some material, and that is at the top of the cylinder where the maze starts. If you have any paths that span the section of the cylinder that is split, you will have to make sure those are open as well
- Roll the marker in the timeline back to the point where you extruded the grooves
- Create a new drawing on the top surface. To make it easier to see the geometry, select "Shaded with hidden edges" from the Display settings. Use the line tool to create a triangle that matches the profile of the groove
- Using the extrude tool, cut through the top edge of the cylinder and move the marker in the timeline to the end to make sure it's on the correct edge
- Use the same process to connect any paths that cross the seam of the cylinder. Because we used a Loft to bridge the gap, it will automatically match the openings assuming they are aligned correctly, as shown in the image
Step 8: Finishing the Bottom of the Inner Cylinder
- Create a new drawing using the bottom face of the cylinder as the reference plane
- Create a circle from the centre of the cylinder to the exterior. Create an offset of that circle equal to the wall thickness you plan for the cap (3 mm) plus a small amount of clearance for the cap (1 mm)
- Extrude the entire face on the drawing to create an area you can grip when you are solving the puzzle. It can be whatever you want, 8 mm seemed to work well for me
- You are done with the hard part! Next, we'll create the pin that rides in the groove and then mesh that with the top cap
Step 9: Creating the Guide Pin
- Locate the area at the bottom where the pin will be located in the closed position. Use the Offset Plane tool to create a plane that intersects the cylinder in the middle of the groove
- To make it easier to see, select Section Analysis from the Inspect menu, and click the new construction plane
- Create a new drawing on the same construction plane to start to create the pin
- Draw a circle from the centre of the drawing that is 1 mm wider than the exterior of the centre cylinder (this accommodates for the clearance on the inside of the cap)
- Draw a line from the centre to outside the edge of the larger circle, intersecting the section where the pin would rest
- Using the line tool, create 1/2 the shape of the pointer, making sure that the shape crosses the circle which represents the inner surface of the cap. Click Finish Sketch
- To create the pin, we will revolve the triangular sketch around it's center axis. Select Revolve from the Create menu, select the triangular area as the profile, and the line running to the center of the circle as the axis.
- Hide the section analysis to show the entire pin to make sure it still fits in the groove
Step 10: Create the Outer Shell
- Using the drawing you created to form the base of the inner cylinder, create another offset from the centre circle by .5 mm. This w ill give you the clearance on the inside of the cap
- Extrude the outside of the cylinder to the top of the inner core. Make sure that New Body is selected in the Operation field to create a separate body
- In order to give a little clearance for the top of the lid, extend the height of the cylinder by 1 mm using either a Push/Pull or Extrude operation
- Create a new drawing at this new top edge and create a circle the diameter of the exterior of the cap. Extrude the top cap to the same thickness as the walls
- Combine the outer cap and the pin together into one 3D printable object by selecting Combine from the Modify menu, and selecting the cap as the target body, and the pin as the tool body. Make sure that Join is selected, and click OK to combine. Tip: select the two bodies to join by clicking on them in the Browser Tree on the left side of the screen. It's much easier than trying to tumble the model around to find the bodies
- If you hide the inner core and look inside the cap, you should now see the pin on the inside surface
- That's it you are done! If you want to do things like add a chamfer, or a logo in the top of the cap etc, now's the time to do it and you are ready for 3D printing
Step 11: 3D Printing Your Parts
- These parts have been designed to be printed on any FDM type printer without needing any supports. You can see from the section analysis, that all of the features are created using a 45 degree overhang which allows you to print without needing supports
- Of course you can also print this using a SLA printer, which would mean you can make the walls of the grooves steeper or even square
- The main challenge I've found with some of these parts is making sure that they are firmly on the printer bed as they can come off when you are printing tall skinny things. I've found using a raft gives me the best results, but as long as you have a well dialled in printer you should be fine
- FYI settings I used for the examples you see in here:
- Printer: Craftbot Plus
- Material: matte PLA from Overture, silver and copper silk PLA from Eryone
- Temperatures: 199 / 70 for hotend / platform
- Layer Height: .2 mm
- Print Speed 55 mm/s
Step 12: STL Files
If you just want to skip straight to the print and play part, here are the STL files for the parts that were produced as a result of this instructable.
UPDATE: I've made some small tweaks to the original STL files to make the cap fit a little more snugly (basically increased the size of the pin in Step 9). In addition, I've also created a version with a smaller size groove for the maze which means the maze is a little longer and more of a challenge.
The process is the same, but I set the grid to 4mm, created the maze as before, and then offset it by 1.9mm each side of the line. When extruding the maze into the cylinder, it was extruded 2 mm instead of 3, with a k-43 degree angle to form the groove. Repeat step 9 to size the pin to the new groove size and end position and those are all the changes you need.
The STL files for both size of maze are below, and I've included a small insert that fits into the design at the top of the cap which may help you along if you get stuck :¬D)
Step 13: Circle Version!
When looking at making the maze pattern, it struck me that there's probably no reason you have to stick with horizontal and vertical lines, so I thought I'd try a version that includes some circles. So I came up with the random pattern you see here, and are ready to print it off. I have no idea whether it's going to be easier or harder to do, but it sure looks interesting.