# Labyrinth Puzzle Box

27,763

392

38

## 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 ( https://www.instructables.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
• That's it - using this same approach and steps you can design any kind of labyrinth box, easy or hard, with the maze on the inside or outside of the cylinders, even do the nesting variations where you have multiple mazes nested inside each other. Hope you found this useful, having fun making your labyrinth boxes

## 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.

## Recommendations

127 6.3K
53 8.5K
20 2.6K
88 8.3K

• ### For the Home Contest

A clever device! It could be made more difficult if the 'peg' was further from the rim, i.e. deeper down inside the tube. That would make it less easy to see which bit of the track you're currently following.

Made one and didn't like the vertical Z seam (probably my printer) so decided to embed a pattern. Chose a sword because it has straight lines. First pass had the pattern raised and printed on the surface. Not much contrast. Second embossed in the cylinder. Better and might be improved with paint. Third printed the sword in two colors and glued to the cutout in the cylinder. Tried various colors and settled on the hilt in black and the blade in grey. It is a gift to a puzzle nut so I am not willing to attempt to solve.
I think this is justification to get a 3D printer with multiple extruders. Thanks for posting.

That looks epic!

Made it as well, such a well written and executed little project, cheers & thanks!
printer: Ender 3, black (PLA) and bronze silk filament (PLA+PETG)

Thanks! That looks sweet - especially that bronze filament, great job!!

Thanks for a great Instructable. I've learned some new tricks in Fusion 360, as well as being able to create one of these for myself. I am in the middle of producing one to fit inside a soft drink can that has been sliced at the top. The maze is on the inside panel of the outer tube, not on the outside of the inner tube. That is so they can't see any of the maze while they are trying to get it out.

I will also then have a second tube inside the first, but I see someone else has already thought of that. Mine will be used as a Geocache container. It will look just like a piece of rubbish on the ground. Once found, they will then have some fun trying to open both tubes to get to the log.

That's a fantastic idea! Please post back a photo here when you are done - I'd love to see that!!!

This is the cache so far. I still need to create the final centre tube to hold the cache log.

Also, when creating the maze part in Fusion 360, I found it easier to draw it as construction lines, then create the offsets as normal lines. That way, it is easier to work out what is what, rather than turn the maze lines to construction lines after the offsets.

Brilliant! That's awesome. Thanks for the tip - it can get super confusing, especially when you are making a more detailed maze.

I love this, it's fantastic. There is a project available online that generates these given your required size and difficulty etc. The project is available here: https://www.me.uk/puzzlebox/ for anybody who is interested. It's nothing to do with me, I just got told about it and have printed a few

Many many cool points for doing it yourself!

That is super cool! And here I am, doing it by hand like a sucker ;¬D) Thanks for sharing the link!

Is there a version of this for Inventor?

Hi William, unfortunately I haven't used Inventor, so I can't speak to the differences in the approach, but I suspect it's similar. Because there is no Wrap command to get the maze path onto the surface of the cylinder in Fusion 360 you have to go through the whole sheet metal unfolding process. If Inventor does have a wrap feature I suspect you could use that and save yourself some steps.

Thanks for revealing the printer used and the tut on how to design in F360. When you describe the progression in fuse, it is 100% that you'll create the part.

Also, most anyone can use 360 free. Be honest when choosing the level. Students and any biz earning less than 100 k is eligible.

Thnx

Ge begint met het tekenen van een cirkel en verder spreekt ge over een cilinder. En wat is dan de hoogte van die cilinder? Wat is het nu eigenlijk. 1 keer zie ik 25mm staan op het voorbeeld en daarlangs 40mm ik begrijp het niet meer. Ik hoop dat dit ook voor beginners bedoeld is. Ik heb Fusion 360. U spreekt over het snijgereedschap maar waar vind ik dat, bij mij staat trouwens alles in het Engels.

Hallo Guido, de basis van het maken van de holle cilinder is: maak een tekening met zowel de binnen- als buitencirkel erop. Wanneer u vervolgens het gebied gaat extruderen, kunt u alleen het gedeelte tussen die twee cirkels selecteren en dat gedeelte extruderen. Het snijgereedschap bevindt zich in het menu Wijzigen en heet Trim (in het Engels). U kunt het ook selecteren door op "T" op het toetsenbord te drukken. Als de tool is geselecteerd, zal Fusion 360 elk stukje geometrie dat kan worden verwijderd uitlichten, en als je erop klikt, wordt het verwijderd. Hoop dat dat helpt!

Since I don't have a 3D printer, how do i purchase one of the maze's

Hi there, the easiest way would be to download the STL files from the instructable, and then search online for a 3D printing service. You will then be able to upload the STL files and get a quote for them to make one and send it to you. I have no idea what the cost would be, you can look at a service like https://www.3dhubs.com/3d-printing/ and the nice part about it is that you can select the material and colors you like. Hope that helps!

very cool puzzle! wonder how difficult it would be to make a 'nesting' puzzle a la matryoshka dolls (russian nesting dolls) - that would be fun?
thanks for posting - will have to wait to get out of covid lockdown to access my public 3D printer - darn

Hiya, thanks for the shout out! Nesting puzzles are definitely a lot of fun. The four parts at the top of the main image in the instructable are exactly that - the smaller one goes into the medium one, and then that assembly goes into the larger one which is finished with the top cover.

The process to design the puzzles is basically the same as shown here, the main differences are that you would repeat Step 5, only placing the drawing on the inside surface of the unwrapped sphere. You would also need to consider the thickness of the cylinder as well as the depth and width of the path, to make sure that you don't end up with holes in the cylinder. So for example if you make the cylinder wall 5mm thick, you can have a maze path on either side with a depth of 2mm and still have a 1mm wall between them where the paths cross. And a path of 2mm deep would mean that the width of the top surface of the path would be 3.8 mm wide (1.9 mm offset from the centre of the path) which would allow an angle of 44 degrees for the side walls of the path, giving you that V shaped groove (which is ideal for 3D printing).

The second thing to keep in mind is that when the inner components are completed together, the base of the inner cylinder needs a slot aligned with the opening at the top of the outer cylinder in order for it to fit into the next cylinder, but again the steps in this instructable can be applied to make that happen. Definitely something I'd like to try in the future, and if/when I do I'll add some additional steps to show how it's done.