3D-Printed Stylish Wind-up Motor Car

Growing up playing LEGO and Gundam, I have always been fascinated by the process of putting together individual pieces to build something significant. I want to use this final project as an opportunity to explore the workflow of building a fairly complex design. On top of that, all the models and prints I have done for this class so far are static. It would be both challenging and fun to build something that can move.

When looking for inspirations, the idea of the music box came into my mind, which is an automatic musical instrument in a box that produces musical notes usually powered by wind-up motors. Music box has a rich history in both Asian and European countries and it represents brilliant engineering and craftsmanship. My initial thought was to build a simple music box, but it requires precise engineering that is way beyond my one quarter experience with digital fabrication. However, the idea of a wind-up motor does capture my attention. After some research and thoughts, I couldn't think of a better idea than building a 3D-printed wind-up motor car. I mean, who doesn't love cars?

I am going to use this instructables to fully document my final project -- it will not only contain the parts and how I model them, but also my learning process and how I approach the final product step by step. As a result, it is going to be long.

Here's the outline of this instructables:

1. Understanding of the wind-up mechanism and the basics of a toy car;
2. Modeling a wind-up engine set in Fusion 360 following this tutorial on Youtube by gzumwalt;
3. Modeling the transmission, frame, and wheels.
4. My attempt to make the car stylish by adding Voronoi patterns to the frame and wheel.

All the STL files are attached in the end. If you are only interested in printing and assembling the car, I also have printing and assembly instructions.

Finally, I want to give a huge shoutout to Greg Zumwalt (gzumwalt) for making an awesome tutorial of a wind-up motor car on Youtube. The step-by-step video tutorial means everything to someone like me who is new to wind-up motor design and Fusion 360.

1. Fusion 360 (with SpurGear and Voronoi Studio add-ins);
2. Ultimaker-Cura 5.0.0;
3. Ender 3 Pro;
4. PLA filament of different color;
5. Four 40*3.5 O-rings.

In short, the key to a wind-up mechanism is conservation of energy. There's usually a key or a knob which allows you to turn or rotate against a coil or spring. Since you're doing work against the spring's tendency to expand, the energy will be stored as potential energy once it is compressed. When you release the knob, the potential energy will be released, which will trigger the gear attached to spin. This will in turn drive other gears and mechanisms inside the toy to work.

For wind-up motor design, the end of the spring is usually fixed. A knob, which goes through the center of the spring and a gear, will be used to "add" energy to the system. Once the spring is released, the gear attached to the spring and knob will rotate, which drives the gears it is connected to. In this way, the whole system is moving. One thing worth noting is that there is a ratchet tooth in the inner of the main gear. The ratchet, together with a pawl, will only allow the gear to rotate in one direction.

A toy car usually consists of an engine set to provide energy, a transmission set to deliver the energy to the driving axle, frame and wheels.

Since I am new to Fusion 360 and engine set design, I decide to follow the Youtube tutorial by Greg Zumwalt for all the parts in the engine set.

I create a new component called knob and made a sketch for it. The center profile of the knob consists of a 6mm*6mm square and a circle on top of it. Then I make a 10mm circle for the knob bushing. Then I create the initial gripping surface segment of the knob and use a circular pattern to complete the profile.

The knob is finished with 3 extrusions. I used the parameters in the tutorial. I extrude the knob profile 24mm with a taper of -3 degrees. I extrude the knob bushing -5.2mm and the knob axle -33.2mm.

Finally I add color to the knob body to give it a finished look. This can be found under Modify->Appearance->Plastic->Opaque.

Next is the energy spring. For this part, I follow the tutorial to use the Fusion 360 built in Coil as the prototype and modify it to suit my needs.

Create a new component called energy_spring. Create a spring coil with the Fusion 360 coil, which can be found under Create->Coil. I use "Spiral" as the Type, 8mm for Diameter, 5 for Revolutions, 5 for Pitch, "Square" for Section, and 2mm for Section Size.

Then I create the sketch for the spring by projecting the coil and the knob axle. I increase the knob axle 0.1mm for tolerance. I add a 14mm centered circle for the spring hub and delete the unnecessary sketch. Then I add a spring end to the sketch by adding a 12mm diameter circle on the right, connecting the spring to it, and filleting it.

Finally, I extrude the spring for 9mm and the spring hub for 9.5mm. I add color to the spring and properly position it with the knob.

Next is the main gear. This is the gear that has an inner ratchet tooth.

I first use the "SpurGear" add-in to create a gear profile. This can be found in UTILITIES->ADD-INS->Scripts and Add-Ins->SpurGear(Python). The parameters I use for the gear are in the screenshot.

Create a new component called main_gear and project the 24 tooth gear just created. Create a 45mm diameter circle as the outer edge of the pawl socket. Then, draw a single ratchet tooth spanning 15 degrees and complete the pawl socket profile with a circular pattern. Make the sketch for the hub.

The main gear is finished with 3 extrusions. I extrude the gear teeth 4mm, the hub 2mm, and the ratchet teeth 6mm.

The pawl works together with the ratchet teeth in the main gear to ensure the main gear only spins in one direction.

I create a new component called pawl, and create a sketch for it.

I project a single ratchet tooth from the main gear into the sketch and provide a 0.2mm tolerance to it by offsetting the curve. Then I project the spring axle hole into the sketch and create the profile for the pawl hub. Then I make a centered circle with a diameter of 32mm and a line of 19mm and two copies of it with +-2mm offsets. I delete the extra sketch and use the 3 points arc to connect the "arm" of the pawl with its end. Then I create the remaining pawl arms using Circular Pattern to duplicate it for 2 additional times.

Finally, I extrude and properly position it between the spring and the main gear.

The second gear is directly connected to the main gear to transfer the energy released from the spring.

First, create an 8 tooth gear with SpurGear. The parameters shown in the screenshot.

Create a new component called second_gear and project the gear teeth and the center hole from the main gear, as well as the profile of the 8 tooth gear just created. Move the gear profile to the proper position and rotate the 8 tooth gear profile 360/16 degrees for the best fit. Then, sketch the hub and use the circular pattern to finish the profile for the second gear.

The second gear is finished by extruding the 24 tooth gear profile 4mm and extruding the 8 tooth gear profile 10mm.

Position the second gear in the right position, and this concludes the engine set.

The floating pinion set consists of an 8 tooth gear as well as an axle.

This floating pinion is an important part of the wind-up motor car and also a brilliant design by Greg Zumwalt. Essentially, it is a gear that traverses a guide slot. It engages the spring motor with the drive axle when spring energy is present and disengages the drive axle when the energy is depleted. In this way, the car is able to coast rather than stop immediately and moves a longer distance.

Create a new component called floating_pinion and create a sketch. Project the 8 tooth gear from the second gear and change the center hole diameter to 6mm. Then, extrude the profile 4mm and align it with second gear.

Create a new component called floating_pinion_axle and create a sketch. Project the center hole in floating_pinion and reduce it by 0.1mm for tolerance using the offset. Symmetric extrude the axle profile 8mm and position it properly.

The driving gear is connected to the floating pinion and is used to drive the axle that the rear wheels are connected to and move the car.

Create a new component called driving_gear and create a sketch for it. Project the floating_pinion to the sketch and create an axle hole with a hexagon with a parameter of 3.57. Here I choose the hexagon for the shape of the driving axle because it looks cool and has a smaller rotational initial. Extrude the driving gear 4mm and put it in the right position.

Create a new component called driving_axle and create a sketch. Make a hexagon with a parameter 3.56mm (1mm less than the driving gear for tolerance and fit) and symmetrically extrude it 26.7mm.

Now we have just finished all the gears needed for this car.

The purpose of the frames is to hold everything together. Basically it needs to encapsulate the engine set and provide space for the floating pinion and driving axles.

Create a component called frame_right and create a sketch for it. Project the center holes from driving gear, floating pinion, second gear, and main gear. Create the front and rear drive axle hole profile by making two circles of diameter 8.875. Do the same thing for the front drive axle. Then, create the floating pinion guide profile by keeping the area that the floating pinion sweeps through when rotating around the second gear for 26 degrees. Then, create the profiles for the crossmember, knob hole, and crossmember socket. Use the Fit Point Spline to join the center points of those profiles to create the base shape of the frame. Offset the curve in both directions for 7mm and delete the extra elements. Then, draw the curve to encapsulate the front and rear end to finalize the frame shape. Finally, extrude the frame 4mm, the spacer -11.6mm, shoulder -24mm, and the guide 17.6mm.

The left frame is almost the same. Create a new component called left_frame and project the left_frame into the sketch. Slightly modify the profiles for crossmembers and the socket for tolerance and fit and extrude.

Position both the right and left frames.

The final parts left for this car are the wheels. I will have different sizes and outlooking for front and rear wheels to make it more fun. However, all wheels will have the same structure -- hub, pattern, and outer loop. For this part, I will use the Voronoi Studio from the Autodesk App Store. Voronoi Studio is a very easy-to-use add-in that allows you to create a large variety of Voronoi designs both in 2D and 3D. You can get the Voronoi Studio here.

I create a new component and label it as front_wheel. I project the axle into the sketch and enlarge it by 0.1mm for fit and tolerance. The front wheel has a diameter of 45mm. I extrude the hub profile for 9.7mm and extrude the wheel profile for 8.3mm as a new body (do not choose join as I will manually join them later).

The next step is to use the 3D Voronoi Studio to add some patterns to the wheel body. Click 3D Voronoi Studio, which is under the CREATE menu, and select the wheel body as the Body to Fracture. Then click the Distributors to customize the patterns on the front wheel. 3D Voronoi Studio comes with 18 different distributors, and for each distributor it gives you the full ability to customize. It also has Live Update and Preview features. I highly recommend playing around with it a little bit, trying different distributors and other settings to choose the best pattern you like.

Specifically for the front wheel pattern. I choose a spiral distributor with 1mm Weld Threshold. I change the Divisions to 10 and 45% for the Radius 1 Size. I also choose to generate a Circular Pattern with 6 Quantities.

In the Fragments section, I unchecked the Fragments so it will only generate the Gaps for me, which is perfect for the wheel pattern. The final result produced by the 3D Voronoi studio with my parameters is shown in the attachment.

Finally, I offset the wheel profile by 2mm and extrude for a shell and join the three bodies to form the front wheel component.

This car is designed to be a rear-wheel drive car. For the rear wheels, I explore a different Voronoi pattern and design it 5mm larger than the front wheel to create some sports car aesthetic.

The whole process is the same as the front wheel. This time, I decide to try a combination of spiral distributors since Voronoi Studio 3D allows me to easily translate and duplicate the distributors. I first create a Spiral distributors with 6 divisions and 35% Radius 1 Size. Then, I duplicate the same distributor 4 more times, on left, right, top, and bottom of the circle respectively. The final result is shown in the image. I would argue it might be a little overly fancy, but it looks cool.

Now it's time to put every part in position and have a look at the car in Fusion 360.

I think I might have messed up the orientation of the frames in the Fusion 360 but I have fixed them in the STL files.

I have attached all the STL files here, as well as a link to a zip file that contains everything on the Google Drive.

Since applying 3D Voronoi patterns on the wheels is a huge success, I decide to add some voronoi patterns on the frame to make it more stylish and reduce the weight.

My plan was to make a copy of the left and right frames and then add patterns directly on them. However, I got "The current version of 2D Voronoi Studio add-in does not support profiles with transformed parent component(s)" error. I was not able to get rid of it so I exported the frames as individual files and edited them separately. I would appreciate it if people can offer any clue to this error.

I first offset the frame sketch to generate some areas where I can add Voronoi patterns. Then for each area, I use 2D Voronoi Studio and select the targeted area as Profile. Just like 3D, you can choose different Distributors and customize nearly everything. I highly encourage you to choose different options and play around with it. For Distributors, I choose the default Profile and I set the Weld Threshold to 0.4mm, which is the size of my printer nozzle. Then in the sketch, I unchecked the Border Padding and Cell Padding. Finally, in the Extra outputs, I click the Extrudes to have the Voronoi pattern cut from the original frame body.

My final results for the frames are shown in the images.

I have also attached the STL files for the Voronoi frames.

Note: Fusion 360 crashed a few times when I apply 2D Voronoi Studio on the frame. Make sure you have saved the file before moving forward.

 Depending on your printer and filament, the printing parameter may be different. Here are some general instructions I have:

Printing temperature: look carefully at the recommended ext. temperature of the filament.

Printing Surface: 60 degree C.

Infill: I use 15-20% for the frames and wheels and 30% for the engine set. My final prints are pretty sturdy. As a result, I recommend even lower infill to reduce the overall weight of the car.

Build Plate Adhesion: None. All the parts can be printed without any build plate adhesion. It is strongly recommended to print the engine set without a base to avoid imperfections in the gears so that they work as smoothly as possible.

Print failure happens all the time. Make sure you level the bed and there's no jam in the nozzle or tube before printing.

You will need four 40*3.5 O-rings on the rear wheels as tires! No car can move without proper tires!

Follow the images in sequence to assemble the car.

Everything should fit smoothly once you have put everything together. Sometimes you need to manually "clean" the print a little bit to make sure everything works well. For example I need to manually clean the hole for the front axle in my right frame once due to in-perfect print.

Hope you enjoyed it!

As proud as I feel for my car, I still want to try out more and make it a work in progress. I am going to work on it over the summer to make it better. Currently, the car drives itself with the wind-up motor. However, the distance it travels is not super far. My primary focus would be reducing the overall weight of the car. Here's a list of things I want to try:

1. Trying to print the parts with a less percentage infill. Currently the engine set parts are printed at 30% infill and other parts are printed at 15%-20%. I feel there’s still a lot of room to reduce the infill to make the weight lighter.
2. Other design patterns on the frames. Other than Voronoi patterns, I may make it completely hollow.
3. Trying generative design on the frames and wheels. Although I am not confident that it will reduce the weight significantly, I am very interested to see the new aesthetic it may generate on my car.
4. Adding a rear spoiler to add some sports car aesthetics.