I have a phone that I really like - the Sony Xperia X Compact. The reason I bought it was really simple: I wanted the smallest, nicest Android phone I could find with a good camera. I never thought the future of smart phones would be the goliaths everyone carries around nowadays.
I haven't found any cases I like for the phone. They tend to make it way more bulky, which defeats the purpose of having a small phone. So I decided to spend some time this weekend prototyping a smaller, minimalist aesthetic phone case.
I carry the phone without a case, and have dropped it quite a few times. Only the corners seem to be wearing down, so my focus is on those.
My design criteria:
(1) The case should only minimally change the overall size of the phone.
(2) The case should add very little weight to the phone.
(3) None of the buttons should be obstructed. Same for the camera, light sensor, speakers, or headphone jack.
(4) The corners should be fully protected. Existing damage should be covered up.
(5) I should be able to set the phone on a surface without the body contacting that surface.
(6 - bonus) I should be able to put an ID and credit card into the strap to replace my wallet from time to time.
Step 1: Plan of Attack
Here's the design and prototyping process I'll use:
(1) Identify important features of the phone. Set these up as User Parameters.
(2) Make an initial, 4-cornered CAD model based on measured features of the phone.
(3) Print the prototype and do a fit check.
(4) Iterate User Parameters until I have a good solid fit. This will probably involve decreasing both Width and Length so that the phone case has some tension.
(5) Once I'm happy with all the fit checks, I'll print a final version with the thinnest case possible.
Step 2: Identifying Important Features
I'll be rapid-prototyping this phone case, so I'm going to use good design habits to save myself any headache down the road.
The idea is to identify any geometries I think will be important for the fit of the case, measure them before starting the CAD process, and be able to quickly change them during fit checks. As I iterate phone cases, I'll make tweaks to these values to fit the phone more securely.
So the very beginning of the design process is to either sketch or quickly generate a model of the object you're interested in. In this case, I'll start with my phone, and build the case up around it. It's useful to have this diagram on-hand to reference as you build the CAD model.
Step 3: Setting Up User Parameters
Before I even start modeling the phone or the case, I'll input these user parameters, cross-referencing the diagram I built in the last step. You can create a new User Parameter by pressing the green "+" sign (circled in red).
You'll want to measure these values with as much accuracy as possible. Use a pair of calipers and maybe a set of radius gauges. The more accurately you input your initial values, the less times you'll have to iterate to get a solid fit. But don't go overboard: most 3D printers don't print with enough precision to perfectly reproduce your initial values.
I'm also adding a few unmeasured values (fillet sizes) to help make the phone case stronger and more aesthetic. I can experiment with changing these values in the CAD environment to get a look I like before sending prototypes to the printer.
Step 4: Model the Phone
Start a new design in Fusion 360. Save the design, and give it a name. I named mine "Practice Case", although I ended up using this file to print my phone case prototypes.
Right-click on the name of the design and select "New Component". Name the new component "Phone Body." Activate that component.
Now make a sketch on the ground plane, using a Center Rectangle at the origin. Keeping the phone centered at the origin will make it easier to mirror components later on.
Give the rectangle the User Parameter dimensions "Length" and "Width".
Now end the sketch and select "Extrude." Select the rectangle and extrude to the User Parameter "Thickness".
Step 5: Model the Other User Parameters
Use the Fillet tool to add the two fillets that were selected at the beginning of the design process.
This is also a good time to add any geometries you think the case might interfere with. For my Xperia phone, the only port I'm worried about is the headphone port, so I add that by extruding a circular cut into the end of the phone in the proper location.
Now, experiment with your User Parameters! Change them all and make sure that the model responds properly.
Step 6: What If Your Phone Is Different?
My phone has a pretty unique geometry in a world full of iPhone-looking bezel monsters. The approach I've taken here can absolutely be used with other types of phones, but you'll be interested in other features when you input your User Parameters. Here's an example.
The rest of this process should work just fine based on any phone geometry (I think....).
Step 7: Start Modeling the Phone Case
The first step I took here was to model a single corner piece. Soon, we'll mirror that piece across the phone's body, then mirror again to make 4 corners. The dimensions of the corner piece will be based on some User Parameters, especially "StrapThickness", which is a User Parameter that expresses how thick I want the case to be.
Right-click on your design name, and select "New Component". Name the new component "Case." Activate that component.
Start a sketch on the base plane, and give it some dimensions:
The distance from the edge of the phone to the outer edge of the case should be "StrapThickness". You should see the lines along the edges of the phone turn purple. That's super important: it means those lines are adaptive, and will change their location if you change your User parameters!
The other two dimensions are up to you. In my case, I can avoid my screen by making the corners about 14mm x 6.35mm.
Now stop the sketch and extrude the corner. Use your User Parameters! In one direction, you want to extrude by "StrapThickness." In the other direction, extrude by "Thickness + StrapThickness" so that you cover the thickness of the phone plus the thickness of the case.
Throw a fillet on there. If you want the case to hug your phone, use the same radius as below ("SideRadius").
Step 8: Cut Out the Inside of the Case Corner
Subtract the phone body from inside this first case corner using "Modify -> Combine." Select the case corner as your Target Body and the phone as your Tool Body. Use "Cut" as your operation.
Make sure to check the mark next to "Keep Tools" so that the operation doesn't delete your phone body entirely.
This is a good time to try changing your User Parameters a little to make sure the cut adapts accordingly.
Step 9: Mirror the Corners
Activate the top-level design. Make the Origin visible by clicking on the light bulb next to it. We'll mirror the case corner about one origin plane, then the other. This is why we placed our initial phone body rectangle right at the origin.
By selecting "Component" as the mirror type, you are making an exact copy of the original corner - not only that, but updating the original corner will update the new one and vise-versa!
Now mirror the original and new corner components about the other plane.
We'll combine all these 4 corners into a single component after adding some tension straps to hold them together.
Step 10: Add a Strap
The criss-crossing back straps are really the crux of this design. We want them to provide enough tension to hold the four corners snug around the phone, and they also should let us carry some cards or cash around.
Activate one of the corners.
Flip the part over and start a sketch on the back plane of the phone. Draw a line from corner to corner, and make it a construction line. Then, use constraints to make two other lines that are coincident to the edges of the corner pieces (these should turn purple), parallel to that construction line, and symmetrical about the construction line.
Add a dimension to give them width. I'm using a User Parameter called "StrapWidth".
Stop the sketch, and extrude the strap with the thickness "StrapThickness." Alternatively, you can use some reference geometry to extrude it to.
Step 11: Combine Corners and Straps
Now, just mirror the corner that now has a strap attached to it across the center plane of the phone.
Hide or suppress any corners you don't need anymore. All of the case pieces we've used up to this point are actually just tools to make one final case!
We'll use the act of combining these parts to make a new component, which is what we'll work with to get the case ready for printing.
Use "Modify > Combine" and select all the four components. Use the "Join" operation. We'll keep the tools, but make them no longer visible to start adding fillets and preparing the design for printing.
Select the check mark next to "New Component." Name the new component "Combined Case." You can now hide all the tools we used to make the case.
Step 12: Add Fillets to the Design
We're almost ready to print the first prototype. First, we want to add fillets wherever there is a sharp corner. It's good practice to assign fillets User Parameter values. In one case here, I decided to add a fillet that's 1/2 the radius of an existing fillet. Doing this makes it really easy to tweak these values and see how it looks before actually printing the part.
We aren't adding fillets just because we want to make the case look organic and aesthetic - they serve an important functional purpose. Any time stress is put on a sharp corner, that's a point where a crack can start to propagate, leading to failure of the part. In engineering, we call a sudden corner like this a "Stress Concentration." Fillets reduce the magnitude of that stress concentration, and make the part last longer.
Some of the fillets I'm adding here serve this purpose. Others are just for looks. The question is always whether we can use a fillet to prevent stress concentrating at a sudden changing geometry.
When stress cracks start to propagate on passenger airplanes, technicians drill circular holes at either end of the crack, basically using a fillet to reduce stress concentration.
Step 13: Prepare the 3D Print
To prepare the case for a 3D print, use Fusion's "MAKE" command and save the STL file.
Now, open the STL file in Cura, or the slicer of your choice. Set up your materials. I'm making my case in TPU, a flexible, stretchy material.
This particular geometry is pretty hard to print without a second extruder to lay down support material, so that might be necessary - then again, I've seen people do some pretty amazing things using the print material as support.
In any case, we use an Ultimaker 3, which lets me print in TPU as a build material and PVA as a dissolvable support. The STL came in at the wrong orientation, so I turned it 90 degrees.
I'm using 100% infill, with a Fine (0.1mm) profile. I'm also using a Prime Tower for higher print quality. I always like to check the layers generated by the slicer before sending the gcode to my 3D printer.
Step 14: Rapid Prototyping the Design
I have now printed 3 versions of the case.
The first case had corners that were just too small. But they fit the case pretty snugly, so I didn't need to change the height or fillet dimensions of the phone in later iterations. The straps don't provide enough tension to hold the edges against the sides of the phone, and the case pops of easily. I think it's likely that printing this case with a more rigid material would work well, but the TPU is too elastic for this design to work well.
The V1 straps weren't quite tight enough, so I decreased the User Parameters "Width" and "Length" by 0.05in each to pull the corners closer together. I also increased the length of each corner to come up right to the edge of my phone's screen. The V2 case was almost tight enough to hold the case tightly on the phone, but it kept falling off in my pocket. I decided I needed to add two more support struts to give it stability.
Step 15: Rapid Prototyping the Design
With the support struts added, the case fit very nicely. The small changes to the Width and Height dimensions were ideal to give a little extra stretch so I can fit a couple cards or some cash on the backside of the phone.
The 4th iteration of the case is on my 3D printer now. I'm happy with the current design, but want to see how thin I can make the case. I've moved down from 0.05in thickness to 0.03in.