- Implement 2D & 3D geometries and explore modification tools on Fusion 360
- Understand efficient techniques used to improve dimensional accuracy, tolerances and minimize design time
- Convert models to STL format for 3D printing
For this project, you will need
- Autodesk Fusion 360 on your computer
The Raspberry Pi 3B+ is among the most commonly used controllers for prototyping. In this tutorial, let’s look at how to design a casing for the raspberry pi. We will go through the entire design process step by step, followed by the procedure for 3D printing. The outcome of this course will be to get you familiarized with the various CAD tools that will help you design enclosures to give your projects a finished appearance.
We can design the case in many ways. We can manually use a Vernier Caliper and measure all the required dimensions of the board as reference for the design for the case. As you can imagine, this will be a tedious, time-consuming process and subject to a lot of errors. The better alternative would be to refer to the datasheet of the manufacturer and find out the dimensions already measured with great accuracy and use that as reference. Usually, this is the procedure followed. However, for popular boards like the raspberry pi 3, there are pre-existing CAD models of the board on open source websites like GRABCAD. We will use the dimensions of the already designed board as a reference to drive the dimensions of our case.
Download the following file from Grabcad to get started. Let’s start designing!
- Start by opening Fusion 360 on your system and save your file in an appropriate location. Always remember to save your file on a regular basis, to prevent data loss after having invested a lot of time and effort into your designs.
- Next, click on the data panel icon at the far left corner to open the data panel. Upload the downloaded .stp file into the appropriate project folder. You can create a new project folder at this stage, if you hadn’t done so in the previous step.
Uploading the downloaded file
- Once uploaded, right click on the file and click on ‘Insert into current design’. Use the rotation icon to rotate the design by 90 degrees until it is flat as shown in the image:
Place the file flat on the platform
- Click on the ‘ASSEMBLE’ drop down box and select ‘New Component’, and rename it as case.
- On the top right hand corner, toggle to the right view of the model of the board. You can see that the bottom most portion of the board’s pins are below the red origin line. We need to account for the thickness of our casing, and ensure that the base of the case is aligned with the red origin line. For this reason, let us move the entire Rpi model upwards by 5.5 mm, where the thickness of the case is 3.5 mm at the base, and the base of model was already 2 mm below the origin line to begin with. Therefore, adding the dimensions will give us 5.5 mm. You can do this by selecting the entire Rpi and using the Move command.
Board’s pins below the red origin line
RPi model moved upwards
- Use the keyboard shortcut ‘R’ to activate the rectangle feature. Click on Capture Position to retain the moved position of the board. What we are doing now is called 2D sketching. You will need to select a plane on which to sketch. Click on the bottom XZ plane to begin sketching.
- Under create, select Rectangle followed by centre rectangle. Click on the origin and use 91 mm as the length and 64 mm as the width of the rectangle. These dimensions were obtained by trial and error to ensure that it encloses the Pi appropriately.
- Press ‘e’ to activate the extrude command. Extrude is a process of converting a 2D drawing into a 3D model. We will extrude the model by a height of 30 mm and hit enter. To see if the there is sufficient space provided, we will need to see through the box. For this, reduce the opacity of the box so that we can see the inside while still working with the box. This option can be found by right clicking on the case part within the browse tab.
- Let us give rounded edges to the box by hitting the ‘f’ shortcut to activate the fillet command. Select the 4 vertical edges and a fillet radius of 5 mm. Repeat the process for the bottom and top edges with a fillet radius of 2.5 mm. Your model should now look like this:
- Let us know make the box hollow. Under ‘MODIFY’, click on the shell command and select only the body of the case under the part drop down menu found under the browser. Select a shell thickness of 2.5 mm. This represents the thickness of the walls.
- Next, we will need to create holes for board. To create holes, we will need to cut out the top of the box temporarily. We can do this by click on inspect followed by section analysis. Click on the top of the box and drag the cursor down by any suitable height, say 20 mm and click ok.
- Next, click on new sketch and under create sketch, click on project, and select the four holes as shown below:
Selection of the four holes
- We need to provide some tolerance to the holes by using the offset command under the modify tab. Click on offset and provide an offset of -0.3mm (radius) or a total tolerance of 0.6mm as we are dealing with a circle. Repeat the offset for the other 3 projected circles.
Offset to provide tolerances
- Now, use the keyboard shortcut ‘e’ to select the extrude command. Select the four projected circles and extrude until holes at the four corners are formed. It will automatically be set to cut operation when extrude is selected.
- Now we need to create slots for the ports of the raspberry pi. For this, repeat the section analysis step cutting it along the width. We could directly do this on a plane of the wall of the case. However, if we decide to change the wall design later, it could be problem. For this reason, create an offset plane under the Construct option.
- We will make the slots in the same manner that the holes were made. Create a section plane under the ‘INSPECT’ option and drag the plane until the connectors are sliced in approximately in half.
- Now, create a new sketch on the newly created plane, and draw an outline of the ports on this plane. Change to the right view using the view toggler on the top right-hand corner.
Draw port outlines
- We need to give some tolerance to the holes. Use the ‘o’ keyboard shortcut and select the three squares. Offset each by 1mm on the outside, by using -1 mm as the input value.
- Let us now cut out the squares drawn from the case. For this, use the extrude and set the operation to cut. Then, select the extent to ‘to object’ and select the inner wall of the case. (If you are unable to make the selection, it would help to create another section plane and cut the case in half horizontally). Repeat the same for all the slots required for the case. Make sure to include one for the camera input and the SD card slot. After the holes are cut out, your model should look like this:
Cutting of slots
- Let us now split the case in half and create some snap fit joints. We need to split the case longitudinally at the midplane. To construct the mid plane, click on ‘Midplane’ under the ‘CONSTRUCT’ option.
Construct the mid plane
- Next, under ‘MODIFY’, click on ‘Split Body’ to split the case into two halves, using the midplane as the cutting tool. Now, we have two faces which can be 3D printed with a flat side on the build plate of the 3D printer.
- We will now create a snap fit joint for the cases. The snap fit joint we will be looking at is the cantilever type. First toggle view to the side of the case with the Audio out, as shown and draw a rectangle 6mm wide by 3 mm height, ensuring that it is a suitable distance away from the neighboring components. Then, extrude and cut out the hole by using ‘to object’ and the inner wall of the case as reference. See the image below for the dimensioning we have used:
Snap fit joint slot
- Hide all other bodies except the bottom of the case for convenience. Sketch on the plane of the slot using the line command and create the following profile as shown:
Dimensioning of the slot
- Extrude the drawn profile, selecting join as the operation. Hide the bottom body and make the top body of the case visible so that it joins only to the top body. Use thickness of the snap as 5 mm.
- We will now add chamfers to the snap. Select chamfer from the ‘MODIFY’ drop down list. Chamfer the bottom front edge by 2 mm and the top front edge by 1 mm. Chamfer the back top edge by 3 mm. The final result should look as shown:
- Finally, we will mirror the slot and the snap to the other side. We can do this using the mirror command. Under ‘CREATE’ click on the mirror option. First select the extruded cut out and mirror about the right plane as the plane of reflection. Select pattern type as ‘Features’ as shown.
Mirror the slot
- Repeat the same for the snap, but this time we need to manually select the chamfer and fillets made on the bottom right hand corner as shown in the figure. With that, we’ve now created a completed Raspberry pi 3B+ case that is ready to be 3D printed! This is the final output after adding the material and some rendering. There are several materials and lighting that you could explore!
Raspberry pi 3B+ case
- Right click on the top and bottom bodies of the case under the Browser click on save as STL, and save these as individual parts which can be printed individually and assembled.
This will be a challenging part to design for a novice; nevertheless we are sure that it would have given you lucid insight into the various features that are available with Fusion360 and the techniques used for accuracy and efficiency. We are certain that after this, you will be able to approach various enclosure designs with ease.