CM5 Carrier Board

[danic85]

Carrier board pin mapping

The below tables detail the pins in use for the various protocols. I am not including pins for voltage or ground as this should be managed separately. See below for considerations here.

I2C

Device	Pi Pin
SDA	GPIO 2
SCL	GPIO 3
Power	5V / 3V depending on device

I2S

Device	Pi Pin
LRC / WS	GPIO 19
BLCK / SCK	GPIO 18
DIN (amp)	GPIO 21
L / R	GND OR 3V
SD (mics)	GPIO 20
Power	5V amp, 3V mics

UART

Device	Pi Pin
TX	GPIO 14
RX	GPIO 15
Power	Managed by connected device, grounds must be linked!

SPI

Device	Pi Pin
RST	GPIO 27
CS	GPIO 8
DC (DS)	GPIO 25
SDA (DIN)	GPIO 10
CLK (SCL)	GPIO 11
Power	3V for display, could be 5V on other devices

Neopixel SPI

Device	Pi Pin
DIN	GPIO 10
Power	5V

Other Consideration

Pi Pin	Notes
CAM / DISP	Expose both ports for cameras
USB-C	Expose USB-C for programming
Disable eMMC boot	Required for flashing CM5 without SD card
USB-A	Expose single USB-A for additional modules
40 pin GPIO	Expose 40 pin GPIO for additional modules
Power	Expose VIN (5.1V, 5A) / GND for power supply

Headers are expected to be 1.27mm pitch for signal (half the size of the most common headers) and MORE THAN 2.54mm pitch for power (as this is only rated at 3A), in order to handle 8A current.

Similarly, PCB trace width must be appropriate on the 5V and GND lines: https://www.pcbway.com/pcb_prototype/trace-width-calculator.html

Modules require 5V and 3V power, and those installed directly on the board (I2S devices) will need power supplied via the board.
Ideally, any 5V power should be fed directly from the power management board to the components. This keeps the board form factor small and allows the power on the board to be dedicated to the CM5.

[danic85]

Notes on creating a carrier board

A few files needed:

CM5 IO board KiCad Files:
https://pip.raspberrypi.com/categories/1098-design-files

Optionally, ShawnHymel's CM5 carrier template https://github.com/ShawnHymel/rpi-cm4-carrier-template
Move 'hardware' folder into KiCad base folder (documents) to use.

Sheet contains multiple sub-sheets.
Use 'labels' to connect pins across sheets, global labels may be the best approach

To add components, find them on the supplier website, download the component footprint etc.
Ensure naming is correct:
Folder, .pretty (footprint)
Folder, .lib (library)

Move folder to libraries folder in current project.

In KiCad: manage symbol libraries. Project specific, add existing, select folder.

Add to sheet, update property values as these are what the BOM references:
Manufacturer
MPN
Digi-Key Part Number (as an example)

'Cut tape works well for single items.'

Considerations:
Add power LED.
Solder jumper between 'nBoot' and Ground if flashing. This is the 'disable eMMC boot' pin.
Add screw fittings

Design rules can be updated in KiCad to match manufacturer.
Board setup also needs Net Class configured. Default Clearance and Track Width should be 0.2mm to match CM5 connectors.

USB Data also needs calculated clearance and track width. To create differential impedance. (See octavosystems note https://octavosystems.com/app_notes/osd335x-design-tutorial/osd335x-lesson-2-minimal-linux-boot/osd335x-lesson-2-usb-circuitry/)
USB data is "coupled microstrip line" Board thickness and other variables determine this. See Shaun Hymels CM4 board videos for more info.
Calculate differential pair width and gap (DP) in net classes. Assign to appropriate nets.

CM5 connector is a 'Hirose' connector.

Add Footprint, Fiducial, 1mm. Opposite corners. Help pick & place machine align the board.

[danic85]

I have made some concessions for v1 of this board as I don't want to over-complicate the design for the first version. I'm removing the USB-C and USB-A ports, (as well as the other ports I won't be using). I may add them later. This will mean that the board will not be able to flash a CM5 directly.

I have added the INMP441 directly to the board with the appropriate capacitors and resistors, detailed in the datasheet: https://invensense.tdk.com/wp-content/uploads/2015/02/INMP441.pdf. Specifically, a 100K pulldown resistor on the SD pin and a 0.1uF capacitor between VIN and GND.

The MAX98357A is more complicated, fortunately Adafruit's circuit is available under this license which means I'm able to copy their schematic:

However, because I have no faith in my PCB design skills I have also added a solder jumper that must be bridged to enable this module. This means that I can disable it and use one of the adafruit modules via the I2S breakout pins if there are issues with this version of the board.

The current version looks like this:

[danic85]

I'm reasonably happy with the board layout and the DRC is passing (except for a few issues I've flagged as warnings as they are problems with the stock footprints that shouldn't impact the production, and I can adjust if they do).

The layout looks like this:

Next step is to route the tracks, so I need to calculate the thickness of the 5v bus to the hirose connectors so that it can handle the current, then complete the rest.

It's currently set as a 4 layer board, and I think I'll need them all. I plan to include two GND zones on either face layer as that seems to be best practice.

[danic85]

I have merged the source from feature/cm5 to develop because, it turns out, none of the changes are specific to the CM5 board, and are in fact just general improvements to the framework.

Once I have the new PCB assembled I'll work on fully testing everything in develop, so it made sense to have the source in one branch.

[danic85]

Board has been printed and assembled, and actually works (at least the initial boot). I will continue testing. I have attached the final design:

[danic85]

The microphone and amps are both working well. The camera isn't recognised but I suspect that is configuration as I didn't test that on the IO board either.
For the other modules I'm just waiting for some pre-assembled connectors because I can't crimp the tiny JST connectors to the wires... My crimp-fu is not strong.

[danic85]

The pre-assembled connectors arrived and I'm pleased to say that the I2C, GPIO and SPI interfaces are all working as expected. The camera does not (no cameras found), but I expect that is a configuration issue as I didn't really change anything there from the IO board that this PCB was based on.
The speaker still works intermittently (depending on the restart of the device), but that was the case with the IO board as well so I suspect that's a driver config issue.

Overall, I'm fairly pleased with the board. If I can get the camera(s) working I will be able to begin building the head.

Current draw hovers just below 1A @ 5V, even with the screen, ear servo, and motion sensor connected and the code running. If the code isn't running it sits at around 0.5A @ 5V. So there are clearly some efficiency improvements I can make to the software that will extend the battery life.

[danic85]

The MIPI CSI/DSI (camera / display) port 0 works with the Raspberry PI AI Camera. I haven't tested port 1 yet, as I need to bridge the two solder connectors, but I don't have plans to use that in this version so I'll test it at a later date.

Besides that, everything is tested and working perfectly!

[awright424]

any plans to make the files available for this?

[danic85]

@awright424 Definitely the plan, in some form, at some point. But, this is still very much a work-in-progress and the technical complexity of recreating this is quite high compared to previous versions so it may not be something that most of the community can reproduce. I may end up making it available as a board with the SMD components already included rather than assuming everyone has the capability of doing that themselves.
Watch this space!

[awright424]

I just need the kicad files. I am scared of differential routing etc. I attempted one board had them produced from jlpcb and assembled and it was a good initial try but the boards didnt work. I will be updating them and building myself next time.

[danic85]

Creating a feature branch for the changes relating to cody testing and integration. Includes the new 'eye' code using the TFT display.

#139

[danic85]

Just to follow on from the updates above: The carrier board is a difficult thing to recreate. The components are small and most require surface mounting with solder paste, a microscope (ideally) for placement, and a reflow oven or heat pad.
I can't make the assumption that everyone has access to the above, or the capability to build this themselves. It's more 'industrial' than most makers ever need to do.

So, for that reason I'm interested in understanding how much interest there is in making the board accessible, and in what way.

Please react to this comment with the appropriate symbol to take part in the survey:

1. 🚀 I would buy the carrier board with all the SMD components in place, so that I could add the CM5 and any connections to off-board components myself (camera, i2c, tft display etc. See here).
2. 👀 I want to do it all myself, make the gerber files available.
3. 🎉 I would buy a full kit of the electronics to build the robot so that I don't need to source the parts myself. I'd 3D print the models myself.
4. 👎 I'm not interested in using the CM5 or carrier board.
5. Other (please comment below).

Some more context on the components used in this build for the head here (Everything under 'Raspberry Pi 5 Carrier Board' in that list would come pre-installed in option 1).

[dburgess100]

1 - I'd buy the carrier board. I don't have the SMD equipment or experience. I'd prefer to print and source the rest of the materials myself.

[BucketHatGirl]

1 - I need a very slim board for building a slim open source tablet and this seems like the perfect one