Add PocketBeagle

[twam]

Datasheet: https://github.com/beagleboard/pocketbeagle/wiki/System-Reference-Manual#70_Connectors_
Images:

---

Thanks for creating a pull request to contribute to the KiCad libraries! To speed up integration of your PR, please check the following items:

• Provide a URL to a datasheet for the symbol(s) you are contributing
• An example screenshot image is very helpful
• Ensure that the associated footprints match the official footprint library
• If there are matching footprint PRs, provide link(s) as appropriate
• Check the output of the Travis automated check scripts - fix any errors as required

[CLAassistant]

All committers have signed the CLA.

[poeschlr]

Connector might not really be the correct repo for this. Might this better fit into the modules lib?

[myfreescalewebpage]

Hi @twam

Same comment already made by Rene, can you move this to "MCU_Module" library ?
Moreover, you have made 2 parts, but as single one is required, this is two headers to be connected to the same module. You can make a single unit with all pins, or two units in the same symbol.

Cheers,
Joel

[twam]

If I make a single part, then it is not possible any more to use the usual connector footprints. Or do I miss something?

[myfreescalewebpage]

No, this will require to create a specific footprint too, with all pins. This has the advantage to grant the distance between the two connectors, and also to create a silkscreen.

I don't know the position of @poeschlr but I don't think it is good to have the board split in two different symbols...

[Misca1234]

Agree, this should be one symbol to match a dedicated foot print as Joel points out
Perhaps you should add the prefix P1_ and P2_ to the 3.3V and %V names so the designer knows what connector they are connected to the other pins seems to have unique names.

I guess the data sheet link should be
https://github.com/beagleboard/pocketbeagle/blob/master/PocketBeagle_sch.pdf

Look what I found
https://github.com/beagleboard/pocketbeagle/tree/master/KiCAD
They actually made the design in KiCad with sch and foot prints, let me poke around here, we might be very lucky

@twam
Do yo uwant me to make the foot print or do you want to do it yourself?

[twam]

I can adjust the file and/or create the footprint. However it will take ~4 weeks due to other obligations.

[Misca1234]

Actually I could not resist so I made it last night, I had to bring up the boards PCB t get the right measurements.
I can push this and then you can add the symbol if you want.

P1 is pin 1-36 and P2 is 37-72

[Misca1234]

Foot print push is here
KiCad/kicad-footprints#1350

[myfreescalewebpage]

Thanks @Misca1234 to help this PR :)

[Misca1234]

np, the lack of measurement triggered my desire to find them ^^

[twam]

Finally managed to update the footprint. I hope I have tackled all wishes :)

[myfreescalewebpage]

@twam I was waiting for update following footprint proposition, I have not performed the review at the moment, but will do asap (today).

[myfreescalewebpage]

@twam here are my comments:

• The correct name for this symbol should be PocketBeagle
• Do you have a better documentation link for this, a datasheet, not a schematic ?
• Spelling error in keywords : "beagleboard"
• Description is too long and not detailed, can you short this, add some kind of information about quantity of RAM/FLASH etc ? See for example how the other module symbol are described.
• "AIN.VREF+" is positive power supply and should be moved to the top of the symbol
• "AIN.VREF-" is negative power supply and should be moved to the bottom of the symbol
• "3.3V" is positive power supply and should be moved to the top of the symbol
• "VOUT" is positive power supply and should be moved to the top of the symbol
• Name of pin 46 is "GPIO52"
• GND pins should be stacked
• AIN pins are Input
• RESET is Input
• PWR.BTN is Input
• BAT.VIN is Power Input and should be moved to the top of the symbol
• BAT.TEMP should be passive to avoid ERC errors
• I wonder about the USB1 pin types, ID and VBUS are probably Input, and DRVVBUS is probably Output isn't it ?

Better datasheet link will be interesting to fix the above comments and have a clear overview of the device.

Cheers,
Joel

[twam]

I haven't found a (PDF) datasheet. I also like to use the https://github.com/beagleboard/pocketbeagle/wiki/System-Reference-Manual but declared the Schematic as a datasheet as this was suggested by @Misca1234

[myfreescalewebpage]

I think the manual https://github.com/beagleboard/pocketbeagle/wiki/System-Reference-Manual is better in this case, it contain much more informations !

[myfreescalewebpage]

My last comment:

• Description: please remove extra spaces between values and units (GHz and MB)

Else, great job!

Thanks,
Joel

[myfreescalewebpage]

Footprint merged, just need the last fix in my previous comment to merge this symbol.

[twam]

There you go. Thanks for the thoughtful review!

[myfreescalewebpage]

@twam please do not force push, this breaks the commit history and make the review more difficult.
Else, this is OK for me, merging.