Need to know which specific part number was ordered, potentially making the current one incorrect (was it the VCNL4040M3OE-H5?).

Create the NTB0104GU12 footprint based on the manufacturer's given recommended reflow soldering footprint and assign it to the respective symbols

Add BLM18PG121SN1D chip ferrite beads to the GNSS, proximity+ambient light sensor, and IMU +3.3V power pins

Use PAM8301 manufacturer's TSOT26 recommanded pad layout modified from KiCad's official SOT-23-6 footprint

A combination of Macronix's "Recommended PCB Pad Layouts for 8-USON & 8-WSON Packages" (page 4) and "Macronix 209mil 8-SOP and 6x5mm 8-WSON Dual Layout" app notes were used in conjunction with KiCad's official DFN-S-8-1EP_6x5mm_Pitch1.27mm footprint to give a well-rounded pattern.

Use manufacturer's recommended land pattern for 74LVC1G32GW, NUP5120X6, and 74AUP2G08 (U1301, U1501, U1803), use more accurate VSSOP-8_2.4x2.1mm_Pitch0.5mm 3D model for 74LVC2G241 (U701), include SOT-563 3D model for NUP5120X6

Used manufacturer's given stencil/solder paste and solder mask dimensions whenever given. Some of KiCad's official footprints do not necessary align with the manufacturer's recommended footprints.

added drawing sheet for pcb with board dimensions

The offset from the main-board to the SoM was measured to be very close to 4.0mm by adjusting the offset and double checking the spacing, it should be fairly accurate when determining the amount of space available (some double checking required).

Create PAM2841GR footprint and assign it, also assign its 3D model to KiCad's offical DFN-4 model, remove back solder mask to thermal relief vias on the footprints which have them, add thermal relief vias to the AR8031's exposed pad (EmCraft's baseboard has them)

Make use MIC5365's SC-70-5 package instead of the SOT-23-5 package since it is a lower cost and is more available, assign it the official SC-70-5 3D model

Used Microchip's "Package Specification" document which on page 41 shows the recommended land pattern for their SC-70-5 packages (nominal pad dimensions are given but spacing is shown as min/max, used these values +/- 0.05mm for headroom).

The MIC5365-2.8YD5's recommended land pattern in the datasheet has inconsistent dimensions, so reasonable values are used based on the given TSOT-23 package's dimensions and KiCad's official SOT-23-5 footprint.

Create and assign RT8070 3.3V buck converter's footprint, import and assign its 3D model from the official KiCad repo

Re-export the BoM after bring the WLAN+BT M.2 sheet to page 18 and redoing the reference designator numbers.

Add the BQ25896 charge controller's missing pins which may make the schematic a bit ambiguous, reduce the value of the VBAT_REG LED's current limiting resistor to 1k in order to make it a bit brighter

This commit is thanks to our design reviewer's feedback.

Move the ground connection on the USB-C receptacle from the shield pin to the GND pins (shield is still connected to GND via the 0 ohm resistor), make the cap between the receptacle's GND and shield NC

This commit is thanks to the feedback from our design reviewer

Update Bill-of-Materials format and include missing SEC1110 datasheet link, fixed lingering component properties typos

Add AC coupling caps to the HDMI_AUXP/N diff pair which were mistakenly left out, fix a couple typos/errors that were made when transitioning to the new top-leve sheet, make the M.2s' I2C RX TX hierarchical signals consistent and clearer

Hopefully all lingering errors have been caught, this will likely be the schematic commit that gets reviewed (fingers crossed).

Assign TLV3201AIDBVR footprint based on the SOT-23-5 official footprint using the given solder mask clearance and pad clearance parameters, assign the QFN48 3D model to the ETH PHY footprint, make some minor adjustments to the front sheet's layout

Create AP22814 footprint and assign it to the respective symbols, use DFN-6-1EP_2x2mm_Pitch0.65mm 3D module for AP22814

Reorder USB-C's diff pairs based on layout simplicity as done on EmCraft's Rev 2 baseboard (requires Lane Polarity Inversion), add 2 and 3-channel differential filter & TVS IC footprints (used with USB-C and HDMI), import USB-C receptacle 3D model

Used a scaled version BGA-256_16x16_17.0x17.0mm_Pitch1.0mm 3D model for the filter&TVS diff pair chips, the perimeter balls are not very noticable at this shrunken scale and can be replaced later on (placeholder).

Move haptic motor connector footprint position such that 0,0 is between the through hole, this should make it so that its placement coordinates is closer to its center of mass

Remove emcr_mx8m.* files as they're no longer used, rename Purism_landscape.kicad_wks file to purism_landscape.kicad_wks (prefer all lower case letter for ease of use)