Standards - PCB
- Forest Zhou
Mounting
Hole Type
The M2.5 hex standoff component shall be used for PCB mounting. The hole shall be 2.7mm in diameter, with a keep-out area 6mm in diameter. Mounting holes shall be low voltage ground where applicable.
Placement
Holes are placed in corners with the centre 3.5mm from the edge.
Size
Boards to be mounted on top of battery modules shall be 70 x 100mm with mounting holes located 3.5mm from adjacent edges in each corner.
Traces
Width
Standard signals shall use 50ohm traces with an impedance profile set in Altium. Use Saturn Toolkit to calculate required width for higher current applications.
Routing
Generally, traces should enter pads through the centre. This is more for stylistic purposes, but will also prevent unintended acute angles and make the routing a lot neater. The marks in green indicate the desired routing path. In areas were space is a constraint, traces exiting at a 45 degree angle through the corner of a pad is also acceptable.
Vias
Standard Size [pad/hole] (mm)
2 Layer: 0.5/0.3
Multilayer: 0.45/0.2
For higher current applications, many standard vias offer more current carrying capacity per area than one very large via. Controlled impedance signals at or above USB High Speed (480Mbps) shall have controlled impedance vias. Saturn toolkit can be used to calculate via impedance and current carrying capacity. Standard JLC plating thickness is 18um, and the expected temperature rise shall be no more than 25C.
Stitching Vias
Comprised of standard vias(see above) placed on an offset 5mm grid, with 1mm clearance to pads/traces/board edge. Sometimes they can be more dense due to smaller board size or specific requirements.
Test Points
Size
SMD test points shall have an exposed copper area of at least a square with edge length of 1.27mm.
Through hole test points shall be un-tented PTH with a 0.7mm hole and at least a 1mm pad diameter.
Location
SMD test points are required for power rails and any analog voltages being measured by an ADC. Both SMD test points and 2.54mm headers are required for digital communication busses.
Thermal Relief
Thermals should be present unless there is sufficient reason to remove them. Some reasons to remove thermals include high current paths in a switcher, or when a thermal cuts down significantly on the area of a polygon. Generally decoupling caps should have thermals.
Logo
The top layer silkscreen shall contain the following graphic, with text under the “Midnight” letters in the following format:
[Car#] [BRD Name] Rev [major.minor]
ie. MSXV Controller Board Rev 1.0
Silkscreen
Designators should be visible if space allows. When space is limited, prioritize key components such as ICs. This way, it is easier to identify which section of the circuit you are looking at.
The standard silkscreen text has the following properties:
Mirror: Mirrored for bottom overlay
Text Height: 0.8mm
Stroke Width: 0.2mm
Font type: Stroke
Font: Default
Board Colour
PCB colour shall not be black or white due to the minimum solder mask sliver being larger for those colours.
Component Spacing
Small SMD components shall be spaced at least 0.5mm apart, or such that their outermost silkscreen lines do not more than fully overlap, whichever is greater.
Solder Paste Stencils
Stencil opening rule shall be set to -20%. Individual footprints may override this rule, such as fine pitch (>= 0.5mm) pads having a smaller paste opening to prevent solder from shorting the pins together.