Part Review Checklist

Owned by Farris Matar
Last updated: 2023-07-07 by Stanley Hao
3 min read

In order to standardize part creation and prevent any issues with symbols and footprints from being manufactured, part reviews will be introduced. Part reviews should be completed during the schematic review for each new part that was designed for the project. It is the project owner’s responsibility to keep track of the parts they added to the libraries and ensure they are reviewed alongside the schematic.

Part Properties

Ensure the properties table for the part includes the following properties. Bolded properties should be set to be visible. Be sure to label the properties exactly as they are shown below. Additionally, be sure a Supplier Link is added to the part.

Part Type

Required Properties

Part Type

Required Properties

Capacitor

Manufacturer 1, Manufacturer Part Number 1, Supplier 1, Supplier Part Number 1, Package, Value, Voltage Rating

Diode

Manufacturer 1, Manufacturer Part Number 1, Supplier 1, Supplier Part Number 1, Package, Voltage Rating, Current Rating (if applicable)

ICs

Manufacturer 1, Manufacturer Part Number 1, Supplier 1, Supplier Part Number 1, Package

Inductor

Manufacturer 1, Manufacturer Part Number 1, Supplier 1, Supplier Part Number 1, Value, Current Rating, Saturation Current, DCR

MOSFET

Manufacturer 1, Manufacturer Part Number 1, Supplier 1, Supplier Part Number 1, Package, Vds Max, Vgs Max, Rdson

Resistor

Manufacturer 1, Manufacturer Part Number 1, Supplier 1, Supplier Part Number 1, Package, Value, Power Rating

Schematic Symbol Checklist

If this is a new symbol, there should not already be an existing symbol that could be used (i.e. do not make a new Schottky diode symbol, unless the existing symbol does not have the same number of pins)
Symbol should be done in mils. All pins should be placed on a 100mil grid
Pins should only come out from the left and right sides. An exception can be made for op-amps and FETs
Parts should show ALL pins - i.e. if a MOSFET has 4 drain pins, all 4 should be included as separate pins
Pin numbering should match the datasheet exactly
Power should be in the top left. If the part is a voltage translator, input power should be in the top left, and output power should be in the top right
GND should be in the bottom right
Proper designator should be used for the part
Active low pins indicated with an overbar notation or with a “_n” following the pin name
Pin names should be visible if the part is an IC. Symbol pin names should match pin names used in the datasheet
Description should include the description copied from Digikey

Schematic Symbol Naming Convention

<insert naming convention here…>

PCB Footprint Checklist

If this is a new footprint, there should not already be an existing footprint that could be used (i.e. do not make a new 0805 footprint for chip resistors/ceramic capacitors)
Avoid using 0402 or similarly sized components, as they are very difficult to work with due to how small they are. Do NOT use 0201 components
Footprint should be made using the WARG stackup
Correct pad sizes and locations
Corner radius for pads should be 15%
Solder mask expansion for all pads set to 0.05mm, verify Top Solder shows solder mask for all pads
For through-hole pads, verify both Top Solder and Bottom Solder show solder mask
Paste mask expansion for all pads set to 0mm, verify Top Paste shows solder mask for all pads (surface mount components only)
For surface mount footprints, pads placed on Top Layer
Silkscreen border included on Top Overlay layer (optional)
Pin 1 designator included on silkscreen (Top Overlay) if applicable - use a 0.25mm radius circle next to pin 1
.Designator string is included and centered on the origin on Mechanical 9 layer. Use TrueType Arial font with 60mil text height
3D Body and border on Mechanical 13 layer
Centre cross and courtyard on Mechanical 15 layer (courtyard is optional)
Nothing on any mechanical layers except mechanical 9, 13, and 15

PCB Footprint Naming Convention

<insert naming convention here…>