USB data lines D+ and D- have 39R series resistors
I2C have pull-up resistors (unless they are already internal to a device)
Do not rely on standard Altium libraries (pinouts and footprints can be wrong). Use Beta Solutions libraries and add to it. Make sure variable labelling is consistent.
P-Ch MOSFETs have their SOURCE connected to the high-side voltage (e.g. Vcc)
N-Ch MOSFETs have their SOURCE connected to the low-side voltage (e.g. ground)
Make sure voltages are not applied to any pins of ICs that are shut-down by removing power (unless the are designed to handle it). Leakage currents can occur.
Systematically check BOM with every component on schematics to weed out labelling errors and component variant problems.
Make sure schematics compile
Solder mask layer is visible on all component pads
Remove very thin slivers of solder mask that will not ‘cure properly’. IMP minimum is 6mill (0.1524mm)
Appropriate test points included. Untented vias can be used as test points when space is a premium. Make sure there are enough ground test points (both analogue and digital if applicable) for connecting multimeter leads and the ground connections of oscilloscope probe leads.
Tracks that could be useful for debugging are accessible from the top or bottom layers (i.e. not completely buried in the middle layers if possible).
The way the PCB is mounted is considered and taken account for (e.g. screw holes or sticky pads)
No reference to client if requested (due to intellectual property protection)
The layer stack-up is specified (core/prepreg/copper material and thickness’s)
The impedance is specified (if applicable). This is normally related to the stack-up.
Component links (between schematics and pcb file) are updated. This is done from the PCB editor.
Mechanical layers are used correctly. This default is:
M01: Board outline and routed cut-outs
M02: PCB Info
M11: Top Dimensions
M12: Bottom Dimensions
M13: Top Component Outline And 3D Body
M14: Bottom Component Outline And 3D Body
M15: Top Courtyard
M16: Bottom Courtyard
No acute angles (typically set minimum angle to 85 degrees)
No silkscreen over pads (clearance 0.01mm)
Track and gap (typically 0.2mm)
Minimum annular ring (typically 0.1-0.3mm)
Minimum hole size (typically 0.2mm, 0.1mm for lazer drilled)
Polygon connect style to via by direct connect
Polygon connect style to all other by thermal relief
As a general rule, make the polygon clearance to anything at least 2x the minimum track clearance. Shorts are more likely to occur between a large polygon and a track rather than between two tracks.
Flip the board (shortcut V, B) when routing and checking correct pin connections on the bottom layer of the PCB (otherwise pins will appear the wrong way around)
Make sure similar amounts of total copper are on each layer. A good way to ensure this is to fill each layer with a plane (either ground or a power plane). This is to prevent the PCB from going ‘banana’ during manufacturing.
Large fiducials are placed as far apart as possible on PCB (typically two, one in each diagonally opposite corner on a square board). Micro fiducials are placed on the diagonals of fine pitch chips (such as BGAs).
Circular speckles of solder mask are applied to chips with large exposed pads rather than the entire area, to prevent the chip from floating during reflow soldering. This applies to chips such as QFN and DFN.
Large exposed pads on the undersides of SMD packages are connected following the instructions on the datasheet. Most are either connected to ground or left floating.
Tracks and vias are large enough to handle their current requirements.
Appropriate pull-back on power planes and clearances on polygons and tracks from the edge of the board. 0.5mm is typical
Vias are tented (except for test points). This is so that silkscreen can go over them.
Ground vias are peppered all over board
Ground vias are placed around edge of the board
Polygons are set to direct connect with vias
Polygons are set to thermal relief connect (typically four connections) with component pads
Make sure vias are not cutting into component pads
Connector pins are labelled, either numbered or described (especially if using terminal blocks)
Test points are labelled
Rebuild all polygons
DRC (design rule check) is carried out
Lock all PCB objects
Find out whether manufacturer wants paste on fiducials (not usually)
Make sure Gerber output contains all the required files (including a file for every copper layer)
Do not send the keep-out layer to the manufacturer. Some people use it just as a board outline, while others use it to also prevent Altium from drawing on layers in other specific places on the PCB (such as adding clearances to objects). This creates confusion. Use Mechanical 1 to define the board outline and any routed holes.
Make sure manufacture information is added to the top copper layer (copper layer is good because it is included in Gerbers). This should include:
What layer defines the board outline
Who determines soldermask expansion (customer or sometimes manufacturer)
Number of layers
Minimum track clearance
Minimum annular ring
Minimum hole size
How many individual boards are on a PCB (if it has been panelised)
How board are going to be cut (e.g. v-scoring or routing, if panelised)
Include additional images with PCB project to instruct manufacturer on how to build/assemble PCB. These include images for counter-sunk holes and components which need gluing
Zip up PCB project and place in release folder
Changes/notes file created (such as readme.txt). This can be incorporated into Altiums project structure.
Once the PCB has been submitted, PCB project folder is stored and locked or committed so that it can be referred to in the future.
Make sure version and revision numbers are labelled correctly both in project documents, folders, and zip files.