Make a product: Schematic / PCB release checklist

Part number should be of the form:
nnnnnnnn-vvv rrr
Where nnnnnnnn is the base part number
Where vvv is the variant number
Where rrr is the revision indicator (Rev. A, Rev. B, Rev. C, Eng. A, Eng. B, Proto A, Proto B, et cetra)

On "full" designs, have a cover page with specification. (Not needed for quickie jobs.)
Be sure to have a title block, including part number, revision number, sheet info, etc.
Don't be afraid of multiple pages and using blocks. Use net-name connections to your advantage.

When choosing the part, verify RoHS / LeadFree, and that there are no other limitations (max temperature, no-water-wash, et cetra). If any special requirements exists, make sure that is noted on the schematic.
Cross check the mfg part number and device footprint between the datasheet and Digikey/Mouser.
Verify that the mfg. part number corresponds to the desired footprint. Cross check Digikey and the datasheet.
Do a digikey/mouser scrub.
Confirm that each pcb part has the correct p/n and footprint. Look at a sample of each component type to make sure it "looks right".
Identify key components for performance/safety reasons -- indicate no-substitution for these items.

Make sure connector clearances take into account the Z height as well as PCB footprint.
Make sure there's plenty of room to route cables, and to connect/disconnect any internal connectors. Make sure your fingers (or tools) can get in there!
The schematics should have a drawing showing connector pin-order for easy reference. Include the drawing of the mating cable, too.

Define board size. Verify that the board size will fit in the intended enclosure.
Make sure you define a 3/8" rail (or component clearance) on parallel edges so that the board can sit on the reflow oven conveyor
Locate the board "origin" 1-inch from the edges of the PCB document.
Draw the outline of the board on a mechanical layer, and put dimension information.
Draw the keep-outs of the board.
Make use of multiple drawing/mechanical layers to write in comments, add mechanical outline information, show tab-routing details, silk-screen notes, et cetra. Enclosure drawing should be in here, too.

Board hardware (PEM nuts) should have location markings.
The BOM should specify part number, diameter, threaded/non-threaded.
Board hardware holes should be unplated
Large mounting holes for solder-mounting should have large spacing to traces and vias to prevent bridging. (Hint: create a design rule to enforce this on specific holes/pads)
Make sure all mounting holes are the right size, have the right annular ring, and that any hardware that come in contact with the PCB will clear components, vias, and traces.

Verify that pin #'s are correct, and that there are no duplicate / overlapped pads
Verify that the footprint matches the drawing, and that both are drawn with the same orientation (sometimes, mech. drawings show details from the under-side)
It's helpful to create a separate mechanical layer just to take measurements.

Make a BOM showing component mfg, p/n, digikey p/n and footprint.
Generate a preliminary BOM to review. Confirm that each schematic part has the correct p/n and library part. Make sure that the library part is non-generic.
Be sure to specify panelization information in a drawing. If 1-up'ing the board, make sure there is component clearance on parallel edges of at least 1/4" on each side. If N-up'ing, make sure the panelization will fit on a standard panel. (18"x24" panel?)

Make sure part numbers and revision information is up to date on the schematic & PCB.
Save a dated copy of the schematic and the PCB.
Export PCB file in ASCII format acceptable to the board house.
Generate a final BOM. All relevant info should be generated from the schematics, and not require manual edits.
Print PDF of the schematic, and the board assembly drawings.
Generate CAM files: create Gerbers, pick-and-place data.
Put together a "Readme" file, specifying contact info, build notes, board construction details (thickness, layers, plating type, RoHS/NoPb process, UL/NoPB markings as needed, et cetra, water-wash ok). Text file listing filenames and their use.
Add any assembly pictures or drawings.
Add any mechanical drawings and CAD models if appropriate
Put together a separate ordering info document specifying turn-around time and quantity

There should be at least a preliminary product documentation.
There should be a complete board test/checkout procedure for pilot/production runs. (Not needed for initial prototypes).
Manufacturing fixtures (jigs, wiring harness, testers, etc.) should be designed and documented as well.
Provide plenty of pictures.
Maintain a post-release bug list / improvement list / ECO list to be incorporated into the next revision.

Make a product