PCB finishing touches - Silk

[mrburnzie]

Currently in the "finishing touches" phase of a project. I'm adding logos and other info like project name, version and date to the silk screen.

What are some things that you add to the silkscreen?
What rules are you following?
Are there some guidelines even for this?

All the best.

[nvmR]

I always add a box in the silkscreen with # in front of it - for board serial number. Either write in it using permanent marker, or place a sticker with a bar code.

[Rerouter]

If there is room, for any connectors I will try and fit in the pinout,
If there is room under a DIP part / module, I'll write on the underside of its pinout its pin names,

if there is a power input, I'll add the polarity and voltage range
etc, documenting the board so when I come back to a project in 3 years, I dont have to curse myself too loudly

[Terry Bites]

Mark out areas that operate at differing voltages. eg mains and low voltage areas, mark out isolation barriers.
HV warnings etc
Test points. eg TP1 12V

[Infraviolet]

Definitely mark which signal pin is which on any connectors going in or out of it, especially if any connectors are headers for standard 2.54mm pins where you'd be plugging in individual wires (potentially in any order) rather than plugging in whole multi-way cable assemblies at once.

I wouldn't tend to bother with marking pinouts of individual chips though, the only time you'd need to refer to those is during debguging, for which you'd probably have the full schematic and board diagrams to hand at the time.

[nvmR]

oh, how did I miss my favorites.
Diode directions (including leds), and pin #1 for each and every device. a small dot can suffice.

It is also fun to do a picture as a silkscreen. Some eye of Sauron, or logo from your favorite movie!

[thm_w]

https://pcbchecklist.com/

[Siwastaja]

+1 for pinouts and other documentation, especially for prototypes.

[Uky]

My experiences with PCB design:

The vendors I have used accepts 1mm text hight as the minimum. Others can do even smaller but its getting more and more difficult to read.

For small text sizes: Use 0.1 mm apperture. Keeping the relation "apperture/text hight" to ~0.1 will provide good readability.
Compress the texts, minimizing distance between characters and by making text hight > text width.

I always design polarized thru-hole component (copper) pads with a square for positive (electrolythics), cathode (diodes), DIL-foot prints with a square for pin #1.
If ordering prototype boards without silk this eases populating the board.

Place reference designators outside the foot print and closest to Pin #1 if possible.

Do not allow silk screen inside (underneath) any multi-pin foot print. Many PCB packages have "auto symbol creation" but they almost always create and place the silk in the wrong fashion.
Once populated, silk inside sometimes then hides pin #1 indicator.

When creating a footprint: Design the silk screen (outline) so that it does not cross any pad. Some PCB packages can automatically remove such silk screen elements
but IMHO it is better to do this already at the fp design stage.

And as others have suggested: For test points - add test point signal descriptions in the silk screen.

And finally: turn off all layers except silkscreen, copper pads/pins and vias. Check that no silk sits above (SMD)/pins or vias and that all texts are oriented in the same way, readable from left to right or from bottom to top (or the other way around if preferred).