Many times I have seen PCB's where the top layer white ink overlay has been crap. Like with writing software, consistency, clarity, ease of use and effective communications to the next poor bunny is almost everything. It is worth the extra effort to make PCB artwork look like it was done with pride. Here are some suggestions that might help others - you can agree or disagree. I would be interested to know of any other good practices others have used for top overlay.
(1) Pin 1 markers. Don't use circles on footprints at pin 1 markers. They look like fly vomit or soldered vias to those of us with challenged eyesight. Moreover, sometimes they are ambiguous between components for example when in a neighbourhood of SOT23s close together. A small slightly isosceles triangle as a pin 1 marker on a footprint stands out very clearly, even if it is tiny. It is unambiguous. No-one makes triangular vias and flies don't vomit up triangles.
(2) Wherever possible, place your component designators so the bottom of the letters are facing the component. If this cannot be done as in the case of a number of resistors "in parallel" next to each other, place the designator with the first character (eg: the R in R123) closest to its respective resistor. This tends to reduce ambiguity and confusion. Reading designators upside down is a mild inconvenience compared to guessing which SOT23 is Q12. Keep the designators, as far as practicable to the same font size, and of course, type.
(3) Make the character line thickness to 1/5 of the character height on non-TrueType fonts. This seems to yield the clearest characters for the average PCB. For example, a 1.5mm high character can have a 0.3mm line thickness.
(4) Keep designators at a consistent distance, as far as practicable, from component bodies. Spend some time aligning designators for equal spacing and offsets from the component bodies, so it looks really neat and professional. Neatly aligned designators impresses chicks.
(5) Back annotate so that the PCB designators are all relatively near each other in a logical pattern physically. Some people think this is bad practice, but there is nothing more frustrating when for example you cannot find R23, but can find R21, R22 and R24 amongst a sea of components. If this sounds trivial, just ask any debug technician how much time is saved when he can actually find components quickly and easily on a PCB.
(6) Use consistency in labelling. Make it look professional. Use smart abbreviations as required. Use underscores to join nearby words if it removes ambiguity. For example: "PWN IN PWR OUT" is much better written as "PWR_IN PWR_OUT". Labels for users to read may be larger than the component designators so they stand out.
(7) Mark the PCB next to connectors screw terminals with what the terminal function is. For example: "+5V 0V -12V", and under it "POWER IN".
(8 ) When making footprints, make the outline of the component to avoid ambiguity and or mistakes when the part is inserted.
(9) Be aware of the PCB's manufacturer's capabilities. A quality manufacturer can print small fonts with clarity, whereas some cheapo manufacturer might just blur the characters. With good manufacturers, you may be OK using a serif font rather than a san-serif font.
(10) Use correct spelling. I have seen "RECIEVER" printed on a board (and in source code). If someone laying out a PCB cannot spell "RECEIVER", they should not have graduated from junior high school. There is no excuse for bad spelling. If you make typos like I do, have someone review your work.
(11) Have a library of marks and logos, such as RoHS and company logos etc as graphical components. Don't manually add them each time you do a board. It is a time saver.
(12) I could be wrong here, but use "REV 1" rather than "VER 1" Revision implies a sequence of modifications to the same product. Where version implies multiple versions exist at the same time. I use "REV 1".
(13) Place as much instructions as practical and useful to the user on the board. Motherboard manufacturers are really good at this. Avoid having users read the manual for connections, which might be out of step with the PCB revision.
cheers,
Dave