I'm working on a fairly dense PCB at the moment and I'm having trouble fitting in all the component labels.
What is the minimum readable standard size for component designators on the silkscreen?
For example: What should the width and height be here?
0.6mm high 0.2mm width lines is usable (a bit fat) in default stroke font.
You could try a bit smaller than 0.2mm width, 0.18 or 0.15mm (6 mils).
Best to work with your PCB vendor, not all can reliably reproduce such fine lines on the silk screen layer. In general, I've seen more problems with lines coming out too light and breaking up than being too heavy and becoming unreadable as a result.
On my own boards, even the most dense, I never go below 25 mil height by 5 mil stroke, and I even hate to go that small because it's practically unreadable. Generally speaking a "safe" designator size is 45 mil height by 10 mil stroke. There will most definitely be cases where this is much too large, so I would say use a size as big as you possibly can, but no smaller than 25 mil by 5 mil.
When arranging designators on dense boards I sometimes find it useful to group designators together slightly away from their respective components, and draw rectangles and lines to indicate which "group" of components they go with. I generally do this for diodes, resistors, and capacitors. Sometimes the lines may not even be necessary, especially if your components are in a unique shape which you can imitate with the silkscreen (see below).
There are a number of tricks that help make positioning designators easier, even when they are relatively large. Whether or not to include lines "grouping" the designators and components together is completely up to you as the designer. Just keep in mind that clarity is key. If you don't make it clear which designators go with which components, your board house will keep coming back and asking you for clarification.
I find the minimum readable size is 15mil height by 5mil width. You can go smaller then that but you may find it hard to read the board at that point.
Well, then just leave it off. Is there a specific reason you require it? Make sure you create a well-readable assembly plan and you should be good to go.
On technical side, possibility to print small text is up to PCB manufacturer. You should consult with yours. Normally they should provide data on minimum line width and height of text. If only minimum line width is given, least reasonable height of digit and capital letter is 5x of line width (say, for "8" they should print 3 horizontal strokes and 2 gaps between, giving 5 line heights total).
On ergonomic side, consider human limits to read. First, there's least perceived size of letter. Per ISO 9355-2 it is 15 arcminutues. Second, there's least comportable read distance, which is about 40 cm. This gives least reasonable letter size of 40cm * (15/(60*180/pi)) = 1.75 mm. While most people can read below this limit, it is recommended to use magnifying devices with smaller letters. However in most modern designs text height is about 1 mm or even below, and magnifying glasses are widely used in manual PCB assembly.
