minimum font size for PCB's

[Simon]

I'm trying to cram as much as possible into my boards and in order to actually make it worth while using 0805 over 1206 I should also use smaller text (something diptrace could not do  ) but how small can I go ?

[mikeselectricstuff]

Depends on the manufacturer - some will include silkscreen line widths in their capabilities specs - Eurocircuits quote min imum line with 0.17mm and character height 1mm.
It will also depend on what process the manufacturer uses.

[Simon]

Well the size diptrace forced me to use seems to be 1.6mm so 1mm is progress. I'm just wondering what is common as I don't want to lock myself to one manufacturer.

[rich]

Hmm, I have a dip trace board here where I can barely read the silk screen due to its thinness. Font size 4, line width 0.15mm. I suspect the actual silk screen wasn't printed that thin.

[KuchateK]

You can make smaller font on component markings in DipTrace.

Go to View > Component Markings > Font. Size 3 is approx 1mm. Default size 5 is 1.6.

[Simon]

Well I'm using KiCAD now where I can actually tell it what I want never mind "sizes"  but I need to come up with something that I use as standard that is as small as most manufacturers will handle and that I can read.

[Bob F.]

The info I have to hand is:

OSH Park: "Lines thinner than 5 mils will be fattened to 5 mils (0.127) "
Elecrow: "Minimum silkscreen text size: 32mil (0.813mm)"
ITead: "silkscreen line width min: 6mil (0.152mm)  silkscreen text height min: 32mil (0.813mm)"
Ragworm: not specified.

6mil lines x 32mil high per char is looking like a working minimum but one can only guess on the quality of the finished text if one pushes those limits.

Cheers, Bob.

[rich]

Where I can, I use 1.2mm for legibility without magnification, but will go smaller/larger depending on layout constraints. Anything less than 1.2mm and I print out a zoomed copy to use as a reference on the bench so making the effort to put the designators in sensible positions is rewarded in the print out even if the silk screen is nearly illegible.

If you are trying to choose a house style for your own work, consider what pitch you will be laying your 0805s out and choose something which works. Say 1.8mm between centres would suggest something of the order of 1.4mm could work for you.

Obviously user instructions and pinouts as large as you can make them within reason.

Not sure how useful this image is now, but I've taken it already and will upload it . These markings are 0.7mm/0.15mm pcb manufactured by Elecrow low-cost service who's rules are 0.8mm/0.15mm so it's not a surprise the eye of 'R' is filled. Shaky camera doesn't show it at its best but for size reference: U5=SOT23-6; C13, C15=0805; R32=0603 all with 0.7mm characters.

[Simon]

Thanks rich, I think i will standardise on 0.8/0.15, I also print out an enlarged PCB layout to help me locate parts when assembling. It's just stupid to have have the board full of silkscreens that will never get read.

[mikeselectricstuff]

If a board's going to be machine assembled there's little point in putting part refs on, though things like polarity and pin-1 marks are essential to spot any errors.
 
Labelling test points can often be a better use of space, as these will help any time a board needs faultfinding.   

[sleemanj]

Hmm, I have a dip trace board here where I can barely read the silk screen due to its thinness. Font size 4, line width 0.15mm. I suspect the actual silk screen wasn't printed that thin.

Silk is pretty variable dependin on fab.  I have used vector size 4 normal width with diptrace fabbed through dirtypcbs and it was fine. http://dangerousprototypes.eu/forum/viewtopic.php?p=60821

PS: I think "size" and "pt" is probably the same in DipTrace, don't know why they use two names.  A point is defined as 1/72 inch if you don't know, which makes 4pt just shy of 1.5mm (but that doesn't necessarily translate to a dimension of the characters in the font, typography units are silly).

[T3sl4co1l]

Most fabs will do 30/6 mils (height / line width -- applicable to standard stroke fonts) just fine.  I've done 25/4, which is pushing it on legibility (let alone readability without magnification), even for the better fabs.

The minimum line or graphic width is usually something like 2 mils, which is probably a spotty line, if you actually use one.

Tim

[Karel]

Eurocircuits quote min imum line with 0.17mm and character height 1mm.

That's only an advice from their side. We use 0.8 for size and 15% for ratio in Eagle which equals
0.8mm character height and 0.12mm linewidth. This goes fine with Eurocircuits.

[exmadscientist]

My standard for OSH Park's 4-layer service is 0.6mm height/0.127mm stroke (24/5 in mils), which I find matches decently well with 0603 parts. For more tightly packed custom-spec boards I go down to 0.5mm/0.1mm (20/4) which I've had no trouble with. It does usually require magnification to read, but those boards are always machine-assembled anyway, and having the designator helps with the inevitable prototype troubleshooting and rework.