Correct size for the silk screen layer

[gyuunyuu1989]

Component silkscreen contains the outline of a component, a circle or some other marking to indicate pin 1, text that states the component designator or some aspect like polarity. So far I have not found any clear guidance regarding how the things on the silk screen should be sized.

Components come in various sizes and shapes. This ranges from small 0402 chip resistors to really massive BGAs with 1000s of balls. Some components are polarized and putting them the wrong way will cause design failure. ICs usually can only be put in one way.

This confusion is related to component outline and component text:

1. Component outline thickness on silkscreen. Should it always be 0.1mm?

2. Component outline distance from copper pads. It is not clear how far the outline should be from the copper pads. This is confusing because some components (e.g SMD resistors and diodes) are so small that they fit fully inside the copper pads and the package does not expand outside of them. However, other packages are so large that copper pads become hidden under them partially or fully.

4. Text font, size and line thickness. This is the text used to represent the component designator. smaller components need smaller font size. But too small and it won't be clear or will be hard to read.

As you can see, the questions are quite basic. Since there are so many different packages, there is no one size fits all. The question is, what is the proper way to do this. The silk-screen can't go over copper pads. It can't be so small that it can't be read or can't be printed reliably. It needs to mark polarized components correctly so its clear where the pin 1 goes. There is certainly a lot more to them silk screens.

[qdrives]

Step 1 -- https://www.eurocircuits.com/pcb-des.../legend-print/

1) No. My standard is 0.2mm for the legend layer. But do have some smaller components (0603) that have thinner lines. Text is more often thin.
2) See the guide and yes, small components (like <= 0402) do not have a legend.
3) Use the courtyard for boundary. I always place the legend lines outside the normal size of the components so that they are visible after the component is placed.
4) For user interaction components (connectors, jumper, buttons, LEDs, (non-resettable) fuses -> Text height 2mm, 0.2mm thickness. Other components 0.7...1mm and 0.1mm thick -- IF useful.

5) Place the designator close to pin 1 as an additional pin 1 mark.
6) Have polarity marking still visible after components are mounted. This could be at an angle.

[gyuunyuu1989]

I am able to come across documentation from manufacturers for the minimum possible line width and spacing that they can manufacture. However, the minimum is not necessarily the best. For text we need something that can be read even when the print is small.

Is there say a table that lists the outline line width, text height and text line width to use during footprint creation of different sizes components for the best result from human observer perspective? The issue comes with these two terminal devices because they can get actually really really small. Ultimately silk screen has no functional use in the PCB since it does not play any role in its operation. It only exists for the human use. We can't read smaller than certain size without using microscope. There would be other constraints on silk screen imposed by human observer as well.

[qdrives]

Oh do not worry about a microscope for silkscreen. The printing process is not good enough to allow a microscope to sense if it were to small.

However, the most important aspect here is the 'printing' technology. How is it applied.
I have seen text on a board with Altium settings:
0.7mm height, true type, Arial.
That true type aspect is very important as in "stroke" size, this would be something like 0.4mm height and 0.07mm thick.
This would be using screen printing. This text was readable with the naked eye.

However, if the silk is printed like a inkjet printer, the quality would not be so good and you would need 1mm height and 0.1mm thickness.

[gyuunyuu1989]

OK, so what text height and thickness should I use usually for SMD parts (starting with 0603) and ICs (like DIP, BGA .e.t.c)?

[qdrives]

How much space do you have on the board?

For most components, I do not have the designator on the silk screen, but because I want a reasonable size and there is not enough space to show them all.
And if we cannot show it for all of them, then why bother about the rest? Except again, for the 'user interaction' components (See pont 4 in my first comment).

So in the end, it is up to you.