Why do some PCBs have the courtyard in the silkscreen layer?

Question

I've seen quite a lot of PCBs which have the passive components outlined all the way in their silkscreen.

Something like this:

Here there is an outline around each passive which goes (almost) all the way around, and seems to be sized exactly the same as the courtyard - the lines for components placed side by side overlap.

This style is apparently very common in high-volume stuff designed and mass produced in China - in this case a Bluetooth module, but I've seen lots of other boards which are the same.

Why is the silkscreen done in this way?

Is there a functional reason for it? Is there some way it makes assembly or inspection easier at volume?

Answer 1

Picture the workflow for initial prototypes on a long string of resistors like on that board. If not for the outline, you'd be forced to start at one end and proceed to the other, or risk getting off by half a component.

Answer 2

I do this all the time, the main reason being it allows a nicer visual appearance. The other nice thing about it is it enables a PCB designer to space components with minimum width between them.

Space can be a major factor on many PCB designs, nothing the minimum width can dance space (and make the design smaller)

Answer 3

Makes visual inspection of correct component placement easier to spot. Or to identify missing components. For example, I see two sets of pads with no components installed.

Answer 4

Silkscreen borders make the PCB layout easily readable by humans. They are not useful for automated PCB population or AOI.

Modules for electronics enthusiasts need to have readable PCB layouts because a lot of eyes will be looking at those PCBs. Mass-produced PCBs in finished products which are not intended to be serviceable often have little silkscreen, sometimes only identification codes.

Answer 5

The courtyard and the silkscreen are different things. The silkscreen is visible on the board, the courtyard is a design concept and visible only in the PCB Design Application.

Generally the silkscreen outline is slightly smaller than the courtyard outline. Courtyards can touch each other, so if the silk outline would be the same, two resistors would have a shared silk line if their courtyards touch. So the silk line must be a bit on the inside of the courtyard to make sure that there is some space between the silk lines of two different components as you see on boards.

The silk outlines and courtyards are suggested by the IPC-7351C document. In IPC-7351B the courtyards were rectangular, they can now be "arbitrary" and more closely follow the component's outline. The silk outline for resistors, diodes and capacitors are not rectangular either.

Below you can see a detail of one of my boards. I haven't updated the outlines of all my components yet - the lines in blue are the silkscreen lines, the lines in grey are the courtyards. You can confirm that this is inline with my explications above.

---

Ben Voigt's remark caused me to look in more detail. The picture has some cases where the shared lines are larger (around the crystal) and other cases where the lines are smaller (between the columns on the far right). So it seems that the designer may have done one or more of the following:

• Not use courtyards and only had silk lines, using them as some kind of courtyard;
• Not respect design rules if he did have actual courtyards.
• Had overlapping "courtyards" (for the cases where the silk line are smaller) - and this resulted in the production files being automatically adjusted to avoid having silk on the pads (these adjustments may be made by the PCB design tool, and are in my experience also applied by the manufacturer).