FEDEVEL
Platform forum

simeon , 11-30-2024, 02:45 AM

Is it true that silkscreen on top of the solder mask expansion won't give me an error or are the rules in the settings wrong perhaps?

simeon , 11-30-2024, 02:48 AM

Edit: Ahaaa, I see that in the rule it has two **Clearance checking modes**. Which one of the two should I be using? Currently it is checking relative to the copper and not the solder mask opening, hence no error present I'd assume.

Which one should I use or is preferred to be used?

Robert Feranec , 11-30-2024, 06:48 AM

I don't have altium here, please could you attach a screenshot?

QDrives , 11-30-2024, 04:11 PM

It depends... It depends on the fabricator capabilities and other settings.
Take https://www.eurocircuits.com/pcb-design-guidelines/legend-print/
There they state 0.1mm from exposed copper. If you have a solder mask expansion of 0.05mm, then it is 0.05 from solder mask opening.
However, for your fiducial, you may want to check that manually too.

simeon , 11-30-2024, 05:55 PM

@Robert Feranec The 'clearance checking mode' option for the 28Pins project. But I guess it is manufacturer dependent as @QDrives mentioned, so I assume it wouldn't matter?


I didn't get it completely. So there ar two things about it basically:
1. **The legend must have the following minimum clearances.** Exposed copper (or surface finished copper): 0.100mm
2. **Legend print is designed to be printed on top of the Soldermask except for traditional single sided PCBs with through hole components where the legend is printed on the Top side of the PCB directly onto the laminate.**


Based on the second statement, does that mean that there can be no silkscreen on top of the solder mask opening of, in this case, the fiducial? What did you mean with *having to check that manually for the fiducial*?

QDrives , 11-30-2024, 08:06 PM

Again it depends.
There are fabricators that simply remove all silkscreen which is on top of solder mask (openings). The reason here is that it is very simple to do (automatically).
Strictly speaking, the silkscreen should not be over (exposed) pads -- which are used to solder components on as it would block the solder from attaching to the pad.
However, they may also opt for the clearance from the exposed copper.

Then it depends on the solder mask expansion that you set or the fabricator uses IF you choose to use a clearance compared to solder mask openings.
As solder mask expansion can be as little as 30um for LDI and up to 100um for PI https://www.eurocircuits.com/pcb-design-guidelines/soldermask/.
If you keep 100um from the solder mask openings and PI is used, then the clearance is 200um from the exposed copper.

If you keep the silkscreen clearance compared to exposed copper, silkscreen can be 'drawn' in the solder mask opening of a fiducial reducing the reliability of it.
I personally always check the fiducials that they are clear an open correct -- silk screen, solder mask and, most importantly, polygon pours.

Robert Feranec , 12-01-2024, 04:03 PM

@QDrives explained it very well.
You can set it the way which is better for you. Basically this rule mostly exists to tell you about possible places you may want to check (e.g. remove silk from pads or in your case from the unmask area around fiducial). But often you probably notice this problems by yourself anyway and most PCB manufacturers will remove silkscreen from pads automatically.