Silkscreen over Solder Mask - OSH Park

Layout Footprints
1

Today I received a prototype board from OSH Park. It has missing silkscreen items.

The first conclusion was made that silkscreen is not allowed over copper, nor allowed over board; in ohter words, must be over “solder mask”. However, this is not always the case. In the Windows version I am using I can not detect that there is anything out of the ordinary.

However, a friend of mine running a recent nightly build of KiCad in Linux noticed this:

1920×1029 119 KB

That^^^ is is my Win file viewed in his Linux build.

This is what I have on my screen:

1017×651 21.8 KB

Over the phone we discussed and selected all the same render and layer check boxes.

We are not 100% certain what exactly is going on at the moment. This post is to see if others have any extra insight to help pin down what is going on.

KiCad is great. OSH Park is great. I have zero complaints at the moment. I would like all of my silkscreen to show up though.

All suggestions/comments welcome.

Thanks in advance.


^^^ On Edit: Photo of the board.

2

I’d ask what it looks like on the gerber but I see that take KiCad files direct. Did you submit KiCad or gerber?

1 Like
3

I submitted a Gerber.

That is one of the next steps to check. Just trying to ask if anyone already knows without us checking everything.

Thanks for your reply.

4

For comparison of your KiCAD versions:
Both go to the KiCAD main starter and under Help click on the About page.
Then copy the version info (button at right bottom corner) and compare what it says there.

I guess:
Seems your friend has ‘show pad clearance at all times’ active under display settings or thereabouts.

(nightly version screenshot!)

To your problem:
OSHpark seems to have a tolerance that they apply to the clearance, and if bigger your line will be removed ( which they naturally don’t state on their spec page) :slight_frown:
Those silkscreen lines are (if normal 0.15 mm thick) less than 0.15 mm from the soldermask edge and just barely 0.15 mm from the copper, for the areas where you got in trouble.
My rule of thumb is 0.25 mm for center of silkscreen to edge of copper (for 0.15 mm silkscreem), if in doubt (=current grid would nudge it closer) even a tad more - at least that’s what I do.

PS:
KicadLibraryConvention-2.0

7.3.3 Silkscreen clearance
Silkscreen must not be placed over pads
Silkscreen must have at least 0.2mm clearance around pads

… you see, my personal 0.25mm from center of silk to pad edge rule of thumb is even a bit tight for the KLC (0.25mm - 0.15mm/2 = 0.175 mm < 0.2 mm)

PPS: I have noted down in a txt file a silkscreen tolerance of 0.12mm for cheap/economical fabs.

PPPS: if that footprint (or others with same problem) is out of the official libs you should correct them and make a pull request to get them updated. :hugging:

5

Well, this just popped up in another thread. We might have our first real test.

First public version of KiPadCheck.py is available on Github

Please make comments or ask questions in this thread1

6

Thank you. I will point him to this answer.

It was just a little bit frustrating to avoid Silkscreen on copper, when I also needed to avoid Silkscreen on board.

And then to find that I needed to avoid Silkscreen on some other dimension.

7

That’s part of the experience… some fabs can’t do full circles on silkscreen (ask how I know :wink: ) or will ignore your soldermask over copper pads (ask how I know :wink: ) etc. pp.

If you do prototypes, this is no biggy.

If you do production, do proto run(s) and make sure the company you order from doesn’t swap fabs between trial/production (Elecrow for example does this) and make sure you nail most of the problems beforehand (= make your design as idiotproof as possible).
This also includes to not get too close to the minimum tolerances/specs they are able to do, unless you absolutely have to.

PS: where did the footprint came from btw?
If you did it yourself, rework it along the KLC and check all others you got. It’s really sensible rules they are having in there.

8

You do not want to know… LOL.

Reality is that I can not quite remember; but it is more then likely a personal “hack” of mine.

The KLC is great for “compliance”. But I don’t think my company wants to comply with others my designs at this time. For example, I really dislike (hate) the diode silkscreens in the KLC.

I think the KLC needs to be what the KLC is; but I think I can do better for my needs.

I’ll try to get a photo of a portion of my board silkscreen with better lighting tomorrow.

Thanks.

9

The latest version of KiPadCheck enables the text thickness and graphical item width check when checking those silk items against the copper in pads.