Silkscreen text outline width is too thick, creating blurry text


#1

I’ve been creating boards and having them manufactured by OSH Park. When I get them back, the text always looks quite blurry. They indicated that the problem was the outline stroke of the text was 8 mil lines, making small text (1-2mm size) look very blurry the problem was with the gerber files I supplied.

Hand tweaking the silkscreen gerber to use a thinner stroke yielded much better results.

  1. Perhaps the text tool could be smart and specify a proportional stroke width on the text? Seems like this is much too thick for small text sizes.

  2. Is this adjustable somewhere for me to tweak it now?

Thanks,
—Joey


Low quality of silkscreen text in gerber files
#2

Thanks Joey, I’ll put a bug in the tracker to investigate this further!


#3

Awesome, thanks.

The board I’ve been working on is:
https://upverter.com/joeyhagedorn/f3f2c238aae66400/DC-002/
I exported gerbers from revision 4881.

Resulted in this blurry text:

The OSH Park folks gave me a workaround:

It looks like what they’re doing is drawing the outline of the text using 8 mil lines. That’s a really thick line, so it makes the text look really muddy.

It is possible to manually edit the gerber and shrink the size down. For example, if you open up the “top silkscreen” gerber (the one ending in .GTO), and change the line that says :
%ADD11C,0.2032*%

to:

%ADD11C,0.1*%

The text looks a LOT sharper on upload.


#4

You’re right, thats pretty ugly. Looks / sounds a little like its just an oshpark issue. Let me chat with @StephenHamer and see what we can figure out.


#5

Hi all, we’re seeing the same issue with Sierra Proto Express. We have a board in with them and they’re reporting that the text will come out blurry/unlegible if printed as-is. The workaround seems to work, though!


#6

Any fix for this issue? I see the same thing with a different fab house. If you inspect the gerber data it appears that the line width applies to the outline of the text. If you scale the text up you see it pretty clearly.


#7

I was playing in a cam editor and it looks like you’re generating ‘non filled’ text. This is Altium’s CAMTastic. It has the ability to generate filled and non filled text (with true type fonts). Have you considered adding this feature?


#8

I can confirm the blurriness on boards from MacroFab as well.


#9

Text on copper layers renders nicely (filled, not outline) in the gerbers. Can Upverter just use that same algorithm on the silkscreen layers? Why is it different to start with?


#10

I had the same problem with all my designs. The problem is related to how Upverter outputs the Gerbers for top and bottom overlay layers. It happens that, instead of generating the Gerbers from the center of the line, Upverter considers the overlay outlines! If you analyse your GTO or GBO in a CAM tool you will notice that a simple dash (-) will generate not a line, but a rectangle.
Original design (top & bottom copper and top overlay):

Resulting gerber from CAM viewer:

Most of PCB manufacturers will use their minimum silkscreen thickness capability on the outline. So they will use something like 4 to 8 mils as the text outline not the text center like (because there’s no such think in Upverter!). That’s why they will result in blurry text.

I don’t think there is a solution for this. Some workaround may work for your design/fabrication like manually change the outline width to fab’s minimum capability and ask them to fill the boundaries of the resulting polygons.

Regards,
Daniel


#11

@zak This is clearly NOT just and oshpark issue. A cursory review of the original post and upverter-made gerber files show that the gerber output is not faithful to the design shown in the upverter eda tool. Further, this issue has be present for more than 2 years!

An export from today shows that text is exported with a border but in the correct geometry. This is gerbv vs. upverter:

An export and produced board from Dec. 2014 show the same bug including on the production board:

Looking at the gerber files for silk and copper layers show that text is exported with an aperture of “%ADD11C,0.2032*%” which means circular with diameter of 0.2032 mm (8 mil). We can confirm that rendering of gerbv is correct by editing the gerbers to use a circular aperture of 0.0 mm diameter and noting that the geometry exported is correct.

The correct way to render text seems to be either a line-based font with user-selected (or scaled) width (aperture), or to render it as you are now but using polygon fills (G36/G37). Please consider using some resources to fix this long-standing bug.


#12

Did this ever get resolved. I’m having the same blurry text issue. I really like Upverter and would consider the paid version but it is worthless if you can’t get clean gerber files.

Any help would be appreciated.


#13

No, this did not get resolved and it’s still a problem. I included a link to this thread in an email to @zak about 6 weeks ago, but never heard back on that either.

I agree that Upverter has some big shortcomings around exporting, especially for production & assembly. That’s a real shame, because it’s an area where I’d expect a SaaS offering like Upverter to really shine above the competition.


#14

@ihartwig @mcbuilder22 @daniboy @jasonmills @seveibar @shisalabs @EnTg888 @joeyhagedorn

Hey Everyone,

Thanks for your patience with this item. We recently released code that fixes the silkscreen issue. The project will require a change (eg. move a silkscreen item) to initiate a re-generation of files.

If you’re still seeing issues with the silkscreen let us know.

Cheers,
Patryk


#15

That appears to have fixed the issue.

That was an issue that was keeping me from using Upverter.

Thanks