Footprint text on mask layer not included in gerber output

Layout Gerbers (GerbView)
1

I’ve got an issue with gerber generation. I have text for PN and and revision to be placed in exposed CU so the mask should be clear over it.

In PCBNew I have the following section of bottom CU
image
and mask
image
(Note edge cuts also included both times)

In the gerbers I get the following bottom Cu

image
image557×566 20.2 KB

and mask
image
image630×572 13.5 KB

which does not show the PN: and Rev: text

The gerber views are from gerbv but the kicad gerber viewer shows the same.

I’m assuming I’ve missed something in either the layout or gerber generation

So the text properties

image
image953×828 33.4 KB

and the plot settings
image
image823×711 31.2 KB

Any thoughts on what I may have missed?

Oh and Kicad Version
Application: kicad
Version: (5.1.0)-1, release build
Libraries:
wxWidgets 3.0.4
libcurl/7.61.1 OpenSSL/1.1.1 (WinSSL) zlib/1.2.11 brotli/1.0.6 libidn2/2.0.5 libpsl/0.20.2 (+libidn2/2.0.5) nghttp2/1.34.0
Platform: Windows 8 (build 9200), 64-bit edition, 64 bit, Little endian, wxMSW
Build Info:
wxWidgets: 3.0.4 (wchar_t,wx containers,compatible with 2.8)
Boost: 1.68.0
OpenCASCADE Community Edition: 6.9.1
Curl: 7.61.1
Compiler: GCC 8.2.0 with C++ ABI 1013

Build settings:
USE_WX_GRAPHICS_CONTEXT=OFF
USE_WX_OVERLAY=OFF
KICAD_SCRIPTING=ON
KICAD_SCRIPTING_MODULES=ON
KICAD_SCRIPTING_PYTHON3=OFF
KICAD_SCRIPTING_WXPYTHON=ON
KICAD_SCRIPTING_WXPYTHON_PHOENIX=OFF
KICAD_SCRIPTING_ACTION_MENU=ON
BUILD_GITHUB_PLUGIN=ON
KICAD_USE_OCE=ON
KICAD_USE_OCC=OFF
KICAD_SPICE=ON

2

I’d suggest finding those strings in the design file with a text editor, and comparing them.
If one works, and two do not, it’s then spot-the-difference.

3

Please report this bug at https://bugs.launchpad.net/kicad

The text items are being plotted as negatives (knock-outs), which are inverted by the layer.

–Edit–

Actually, I just noted that your version information is old, so I posted the bug with as seen in 5.1.4 so that we can address it.

1 Like
4

Thanks @Seth_h, I take it there’s no workaround?

@PCB_Wiz, here’s the two text’s in different layers. AFAICT the only difference is the layer.

 (fp_text user PN: (at -20.955 -6.985 180) (layer B.Mask)
  (effects (font (size 2.54 2.54) (thickness 0.508)) (justify left mirror))
)
(fp_text user PN: (at -20.955 -6.985 180) (layer B.Cu)
  (effects (font (size 2.54 2.54) (thickness 0.508)) (justify left mirror))
)

Robert

5

My first glance had those as 3 strings, but I think the top text has sharp corners, so it must be shapes ?
so my suggestion thinking one worked, did not apply to all-text…

I think seth_h may be right
The text items are being plotted as negatives (knock-outs), which are inverted by the layer.

Perhaps there is a workaround.
There was an earlier thread about negative text, and someone did a gerber merge utlility that takes two gerber files and combines them as LPD / LPC (plot Dark / Plot Clear (inverted) )

Or, you could create a simple rectangle as your no-mask, for the text to show thru ?

1 Like
6

@PCB_Wiz The gerber merge would be kind of hard to maintain since it would need re-applying on each generation. The rectangle is definitely trying.

Yep, the rectangle does indeed get plotted as expected to the gerber so that should work for this case. Might not work for everyone that runs into it but it’s sufficient for this particular instance of the problem.

Thanks
Robert

7

You can place the text on the board as a text item instead of inside the footprint. We’ll get this fixed for 5.1.5.

3 Likes
8

Yep, that seems to work. So two work arounds available.

9

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.