Fab shop caught this. I have a 0.4mm pitch BGA, with copper pads 0.28mm dia, mask opening 0.254mm (mask clearance set to -0.026mm).
Not sure if I can attach images here, but on the board the mask looks exactly as it should. However when I generate Gerbers, the Gerber mask file shows “teardrop” connections between adjacent pads. The actual pads are not exactly round, but they look like if they were round and then you “pulled” each circle toward the adjacent pins. Generated PDF of the Gerber and it’s the same.
I’ve asked the shop if they can fix this on their own, and I expect they can, but obviously I’d like to figure this out so my Gerbers are correct.
If anyone has any ideas please let me know asap!
Thanks in advance
Dan
Can you reproduce your problem in a small example board that you can post so others can look at it?
Bear in mind that this is a forum for KiCad users, and not the official channel for bug reports. Check this FAQ for more information on filing a bug report:
https://forum.kicad.info/t/i-found-a-bug-what-now/9452
Doing some testing here with the Gerber settings. This might be a limitation of the “Default Line Width” in the Gerber generation settings. I can’t set it below 0.02mm. If I make it bigger, the problem seems to be worse. So maybe I need to be able to set it to << 0.2mm? Can anyone confirm that this is the issue? And hopefully it’s on a list of things to visit in future revisions.
I am using
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
The issue is with your Board Setup rules for “Solder Mask minimum width”
You can set it to 0 and allow your fab house to expand based on their process. 0 is what you see on screen.
3 Likes
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.