search

KiCad / Housings_SSOP.pretty

Shrink Small Outline Package footprints
5 stars 31 forks source link

Pin 1 indicator is not visible on manufactured boards due to silkscreen-to-mask clearance #15

Closed mrnuke closed 8 years ago

mrnuke commented 8 years ago

The small line that is supposed to be the pin 1 indicator is too close to pad 1. Once soldermask clearance is taken into account, the silkscreen line would end up falling on bare FR4. This happens with 0.15 mm pad mask clearance.

I've tested Oshpark and seedstudio, and with both manufacturers, the pin1 indicator line is removed, and there is no way to identify the correct orientation of the footprint.

img_20160725_210323

SchrodingersGat commented 8 years ago

I have addressed this in https://github.com/KiCad/Housings_SSOP.pretty/pull/12

In future please feel free to make pull requests yourself to fix these issues :)

CarlPoirier commented 8 years ago

12 is merged, so closing the issue. Thank you @mrnuke for reporting it.

mrnuke commented 8 years ago

These are manufacturing examples with git commit 2933ce3

sssop_mfg ssop_mfg_scan

mrnuke commented 8 years ago

This specific example was manufactured at oshpark, with default kicad settings. oshpark's reference rendering is included below.

mfg_render

michal777 commented 8 years ago

The mask clearance looks quite big. The footprints in the library has not the mask clearance defined so they use global settings. Maybe you have set it too large? I guess the setting should be zero and the manufacturer modifies mask according to his technology. I've used the the clearance set to zero and my boards looks fine (it may depend of manufacturer).

mrnuke commented 8 years ago

Mask clearance was set to 0.2 mm (8 mil). For oshpark, the tightest is 0.15mm (6 mil), and that sort of figure seems to be common among commodity manufacturers.

I see two ways to go about this.

  1. Say mask clearance must be at most so and so, and call this a user error.
  2. Say that if a process is capable of manufacturing the feature size, the footprint should work with such process.

In my opinion, assuming a clearance of 0.15mm would work, a difference of 0.05mm should not cause such a dramatic outcome on a human-visible feature.

SchrodingersGat commented 8 years ago

@mrnuke can you post a screenshot of the silkscreen gerber layer you sent to OSHPark? Comparing the screenshot of the KiCad render with the boards you received, it looks to me like the silkscreen should have been on the final board.

The middle part (SSOP-16_4.4x5.2) for example, the top line does not look like it should intersect with the solder mask at all - it looks like it has been completely removed, either by OSHPark or by KiCad when it was plotted...

michal777 commented 8 years ago

Looks like they added their mask clearance to yours. Won't they accept just zero mask clearance on gerbers?

mrnuke commented 8 years ago

I uploaded the kicad_pcb file [1] directly. If you zoom in enough, there shouldn't be an overlap with soldermask (there's a clearance of 0.025mm/1mil).

[1] https://gist.github.com/mrnuke/10e3027b3196ba24202a1db71d90fb26