search

KiCad / kicad-footprints

Official KiCad Footprint Libraries for Kicad version 5
https://kicad.github.io/footprints
Other
617 stars 714 forks source link

missing silkscreen on 0402 passives #799

Open Shackmeister opened 6 years ago

Shackmeister commented 6 years ago

Hi guys (probably @poeschlr the most)

I just used updated some of the 0402 passives, and noticed the missing silkscreen. At my company we typically use 0402 for everything and likes to handsolder the first prototype. The missing silkscreen quickly makes it harder, since a bunch of resistors will look something like the image below. resistors_no_silk I would like to recommend 2 different styles which could be used to clear up the confusion this might bring. The second one would however require a KLC change since silksceen under the component, to aid assembly, is only allowed for THT components.

Style 1, should be fully KLC compliant: r0402_2_lin

Style 2, not KLC compliant r_0402_1_line

poeschlr commented 6 years ago

Sorry the later one is not a good idea. Silk under the body is no good. (Increases risk of tombstoning)

For 0402 imperial there is just too little space to get decent silk in there. For the default line width of 0.12mm i would get 0.1 clearance to the pads with just 0.04mm long line. (So basically a dot)

For this reason it was decided not to include silk in parts smaller than 0603 imperial.

Edit: If we ever add handsolder variants for these, then it might be feasible to include silk as you suggest in the last picture.

right now the script generates silk as long as the line lenght is at least 0.3mm with a pad to silk clearance of 0.1mm (0.2mm clearance if possible -> so for large parts)

Shackmeister commented 6 years ago

Tombstoning risk is absolutely true, totally forgot about it.

with 0.1mm pad to silk clearance, and 0.1mm silkscreen thickness I get a length of 0,15mm (exluding the line end rounding, so 0,25mm line in total) which I think looks fine, and not like a dot.

r0402_0 1

Shackmeister commented 5 years ago

@poeschlr would you consider this a viable solution or should I close this issue?

evanshultz commented 5 years ago

I support adding silk to these small chip footprints.

Why limit silk length to 0.3mm min? Even smaller would still show up as a line in silk and help to guide part placement as mentioned above. This is valid for for hand soldering and reflow.

And why 0.1mm min spacing? I wrote up that IPC 7351C should use the line width at https://github.com/KiCad/kicad-footprints/issues/439, which would be 0.12mm. At least the 0603 is still using 0.12mm line width so I'm not sure where we draw the line for "high density" as mentioned in KLC.

Shackmeister commented 5 years ago

yesterday I was debugging a USB connection which didn't work. Turns out the apprentice has soldered the resistors this way :) 47143318_200643230869504_6329078706627149824_n

poeschlr commented 5 years ago

To be honest i am not sure where the IPC rule comes from. All manufacturers i ever used had it dependent on the copper thickness and relative to the mask cutout. Nowhere did they ever mention that it depends on line thickness. But i can setup the script to use this.

I will take a look at this within the next few weeks.

Regarding min line length: How about double line width? That way it should really still be a line and not a dot.

Shackmeister commented 5 years ago

double the line width, is that including the lineends? I think the line length of 0.15mm looks fine (excluding lineend), with 0,1mm, as suggested above, looks quite fine