Hello, I’m trying to route a micro-HDMI connector using the KiCad (7) footprint ‘HDMI_Micro-D_Molex_46765-1x01’.
This footprint has a keepout zone under the connector, and two signal rows. What is the recommended way of routing signals to the inner row? There is literally no room for traces if we respect the keepout zone.
Is the only way using via-in-pad? With pretty thin pads too?
Or is the keepout zone “erroneous”?
The keepout zone is in the manufacturer’s mechanical drawing so it looks right. https://www.molex.com/content/dam/molex/molex-dot-com/products/automated/en-us/salesdrawingpdf/467/46765/467651001_sd.pdf?inline
You’ve got maybe 16 mils / 0.4mm between the pads and the keepout so you should be able to get some vias in there if your design rules are tight enough. If your fab process allows for via-in-pad that would be an option too but I don’t think it’s necessary - if your process allows for via in pad I’m sure it also supports vias small enough to fit in the gap.
Just looking at JLC’s design rules, the 2 layer rules don’t allow vias small enough to fit, but the 4 layer design rules let you use vias down to 0.25mm.
Thanks. Looking at JLCPCB specs, they can do 0.15(hole)/0.25(ring) vias for >= 4 layers, but say that 0.2/0.35 min is preferred. But they have a 0.254mm via-to-trace min clearance. So that wouldn’t fit. Unfortunately. Looks like those micro-HDMI connectors require relatively advanced capabilities.
Good point. Yes, these look pretty annoying to route 
To be honest it’s not obvious to me why the keepout is needed.
It’s not uncommon for connectors with a metallic shell that lies on the PCB - my guess is that the heat during reflow may cause the soldermask underneath to melt and could cause some short-circuits.
0.15 / 0.25 vias are much more expensive. If you want to avoid an extra cost stick to 0.30 / 0.45 if possible.
Yes I’ve looked at prices - it’s not overly expensive either, but there’s certainly an added cost.
I found some TI notes with micro-HDMI layouts and they just place very small vias at the bottom of the pads in the inner row. So technically that’s via-in-pad, but since the connector’s pins do not sit on those vias, I think you shouldn’t need to have those vias plugged (which is definitely the most expensive). Not really any other approach anyway.
I saw some dev board with a micro-HDMI connector, on which they routed traces and vias in the “keepout” zone. I don’t think it’s really good practice, but I guess that’ll work for a dev board. I don’t think I would do this for a end-user product.
The “Keepout” area is very likely because solder mask just is not guaranteed to be an isolating layer. With both a silkscreen rectangle and solder mask, you can put two layers of paint over each other, but such a construction is still “out of spec”. It is possible those “other people” used a guaranteed good solder mask, or maybe even selective conformal coating, or put some tape in between. But they also may have guessed it may be “good enough”, or just missed it at all. It’s easy to make mistakes like that on complex PCB.
be cautious with that. as the whole pad will be pasted, the solder paste will also have direct contact with the via. one of the big problems with vias in pad is, that they channel the paste through to the other side of the board due to capillary effects, with that pull the paste away from the actual pins of the component and create fragile or no connections.
One solution to this is to place square of Kapton tape in the keepout zone, post stenciling most likely, with a pair of tweezers. OR you can add a type of heatproof conformal coating in the region (thin, bus…) Itr might be OK to place pre-stenciling if it doesnt lift the stencil too much.
I would regard 0.35 / 0.2 vias as “insane” for this application. And 0.15 drill is “smoking something”.
Suggest a 0.5 / 0.2 if you must or just use an easy 0.6 / 0.3 and interleave them under the Kapton Tape.
Also, it should be remembered that thinner PCBs are more suited to small drills. All my PCBs with 0.2mm drills are 1.2mm or less. They’re also better for high speed boards, the vias are not so long.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.