SparkFun Forums

[treez]

Hello,

why is it that putting a via near a pad of the same net makes a board non-manufacturable?

-Also, why is it bad practice?


I have been told to re-do a double-sided layout because i have a few 0.6mm/1.2mm vias just 0.1mm away from SMD resistor pads of the same net.

...the via "restring" is not touching the pad of the resistor....as i said, it is 0.1mm away...and in any case, it's of the same net.

(-the vias are 0.6mm drill, and 1.2mm overall diameter)


So do you know why this is a bad thing?

[leon_heller]

The software is too dumb to avoid flagging it as an error?

It could conceivably cause problems with things like ground loops, or unwanted feedback, if connections not intended by the designer are made between tracks on the same net.

[Roko]

You typically want to avoid having vias too close to pads, since the vias can suck solder away from the pad due to capillary action. Remember that there's a minimum width required to ensure a complete solder-mask. A 0.1mm solder mask width might not be manufacturer with any reliability by your PCB house. You'll want a complete, reliable solder-mask between the via and pad to prevent solder from getting sucked in. It's also good practice to ensure you force solder-mask tenting on your vias to try and prevent solder from getting sucked into them.

If you're hand-building this board, or doing small quantity with relatively small vias, it often won't be too much of a problem/ However, if you're doing larger volume production with reflow soldering you'll start to have increased failure rates due to bad solder joints.

That being said, sometimes it's fine to have a via in a pad, i.e. if you're putting vias directly under a ground slug on, say, a QFN component. I do this all the time, including in mass production with RF circuits, and it's never caused me problems. With enough solder paste it doesn't matter if some of it gets sucked into the via, as you'll get a solid connection anyways.

Putting via's near or in something like a 0402 pad, on the other hand, can start causing you problems really quick with bad solder joints, tomb-stoning, etc, so you'll want to avoid that if you can. Putting vias on the signal pads of the QFN (as opposed to the ground slug) could also suck away the solder before it has a chance to adhere to the lead on the IC, especially if the part hasn't settled properly yet.

There are technologies out there for putting viass in pads, like plugged and/or microvias, but those tend to increase the cost of a PCB significantly.

[MichaelN]

...the via "restring" is not touching the pad of the resistor....as i said, it is 0.1mm away...and in any case, it's of the same net.

If it's of the same net, and it's really close, why don't you just connect it with a piece of track? As Roko says, there can be issues with "tombstoning", but there shouldn't be any issues actually making the PCB itself.

...That being said, sometimes it's fine to have a via in a pad, i.e. if you're putting vias directly under a ground slug on, say, a QFN component. I do this all the time, including in mass production with RF circuits, and it's never caused me problems. With enough solder paste it doesn't matter if some of it gets sucked into the via, as you'll get a solid connection anyways.

I agree. Also, if you "tent" the vias on the other side of the PCB, I find I get almost no wicking / "stealing" of the solder into the vias.