I was looking at an example board schematic provided by TI and I noticed something rather curious: vias were placed directly on SMD pads. Is this a normal/acceptable practice to follow? Or is it recommended/better to put a short trace and then have a via?
- Anybody can ask a question
- Anybody can answer
- The best answers are voted up and rise to the top
Vias in the pads are useful in high speed designs since they reduce trace length and therefore inductance (i.e. the connection goes straight from pad to plane rather than pad-trace-via-plane)
They are also useful for Micro-BGA designs, where space is very limited and traditional fanout techniques cannot be used.
A via-in-pad (or capped/plated via) is not to be confused with a "tented via", which is a standard via with soldermask covering the hole (hence "tented")
To illustrate the advantage, here is an example of a TQFP footprint fanout with standard vias and via-in-pads:
It's easy to see why the via-in-pad version is preferable for high speed designs that need to keep inductance low.
The reason it's more expensive is due to the complex process (compared to standard vias) and potential problems (e.g. plating bulging with expansion of plug, or dimpling)
Here is a run through of the process:
In general it's bad practice: the solder paste may get sucked in the via capillarily, leaving too little to solder the part's connection. I would place the via as close as possible next to the pad, with a narrow connection which won't draw the solder paste from the pad.
There's a technique called tented via which avoids this by covering the top of the via, but it's covered with solder mask, so that's not usable on a pad.
Staggered microvias don't require plugging and the copper caps, but are buried vias, so also expensive.
When ordering PCBs to be manufactured, you can expect the vias to be drilled slightly off. Depending on how far this "slightly" is, the via might mess things up.
I'm sure TI has the best quality PCB manufacturing available. If you're using a cheap PCB manufacturer though, you may expect some visible imperfections.
Sometimes putting vias on pads is recommended. A power component soldered on to the PCB will very often have numerous vias connecting its big thermally conductive ground pad to the GND trace on the bottom layer. In high frequency designs you have to take into account the trace lengths of your PCB. It may sometimes be beneficial to put a via directly on a pad to reduce trace length.
It is sometimes done with BGA devices, or to minimise inductance. The vias need to be plugged, which is very expensive.
No, no, no, no, no. Don't place vias on the pads*. The solder will suck into the via and create a faulty soldering. The solder joint will not have enough solder to be reliable.
This practice is expressly forbidden in any company taking their work seriously. I have worked e. g. at a major manufacturer of telecom equipment: Don't even think about via-in-pad.
I have seen a number of such solder joints. And I have seen such joints crack up after a while, losing contact.
In our design rules I have defined this as no-go. There shall be at least 100um solder mask between the pad and the via, exactly to avoid this problem.
If your assembly house makes sloppy work they will let you do this. If they are careful they will ask you to move the vias out of the pads.
*Exceptions: -Certain RF applications may need the pad in the via, but then the common practice is to use many vias.
-BGAs may require via-in-pad because there may not be enough space to route the board otherwise.
-Certain pads for power dissipation use vias in the big pad to conduct the heat away.