Electrical Engineering Stack Exchange is a question and answer site for electronics and electrical engineering professionals, students, and enthusiasts. It only takes a minute to sign up.
Sign up to join this community
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?
Example:
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)
You have to check whether your PCB house can do this though, and it may cost more (via will need to be plugged and plated over to provide a smooth surface) If you can't put the via in the pad, putting directly adjacent and using more than one can help reduce inductance.
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)
This document discusses various plugging techniques.
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.
edit
Fake Name comments that I forgot to mention plugged vias, and they may indeed be a solution. I didn't mention them at first because I've never used them, and can't comment on possible pitfalls. Oli's answer has a very nice illustration of the technique and everything just screams "expensive!" (anywhere between very expensive and Damn Expensive™). You may need plugged microvias though for a small pitch BGA, like 0.5 mm.
Staggered microvias don't require plugging and the copper caps, but are buried vias, so also expensive.
I'm talking with experiences not imaginary recommandation with no actual evidence to back it up. You already asked for the smd pads not BGAs, nevertheless I saw many answers that only cover up for BGAs/ICs fanouts not the passive components.
To put it short, yes you can but you need a little care along the way.
Via in pad is a bad thing if your via's hole occupy more than 30% of the pads area AND if your pad is too small too! If your pad be too small and you use mechanical drill this might blow out the pad. In this case your manufacturer may recommand to you that use laser drilling instead of mechanical drill and it surely cost you more. Moreover in the assembling proccess to avoid sucking out solder paste you need to resin plug these vias too which again cost you more.
But all these recommendation are only for the BGA parts, If your pad be big enough and your hole size be small relative to the pad size (like the TI board you mentioned) you don't need any laser drilling nor plugging the vias because it's effect will be too small to be noticable.
I've had a succesful experience with placing 0603 component (imperial) with 0.3mm via in it and 0402 component (imperial) with 0.2mm vias in it on my board. In both of these cases I had used mechanical drilling with no resin plugged holes.
I doesn't saw any defect on a batch of 1000 board with more than 40 component like the following figure
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:
Placing vias over SMD pads is pretty common and an acceptable practice provided you take good care while designing. Here are some practices I follow when I use Via in Pad:
I don't tend to use through hole via in pad for 0201 passives. The pads for an 0201 are pretty small for a through hole mechanical drill and may damage the pad in the process.
When it comes to 0402 passives, I use a 0.15mm/0.2mm through hole mechanical via in pad.
When it comes to 0603 and 0805 passives, I use a 0.2mm/0.25mm through hole mechanical via in pad.
I even used a 0.15mm hole/0.4mm pad via in pad on a BGA package (DDR3L RAM). Of course my BGA package's pad size was 0.41mm. The via fit in without any issue in manufacturability. Since the hole was pretty small, the common problem of solder flowing into the hole is negligible.
PS: Many people say it is a bad practice but I used this approach in many designs which went into production (5K pcs volume) and they've had no issue since then.
Good luck with your design!
Via-in-pad is generally considered bad practice for automated assembly processes, as the solderpaste may be drawn into the via during reflow soldering and result in a poor quality solder joint between the device pin and the pad. This can be mitigated by using plugged vias, with the associated additional cost.
That being said, this practice is used in specialized RF and harsh environment electronics where hand assembly, or visual inspection and hand touch-up are used to ensure near perfect solder joints at every point. If you're doing a small run to be assembled by hand, this shouldn't be a problem for you.
