Use extra via-stitching by bypass capacitors? - Page 1
Forum section: electronics / beginners

author: Clear as mud
author_rank: Regular Contributor
timestamp: May 27, 2014, 06:21:04 pm
content: I just read this application note from Maxim:Successful PCB Grounding with Mixed-Signal Chips. It's about keeping the path of the current in mind when designing printed circuit boards. I've been designing PCBs for about a year, so most of this is familiar to me, but I have a couple of questions about one of the figures. In figure 14, they show green-shaded areas near the two bypass capacitors. It's on the grounded side of the bypass capacitors, and they have added vias along the trace between the capacitor and the chip. I haven't included extra vias like that in my designs before, and I was wondering why it is a good idea? They didn't explain it in the text of the application note. I think it provides a better path to ground for the DC and low-frequency portion of the signal, but the high-frequency portion still has to come from the capacitor, and it would seem that the via stitching is unnecessary. Or, does it really lower the impedance of the trace a lot, for high-frequencies?If you had a multi-layer board with a power plane and a ground plane, would you want to provide via-stitching on both sides of the bypass capacitor?Finally, are there drawbacks to putting vias in component pads? Some of the vias in that figure appear to be partially underneath the capacitor.

author: marshallh
author_rank: Unknown
timestamp: May 27, 2014, 06:30:46 pm
content: 1. Multiple vias on a cap like that are to reduce inductance. Typical inductance assuming the most common pcb stackup can be 10-15nH. If you are using 8mil vias (common in denser boards) that figure is a bit higher. So using multiple small vias compensates for the increased inductance of each.2. For ic grounding there is probably no benefit to multiple vias per ground ball/pin, as the inductance is dominted by the internal bond wire (or, interposer tracks in the case of a flip-chip bga).3. Don't put vias in pads, because it will "steal" solder paste from the connection into the via, causing a weaker joint. Also, if you have paste on both sides then gas/vapor can get trapped inside the via causing it to blow off ruining one side.4. One place you want to use extra grounding vias is when you have a very fast signal changing layers. Such as a 5gbps differential pair. If you put an additional return path via right next to the actual signal vias you create a more direct reference path for the return current. Same thing as minimizing loop area. It's just turned sideways.

author: marshallh
author_rank: Unknown
timestamp: May 27, 2014, 06:38:29 pm
content: Also regarding via in pad, yes it is possible in some cases. There are several ways you can accomplish via in pad (VIP):1. Squeegee a fine conductive epoxy over the pcb (or through a mask if you don't want all vias to be filled) and then plate the PCB. This gives you a nice plated surface on each side and there is no risk of venting gas from inside the via.2. Via capping - only deposit some epoxy over one side, and then plate. This might be something you use on the backside of a PCB for bypassing under a dense BGA. However the process must be strictly controlled since venting can ruin the other side of the joint.One of the prototype boards I'm using right now has selective VIP by the first method. It cost about $2k extra in setup costs. Because it was a 8layer board it essentially doubled the tooling costs for the run.Another way I've seen but not had the balls to try:3. Put the vias inside the pads, with no capping. Instead, over-deposit paste on the pads (Make paste aperture larger than the copper/mask aperture) and hope that nothing goes wrong. This will probably work better with larger passives and parts, but may fail with 0201's or some such.

author: marshallh
author_rank: Unknown
timestamp: May 27, 2014, 06:48:01 pm
content: Here are some pictures from that pcb, you can see both the filled vias and low-inductance SMPS routing like in that appnote you linked.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: May 27, 2014, 10:39:16 pm
content: Of course, you need some connection to the ground plane, otherwise the chip and cap are just floating...Figures I've heard are more like 3nH per via for an average thickness board. 10-15nH would be including component length and traces back to the IC pins, I would think?Extra vias are handy from time to time; for example, if you want to place a lone bypass cap between planes, you can use four vias, each pair flanking each pad of the capacitor. Place them as close to the centerline as possible, given soldering limitations (keep a minimum solder mask sliver between pad and via, or tent the via, so solder doesn't creep into it; unless you want to go the way of via-in-pad, with its potential benefits and issues). This minimizes the loop area, and probably gives ~2nH total from plane to plane.I don't think you'll see much gain from more than a couple vias. If you want to go whole-hog, your first choice should be ground flood on the top layer; that way you have a short perimeter around all traces and pads, and you can add stitching vias anywhere you please. Note that top side ground changes the characteristic impedance slightly; you have a coplanar waveguide with ground plane:http://chemandy.com/calculators/coplanar-waveguide-with-ground-calculator.htmTim

author: luky315
author_rank: Regular Contributor
timestamp: May 28, 2014, 08:25:58 am
content: Via in Pad works fine with passives in 0603 and even with 0402s if you use small Vias (0.2mm or 0.25mm end diameter).