Bypass Capacitor - Via vs Trace Length

[lodup29]

I’m weighting the impact of placing bypass capacitors beneath their corresponding pin rather than next to it. Looking around, I found a few rules of thumb stating that the parasitic inductance of a via would be around 1.2 nH while the inductance of a trace would be around 1 nH/mm. Considering that the board must follow the IPC-7351B (density A) guidelines which, unless I made a mistake, implies that all components must be at least 1mm apart, I’m under the impression that placing the capacitor on the same side and next to the pin is at best virtually equivalent to placing the capacitor beneath the pin with a via right next to the pad. Yet I found I few guidelines stating that the bypass capacitors should be placed on the same side of the IC. I guess I’m missing something here. Thanks.

 

[keith1200rs]

The only guidance I can offer is experience of testing high speed analogue circuit boards where I have seen worse decoupling performance where the capacitors are on the opposite side of a PCB to the IC. This is at around 1GHz with small ICs. It may not apply where the ICs are large and top tracking would be long.

Keith

 

[lodup29]

The only guidance I can offer is experience of testing high speed analogue circuit boards where I have seen worse decoupling performance where the capacitors are on the opposite side of a PCB to the IC. This is at around 1GHz with small ICs. It may not apply where the ICs are large and top tracking would be long.

Keith

Thanks Keith. May I ask you how close were the decoupling capacitors to the pins (when on the same side)?

 

[keith1200rs]

Thanks Keith. May I ask you how close were the decoupling capacitors to the pins (when on the same side)?

1mm from the edge of the capacitor pad to the edge of the QFN pad. 0.4mm track. 0.3mm via with 0.6mm pad. 1.4mm FR4 (6 layer).

I had tended to put decouplers underneath ICs because with small ICs it can get very crowded trying to get all the parts close to the IC. This is predominantly high speed analogue circuitry, but working with fast pulses. However, I tracked some problems down to inadequate decoupling. Using microprobes I could see a significant difference in the power supply on the two sides of the PCB, even just probing the two sides of the via. Adding a decoupler to the top side fixed it. So, while the calculations may suggest that vias are as good as short tracks, maybe they aren't. Maybe it is the increased resistance of plating vs copper? Maybe my PCB had thin plating? I don't really know, but I know it worked better when the capacitors were on top.

Keith.