|
Many IC's I've seen suggest decoupling capacitors across Vdd to Vss - this is sensible. However some IC's for example the dsPIC33FJ128GP802 has THREE Vss pins and only two Vdd pins (AVdd and Vdd.) So would I put a decoupling capacitor on each Vdd pin, or from each Vdd pin to each Vss pin? |
|||||||||
|
|
I believe the general rule is 1 cap per Vdd pin. Are you using a ground plane? If so, don't bother attaching the caps to Vss pins. However, if you are using a ground bus instead, then yeah you should attach the cathode of the caps directly to Vss. |
|||||||||||||
|
|
In the case of that chip, yes, you would. They actually allocate quite a bit of space (pages 21 and 22 in the datasheet) to describing the capacitors required. But, as a general rule, you do want 1 cap per Vdd pin. A ground plane negates the need for decoupling on Vss, if you don't have one you're going to have problems. In the case of the dsPIC linked (and many other chips), each Vdd pin is adjacent to a Vss pin, so just put it right there. There are actually four Vdd pins, and four Vss pins, so they match up: 2xVdd (IO supply), 1xAVdd (ADC supply), and 1xVcap/Vddcore (internal regulator capacitance), along with 3xVss and 1xAVss. |
|||||||||
|
|
You overlooked \$V_{CAP}/V_{DDCORE}\$. If you take that in account you'll see that there's a \$V_{SS}\$ for every power pin.
I only wish Microchip would have placed the \$V_{SS}\$ of pin 8 and the \$V_{DD}\$ of pin 13 on adjacent pins, like it did for pins 19/20 and 27/28. As explained in section 2.3 of the datasheet there's an internal voltage regulator for the core, which needs an output capacitor for stability. That's \$V_{CAP}/V_{DDCORE}\$. You connect a 4.7\$\mu\$F to 10\$\mu\$F between this pin and ground. That's all you need the pin for, the rest is internal. Section 2.2 in the datasheet covers decoupling and shows this schematic:
Some designers will draw power rails in a corner of the schematic and place all decoupling capacitors there. Their excuse is that the decoupling in the schematic itself will clutter it and make it less clear. IMO that's a bad idea. Especially if someone else will create the PCB layout it's not clear where the capacitors belong physically. If you draw them like in the above schematic it's at least suggested which pins a capacitor belongs to and the PCB layout engineer will know that it has to be placed close to the pins. |
|||
|
|
