Take the 2-minute tour ×
Electrical Engineering Stack Exchange is a question and answer site for electronics and electrical engineering professionals, students, and enthusiasts. It's 100% free, no registration required.

This is a subset of a circuit I am building to run motors off a PIC 16F884:

schematic

simulate this circuit – Schematic created using CircuitLab

I noticed last night as I was drawing up my schematics that I might have redundancy in the use of the smoothing capacitors off of the VDD/VSS pairs on the PIC.

My question is: Does the 0.1uF cap off the 7805 have the same smoothing effect for both VDD/VSS pairs thus eliminating the need for the two extra caps off of the PIC?

schematic

simulate this circuit

share|improve this question
2  
It's generally recommended to wait a day or so before accepting an answer, to help stimulate discussion. –  Madmanguruman May 16 '13 at 20:18

2 Answers 2

up vote 8 down vote accepted

Smoothing caps need to be as close to the power pins as possible of the target ICs. Trace parasitics add a whole bunch of invisible components in series with the power and return nets. It's a difficult concept to visualize from a schematic standpoint, since a schematic shows logical relationships (nets) but not physical relationships (how far apart parts are, how convoluted the routing is, etc.)

Unless your PCB layout is such that the regulator, capacitor and power pins are fractions of a millimeter apart, you'll need the local capacitors.

As a rule of thumb, it's always best to add decoupling everywhere you think you may need it on a layout - it's easy enough to not populate parts later, and much harder to add a cap where there isn't room for it.

share|improve this answer
    
+1 for that last point! –  Dave Tweed May 16 '13 at 16:08
    
Having been in both positions, I err on the side of caution. –  Madmanguruman May 16 '13 at 20:17

The purpose of the 100 nF capacitors placed physically close to the microcontroller, is to decouple the varying load any microcontroller represents, from the power supply rails. Thus, those capacitors do need to exist, as close as possible to the supply pins of the device.

Similarly, typical voltage regulators sense their output and use a feedback loop to regulate it, so they need stabilization of the output rails via a capacitor placed physically close to the regulator, to protect against both EMI picked up by the rails and load ripple. So the regulator output side capacitors are needed as well.

If the physical layout of the board is such that the regulator's output pins are physically close to the load device, one of the capacitors could be dispensed with. Do note, though, that this is not a good idea, as the heat generated by a linear regulator is likely to disrupt or possibly damage the microcontroller and support circuitry, or at the very least, introduce frequency variation in clock crystals or internal RC oscillators.

To address the specific case of a microcontroller with two sets of supply pins: Often these pins may be ganged together using a Vcc plane / short fat trace and a ground pour / short fat trace - in which case the need for the additional decoupling capacitor for the second supply rail pair may be non-critical - but still a nice-to-have.

If however the supply rails between the pairs of supply / ground pins have any significant trace length between them, adding the second decoupling capacitor is strongly recommended, for the same reasons mentioned above: Traces pick up EMI, which needs to be shorted to ground.

share|improve this answer

Your Answer

 
discard

By posting your answer, you agree to the privacy policy and terms of service.

Not the answer you're looking for? Browse other questions tagged or ask your own question.