Bypass Caps

The questions is; where to put Bypass caps in the circuit?

Next to a analog or digital device of course, between the VCC and VSS pins.

But, this is only really easy to do on; push boards, protoboards, deadbug or experimental circuits, just push the caps in, and/or solder as necessary.

But then, if you are actually planning to build a complex PCB's (i.e. more than a few devices), it is a lot of work to make sure the right cap (as per the schematic) is next to its associated device. All of the bypass caps are connected in parallel to the same supply and ground rails (i.e. VCC and VSS), therefore on the initial PCB layout they are connected to the same "rats nest" and not really associated with a particular device. The unscrambling task is even more difficult, because bypass caps are typically all the same value.

Some designers just scatter the bypass caps around the board next to a likely devices. Other (better) designers take the time to place the correct bypass caps near its associated devise, as per the schematic - this can be a lot of work!

But, does it matter? - it is only a reference symbol printed on PCB in silkscreen. To me; "Yes, it does matter". And therefore, I make sure the correct bypass cap is next to its associated device as per the schematic.

Schematic Diagram

I use the following technique to make the PCB layout of bypass caps and associated devices easy. On the schematic, I insert a "Zero Ohm" resistor in the supply line (VCC) that feeds each bypass cap. Now regardless of PCB layout software that is used, the initial "rats nest" will suggest close layout of the correct bypass cap with its associated device. From PCB layout perspective, the Bypass caps are NOT directly attached to the VCC rail, but instead, it is connected to the "Zero Ohm" resistor which is connected to the power VCC rail. The associated "Zero Ohm" series resistor is easily located and placed next to its bypass cap (because it is in series and not parallel on the schematic). Its a simple trick that just makes PCB layout much-much easier!

PCB Layout

Also, for most low current devices where 6 mil traces are typical, I use a 0201 "Zero Ohm" device footprint. Instead of an actual device, a simple solder bridge is all that is needed to make the connection. And, this technique makes troubleshooting a new designs all that much easier. A troubling device can be removed from the circuit with a little solder wick.

As Manufactured

As seen in the schematic diagram, B2 is the symbol that I created for the solder bridge.

This technique; may, or may not, be useful for Production Products, but for the Hobbyist it works great!

BTW, I also put in 0201 "Zero Ohm" in all I2C lines, next to each I2C device, for easy initial testing. A bad I2C device can easily take the entire bus down - which is not fun to troubleshoot.

---

UPDATE

Note: I am looking for a more appropriate footprint for an easy to use solder jumper.

A "Zero Ohm" resistor can also be used to enforce and make easier a "star grounding" system for a set of parts. Connect the circuits star grounds to one end of the "Zero Ohm" resistor and the real ground to the other. For a PCB layout, a star isolated ground plane can also be attached to the same point (i.e., multiple isolated ground planes can be used on the same board).

UPDATE 2

I am considering one of the following for future project Solder Jumpers, some additional function and use evaluation is needed.

Proposed Solder Jumpers

• Jumper SJ2 is about 100 mil diameter with 10 mill isolation.
• Jumper SJ1 is a 70x40 mil rectangle with 6 mil isolation.

-