Nuts & Volts - July 2004

In The Trenches

Ground and Power

Proper grounding is critical. It’s a topic that books have been written on. Obviously, I can only touch on the subject here. A ground and power plane are ideal, but often it’s simply too expensive (it doubles the cost of the PCB).

I usually start with a wide ring (0.100” to 0.250”) around the PCB that is my ground. This allows me to easily put large ground areas around the PCB mounting holes (which are typically near the edge of the PCB). That means that a star washer and a metal screw to the chassis make a good chassis-ground connection. It also means that ground traces only have to go to any board edge. This simplifies the layout. If there is any concern about ground loops (more than one ground current flowing in one conductor), I simply cut the ring.

In this way, I can control where and how the current flows in the trace. If the design is fairly simple, I’ll spend extra time and try to make it single-sided and use the second side as a ground plane. There are always more connections to ground than to any other circuit node. Properly understanding how and where ground current flows in your layout cannot be overemphasized.

I use a similar ring technique for power, but on the other side. I carefully avoid the PCB mounting holes so that power/ground shorts will not occur. Running the traces back-to-back creates a small capacitor. This helps to reduce noise on the power line.

When I’ve finished the layout, I increase the width of the power and ground traces as much as I can. If there are large areas without traces, I’ll fill them with solid copper connected to power or ground. More copper often helps and very rarely hurts PCB performance.

Surface Mount

Surface Mount technology (SMT) has added more facets to PCB layout. The parts are very small and the lead pitch (spacing between the centers of adjacent leads) can be very small. It’s usually not possible to run any traces between the leads. This makes routing more difficult and increases the number of vias.

It’s virtually impossible to use a single-side layout with high pin count SMT ICs. The pad sizes and shapes are different for different parts. You will need to refer to the manufacturer for these specifications. Testing and repair need to be considered more with SMT designs because it’s hard to

probe tiny, closely-spaced pins. Think about how can you lay out the board to make servicing easy.

Routing the PCB

The proper placement of traces is something that is learned. The only way to do this is to actually route PCBs. A common and effective technique is to run horizontal traces on one layer and vertical traces on the other layer. (Obviously, this doesn’t work for single-layer boards.) This tends to create boards with a lot of vias.

Don’t run parallel traces closer than necessary. Segregate analog and digital areas. Put ground traces next to sensitive analog lines to act as shields. Do the same for high-speed clock lines to reduce EMI (ElectroMagnetic Interference) and crosstalk. Pay close attention to parts placement. It’s amazing how this can simplify routing.

Do not use an auto-router, unless it’s really smart (and expensive). The typical, low-cost routers only connect points together. They don’t consider the length of the trace, which traces are analog and which are digital, which lines are sensitive, ground loops, etc. As we’ve seen, subtle points can make a significant difference in how the PCB performs.