yzf600:
What benefit do you get from having such planes on the same layer as the routes? Is there anything wrong with just routing power and ground a regular signal traces? Are regular signal traces not wide enough? In other words, what is the best practice? Both a ground plane and a power plane? Two ground planes with power routed as a fat trace?
Greetings (no name supplied),
There are cases where a ground plane is required as the PCB is a component in a critical circuit. Typically, these are RF designs, where circuits must resonate at the correct frequency, and/or carry RF power efficiently (without losses). In very low level circuits (sensors, high resolution A2D and D2A converters, measuring instruments, transducer preamplifiers, etc.) the ground plane acts as a shield or barrier to exclude external electrical noise.
In the days of combinational logic built on bipolar IC processes (DTL, TTL, ECL) a lot of power was consumed and switching caused large spikes on both the power and ground circuits. Ground (and power) planes were added to reduce the inductance of the supply and ground, effectively increasing the noise immunity.
More recent designs using lower power circuits (battery operation in particular), the use of mixed-signal ICs (analog and digital on the same die) and increasing use of RF communications has made the use of a PCB ground plane attractive.
Some circuits fail to operate, or have reduced performance, on a ground plane due to increased capacitance loading and interference from noisy power and ground lines coupling into high impedance and high gain stages. In particular, any device that uses a crystal, ceramic resonator, or NFB (negative feedback) will require that ground planes are removed in critical areas.
It’s not the copper resistance that causes the problem, although high power circuits benefit from “fat” traces or extra weight copper, but the inductance. Small width traces, or traces that run parallel (even on opposite sides of the PCB) will exhibit greater noise, and possibly coupling between the traces. A ground plane can eliminate this problem.
On single and two layer PCBs its a good idea to flood the unused areas to form a ground plane (but not in the areas noted above). Its considered bad practice to leave islands (or orphans) of ground plane that are not electrically connected to ground. Its also possible to section a PCB layer to form power planes of different voltages or power and ground. or two separate ground to isolate analog and digital circuits on the same PCB.
PCBs can be effective without any planes, by routing the power and ground as ‘signal’ traces. There’s a few rules to making this work the first time, mostly its common sense. If in doubt think of the traces as small resistors. What will happen to the circuits if voltage is lossed in each segment of the trace? Will it reduce the available voltage at the end of the line furthest from the power source? Will a heavy load cause voltage drops on the power traces that effect other curcits? Remember that current must return to the power source, so similar losses occur in the ground traces to those in the power traces.
Allowing space to place wider traces for power and ground compared with signals (many of which carry less than one percent of the total current in a given circuit) will help.
Advances in IC processing produces finer feature size (the smallest element in the silicon), but operating voltages must be reduced due to lower breakdown voltages. This leads to greater current for a given processing performance, and makes power design, distribution, and decoupling quite difficult. Many large scale digital devices now use less than one volt for their core, less than three volts for their IO, and consume tens of watts. This translates to tens of amps, which requires fat traces to reduce the I2R losses. Further, the switching regulators used to power these circuits have very large high speed circulating currents that require very careful PCB design and layout.
In my experience, having worked on high speed analog and digital systems, it may take more than half a dozen PCB revisions to get it right. These are just that - PCB layout changes. Not architecture or circuit changes, or substitution of different packages and devices, just placement of traces and scupturing of the ground and power planes, and addition or subtraction of vias.
For BatchPCB level hobby projects adding a power plane may have a very small effect. Critical circuits will likely have hints in their data sheets. I think ground planes are attractive, and I’ve found out the hard way that without “thermals” (breaks around pads and vias on the ground plane) it can be very hard to get good soldering.
Power planes and ground planes are typically not allowed in inner layers of multi-layer boards for a variety of PCB production reasons, and I think they are banded in the new BatchPCB four layer service (can someone confirm this - I hate to spead false info). Also, I wonder if blind vias are allowed (ones that connect inner layers without removing route area on the outer layers?
Comments Welcome!