| Episodes | 47 |
| Mentions | 72 |
| Cited here | 31 |
| First — last | #8 — #713 |
| Top guests | Hank Zumbahlen, Katerina Galitskaya, Eric Bogatin |
| Related | antenna · pcb layout · radio frequency · signal integrity · analog to digital converter |
A ground plane is a large continuous region of copper on a printed circuit board that serves as the return path for signal and supply currents. It is not a perfect equipotential sheet: a plane has inductance, so return current follows the path of least loop inductance rather than spreading evenly across the copper.[128] A power and ground plane pair exists to deliver supply voltage at low impedance and low inductance, which is why the geometry of the pair matters more than the mere presence of copper.[252] Beyond its electrical return function, the plane forms part of the radiating structure of any antenna carried on the board, so purchased antennas are supplied with a required ground-plane size in their datasheets.[446]
Return current
Return current in a plane concentrates directly beneath the forward-going trace rather than spreading over the whole plane, because that arrangement minimises the enclosed loop.[185] The behaviour is frequency-dependent: at low frequencies the current distributes across a wide plane, which can then be treated as a bulk conductor, while as frequency rises the current follows the path of least inductance and hugs the forward path.[185] The concentration can be demonstrated directly with a current-tracing probe, which shows current flowing in one region of the plane and effectively none in adjacent areas.[165]
The return path exists whether or not the designer plans it, since Maxwell’s equations determine where the return current goes; the purpose of a stackup and plane strategy is to take that determination into the designer’s hands as far as is practical.[452]
Return current also does not necessarily flow in the ground plane at all. A signal routed on a layer adjacent to a power plane returns on that power plane instead,[439] and a power plane serves as a return path just as readily as a ground plane, so the widespread assumption that a high-speed signal must return on ground is mistaken.[452] A layer made up of patches of different supply voltages can still act as a valid return plane, provided those power planes are adequately decoupled to ground.[452] As a working rule of thumb a power plane may be treated the same as a ground plane for return purposes, because bypass capacitors hold the two at essentially the same low impedance across the frequencies of interest, although the approximation breaks down in the finer details.[439]
Inductance
The inductance of an interconnect is set by three physical properties: its width, since spreading the current out generates fewer rings of magnetic field lines; its length; and its proximity to the return path.[252] Power and ground planes are placed close together because the currents in them counter-propagate, so the magnetic field of the power current cancels that of the ground current, reducing total inductance and hence the voltage developed when the current changes.[252]
The same reasoning condemns a thin ground trace. Running ground as a single narrow trace across a board is poor practice because the trace is electrically a long wire and therefore high in inductance, unlike a plane.[410] Where such a run cannot be avoided, it should be stitched down to the plane with vias at multiple points along its length rather than tied at a single end, to keep the ground connection low in inductance.[410]
Plane inductance has consequences at the board level. Current flowing across a board between two connectors, acting on the plane’s own inductance, develops a voltage difference between the two sides of the board, so the ground plane itself becomes a radiating element.[645] A return loop formed by a trace and its path through ground can also be resonant at a frequency present in the system; loops of this kind have been the root cause of field failures in instruments from major manufacturers, and such faults are hard to find because no single component is defective.[319]
The plane structure of a board also acts as a bulk capacitor in its own right, and its effectiveness can be compared directly against a discrete bypass capacitor of the order of ten nanofarads.[710]
Stackup
The ideal high-speed stackup sandwiches every signal layer between ground layers, which for a six-layer design of moderate complexity would call for ten layers; commercial practice is to take the minimum layer count that works, so such boards ship as six-layer parts.[439] Where that compromise is made, routing a signal layer adjacent to a positive power plane is almost as good as routing it next to a ground plane, and decidedly better than routing it with no adjacent plane at all.[439]
Stackup decisions should not be delegated. Leaving them to the fabricator optimises for the fabricator’s yield rather than the board’s electrical performance; the result may still work, but the designer is then relying on luck instead of specification or simulation.[252] One specific mechanism is the dielectric fill layer: when a stackup computed for a target impedance comes out thinner than the specified board thickness, the fabricator adds fill to make up the difference and places it in the middle of the board for symmetry and yield, pulling apart any power and ground plane pair that sits there.[252]
A design that carries multiple separate ground planes must define explicitly where those planes are tied together, since they have to meet somewhere, and CAD tools handle that junction awkwardly.[185] A switching power supply can be treated as a self-contained block within a larger board, given its own ground plane and otherwise isolated from the surrounding circuitry.[230]
Automated layout tools address the stackup problem directly: a four-layer stackup can be fixed by inferring which net is ground and which is the most used supply, assigning those two to the internal plane layers and routing everything else on the top and bottom.[626]
Discontinuities
The most damaging thing a layout can do to a plane is chop it up, whether by splitting it with a routed trace or by punching a field of vias through it, since in either case the return current is forced to detour around the break.[439] When a return plane is chopped into islands by multiple supply voltages, the return current cannot stay adjacent to its signal and instead finds another route across the board, enlarging the loop area with a range of undesirable consequences.[452]
Two-layer boards are the common case. Where a two-layer board relies on a bottom-side pour for its ground, every trace routed through that pour breaks the plane, and a plane cut in half can leave the board worse off than the designer expected.[221] In practice the bottom-side plane ends up perforated by the signal routing it must share the layer with, and the resulting cuts are a standard reason to move a revised design to more layers.[395]
Deliberate cutouts are also frequency-dependent in their merit. Cutouts in a ground plane, a standard technique in low-frequency mixed-signal layout for keeping converter noise out, are counterproductive at RF: a high-frequency signal crossing a plane cutout simply radiates, so the trace becomes an antenna.[457]
A mistake in an internal ground plane is far more costly to correct than an error in a signal trace, because the plane connects to every ground reference on the board and each of those references has to be reworked.[68]
Antennas
A PCB antenna does not work in isolation: the board’s ground is part of the radiating structure.[446] An antenna element needs a feed point and a plane behind it, and the plane acts as an extension of the element, so a wire monopole plus its ground plane together form the dipole that actually radiates.[678] Module and chip antennas function only because they are connected to the ground plane of the board carrying them; the same element suspended in free space with nothing to work against would not radiate.[678]
Size follows from this. Lower-frequency antennas require a larger ground plane to radiate efficiently, which is why the low cellular bands are the hardest to accommodate in a small product.[678] Shrinking the antenna element itself buys no radiating performance, because performance follows the size of the ground plane; a smaller element only frees board area or allows the radiator to be moved off the board into the space above it.[678] A ceramic chip antenna is likewise specified against a particular board size, and a product too small to provide that plane will not reproduce the antenna’s rated performance.[175] Antenna types differ in their relationship to the plane, some being designed to work over a ground plane and others requiring no plane beneath them, so the choice of type is constrained by the board and enclosure available.[678]
Placement follows the same logic: an antenna should be placed on the shorter side of the board, in a corner and on the edge, never in the centre, so that the long dimension of the ground plane is available to it.[678] So-called virtual antenna designs radiate from the ground plane itself, so conductive parts bonded into the ground, including a battery, extend the effective plane and can improve radiation rather than degrade it.[557]
A typical wireless module layout is trivial by design: the module and a few passives stitched down to a large ground plane on the layer beneath, with a single controlled-impedance trace running out to the antenna.[453] Development boards for cellular modules provide a large copper landing pad tying the module ground to the board ground, because a substantial reference plane is wanted for antenna performance, and a shield may be fitted under the module as well as over it.[493]
Radio module vendors advise against placing a ground plane under the antenna region of a design, and publish layout documents saying so because first-time integrators frequently do it.[202] Although copper under the antenna is the failure most often anticipated, the more common fault seen in module integrations is a board with no ground plane at all, compounded by poor placement such as switching-regulator inductors sited next to the radio.[202]
Fabrication and assembly
Board fabrication documentation should specify every parameter explicitly rather than leaving values such as pad clearance to the manufacturer, because fabricators adjust unspecified parameters to suit their own process.[393] A fabricator enlarging clearances and removing copper fill around pads without notice can sever a ground pour, in one documented case breaking a ground plane in half on a delivered board.[393]
Planes also affect reflow. Tombstoning of small two-terminal parts arises when one termination lands on a pad tied into a ground plane and the other on a thin trace: the grounded end is coupled to a large thermal mass and cools at a different rate from the other end, so the part lifts during reflow.[172] Thermal relief on pads connecting to internal planes is therefore a design requirement rather than a cosmetic detail, because thick boards with large internal copper layers retain heat and unrelieved pads make bypass capacitors and similar small parts liable to tombstone.[172]
For electrical test, a flying-probe machine can be programmed to hold one probe on the ground plane and touch the other to every non-ground net in turn to check for shorts, but this must be repeated for each power plane and is not part of the default automated test.[682]
Thermal behaviour
Internal ground planes are poor heat sinks despite their copper area, because they are sandwiched between layers of fibreglass, which conducts heat badly.[516]
Prototype construction
Dead-bug construction, in which a chip is glued upside down on an unetched copper-clad board and its pins wired in the air, performs well at high speed because the continuous copper underneath acts as an uninterrupted ground plane.[8] In the related Manhattan technique, small islands are machined or cut out of the copper on a bare board and components are soldered to those islands, while the surrounding uncut copper is retained as the ground plane.[106] Both methods work because soldering a component lead straight onto solid copper gives an essentially inductance-free ground connection, with no length of trace or wire standing between the part and the plane.[56]
Limits of the ground reference
Ground planes on silicon suffer high-frequency inductance effects and are distorted by current injected into them, and an equivalent effect appears on boards as dynamic variation of ground potential from place to place.[704] Because no hard ground reference is achievable on an integrated circuit, on-chip signal paths are designed fully differentially as a matter of course, and thinking differentially is a sound default in any ground-sensitive system.[704]