RF PCB Routing and Related Design Practices
A radio-frequency board is not simply a digital board with a few faster traces on it. Once signals move into the high hundreds of megahertz or into the gigahertz range, the copper geometry itself becomes part of the circuit: trace width sets the characteristic impedance, a right-angle bend becomes a discontinuity, a gap in the reference plane becomes a radiating slot, and a short stub of trace behaves like an inductor. These effects cannot be corrected afterwards by tuning components, so routing discipline has to be applied during layout, when the geometry is still being drawn.
This part of the article covers the routing practices that govern RF and high-frequency boards in practical design work: impedance control and the parameters that determine it, the treatment of trace corners, the structural integrity of microstrip and stripline transmission lines, and the passive functions that ordinary PCB traces can perform, including couplers, power dividers, quarter-wave bias feeds, and the three basic microstrip elements. Each section states the requirement, explains why it exists in terms of field behavior and impedance, and gives the dimension or ratio that satisfies it, so the material can be applied directly at the layout stage.
Highlights:
- Every RF trace on the board is designed to a controlled 50Ω impedance, with microstrip on the surface layer and, when an inner layer is required, stripline on the third layer between two solid ground planes.
- Microstrip and stripline structures stay electrically intact only if the ground reference is continuous: at least 3W of clearance from the plane edge, no non-grounded vias inside that 3W band, no crossing of plane splits, and 2W of spacing to any shielding wall.
- Short trace segments can replace real components, but only with the correct dimensions: quarter-wave coupled lines for a coupler above 20dB coupling, a 70.7Ω branch length of λ/4 for a power divider with a 100Ω isolation resistor, and a λ/4 high-impedance bias line for amplifier supply feeds.
Impedance Control
The impedance of a PCB signal trace is determined by the dielectric constant of the laminate, the PCB structure, and the trace width. In practice, RF signal traces should be routed on the surface layer wherever possible. In some cases they may be routed on an inner layer, and the most common arrangement is a stripline on the third layer. In all of these cases the impedance is designed to 50Ω.
The "PCB structure" part of that sentence carries most of the design risk. A trace on the top layer with a ground plane directly beneath it is a microstrip, and its impedance depends on the width of the trace relative to the dielectric thickness between the trace and that plane. A trace buried between two ground planes is a stripline, and its impedance depends on the same ratio, but with the dielectric split above and below the trace. Because the dielectric thickness is set by the stack-up rather than by the layout, the width needed for 50Ω can differ substantially from one board to the next, even when the same laminate is used. These stack-up and impedance considerations are also important in EMC design, where controlled signal paths help manage unwanted electromagnetic coupling.
The table below lists the impedance-controlled (50Ω) parameters of previously designed PCBs. For a new design with a comparable stack-up, these values can be applied directly.
| PCB name | Laminate | Relative dielectric constant | Thickness | Line width (mils) |
|---|---|---|---|---|
| PA41LCA3 | RO4350 | 3.48 | Layer thickness 0.8mm | 75 |
| GM61MPA3 | FR4 | 4.25 | Board thickness 1.0mm | 60 |
| GMJ2HPA5 | TLX-8-0310-C1/C2 | 2.55 | Board thickness 0.8mm | 87 |
| ED41OPRF | FR4 | 4.25 | Layer thickness 0.35mm | 27 |
| GM61PTRX | FR4 | 4.25 | Layer thickness 0.36mm | 27 |
| GM61PTRX | FR4 | 4.25 | Stripline 0.36 + 1.13 + 0.36mm | 18 |
The table is worth reading as a set of relationships rather than as a list of numbers. The same FR4 laminate, at a relative dielectric constant of 4.25, requires a 60-mil trace when the dielectric below the trace is 1.0mm thick, but only a 27-mil trace when the dielectric is thinned to 0.35mm or 0.36mm. Lowering the dielectric constant reduces the required width for the same dielectric thickness: the 2.55 laminate reaches 50Ω at 87 mils on a 0.8mm board thickness, while RO4350 at 3.48 reaches it at 75 mils for the same 0.8mm layer thickness. The final row shows the stripline case on the same FR4 board: once the trace is buried between two ground planes with a combined dielectric of 0.36 + 1.13 + 0.36mm, 50Ω is reached at only 18 mils, because the field is now distributed above and below the trace instead of being concentrated in a single dielectric layer.
Two practical cautions follow. First, these widths are valid only for the stack-up they were calculated for; any change in laminate, layer thickness, or copper weight requires the width to be recalculated rather than scaled by eye. Second, once the width is fixed, it should be held constant along the whole run. A trace that narrows to pass between pads or widens to fill a gap introduces an impedance discontinuity at each transition, and each discontinuity produces a reflection that adds to the ones from the connectors and the matching network.
Trace Corners
If an RF trace is routed with a 90° corner, the effective line width at the corner increases. Wider line means lower impedance, and lower impedance at that point means a reflection. The corner therefore has to be treated geometrically, and there are two ways to do it: a mitred corner and a rounded corner.
The mitred corner is applied to relatively small bends. A chamfer is cut across the outside of the corner so that the effective width through the bend stays close to the width of the straight sections. The mitred corner is usable up to a frequency of 10GHz.

a: mitred corner

b: rounded corner
Figure 8: The two methods of treating a trace corner.
The radius of the rounded corner must be large enough. As a general rule, the layout should satisfy:
R > 3W
where W is the trace width. A radius that is too small leaves the corner with the same problem as a square bend: the current path on the inside of the bend is shortened and the local impedance drops, so the reflection is reduced but not removed.
Microstrip Routing
When RF signals are routed on the top layer of the PCB, the plane layer beneath the RF signal must be a complete ground plane, forming a microstrip structure, as shown in Figure 9. To keep the microstrip structure intact, all of the following requirements must be met:
- The edge of the microstrip on both sides must be at least 3W away from the edge of the ground plane.
- Within that 3W band, there must be no non-grounded vias.
- RF signal traces must not cross a gap or split in the ground plane of the second layer.
- The electric field at the edge of a microstrip extends sideways, so ground copper must be added between non-coupled microstrip lines, and ground vias must be placed in that copper.
- The distance from the microstrip to a shielding wall should be maintained at 2W or more. (W is the trace width.)

Figure 9 | Structural integrity of the microstrip line
Each of these rules addresses the same underlying issue: the microstrip mode only exists when the return current can flow in the plane directly beneath the trace. At the edge of the ground plane the return current has to divert, and the field is no longer confined to the region between the trace and the plane, which raises radiation and changes the impedance. The 3W band gives the fringing field room to terminate in copper instead of in air. A non-grounded via inside that band is worse than no via at all, because it interrupts the path the return current would otherwise take. A split in the plane beneath the trace is more severe still: the return current is forced to detour around the gap, the loop area becomes large, and the structure radiates and couples into neighboring traces instead of behaving as a transmission line. The 2W spacing to a shielding wall keeps the wall from loading the trace; a metal wall placed too close adds capacitance to ground and pulls the impedance down.
Microstrip Couplers
Coupled microstrip traces are commonly used to sample the strength of a high-power signal and to detect standing-wave conditions. Where the requirements are modest and the coupling is greater than 20dB, a microstrip coupler can be built from two closely spaced PCB traces, as shown in Figure 10(a). When directivity is required, the coupling length L is:
L = λ/4
Here W is the width of the coupled lines, and the microstrip impedance should be maintained at 50Ω.

a: microstrip coupler

b: microstrip power divider
Figure 10: A microstrip coupler and a power divider.
The 20dB figure defines where this approach is practical: the coupled port only receives a small fraction of the incident power, so a lower coupling level would require spacing so tight that etching tolerance dominates the result. The λ/4 coupling length is what separates forward from backward coupling, which is the mechanism that gives the coupler directivity and allows it to distinguish incident from reflected power.
Microstrip Power Dividers
Where the requirements are not demanding, a microstrip power divider can also be formed from PCB traces, as shown in Figure 10(b). The impedances must satisfy the following relationships:
Z0 = 50Ω
Z1 = 21/2 Z0 = 70.7Ω
The trace length LBC from the power combining point B to the resistor at point C should satisfy:
LBC = λ/4
The resistor value is 100Ω.
The three numbers work together. The 70.7Ω branch lines transform the 50Ω system impedance at the input to the two output ports, the quarter-wave length sets the phase relationship that makes the division equal, and the 100Ω resistor placed across the outputs absorbs the difference signal so that the two output ports remain isolated from one another. If the resistor is omitted or placed at the wrong distance from point B, the divider still splits power but the outputs interact, and a mismatch on one output appears at the other.
Basic Microstrip Elements

(a)

(b)

(c)

(d)

(e)

(f)
Figure 11: Basic microstrip elements.
(1) A microstrip segment (a) can be represented by the equivalent circuit element (d):
jωL = jZ0 sin θ
jωC = j(1/Z0) tan(θ/2)
A narrow microstrip has a higher characteristic impedance, so the segment behaves as a series inductance; a wide microstrip has a low characteristic impedance and is equivalent to a shunt capacitance. This is the basis for replacing lumped elements with copper at high frequency, where a real inductor has more parasitic capacitance than useful inductance.
(2) The equivalent circuit element for an open shunt stub (b) is (e):
Zop = ?j(1/Z0) cot θop
When the stub length θop is less than 90°, that is, when the physical length is less than λg/4, the stub is equivalent to an inductive reactance.
(3) The equivalent circuit element for a shorted shunt stub (c) is (f):
Zsh = j(1/Z0) tan θsh
When the stub length θsh is less than 90°, the shorted shunt stub is equivalent to a shunt inductive reactance; when θsh is greater than 90°, it is equivalent to a capacitive reactance.
These three microstrip elements are enough to build a wide variety of microstrip circuits, and such circuits have a certain filtering effect as a natural consequence of their reactance versus frequency. The most widely used microstrip element is the λ/4 microstrip line, and one application example is described below.
Two points on a periodic sine wave separated by a quarter wavelength (90°) have the least influence on each other. When one end of a λ/4 microstrip line is connected directly to ground, or to ground through a high-frequency filter capacitor (for example, 100pF), that end is at AC ground, and the other end behaves as an AC open circuit. For signals whose wavelength corresponds to the line length, the line has an inductive effect. A typical application is the bias and supply circuit of a small-signal amplifier transistor or a power amplifier transistor.
The PCB design points are as follows:
- The bias trace at the output of the power amplifier transistor is λ/4 long, measured from the nearest high-frequency filter capacitor to the signal trace or matching copper.
- The bias trace at the input of the power amplifier transistor is λ/4 long, measured from the nearest high-frequency filter capacitor to the signal trace or matching copper.
- The parallel combination of filter capacitors should be placed together, and their order matters, as shown in Figure 12. The λ/4 high-impedance line should be drawn directly from the pad of the high-frequency filter capacitor.
The quarter-wave length is what makes the bias network transparent to the RF signal. At the operating frequency, the λ/4 line transforms the AC ground at the capacitor into an open circuit at the point where it joins the signal path, so the supply does not load the amplifier, while the DC path to the transistor remains intact. The measurement point matters as much as the length: if the λ/4 is counted from the wrong reference, the transformer no longer presents an open circuit at the signal trace and the bias network detunes the matching. Starting the high-impedance line directly at the capacitor pad avoids a short section of wider trace between the capacitor and the line, which would otherwise add capacitance at the exact point where the impedance must be highest.
Stripline Routing
Some RF signals have to pass through an inner layer of the PCB. The most common case is routing on the third layer, with the second and fourth layers kept as complete ground planes, forming an offset stripline structure, as shown in Figure 12. To keep the stripline structure intact, the following requirements must be met:
- The edge of the stripline on both sides must be at least 3W away from the edge of the ground plane.
- Within that 3W band, there must be no non-grounded vias.
- RF signal traces must not cross a gap or split in the ground plane of the second or fourth layer.

Figure 12 | Structural integrity of the stripline structure
The stripline rules mirror the microstrip rules because the failure mode is the same. In a stripline the field is distributed between the two reference planes, so the return current is split between the plane above and the plane below the trace. A split in either plane therefore interrupts part of the return path, and because the trace is buried, the resulting discontinuity cannot be inspected or corrected after fabrication. This is why the requirement is stated as a routing prohibition rather than a layout preference: the stripline structure is fully enclosed, and the only opportunity to preserve it is at the design stage, where the plane edges, the via placement, and the plane splits are all still under the designer's control.
Taken together, the requirements in this part describe a single design principle applied at different scales. The 50Ω impedance sets the trace geometry, the corner treatment keeps that geometry continuous through bends, the 3W and 2W clearances and the prohibition on plane splits keep the reference plane continuous beneath the trace, and the quarter-wave elements turn short lengths of that same controlled-impedance copper into couplers, dividers, and bias feeds. Each rule is simple on its own; what matters is that all of them are checked before the board is released, because on an RF board every one of them has a measurable effect on the result.
Ground Copper Pour Alongside RF Traces
The spacing from the ground copper pour to the signal trace must be at least 1.5W. Add ground vias along the edge of the ground copper, with via spacing less than λ/20, arranged uniformly and neatly.
The edges of the ground copper must be smooth and flat; sharp burrs are prohibited.
Except for special applications, no excess stub or protruding trace end is permitted on an RF signal trace.
6 Other Design Considerations
Add the characters "RF" to the silkscreen so that PCB fabrication and finished-board inspection follow the dedicated requirements for RF PCBs.
Because RF devices operate at very high frequencies, a protection circuit cannot be placed directly at the device input, making them more susceptible to electrostatic discharge damage than other devices. For this reason, a conspicuous ESD warning mark must be added to the silkscreen during PCB design.
- Transmission Line Models: Microstrip, Stripline, and Reflections
- Special Signal Handling and Via Effects in PCB Design
- Backplane Slot Layout and Board Position Structure for EMC Design
- PCB EMC Design: Module Partitioning and Special Component Layout
- Filter Components and Filter Circuit Design in PCB EMC Engineering
- Handling Split-Plane Crossings and Slots in PCB Design
- Grounding Concepts and Methods for PCB and Backplane Design
- PCB Design Safety Regulations: Markings, Shock, and Fuse Requirements