PCB Propagation Delay: Formula, Calculator & Solved Example

Share:
PCB Design & Signal Integrity
PCB Propagation Delay Calculation for Microstrip and Stripline With Critical Length and Skew Fixes

A signal on a circuit board moves at roughly half the speed of light, and every millimetre of copper adds a few picoseconds. You can work out that delay from the dielectric constant of the laminate, check when a trace turns into a transmission line and fix skew on a bus.

84.73 × √εeff ps/in Microstrip vs stripline Critical length rule DDR length matching Free calculator

How to calculate PCB propagation delay for microstrip and stripline traces, with a worked FR4 example and a free calculator, plus critical length, DDR length matching and skew troubleshooting.

Hello everyone, today we are going to learn how to calculate PCB propagation delay for microstrip and stripline traces, and how to use it for length matching and skew control.
PCB propagation delay
Quick Answer

What is PCB propagation delay and how do you calculate it?

PCB propagation delay is the time a signal edge takes to travel along a trace, and it depends on the effective dielectric constant around the copper: tpd = 84.73 × √εeff ps/in. For FR4 stripline with εr 4.2 this gives 173.6 ps/in or 6.84 ps/mm, while microstrip uses εeff ≈ 0.475εr + 0.67 and gives about 5.45 ps/mm. Example: a 100 mm stripline delays a clock edge by about 684 ps.

What Is PCB Propagation Delay?

PCB propagation delay is the time a signal edge needs to travel from the driver pin to the receiver pin along a copper trace, normally quoted in picoseconds per inch or per millimetre. The dielectric material around the trace sets almost all of it; trace width and the current it carries hardly matter.

Key Facts
  • Light in vacuum needs 84.73 ps per inch, which is 3.34 ps/mm.
  • Stripline delay on FR4 with εr 4.2 is about 173.6 ps/in or 6.84 ps/mm.
  • Microstrip on the same laminate is faster, about 5.45 ps/mm, because part of its field is in air.
  • A trace acts as a transmission line when its delay exceeds half the rise time.
  • Match lengths in picoseconds when nets use different layers.

At high speed a trace and its reference plane form a waveguide that carries an electromagnetic wave. You need PCB propagation delay before anything else in signal integrity, because reflections, ringing and timing skew all depend on how long the edge spends on the line.

Do You Know?

Analog Devices tutorial MT 094 gives a handy number: on a symmetric stripline with εr 4.0 a signal needs almost exactly 2 ns per foot, which is 170 ps per inch.

Advertisement

How Fast Does a Signal Travel on a PCB?

A signal on FR4 travels at about half the speed of light, roughly 146 mm per ns in stripline and 184 mm per ns in outer layer microstrip. The exact speed is c divided by the square root of the effective dielectric constant εeff.

In a stripline the trace sits between two planes, so the whole electric field passes through the laminate and εeff equals the εr of the material. In a microstrip part of the field bends up through air, so the wave sees a lower εeff.

pcb propagation delay microstrip and stripline cross section with field lines
Diagram by Instrumentation Blog showing microstrip and stripline cross sections on FR4 εr 4.2, where the field travels and the resulting delay per millimetre.

Wikipedia describes the microstrip mode as quasi TEM and notes that its effective dielectric constant climbs gradually toward that of the substrate as frequency rises. So microstrip delay from a field solver at 10 GHz can differ slightly from a low frequency estimate.

Quick Tip

Solder mask adds a thin dielectric layer over a microstrip and raises its delay a little. For tight outer layer timing, ask the fabricator for the mask thickness.

How to Calculate Propagation Delay on a PCB

To calculate PCB propagation delay, find εeff for the trace type, take its square root and multiply by 84.73 ps/in, then multiply by the trace length. The constant 84.73 is simply 25.4 mm divided by the speed of light, 0.2998 mm per ps.

Vacuum delay = 25.4 ÷ 0.2998 = 84.73 ps/in
Stripline: tpd = 84.73 × √εr ps/in
Microstrip: εeff ≈ 0.475 εr + 0.67
tpd = 84.73 × √εeff ps/in
ps/mm = (ps/in) ÷ 25.4
Total delay = tpd × length
1
Get εr
Read the laminate datasheet at your operating frequency.
2
Pick the line type
Stripline uses εr directly; microstrip needs εeff.
3
Compute tpd
Multiply 84.73 by √εeff to get ps per inch.
4
Convert units
Divide by 25.4 to get ps/mm.
5
Multiply by length
Use the routed length from the CAD report, including tuning.

The microstrip formula above is the simple approximation used in Analog Devices MT 094, and it ignores trace geometry. Sierra Circuits uses 0.64 εr + 0.36 for wider traces, which gives about 5.82 ps/mm for the same laminate, so always confirm critical outer layer nets with your fabricator or a field solver.

Solved example, stripline, FR4 εr 4.2, length 100 mm
√4.2 = 2.049
tpd = 84.73 × 2.049 = 173.6 ps/in
173.6 ÷ 25.4 = 6.84 ps/mm
Delay = 6.84 × 100 = 684 ps
Rise time 1 ns: Lc = 1000 ÷ (2 × 6.84) = 73 mm
bar chart of delay per mm for air microstrip and stripline with solved example
Diagram by Instrumentation Blog comparing delay per millimetre in air, microstrip and stripline on FR4, with the 100 mm stripline solved example and critical length.
PCB Propagation Delay Calculator
Result
Delay 684 ps at 6.84 ps/mm, critical length 73 mm, treat as transmission line

Change the type to 2 and the same 100 mm trace drops to about 545 ps at 5.45 ps/mm, with a critical length near 92 mm. Once you know the delay, size the copper width for current with our PCB trace width calculator and then tune width for impedance in the stackup tool.

Advertisement

Microstrip vs Stripline Propagation Delay

Stripline is always slower than microstrip on the same laminate, because all of its field lines sit inside the dielectric. On FR4 with εr 4.2 the difference is about 1.39 ps per mm, which becomes 139 ps over 100 mm.

ParameterMicrostripStripline
LocationOuter layer, air aboveInner layer, planes on both sides
εeff at εr 4.2About 2.67 (approximation)4.2
Delay per inchAbout 138.3 psAbout 173.6 ps
Delay per mmAbout 5.45 psAbout 6.84 ps
Signal speedAbout 184 mm per nsAbout 146 mm per ns
Depends on geometryYes, slightlyAlmost no
Shielding and crosstalkWeakerBetter

Altium gives typical values of about 150 ps/in for a 50 ohm microstrip and 171 ps/in for stripline on a Dk 4 laminate, which agrees well with the formulas. Your layer stackup design decides which nets go on outer layers and which go inside, so it fixes their delay before routing starts.

Do You Know?

A 0.1 mm and a 0.3 mm stripline on the same core have almost the same delay per millimetre, even though their impedance is very different.

What Is Critical Length in PCB Design?

Critical length is the trace length beyond which a digital edge sees the trace as a transmission line, and Analog Devices sets it where one way delay equals half the rise time. Above that length you need controlled impedance traces and termination.

Lc = tr ÷ (2 × tpd)
tr = 1 ns = 1000 ps, tpd = 6.84 ps/mm
Lc = 1000 ÷ 13.68 = 73 mm
Analog bandwidth: tr ≈ 0.35 ÷ fmax

The clock frequency is not in the formula, only the edge rate, so a slow clock from fast logic still needs care on long traces. Analog Devices also gives a conservative rule of about 2 inches of trace per ns of rise time, and you can use impedance matching with series or parallel resistors once a net crosses that limit.

Quick Tip

Measure the real rise time at the receiver with a fast probe, because many datasheets quote the slowest case. Edges from modern FPGAs and microcontrollers are often far faster than the clock rate suggests.

PDF
Analog Devices MT 094: Microstrip and Stripline Design
Free PDF tutorial with delay formulas, impedance equations and the half rise time termination rule

PCB Propagation Delay in Length Matching for DDR and Clocks

Length matching uses PCB propagation delay to make all bits of a bus arrive inside the same timing window, and the safe way is to match in picoseconds, not millimetres. Modern CAD tools convert a delay rule into length per layer once you enter the stackup.

Millimetres mislead across layers: 50 mm of microstrip takes about 272 ps, while 50 mm of stripline takes about 342 ps, a 70 ps gap for two nets of the same length. If a controller allowed 10 ps of skew, stripline mismatch would need to stay within 10 ÷ 6.84 = 1.46 mm, so take the real budget from the controller layout guide.

DDR data lanes
Each DQ bit is matched to its strobe within the byte lane, using delay rules per layer.
Differential pairs
The P and N lines must match closely so common mode noise stays low.
Clock trees
Clock branches to several chips are tuned so each receiver sees the edge at the same time.
High speed serial links
Only the pair skew matters, since the receiver recovers the clock from the data.

For pairs, our guide on differential pair routing explains where to place tuning bumps so the coupling is not broken. Serpentines also couple to themselves and to neighbours, so keep loop spacing wide as described in our article on PCB crosstalk reduction.

Good matching habits
  • Set the rule in picoseconds and let the tool convert per layer
  • Include package pin delay from the chip vendor
  • Tune close to the mismatch source
  • Keep serpentine gaps at least three trace widths
Common mistakes
  • Matching only in millimetres across layers
  • Ignoring via and connector delay
  • Tight serpentines that couple to themselves
  • Tuning over a split plane or void
Advertisement

Troubleshooting Skew and Timing Errors

Most skew problems come from matching in the wrong unit, mixing layers, ignoring via and pin delay, or routing over a broken plane. Work through the flowchart below in order, since each check is cheaper than the next.

flowchart to troubleshoot skew and timing errors on a PCB bus
Diagram by Instrumentation Blog showing a step by step skew troubleshooting flowchart for PCB buses, from unit checks to vias, plane gaps and scope or TDR verification.
SymptomLikely causeField fix
One bit fails at high data rateThat net changes layer and runs longer in striplineRematch in ps using per layer delay
Measured delay higher than calculatedReal εr higher than assumedUse fabricator εr or measure with TDR
Pair shows common mode noiseIntra pair skew from uneven bendsAdd a small bump near the bend that caused it
Ringing on a clock lineTrace longer than critical length without terminationAdd a series resistor near the driver

A broken reference changes both impedance and PCB propagation delay, so check the plane under every timed trace using our guides on ground plane design and the PCB return current path. Vias add delay and a discontinuity, and our article on through hole, blind and buried vias helps you pick the right type.

Myth: Wider traces carry signals faster.
Fact: Trace width changes impedance, but the delay per mm is set by the dielectric around the trace.
Myth: A slow clock never needs transmission line care.
Fact: The edge rise time decides critical length, so a fast edge on a slow clock still rings.
Myth: FR4 always has εr 4.5.
Fact: FR4 grades vary and εr falls with frequency, so take the value from the laminate datasheet.
  • Laminate εr taken at the operating frequency
  • Delay rules written in ps, not only mm
  • Package pin delay included for DDR and FPGA nets
  • Solid reference plane under every timed net
  • Critical length checked against measured rise time
  • Final skew report reviewed after routing

To verify PCB propagation delay in the lab, use a TDR or two deskewed channels on a fast oscilloscope, as covered in our article on the cathode ray oscilloscope. Simultaneous switching can also shift edges in time, so review ground bounce before blaming the trace.

Eric Bogatin explains why a signal is a wave travelling between the trace and its return path, and that is why the dielectric sets the delay.

If you are new to layout, start with these PCB design basics and our list of essential PCB design rules. For outer layer impedance, a microstrip impedance calculator pairs well with the delay numbers here, and our guide on high speed PCB signal integrity goes deeper.

PCB Propagation Delay FAQ

What is pcb propagation delay and how is it measured in ps per mm?

PCB propagation delay is the time an edge needs to travel along a trace, usually quoted in ps/in or ps/mm. On FR4 with εr 4.2 it is about 6.84 ps/mm for stripline and 5.45 ps/mm for microstrip.

Engineers measure it with a TDR or by comparing two scope channels at both trace ends after deskewing the probes.

What is the difference between microstrip and stripline propagation delay with example?

Stripline is slower because its whole field sits inside the dielectric, while microstrip shares part of its field with air. With εr 4.2, a 100 mm stripline takes about 684 ps and the same microstrip about 545 ps.

That 139 ps gap is why outer and inner layer lengths cannot be matched in millimetres alone.

How to calculate pcb propagation delay step by step for a stripline trace?

Take the square root of εr, multiply by 84.73 to get ps per inch, then divide by 25.4 for ps per mm. For εr 4.2 that gives 173.6 ps/in or 6.84 ps/mm.

Multiply by the routed length, so a 100 mm trace gives about 684 ps of one way delay.

What is the critical length rule for rise time and trace length?

A trace behaves like a transmission line when its one way delay is more than half the signal rise time. Critical length is the rise time divided by twice the delay per mm.

With a 1 ns edge on FR4 stripline, that is 1000 ÷ (2 × 6.84), or about 73 mm.

Why does my DDR data bus show skew even though lengths match?

The usual cause is matching in millimetres while nets run on different layers, because microstrip is faster than stripline. Vias, connector pins and package delay inside the chip also add time that a plain length rule ignores.

Set the constraint in picoseconds, include pin delay from the datasheet and recheck the report after routing.

Which dielectric material gives lower propagation delay for high speed board routing?

A laminate with lower εr gives lower delay, because delay scales with the square root of the effective dielectric constant. Moving from εr 4.2 to εr 3.0 cuts stripline delay from 6.84 to about 5.78 ps/mm.

Choose by loss, cost and stack availability as well, since delay alone rarely drives material choice.

Advertisement

Related Articles

External References

What We Learn Today

  • PCB propagation delay equals 84.73 × √εeff ps per inch, so FR4 stripline with εr 4.2 gives about 6.84 ps per millimetre of trace.
  • Microstrip is faster than stripline because part of its field travels in air, giving about 5.45 ps/mm on the same FR4 laminate.
  • A trace longer than rise time divided by twice its delay acts as a transmission line, and bus matching should be written in picoseconds.
I hope you like above blog. There is no cost associated in sharing the article in your social media. Thanks for reading!! Happy Learning!!
Sunayana Gadepatil, author at Instrumentation Blog
Author · instrumentationblog.in
Ms. Sunayana Gadepatil is an instrumentation professional, technical writer, and the author behind Instrumentation Blog. With a strong interest in industrial instrumentation, process measurement, and automation, she specializes in simplifying complex technical concepts into clear, practical, and easy to understand insights. Through her articles, Ms. Sunayana shares valuable knowledge on flow, pressure, level, temperature, control systems, and industrial automation for engineers, students, technicians, and industry professionals.
Technically reviewed on

Leave a Reply

Your email address will not be published. Required fields are marked *

Support free learning

Help keep every guide, calculator and tool 100% free

Hosting, software and hours of research go into every article. Even a small contribution helps us publish more in-depth guides for students, technicians and engineers.

  • No paywalls
  • No sign up
  • Free for everyone