Layer Stackups, Vias, and Impedance
Two layers are a budget. Four layers are a ground plane — and a ground plane is the single largest improvement a board can get.
🎯 By the end you'll understand
Why the copper under a trace is part of the circuit, and what changes when you put a continuous plane there. What a four-layer stackup is physically made of — core, prepreg, foil, glass style — and how to read the one Beacon orders. Why characteristic impedance is a property of the stackup rather than a number you copy from a reference design, with the microstrip equation worked twice to show the same 50 Ω asking for a 0.35 mm trace on one board and a 2.8 mm trace on another. When impedance control is genuinely required and when paying for it is waste. And what vias actually cost — in money, in inductance, and in the joints they can starve.
KEY INSIGHTCurrent travels in loops, and the loop's other half is whatever copper is underneath
The two-layer prototype worked perfectly on the bench and rang like a bell on the scope. The four-layer respin had the same schematic, the same firmware, the same parts, and half the noise. Nothing changed except what was underneath the traces.
Schematics draw a signal as a line from a driver to a receiver. That line is half a circuit. Every electron that leaves the driver comes back, and on a board it comes back through copper you did not draw and probably did not think about. At DC the return spreads out to take the lowest-resistance path, which usually means a broad fan through the ground pour. Above roughly the tens-of-kilohertz region the return stops caring about resistance and starts minimising inductance, and the lowest-inductance return path is the one that hugs the outgoing trace as closely as possible — directly beneath it, in the nearest continuous copper.
That single fact is the whole argument for four layers. It says the plane under a trace is not background, it is the other conductor of a transmission line. It says a break in that plane is a break in the circuit, even though no net is disconnected and no rule is violated. It says the loop enclosed between a trace and its return sets how much the signal rings, how much voltage appears across "ground" between two chips, and how much the board radiates. And it says the distance from the trace to the plane — 0.21 mm on the stackup Beacon orders, 1.53 mm on a two-layer board of the same thickness — is one of the most consequential numbers on the entire design, chosen not by you but by a laminate press in a factory.
You do not choose trace impedance. You choose a stackup, and the stackup chooses the trace width that gives an impedance. Anyone who hands you "use 0.25 mm for 50 Ω" without naming the dielectric height, the dielectric constant and the copper weight has handed you a number for a board that is not yours.
CORE CONCEPTWhat layers two and three actually buy
"Four layers gives you more room to route" is the reason beginners state and the least important one. Here are the three that matter, in order.
1. A continuous return under every fast signal
On a two-layer board the bottom side is both the ground pour and the second routing layer, and those two jobs fight. Every bottom-side trace is a slot in the pour; every slot is a detour for some return current above it. On a four-layer board layer 2 has exactly one job — be uncut copper — and every trace on layer 1 gets a return path directly under it whether you thought about it or not. That is the difference between a board that is right by construction and a board that is right if you were careful everywhere.
2. Loop area, and therefore emissions and ringing
Take a 20 mm signal trace. On Beacon's four-layer stack the return runs 0.21 mm beneath it, so the enclosed loop is about 20 × 0.21 = 4.2 mm². On a 1.6 mm two-layer board the return is 1.53 mm beneath, giving 30.6 mm² — 7.3× the area. Differential-mode radiation from a current loop scales with its area, so at the same current and frequency that is 20·log₁₀(7.3) ≈ 17 dB more field. Seventeen decibels is the difference between passing a radiated-emissions scan with margin and failing it outright.
Inductance grows more slowly than area, because inductance depends on the logarithm of the geometry rather than the geometry itself. Working it through the microstrip relation L′ = Z₀·√εeff / c: a 50 Ω trace on the four-layer stack has about 0.30 nH per mm; a 0.25 mm trace on the two-layer board comes out near 131 Ω with εeff ≈ 2.9, giving 0.74 nH per mm. So 7× the loop area buys only 2.5× the inductance — a useful thing to know, because it means the emissions penalty is far worse than the ringing penalty, and people who judge a board by how clean the scope looks will under-estimate how badly it radiates.
3. Low-inductance power distribution — but not the capacitance you were promised
A common claim is that a ground/power plane pair is a free distributed capacitor. Check it on Beacon's numbers. The planes are the full board, 35 × 25 mm = 875 mm², separated by the 1.065 mm core with Dk ≈ 4.6:
C = ε₀·εr·A/d = (8.854 × 10⁻¹² × 4.6 × 8.75 × 10⁻⁴) / 1.065 × 10⁻³ ≈ 33 pF.
Thirty-three picofarads. One 0402 decoupling capacitor is 100 nF — three thousand times more. On a thin-core high-speed board where the planes are 0.1 mm apart the argument starts to earn its keep; on a 1.6 mm four-layer board it is folklore. What the plane pair really provides is low inductance: a wide, short, uninterrupted path from a decoupling capacitor to the pin it serves. Inductance, not capacitance, is what limits how fast charge arrives.
There is a fourth reason, and it is Beacon's real one: you cannot route this board on two layers without destroying the pour. An ESP32-C3-MINI-1 module occupies a large fraction of a 35 × 25 mm outline; add a USB-C receptacle, a battery connector, a buck converter with its inductor, a charger, two I²C sensors, an LED, a button and a Tag-Connect pattern, and the bottom side of a two-layer version would be shredded into ribbons. A pour cut into ribbons is not a plane; it is a set of accidental antennas that happen to be at ground potential somewhere.
HOW IT WORKSInside the stackup: core, prepreg, foil, and the glass in between
A multilayer board is a sandwich pressed under heat. The rigid middle is a core: cured FR-4 with copper foil bonded on both faces, which is where the inner layers are etched. Outside the core goes prepreg — glass cloth pre-impregnated with partly-cured resin — and then outer copper foil. Heat and pressure melt the prepreg resin, which flows, fills the etched gaps and cures, gluing the whole stack into one laminate. Outer copper is then plated up during through-hole plating, which is why "1 oz outer" usually means half-ounce foil plus plating.
FR-4 is not one material. The glass cloth comes in standard styles — 7628, 2116, 1080, 3313 and others — that differ in thickness and in how much resin they carry. Resin and glass have different dielectric constants (roughly 3 and 6), so the mix sets the effective Dk of that layer, and the weave sets how much Dk varies across the board. That is why the fab names its stackups after the glass style.
| Layer | Material | Nominal thickness | Dk (≈1 GHz) | Beacon uses it for |
|---|---|---|---|---|
| L1 (F.Cu) | Copper, 1 oz finished | 0.035 mm | — | All fast signals, power fan-out, most parts |
| Dielectric 1 | Prepreg, 7628 glass | 0.2104 mm | ≈ 4.4 | Sets L1 impedance |
| L2 (In1.Cu) | Copper, 0.5 oz | 0.0175 mm | — | Uncut ground — the reference for everything on L1 |
| Core | Cured FR-4 laminate | 1.065 mm | ≈ 4.6 | Mechanical rigidity; keeps L2 and L3 far apart |
| L3 (In2.Cu) | Copper, 0.5 oz | 0.0175 mm | — | 3.3 V pour plus VBAT and VBUS islands |
| Dielectric 2 | Prepreg, 7628 glass | 0.2104 mm | ≈ 4.4 | Sets L4 impedance (against a split plane) |
| L4 (B.Cu) | Copper, 1 oz finished | 0.035 mm | — | Slow signals, test pads, stitched ground fill |
SIG / GND / PWR / SIG versus SIG / GND / GND / SIG
Given four layers there are two sane arrangements, and engineers argue about them for good reasons.
| SIG / GND / PWR / SIG | SIG / GND / GND / SIG | |
|---|---|---|
| Power distribution | A plane — low impedance, easy, no routing effort | Fat traces on the outer layers; you route every rail by hand |
| Reference for L4 | The power plane, which has splits wherever rails divide | Solid ground — both outer layers are equally safe |
| Routing capacity | Two signal layers | Two signal layers, minus whatever the power traces eat |
| Failure mode | A fast signal on L4 crosses a plane split and its return has nowhere to go | A power trace is too narrow and drops volts, or blocks the routing you needed |
| Best when | One or two dominant rails, few fast signals on the bottom | Many rails and islands, or fast signals on both outer layers |
Beacon takes SIG/GND/PWR/SIG, which is the canon's choice and the pragmatic one for a board whose fast signals — the module's USB pair and its own internal radio — all live on the top layer. The discipline that makes it safe is a single rule enforced in review: nothing on L4 is fast, and nothing on L4 crosses a break in L3. I²C at 400 kHz, an LED data line, a button, and test pads can live on the bottom layer without caring what plane is above them. A 12 Mbit/s USB pair cannot, so it never goes there.
CORE CONCEPTImpedance is a property of the stackup, not of the trace
Characteristic impedance is the ratio of voltage to current a wave sees while it is still travelling, before it knows what is at the far end. It comes from the per-unit-length inductance and capacitance of the trace-plus-return structure: Z₀ = √(L′/C′). Widening the trace increases C′ (more area facing the plane) and slightly decreases L′, so impedance falls. Moving the plane further away decreases C′ and increases L′, so impedance rises. Both effects live in the same geometry, which is why width alone means nothing.
You cannot measure Z₀ with a multimeter — a DC ohmmeter sees a short. It is measured with a time-domain reflectometer on a test coupon that the fab adds to the panel edge, built in the same press cycle as your board.
For a trace on an outer layer over a plane, with everything in mils:
Z₀ = (87 / √(εr + 1.41)) · ln( 5.98·h / (0.8·w + t) )
where h is the dielectric height to the reference plane, w the trace width, t the copper thickness. It is stated as valid for roughly 0.1 ≤ w/h ≤ 3.0 and 1 ≤ εr ≤ 15, and it ignores solder mask, etch taper and the frequency dependence of Dk. Outside that window, or when you are paying for impedance control, use the fab's own field solver.
The same 50 Ω, twice
Work it for a 50 Ω single-ended trace on Beacon's four-layer stack: h = 0.2104 mm = 8.28 mil, t = 1.4 mil for 1 oz copper, εr = 4.4.
√(4.4 + 1.41) = 2.410, so the prefactor is 87 / 2.410 = 36.1.
Setting 36.1 · ln(5.98 · 8.28 / (0.8w + 1.4)) = 50 gives ln(…) = 1.385, so 49.5 / (0.8w + 1.4) = e1.385 = 4.00.
0.8w + 1.4 = 12.4 → w = 13.7 mil = 0.35 mm.
Now h = 1.53 mm = 60.2 mil and everything else is unchanged.
5.98 · 60.2 = 360, and 360 / 4.00 = 90.1, so 0.8w = 88.7 → w = 111 mil = 2.82 mm.
Two point eight millimetres. On a 25 mm-wide board that single trace consumes more than a tenth of the width, and it is not routable past the module. This is why "just use two layers and be careful" is not a strategy for anything with a radio: the geometry stops being buildable long before your skill runs out.
Differential pairs, and the honest question of whether you need them
USB 2.0 specifies 90 Ω differential (with a ±15% tolerance) for D+ and D−. For an edge-coupled pair on an outer layer the usual approximation adds a coupling term to the single-ended result:
Zdiff ≈ 2·Z₀·(1 − 0.48·e−0.96·s/h), with s the edge-to-edge gap. Closer coupling (small s/h) pulls the differential impedance down; a pair spaced several dielectric heights apart is barely a pair at all — it is two independent single-ended traces that happen to run together, and it neither rejects common-mode noise nor holds its impedance.
Now the contrarian half. Impedance control only matters when the trace is electrically long: when a reflection takes longer to come back than the signal's edge takes to finish. The standard rule of thumb is that a trace is electrically short if its one-way delay is under about one sixth of the rise time.
The ESP32-C3's native USB Serial/JTAG runs at full speed, 12 Mbit/s, where the specified rise time is at least 4 ns. On this stack the effective dielectric constant for a 0.24 mm trace works out near 3.2, so propagation velocity is c/√3.2 ≈ 168 mm/ns — a delay of 5.96 ps per mm.
Critical length = 4000 ps / (6 × 5.96 ps/mm) ≈ 112 mm. Beacon's USB run from the receptacle to the module is about 15 mm — about a seventh of the threshold, and shorter than the whole board. The pair is electrically short by a wide margin.
Conclusion: route it as a proper coupled pair with a solid plane beneath, because that costs nothing and buys common-mode rejection and lower emissions — but do not pay the fab for controlled impedance on it. The canon's 22 Ω series resistors on D± sit in the middle of that "line" and are invisible for the same reason: a 15 mm trace at full speed does not behave like a transmission line.
SEE ITStackup and impedance calculator
Pick a board, pick what you are routing, and set the geometry. The impedance follows from the stackup, not from your intentions. The last control is the one that costs money: whether you order controlled impedance, which changes who decides the trace width — you, or the fab.
Three things are worth provoking deliberately. Switch to the two-layer board with the 50 Ω target and watch the required width leave the realm of the routable. Change only the copper weight from 1 oz to 2 oz and watch a correct trace drift several ohms off target, because thicker copper adds capacitance to the plane. And order controlled impedance: the impedance snaps onto target and the widget tells you the fab has just taken your trace width away from you. That last one surprises people. Controlled impedance is not a promise to build what you drew; it is a contract to hit a number, and the fab adjusts widths to hit it on the stackup they actually pressed.
COMPARISONVias: four kinds, three costs
A via is a plated hole connecting layers. The kind you use is a process decision, and process decisions are where board cost lives.
What a via costs electrically
A via is a short vertical conductor, so it has inductance. The usual estimate, with height h and diameter d in inches, is L ≈ 5.08·h·[ln(4h/d) + 1] nH. For a through via on a 1.6 mm board (0.063 in) with a 0.3 mm finished hole (0.0118 in): ln(4 × 0.063 / 0.0118) = ln(21.4) = 3.06, so L ≈ 5.08 × 0.063 × 4.06 ≈ 1.3 nH.
Take that number with the caveat it deserves. Inductance is a property of a loop, not of a piece of wire, and this formula reports a partial inductance that assumes the return is far away. In a real board the effective inductance of a signal via depends strongly on how close the nearest ground via is — put a stitching via 0.5 mm from a signal via and the pair's loop inductance is a fraction of the isolated figure. This is why "add a ground via next to every layer change on a fast net" is real advice and not superstition.
The practical consequences on Beacon: a decoupling capacitor that reaches ground through one via has that via's inductance in series with it, which is comparable to the capacitor's own ESL, so the via can double the effective inductance of the decoupling path. Two vias side by side roughly halve it. And for the RF module, stitching vias along the ground pour boundary keep the plane a plane at 2.4 GHz: the usual guideline is to space stitching at a twentieth of a wavelength or less. In FR-4 at 2.45 GHz the wavelength is about 58 mm, so λ/20 ≈ 2.9 mm — stitch every 3 mm or tighter near the module.
Via in pad
Putting a via inside a solder pad is tempting on leadless parts, and dangerous in the plainest way: during reflow, molten solder wicks down the open barrel and the joint above it starves. The fixes are to have the fab fill the via with non-conductive epoxy and plate over it (an added process and an added cost), or to tent the via with mask (cheap, unreliable on the pad side), or to move the via out of the pad and connect with a short trace, which is free and usually possible. Beacon's only real candidate is the buck's ground pad, and the design keeps its vias just outside the pad rather than paying for filled-and-capped on a 25-unit pilot.
Minimum via drill, minimum annular ring and minimum trace/space are the manufacturer's current published capability, not laws. JLCPCB's standard four-layer process is presently around 0.09 mm minimum trace and space and 0.15 mm minimum via drill; other fabs and other process tiers differ, and every one of these numbers has been revised over the years. Read the capability page the week you design, and put the numbers into KiCad's Board Setup so DRC enforces them for you.
BEACONBeacon Rev A's stackup decision, written down
Here is the decision as it goes into the project's design-intent note — the kind of paragraph that saves the Lesson 5.9 review twenty minutes of re-deriving.
(setup
(stackup
(layer "F.Mask" (type "Top Solder Mask") (thickness 0.01))
(layer "F.Cu" (type "copper") (thickness 0.035))
(layer "dielectric 1" (type "prepreg") (thickness 0.2104)
(material "FR4") (epsilon_r 4.4) (loss_tangent 0.02))
(layer "In1.Cu" (type "copper") (thickness 0.0175)) ; GND — never cut
(layer "dielectric 2" (type "core") (thickness 1.065)
(material "FR4") (epsilon_r 4.6) (loss_tangent 0.02))
(layer "In2.Cu" (type "copper") (thickness 0.0175)) ; +3V3 pour, VBAT/VBUS islands
(layer "dielectric 3" (type "prepreg") (thickness 0.2104)
(material "FR4") (epsilon_r 4.4) (loss_tangent 0.02))
(layer "B.Cu" (type "copper") (thickness 0.035))
(copper_finish "ENIG")
(dielectric_constraints no) ; no controlled impedance ordered — see note
)
)
Four layers, JLC04161H-7628, 1.6 mm, ENIG
Four is forced by R8 (35 × 25 mm) and by the radio: there is no arrangement of this parts list on two layers that leaves an uncut ground pour. 1.6 mm because the enclosure and the USB-C receptacle both assume it. ENIG rather than HASL because the module's castellations and the leadless parts want flat, coplanar pads — it costs more per board and it is the cheapest insurance on the panel.
L2 is ground and nothing else
Not a single trace, not a single split. The rule is enforceable by looking: if L2 has anything on it but copper and via antipads, the review stops. This is the layer that makes every other decision forgiving.
L3 is power, and therefore has splits
A main +3V3 pour, an island for VBAT from the protection pair to the buck input and the charger, an island for VBUS from the receptacle to the charger. Wherever L3 is empty it gets ground fill, stitched to L2 — free copper, better thermal spreading, fewer floating islands.
Nothing fast on L4
L4 carries I²C at 400 kHz, the LED data line, the button, the Tag-Connect fan-out and the four pogo test pads. Every one of those is slow enough that crossing a break in L3 does no harm. The USB pair and everything near the module stays on L1 over solid ground.
Through vias only, 0.6 mm pad / 0.3 mm drill (a 0.15 mm annular ring, inside the 0.13 mm capability and the house 0.25 mm minimum drill), no via-in-pad
Blind and buried vias would move the order into HDI pricing for a 25-unit pilot with no HDI need. The 0.15 mm drill is the fab's stated minimum; Beacon's default via uses it only where the module fan-out is tight, and 0.2 mm elsewhere for yield margin.
No controlled impedance ordered — and the condition that would reverse it
Beacon's ESP32-C3-MINI-1 carries its own PCB antenna, so there is no 50 Ω feed line to control; the only differential pair is a full-speed USB run of about 15 mm, which the calculation above shows is electrically short by more than 7×. Ordering impedance control would add cost, a test coupon on the panel, and a fab-chosen trace width, for no measurable benefit. The condition: if Rev B moves to the ESP32-C3-MINI-1U with a u.FL connector and an external antenna, that feed line is a real 50 Ω transmission line and impedance control stops being optional.
Notice the shape of that decision. Two of the six lines are refusals — no HDI, no impedance control — and each refusal is recorded with the condition that would overturn it. A design-intent note that only records what you did is half a note; the useful half is what you decided not to do and why, because that is the part the next engineer would otherwise re-litigate or, worse, quietly reverse.
WEAKNESSWhere stackups and impedance bite
This is the single most common impedance error and it never announces itself. A vendor's reference layout for a 0.5 mm four-layer board might specify 0.25 mm for 50 Ω; drop that width onto a 1.6 mm four-layer board with 0.21 mm prepreg and you get roughly 60 Ω, and onto a two-layer board you get well over 100 Ω. Nothing fails, nothing warns, and the radio's range is quietly worse than the datasheet promised. Widths are only transferable together with h, εr and copper weight — which is exactly the information reference designs usually omit.
On a SIG/GND/PWR/SIG board, a bottom-layer trace references layer 3. If layer 3 is one solid, well-decoupled rail, that is acceptable — at high frequency a rail bypassed to ground is a ground. If layer 3 is carved into +3V3, VBAT and VBUS islands, then a trace crossing from over one island to over another has its return current stranded at the boundary, and the return goes the long way round through whatever decoupling capacitor happens to bridge the rails. The loop area explodes and nothing in DRC has an opinion about it. On Beacon this is why "nothing fast on L4" is a written rule rather than a habit.
Impedance control costs money, adds a coupon to the panel, sometimes forces a minimum panel size, and gives the fab licence to change your trace widths. Ordering it on a board with no electrically long trace is paying for a service you cannot benefit from. Ordering it without a clear impedance-control drawing naming the layers, nets, target impedance and tolerance is worse: the fab will either ask (delay) or guess (bad). If you need it, specify it properly; if you do not, write down why in the design-intent note so nobody adds it later "to be safe".
KEY INSIGHTHow this connects
- Decoupling, Grounding, and Return Paths (2.5) — the physics this lesson buys hardware for: return current, loop area, and why a decoupling capacitor's inductance is mostly in its route, not in the part.
- From Schematic to Board (5.1) — the stackup is set in Board Setup at the start of layout, because changing it later invalidates every width you have drawn.
- Routing: Traces, Current, and Return Paths (5.6) — where these numbers become copper: trace widths from current, differential-pair rules, and what happens when a trace crosses a split in L3.
- RF and Antenna Layout for the ESP32 Module (5.7) — the reason Beacon has no 50 Ω trace at all, and what the module's antenna demands from the layers underneath it instead.
The stackup is now fixed and the electrical rules follow from it. Next: where the parts go — because placement decides most of the routing before a single trace is drawn.
GLOSSARYKey terms introduced
- Core
- Cured FR-4 laminate with copper foil on both faces; the rigid middle of a multilayer stack, where inner layers are etched before pressing.
- Prepreg
- Glass cloth pre-impregnated with partly cured resin; it melts and flows during lamination to bond the stack and set the dielectric height between an outer and inner layer.
- Dk (εr)
- Relative dielectric constant of the laminate; it sets propagation velocity and, with the geometry, the impedance. It varies with glass style, resin content and frequency.
- Characteristic impedance (Z₀)
- √(L′/C′) for a trace and its return; the ratio of voltage to current a travelling wave sees. A geometry property, not measurable with an ohmmeter.
- Microstrip / stripline
- A trace on an outer layer over one plane (microstrip) versus a trace on an inner layer between two planes (stripline); different formulas, different velocities, different widths for the same impedance.
- Controlled impedance
- A paid fab service: they adjust trace widths for the stackup they actually press and verify with a TDR measurement on a panel-edge test coupon, to a stated tolerance (commonly ±10%).
- Electrical length
- A trace's one-way propagation delay compared with the signal's rise time. Under roughly a sixth of the rise time, reflections settle inside the edge and impedance control stops mattering.
- Stitching via
- A ground via placed to tie pours on different layers together; spaced at or below a twentieth of a wavelength to keep the pour behaving as one plane at the frequency of concern.
ACTIVE RECALLCheck your understanding
Answer in your own words first, then reveal.
1A colleague hands you "0.25 mm gives 50 Ω, I checked it". What three pieces of information must you ask for before the number means anything, and what does the answer change?›
The dielectric height to the reference plane, the dielectric constant of that layer, and the copper weight. Impedance comes from the trace-plus-return geometry, so a width without them is meaningless. On Beacon's 0.21 mm prepreg with 1 oz copper, 50 Ω wants about 0.35 mm; on a two-layer 1.6 mm board it wants 2.82 mm — the same target, an eightfold difference in width. Copper weight alone moves it several ohms: doubling to 2 oz on the four-layer stack pulls a 0.35 mm trace from 50 Ω down towards 46 Ω, because thicker copper adds capacitance to the plane.
2Beacon's USB pair carries 12 Mbit/s over about 15 mm. Justify, with a calculation, why it does not need controlled impedance — and say what you still do about it.›
Full-speed USB has a specified rise time of at least 4 ns. Propagation on this stackup is about 5.96 ps/mm (c divided by √3.2, roughly 168 mm/ns), so the critical length — where one-way delay reaches a sixth of the rise time — is 4000 ps ÷ (6 × 5.96 ps/mm) ≈ 112 mm. A 15 mm run is under an eighth of that, so reflections settle well inside the edge and the trace is not behaving as a transmission line. What you still do: route it as a tightly coupled pair, keep it over solid ground on L1, match the two lengths, and never cross a plane split. Those cost nothing and buy common-mode rejection and lower emissions. What you skip is paying the fab for impedance control and a test coupon.
3Why is "the ground and power planes form a useful decoupling capacitor" close to worthless on Beacon, and what do the planes actually give you instead?›
Run the number: 875 mm² of overlapping plane separated by a 1.065 mm core with Dk ≈ 4.6 gives about 33 pF — three thousand times less than a single 100 nF decoupling capacitor. The plane-pair capacitance argument only starts to matter on thin-core boards where the planes are tens of microns apart. What the planes really provide is very low inductance: a wide, short, uninterrupted return path so that a decoupling capacitor's charge reaches the pin quickly, and a defined reference so that every trace has a return directly beneath it. Inductance is what limits how fast charge arrives; capacitance is what the capacitors are for.
4Beacon uses SIG/GND/PWR/SIG. What specific failure does that arrangement invite, and what rule does the design use instead of avoiding the arrangement?›
Bottom-layer traces reference layer 3, which is a power plane split into +3V3, VBAT and VBUS islands. A signal on L4 that crosses from over one island to over another has no continuous return beneath it; the return current detours to whatever capacitor bridges the two rails, and the loop area — and therefore the radiated field and the ringing — grows sharply. No DRC rule catches it because no net is disconnected. Beacon's rule is that nothing fast lives on L4: only 400 kHz I²C, the LED data line, the button and test-point fan-out, all of which have edges slow enough not to care. Everything fast stays on L1 over uncut ground. The alternative arrangement, SIG/GND/GND/SIG, removes the hazard entirely at the price of routing every power rail as traces by hand.