The properties and role of insulation in PCB manufacturing are usually described as one thing, done by one layer, judged by one number. In a real board the insulation is four different materials — the core laminate, the prepreg that bonds it, the solder mask on the surface and the conformal coating over that — and each is asked a different question: can it hold off voltage, does it still resist leakage after a week at 85 % relative humidity, and what does it do to a signal passing through it. Those three questions have three different answers, and optimising one of them usually degrades another.
One Word, Four Materials
The single phrase “insulation layer” covers four materials that are deposited by four different processes, are between 10 and 60 times apart in thickness, and fail in four different ways. Treating them as one property is the origin of most insulation mistakes, because a design change made to improve one of them is silently paid for by another.
| Material | Typical thickness | What it is actually for | Number that governs it | How it fails |
|---|---|---|---|---|
| Core laminate | 0.05–1.6 mm (0.1 mm and 0.13 mm are common RF cores) | Holds the copper apart over the whole board area; provides the mechanical body | Dk, Df, dielectric strength, Z-axis CTE, Tg and Td | CAF between holes, delamination at reflow, ionic leakage after moisture |
| Prepreg / bondply | 0.05–0.2 mm per ply, 2–4 plies per bond line | Bonds cores together and fills the copper pattern; becomes dielectric after cure | Resin content, flow, gel time, and the cured thickness tolerance | Resin starvation over heavy copper, voids, bond line thinner than designed |
| Solder mask | 15–25 µm | Keeps solder off, and separates adjacent pads | Resolution, adhesion, Dk 3.5–4.2 | Pinholes, blistering, ionic residue under the mask, dendritic growth between pads |
| Conformal coating | 25–75 µm | Environmental barrier over the assembled board | Coverage completeness, cure, adhesion over flux residue | Missed coverage at tall components and connector edges; the classic field failure point |
The thickness column explains most of the confusion. A core is a structural element whose dielectric behaviour is a side effect; a solder mask is a 20 µm film whose structural contribution is nil but whose Dk still shifts a microstrip by 1–3 Ω. When an article says the insulation “protects against short circuits and moisture”, it is describing the solder mask and the coating, and then applying that description to the laminate. The laminate is not a moisture barrier at all — it absorbs water, and that absorption is one of the two mechanisms that destroy insulation in service.
The layer count and the positions are covered in PCB structural layers; what follows is what each of those layers has to prove.
Three Quantities That Are Not Interchangeable
Insulation is specified by three unrelated quantities, and a material can be excellent at one and mediocre at another. Mixing them up produces both false confidence and unnecessary cost.
| Quantity | Question it answers | Typical units | Governed by | Not related to |
|---|---|---|---|---|
| Dielectric strength | Can it survive a voltage surge without breaking down | kV/mm, or kV for a stated thickness | Resin system, voids, thickness, electrode geometry | Dk, Df, surface finish |
| Insulation resistance | How much current leaks through and across it, now and after ageing | MΩ, or Ω·cm for volume resistivity | Ionic cleanliness, moisture uptake, glass weave, hole spacing, bias voltage | Dielectric strength, which can stay high while leakage collapses |
| Dk and Df | What it does to a signal travelling through it | dimensionless, Df often ×10-3 | Resin chemistry, filler, glass content, frequency | Both of the above — a low-Df PTFE is a poor barrier against CAF if the hole spacing is tight |
A design that needs 3 kV of isolation and a design that needs 0.002 Df are almost never the same design. The 3 kV board is a clearance and cleanliness problem, and thick FR-4 with generous spacing solves it; the low-loss board is a material problem, and thin PTFE solves it while making the voltage problem worse. This is why automotive inverter boards and 77 GHz radar boards are built on different laminates even though both are called high-frequency.
Dielectric Strength Is Not a Material Constant
Datasheets quote dielectric strength as a single number in V/mil or kV/mm, which invites the assumption that breakdown voltage equals that number multiplied by thickness. It does not. Breakdown is a weakest-link process: the thicker the sample, the larger the volume of material that must be free of voids, contamination and partial discharge sites, so the apparent strength per millimetre falls as the sample gets thicker.
| Data as published | Value | Converted | What the sample was |
|---|---|---|---|
| TLY-5 (PTFE/woven glass) | 2,693 V/mil | ≈106 kV/mm | Thin film, 5 mil class |
| RT/duroid 4003C | 780 V/mil | ≈31 kV/mm | Standard laminate coupon |
| Generic FR-4, short-time | 500–1,000 V/mil | 20–40 kV/mm | Depends on thickness and test method |
Two laminates with similar dielectric chemistry appear to differ by a factor of three, and the difference is mostly the specimen, not the polymer. The consequence for specification writing is that dielectric strength must always be quoted with the thickness and the test standard; a bare V/mil figure cannot be multiplied by a 1.6 mm board thickness to predict a 48 kV withstand, because at that thickness the failure is initiated by a defect and by partial discharge in the void above it, not by the intrinsic strength of the resin.
There is a second reason the multiplication fails, and it is geometric. On a finished board the shortest path between two conductors at different potentials is rarely through the full thickness of the laminate. It is from an inner-layer copper edge to the board edge, or from a plated hole wall to a plane, and those distances are set by routing and by the artwork, not by the core thickness. A 1.6 mm board with 0.25 mm from the outermost inner layer to the profile edge insulates to 0.25 mm, not to 1.6 mm.
Practical design therefore works from clearance tables rather than from breakdown arithmetic: IEC 60664-1 for mains-referenced circuitry and IPC-2221B for the internal spacing rules, with the plating and hole geometry checked separately. What the material data gives is a sanity check that the resin system is in the right class, not a design number.
Insulation Resistance, and the Three Things That Eat It
Insulation resistance is the quantity that actually degrades in the field, and it degrades slowly, with moisture and voltage doing the work. A new board measures in the high megohms or beyond; the same board after 500 hours at 85 °C and 85 % RH under bias can be orders of magnitude lower. IPC-6012 puts the bare-board acceptance threshold at the 106 Ω level, measured at 500 V DC after conditioning, which is a floor rather than a target.
Conductive anodic filament. CAF is copper that has migrated along the glass-resin interface from an anode to a cathode, inside the laminate, under bias and moisture. It is the dominant long-term insulation failure of FR-4, and it is a spacing problem more than a material problem: the test in IPC-TM-650 method 2.6.25 runs 596 hours at 85/85 with 100 V bias and declares failure below 106 Ω. Hole-to-hole distance, the glass style, and whether the laminate cures with dicyandiamide all move the time to failure by large factors. A 0.3 mm hole pitch on a 1.6 mm thick board is a different reliability class from a 0.8 mm pitch on the same material.
Electrochemical migration. On the surface, between adjacent pads under a solder mask or a coating, the same electrochemistry produces dendritic growth. It needs three things at once: ionic contamination, moisture, and a bias. Remove any one and it stops, which is why cleaning is a functional requirement rather than a cosmetic one. J-STD-001 sets the cleanliness verdict at 1.56 µg/cm² of NaCl equivalent, and that number is the reason a no-clean process has to be qualified per flux rather than assumed.
Ionic contamination and moisture uptake. The laminate absorbs water — PTFE grades around 0.02 %, FR-4 substantially more — and the absorbed water carries whatever ions are dissolved in it. This is why a resistance measurement taken dry in an air-conditioned room proves very little: the conditioning step is the test, not the meter reading. It is also why the moisture sensitivity level and the bake before reflow matter to insulation and not only to popcorning.
One consequence deserves emphasis because it contradicts the intuitive fix: adding more insulation material does not restore resistance once the failure path exists. CAF grows along the interface that is already there. The repairs that work are geometric — more spacing, offset hole patterns, non-functional pads removed from the drill path — and process-based: better desmear, drier laminate, cleaner surface.
Dk and Df: The Insulation Is Also the Signal Path
Every signal on a board travels through insulation as well as along copper, so the same layer that isolates also sets propagation delay and a large share of the loss. Dk sets the delay: velocity falls as the square root of Dk, so a 4.4 laminate runs about 40 % slower than a 2.2 one on the same physical length. Df sets the attenuation, and it does so in a way that is easy to misapply.
For dielectrics the attenuation is closely approximated by αd ≈ 2.6 · fGHz · √Dk · Df in dB/in. What matters is that when two designs are compared at equal electrical length, the dielectric loss depends only on Df: the √Dk term exactly cancels the shorter physical length that a higher Dk buys. A high-Dk material saves area and does not save loss.
| Laminate | Dk (process) | Df | Dielectric loss at 10 GHz | Where it is the right answer |
|---|---|---|---|---|
| Standard FR-4 | 4.3–4.6 | 0.020 | 1.08 dB/in | Digital boards below about 1 GHz of edge rate |
| RO4350B | 3.48 | 0.0037 | 0.18 dB/in | FR-4-compatible process, mixed stacks, cost-sensitive RF |
| RO4003C | 3.38 | 0.0027 | 0.13 dB/in | Antenna and microwave layers needing tight Dk tolerance |
| RO3003 | 3.00 | 0.0010 | 0.045 dB/in | Low-loss PTFE, no glass, stable over temperature |
| RT/duroid 5880 / TLY-5 | 2.20 | 0.0009 | 0.035 dB/in | Millimetre-wave, where 0.1 dB/in is the whole budget |
The 31-fold spread between the first and last row is the reason material selection dominates high-frequency design. But the table also shows the limit of material selection: at 10 GHz on a 0.0027 laminate, the dielectric contributes about 0.13 dB/in while 1 oz copper with a realistic surface roughness contributes about 0.19 dB/in. Past a certain point the copper, not the insulation, is the loss. That balance is worked through in the stack-up arithmetic of high-frequency stack-up design.
Dk also has a temperature coefficient, and it is not small on PTFE: 5880 moves −125 ppm/°C while 4350B moves about +50 ppm/°C and 4003C about +40 ppm/°C. Over a 100 °C excursion that is roughly −1.25 % for the PTFE against +0.4 % for the hydrocarbon, which is a phase shift on a long line, not just a number on a datasheet. Design Dk and process Dk also differ — 3010 is specified at 10.2 as a process value and 11.20 as a design value — and mixing the two in an impedance calculation is a common source of a 5 % error before the board is even etched.
CTE: Matching Is Impossible, Managing Is Not
The original version of this article stated that the CTE of the insulation should match the other materials in the board. In the Z axis that is not achievable with any laminate, and the attempt to state it as a requirement hides the actual engineering, which is to keep the mismatch from accumulating into a via wall crack.
| Material | Z-axis CTE (ppm/°C) | X/Y CTE | Multiple of copper (17) | Consequence |
|---|---|---|---|---|
| Copper | 17 | 17 | 1× | Reference |
| FR-4 below Tg | 50–70 | 14–17 | 3–4× | Manageable with 8:1 aspect ratio limits |
| RO4350B | 32 | 10–12 | 1.9× | Close enough for conventional vias |
| RO4003C | 46 | 11–14 | 2.7× | Needs ductile plating on thick builds |
| RO3010 | 16 | 13 / 11 | 0.94× | Below copper in all three axes, which is why it survives thick stacks |
| RT/duroid 5880 | 237 | 31 / 48 | 13.9× | Aspect ratio capped near 6:1, elongation ≥20 % plating |
| TLY-5 | 217 | 26 / 15 | 12.8× | Same constraint; 1.6 mm over 215 °C expands about 75 µm |
The right-hand column is the whole design conversation. A 13.9× mismatch does not fail because the number is large; it fails when the expansion is restrained, and the restraint is the plated barrel. The three controls that actually work are symmetrical stack-ups (so the board does not bow and concentrate strain at one via), a capped aspect ratio so the barrel can flex over a shorter span, and plating with at least 20 % elongation so the copper stretches instead of fracturing. The through-hole geometry that carries this load is dealt with in PCB through holes.
Above Tg the Z-axis CTE of FR-4 roughly triples, which is why Tg is a specification that matters to reliability and not only to reflow survival. The temperature at which the expansion rate breaks is the temperature at which the via sees its worst strain, and a lead-free profile crosses it. That is the argument in PCB glass transition temperature, and it is the reason a 0.2 mm thicker board can be more reliable than a thinner one at the same Tg.
Heat: The Insulation Is a Resistor, Not a Sink
The original article credited the insulation layer with helping to dissipate heat. The sign of that statement is wrong. Laminate is a thermal insulator by design — if it conducted heat as well as copper there would be no point in copper planes — and it sits directly in the path between a hot component and any heatsink below it.
| Material | Thermal conductivity (W/m·K) | Thermal resistance, 0.254 mm | Rise at 10 W/cm² |
|---|---|---|---|
| Copper | 400 | 0.006 K·cm²/W | 0.06 K |
| RO3010 | 0.95 | 2.67 | 27 K |
| RO4003C | 0.71 | 3.58 | 36 K |
| RO4350B | 0.69 | 3.68 | 37 K |
| FR-4 | 0.30 | 8.47 | 85 K |
| RT/duroid 5880 | 0.20 | 12.70 | 127 K |
The table is deliberately built at 10 W/cm² because that is an ordinary power density under a small surface-mount device, and the numbers are the temperature difference across the dielectric alone — before any spreading, convection or heatsink is considered. Under a 0.254 mm PTFE layer, 10 W/cm² produces a 127 K rise through the laminate; the same heat flux through copper is 0.06 K. The ratio is about 1,300.
Three design responses follow, and none of them is “use the insulation to spread heat”. Thermal vias carry the heat through the dielectric to a plane, and their effectiveness is dominated by the copper barrel, not by the laminate. A thermally conductive laminate helps when vias are impossible — 6035HTC at 1.44 W/m·K turns that 127 K into about 18 K — and costs more than a via array in most cases. And spreading in the plane is done by copper area, which is why the copper thickness decision in PCB copper thickness is a thermal decision as much as an electrical one.
Thinner Is Not Better: What HDI Buys and Pays
In a high-density build the dielectric between layers is thinned to 60–80 µm so that microvias can be laser drilled at 75–100 µm diameter and stacked. That decision is usually discussed as a routing-density choice. It is equally an insulation choice, and the costs land on the same three quantities.
Breakdown margin. At 60 µm the voltage across the layer for a given field is 4 times what it is at 0.25 mm. For a 3.3 V digital layer that is irrelevant; for any layer that also carries a 48 V rail or an isolated gate drive, it is the binding constraint. This is why HDI boards that mix high voltage and fine pitch usually keep the high-voltage nets on the thick core and use the build-up layers only for signal.
Impedance sensitivity. A 60 µm dielectric with ±10 % thickness tolerance moves a 50 Ω line by about ±6 % before etch variation is counted, and the width needed for 50 Ω on a 3.4 Dk build-up film falls to the region where ±25 µm of etch is a large fraction of the width. The tolerance budget is genuinely tighter, not merely harder to hold.
Loss. Build-up films are Df 0.015–0.025, which is an order of magnitude worse than a microwave laminate. A 60 µm build-up layer contributes little absolute loss because it is short in wavelength terms, but a microvia that changes layer through two build-up films adds reflections that the dielectric data does not predict. What the thin layers do buy is the ability to route the signal at all; the electrical penalty is real but usually accepted before the material is chosen. The process side of this trade is set out in HDI production process, and the performance side in HDI PCB performance.
One practical rule follows. When a stack-up is converted from 0.1 mm cores to 60 µm build-up, the impedance target should be re-derived rather than copied, and the high-voltage nets should be checked against the new spacing on the same drawing. Both are arithmetic, and both are routinely skipped because the layer count did not change.
Solder Mask Is Not an Insulation Guarantee
Solder mask is often treated as the surface insulation, and electrically it is a thin film doing a large job. At 15–25 µm thick it is two orders of magnitude thinner than the core it sits on, it is applied over a surface that may still carry ionic residue, and its coverage at pad edges and around vias is limited by the imaging process.
Its dielectric effect is measurable and usually ignored. With Dk in the range 3.5–4.2, a coating over a microstrip lowers the impedance by roughly 1–3 Ω depending on the line width and the mask thickness, and a white mask with a high titanium dioxide loading is worse because its Dk reaches about 6.5. This is the reason impedance coupons must be measured with the same mask as the product, and the reason a bare coupon reads 1–3 % higher than the finished board.
Its insulation effect is limited by coverage rather than by material strength. A 20 µm mask with a pinhole is a 0 µm mask at that point, and the failure then proceeds by dendritic growth across the gap under bias and humidity — the mechanism described in section four. Meanwhile a mask that is properly cured and complete can legitimately be used to gain a pollution degree in the creepage calculation, which is worth more than its thickness suggests. The distinction matters: the mask is a manufacturable barrier whose value depends on the process, not a material property to be read from a datasheet.
Surface preparation under the mask is therefore part of the insulation specification. A finish applied over contaminated copper, or a mask cured with trapped solvent, fails in the field in ways that pass every incoming inspection. The finishes themselves and their process windows are in PCB surface treatment processes.
Creepage and Clearance at Mains Voltage
Once a board carries mains-referenced voltage, the insulation question stops being about material and becomes about distance. Two distances are involved: clearance, the shortest path through air, and creepage, the shortest path across the surface. Both are read from tables keyed to the working voltage, the pollution degree and the material group — and the table is keyed to the peak voltage, not the RMS value.
The peak-versus-RMS distinction is where designs most often fail. A 230 V AC supply has a peak of 325 V, so it falls in the next band of the IPC-2221B table rather than the one the nominal number suggests. In that table the external uncoated spacing steps from 0.1 mm at 30 V to 0.6 mm at 31 V, and reaches 2.5 mm by 500 V — a 25-fold jump across a voltage range that a designer might think of as “low voltage”. Internal layers are allowed less than external uncoated surfaces, which is why a mains isolation barrier is usually placed on an inner layer or made an explicit slot.
Three practical controls follow. Conformal coating can gain one pollution degree, which reduces the required creepage, but only if the coverage is complete and stays complete over thermal cycling. A routed slot is a legitimate way to break a creepage path because it converts surface distance into air clearance. And the board profile matters: 0.25 mm from the outermost inner-layer copper to the routed edge is a common fabrication limit that becomes the controlling insulation distance on a high-voltage board, regardless of how thick the laminate is.
A Selection Matrix
Combining the three quantities with the four materials gives a matrix that is short enough to use. Each row states which property is binding, because that is the one that must be specified and inspected.
| Application | Binding property | Right material class | What to specify |
|---|---|---|---|
| Mains-referenced power supply | Clearance and creepage | FR-4, Tg 150 °C or above, thick core | Spacing per IPC-2221B at peak voltage; CTI class; slot positions |
| Automotive inverter / 800 V bus | Partial discharge and CAF | High-Tg FR-4 or hydrocarbon, thick dielectric | Hole-to-hole spacing; CAF test; ionic cleanliness |
| Millimetre-wave front end | Df and Dk tolerance | PTFE/woven glass (TLY-5, 5880) or 3003 | Df at operating frequency; Dk tolerance ±0.04; design versus process Dk |
| Microwave antenna, cost-sensitive | Dk stability | 4003C or 4350B | Dk tolerance; TCDk; Df at 10 GHz |
| Fine-pitch HDI logic | Density, not voltage | Build-up film on thin core | Layer thickness tolerance; microvia AR; adhesion |
| High-impedance sensor input | Surface leakage | FR-4 with thorough cleaning, guard ring | Ionic cleanliness; mask coverage; coating type |
The matrix has one useful property: no two rows ask the same laminate to do the same job. Where a product needs two rows at once, the answer is a mixed stack rather than a compromise material — PTFE on the antenna layers, FR-4 or hydrocarbon for the digital and power layers, bonded in separate press cycles, because the three press systems cannot be combined in one cycle.
What to Test, and What Each Test Proves
Four tests cover the three quantities, and each one proves something narrower than its name suggests.
Insulation resistance, at 500 V DC after humidity conditioning, against the 106 Ω class threshold. Performed dry, it proves the board is not shorted; performed after conditioning, it proves the material and the cleaning are adequate. The conditioning is the test.
Dielectric withstand (hi-pot), at a specified AC or DC voltage for a specified time. It proves there is no gross defect in the dielectric at that voltage and thickness — and nothing about long-term ageing. Repeated hi-pot on finished assemblies is also a stress, so the test voltage and the number of applications belong in the drawing rather than in a shop-floor habit.
CAF testing to IPC-TM-650 2.6.25, on a dedicated coupon with the production hole pitch. It proves the laminate, the glass style, the drilling and the desmear are a combination that survives 596 hours of bias and humidity. It is a qualification test, not a lot acceptance test, and its value is entirely in using the real hole spacing.
Ionic cleanliness, by resistivity of solvent extract, against 1.56 µg/cm² NaCl equivalent. It proves the surface is clean enough that migration needs a defect rather than a residue, and it is the cheapest of the four to run per lot.
The acceptance documents tie these together: IPC-6012 for rigid boards, IPC-6016 for HDI, IPC-A-600G for visual criteria, and the coupon design that makes the measurements meaningful. A drawing that names the standard without naming the coupon geometry leaves the fabricator to choose what to measure, which is how a board passes inspection and fails in the field.
Eight Statements About Insulation That Do Not Survive Measurement
Each of these appears in supplier copy, and each is wrong in a way that changes a decision.
| Statement | What is actually true |
|---|---|
| The insulation layer helps dissipate heat | It is a thermal resistance in the path. FR-4 conducts 0.30 W/m·K against copper’s 400; 0.254 mm of it adds 85 K at 10 W/cm². Heat is moved by copper and vias |
| Its CTE should match the other materials | Unachievable in Z. 5880 is 237 ppm/°C against copper’s 17. The controls are symmetry, aspect ratio and ductile plating |
| A higher Dk means better insulation | Dk describes storage of field, not resistance to breakdown. A high-Dk material can be a poor barrier and a good capacitor at the same time |
| Dielectric strength × thickness = withstand voltage | Breakdown is weakest-link; thick samples show lower strength per millimetre, and the real path is often to a board edge, not through the core |
| The solder mask insulates the surface | A 15–25 µm film with a pinhole is no film at that point. Coverage and cleanliness decide, not material grade |
| Insulation resistance is a fixed material property | It is a system property that falls with moisture, ions and bias. Measured without conditioning it says almost nothing |
| Spacing can be calculated from RMS voltage | Tables are keyed to peak. 230 V AC is 325 V peak and lands one band higher than the nominal number implies |
| Thinner dielectric is always better for density | It also cuts breakdown margin, tightens the impedance tolerance to ±6 % from thickness alone, and shortens the CAF path |
Conclusion
Insulation in a PCB is four materials and three numbers, and the useful engineering begins when they are kept apart. The core and the prepreg carry the voltage and set the loss; the solder mask and the coating govern surface leakage and are only as good as their coverage. Dielectric strength is a thickness-dependent, weakest-link property that cannot be extrapolated; insulation resistance is a system property that falls under moisture and bias, through CAF inside the laminate and dendritic growth on its surface; and Dk and Df decide what the signal pays, with the loss per unit electrical length fixed by Df alone.
The two statements worth correcting from the common description are the ones with the largest design consequences. Insulation does not help dissipate heat — it is the thermal resistance that thermal vias exist to bypass, and 0.254 mm of PTFE adds 127 K at 10 W/cm². And its CTE cannot be matched to copper; on a 5880 build the mismatch is 13.9×, managed by symmetric stacks, a 6:1 aspect ratio limit and plating with at least 20 % elongation.
XCE PCB builds to those constraints on both conventional and high-frequency stacks: 2 to 72 layers, panels to 600×1200 mm, impedance held to ±10 %, samples in as fast as 24 hours, inspected to IPC-A-600G and IPC-6015, with CAF coupons drilled at the production hole pitch rather than at a convenient one. The copper that does the actual heat spreading is described in copper thickness, and the bonding step that sets the cured dielectric thickness in lamination.
Frequently Asked Questions
What does the insulation actually do in a PCB?
Is a thicker dielectric always better for voltage?
Why does insulation resistance drop after humidity exposure?
Can solder mask be used as insulation for mains voltage?
What Dk and Df should the insulation have for high frequency?
How can you prove the insulation is good?
Need the Dielectric Checked Layer by Layer?
Send us your Gerber files and requirements for a manufacturability review and a tailored quotation.
sales1@xcepcb.com
+86 180 3341 4657