Concept renderMost wearables and trackers start on FR-4. Pick a mid or high Tg grade for lead-free assembly, use polyimide flex where the circuit must bend, and use rigid-flex when a fold can replace connectors. A low-loss RF laminate pays off mainly for long RF lines or high frequencies. Confirm every value on the laminate datasheet.
PCB material sets how hot a board can get in assembly, how much RF signal it loses, and whether it can bend. This guide compares datasheet values and ties each choice to a device type: a tracker, a band, a ring or a voice badge. It contains no Duobay price and no test result.
Values come from the maker pages and guides listed under Sources, accessed November 5, 2026. Laminate data sheets are revised, so confirm each value on the current version before it goes in a fab note.
What PCB material types are there, and what is each one for?
Five families cover nearly every small connected device. FR-4 is the default. The others solve a specific problem: heat, bending, folding or RF loss.
| Material | What it is | Where it fits in a wearable or tracker |
|---|---|---|
| FR-4, mid Tg | Glass-reinforced epoxy laminate. The IS400 page calls it a lead-free, mid Tg epoxy laminate with a Tg of 150 °C. | The main board of most trackers, docks and chargers, and the rigid parts of many wearables. |
| FR-4, higher Tg | The same family with a resin that softens later. 370HR lists a Tg of 180 °C. | Thicker or denser boards, more reflow cycles, or a hotter use case. Check the datasheet rows for delamination time and Z-axis expansion. |
| Polyimide flex | Copper on a polyimide film. Pyralux AP is described as an adhesiveless, all-polyimide double-sided copper-clad laminate. | Bands, rings, hinges, sensor tails and battery tails, where the circuit has to bend to fit or move. |
| Rigid-flex | Rigid board sections and flex layers built as one board. The Pyralux AP page lists rigid-flex constructions among its uses. | A device that folds two or three boards into a small shell and would otherwise need board-to-board connectors. |
| Hydrocarbon ceramic RF laminate | A low-loss rigid laminate. Rogers says RO4000 materials can be fabricated using standard epoxy/glass (FR-4) processes. | Long RF lines, filters or antennas at higher frequencies, often only on the outer layers of a mixed stack-up. |
Sources: Isola IS400, Isola 370HR, Pyralux AP, Rogers RO4000 data sheet, as of November 2026.
Ceramic and metal-core boards also exist. This guide leaves them out, since none of the sources above covers them.
Which FR-4 PCB grade do you need?
"FR-4" on a drawing does not define a material. Two FR-4 laminates from the same maker can differ in Tg, heat resistance and RF loss. The table puts a mid Tg grade and a higher Tg grade side by side, using the values each product page lists as of November 2026.
| Property | Isola IS400 | Isola 370HR | Why it matters |
|---|---|---|---|
| Glass transition (Tg), by DSC | 150 °C | 180 °C | The temperature where the resin turns soft. A higher figure gives more margin in lead-free reflow and in hot use. |
| Time to delaminate at 260 °C (T260) | More than 60 minutes | 60 minutes | Shows how the board holds up under heat. Compare only with the same test method. |
| Time to delaminate at 288 °C (T288) | More than 10 minutes | 30 minutes | Same as above at a higher temperature. This row separates the two grades more than T260 does. |
| Z-axis expansion, 50 to 260 °C | 3.3% | 2.8% | Lower expansion through the thickness puts less strain on plated holes and vias during reflow. |
| Dk and Df, summary table | Dk 3.90, Df 0.022 at 500 MHz | Dk 4.04, Df 0.0210 at 2 GHz | The IS400 summary stops at 500 MHz. Its core data tables list values up to 10 GHz for each construction, and they vary with resin content, so read the row for your core. |
| IPC-4101 slash sheets listed | /97, /98, /99, /101 | /98, /99, /101, /126 | The slash sheet is how a fab note can allow an equivalent material from another maker. |
Sources: IS400 product page and 370HR product page, test methods as listed there, as of November 2026.
What Tg actually tells you
Tg is the point where the epoxy changes from glassy to soft. Above it, the board expands much faster through its thickness. The 370HR page shows this: 45 ppm/°C below Tg and 230 ppm/°C above it. That expansion pulls on plated holes, so a board that sees several reflow passes, or a thick multilayer stack, benefits from a higher Tg and lower total expansion.
Tg alone does not rank materials. Read T260, T288 and Z-axis expansion with it, and compare values only when the test method matches, as it does on the two pages above.
How to call out FR-4 in a fab note
Both pages list IPC-4101 slash sheets. IPC-4101 is the specification for base materials for rigid and multilayer boards. IPC's preview of revision F is dated February 2026, and its purpose section says it is to be used for procurement and quality assurance activities (IPC-4101F preview, as of November 2026). The full standard is paywalled, so we quote no slash sheet requirements. A fab note can name a laminate and allow an equal material by slash sheet, which gives the fab room to source and gives you a defined floor.
When does a flex PCB make sense, and how do you design one?
A flex PCB earns its place when the circuit must follow a curve, fold into a shell, or move with a hinge. Bands, rings and sensor tails are typical. The base is usually polyimide film. Pyralux AP, one polyimide laminate for flex and rigid-flex, lists dielectric thicknesses from 25 µm to 150 µm and copper of 18 µm or 25 µm, with a Dk of 3.2 at 10 GHz (product page, as of November 2026).
IPC-2223 is the sectional design standard for flexible and rigid-flex printed boards, to be used together with IPC-2221. IPC's preview of revision F is dated May 2026 (IPC-2223F preview, as of November 2026). The full standard is paywalled, so the rules below come from a fabricator's public flex design guide, as of November 2026. Treat them as starting points to confirm with your own fab.
Flex design rules from a fabricator guide
| Rule | Guide value | Why it matters |
|---|---|---|
| Bend radius, single-sided | Flex thickness x 6 | A tighter radius risks cracked copper or coverlay that lifts. |
| Bend radius, double-sided | Flex thickness x 12 | Two copper layers make the flex stiffer, so it needs a wider bend. |
| Bend radius, multilayer | Flex thickness x 24 | Each extra layer adds stress in the bend. |
| Bend radius, dynamic flexing | 100 x the finished thickness | The guide treats a board that flexes fewer than 100 times in its life as static. A hinge or a band that bends daily is dynamic. |
| Copper type | Rolled annealed copper on polyimide cores | Thinner copper also bends more easily. |
| Traces in the bend | Perpendicular to the bend line, with rounded corners, staggered between layers | Stacked traces on two layers stiffen the bend and raise stress. |
| Holes and parts near the bend | No plated holes or components in the bend area. No vias in the flex section of a dynamic board. | Plated barrels and solder joints crack when the copper around them bends. |
| Parts on flex | Add a stiffener where components sit on a flex section. | The stiffener keeps solder joints from flexing. |
| Rigid-flex transition | Leave enough space between the rigid-flex transition and the bend point. The guide gives no number. | The joint between rigid and flex is the weak spot. |
Source: Sierra Circuits, flex PCB design guidelines, as of November 2026.
The dynamic rule matters most for wearables. A band that opens and closes on the wrist every day bends many more than 100 times in its life. If the radius the shell allows is smaller than the guide value, change the shell, thin the flex stack-up, or move the bend to a part with no copper crossing it.
When rigid-flex replaces flex plus connectors
Rigid-flex builds the flex layers into the rigid boards, so there is no connector at each end. That saves height and removes contacts that can loosen in a drop. The cost is a more complex build. Each fab has its own rigid-flex limits, and a design change usually means a new panel. A common middle path for a first prototype is two rigid FR-4 boards joined by a separate flex jumper. Move to rigid-flex once the fold and the shell are stable.
Do you need a high-frequency laminate for Bluetooth, Wi-Fi or LTE?
Often not. FR-4 loses more signal per inch than an RF laminate, but on a small device the RF path from radio to antenna is short. The table compares a high Tg FR-4 with a common hydrocarbon ceramic RF laminate, as of November 2026.
| Property | Isola 370HR (FR-4) | Rogers RO4350B |
|---|---|---|
| Dielectric constant (Dk) | 4.04 at 2 GHz; 3.92 at 10 GHz | 3.48 ± 0.05 at 10 GHz (process); 3.66 for design, 8 to 40 GHz |
| Dissipation factor (Df) | 0.0210 at 2 GHz; 0.0250 at 10 GHz | 0.0031 at 2.5 GHz; 0.0037 at 10 GHz |
| Tg | 180 °C by DSC | More than 280 °C by TMA |
| Processing | Standard FR-4 process. | The datasheet says it can be fabricated using standard FR-4 circuit board processing techniques, without the sodium etch that PTFE materials need. |
Sources: 370HR product page and Rogers RO4000 data sheet, as of November 2026. The test methods differ between the two makers, so treat the comparison as a rough guide.
Near 2.4 GHz, the RF laminate's dissipation factor is several times lower. That matters for long lines, filters and PCB antennas. For a short 50 ohm feed from a module to a chip antenna, the extra loss on FR-4 is often small enough to accept. Run your own numbers with the trace length you actually have.
Two vendor notes point the same way. TI's AN043 for a small 2.4 GHz PCB antenna recommends using the same thickness and type of PCB material as the reference design, and says a thicker or thinner board can be compensated by making the antenna slightly shorter or longer (AN043, as of November 2026). Espressif's ESP32-S3 layout guide recommends a four-layer board, points to its stack-up for a 50 ohm RF trace, and says PCB antennas should be validated by simulation and by real-world tests on a development board (layout guide, as of November 2026). The material and thickness are part of the antenna design, so changing them means retuning. For tracker antennas, see GNSS antenna placement in small trackers.
How do you choose a PCB material for a wearable or tracker?
Start from the device form and the radios, then check the few rows of the datasheet that matter for that case. The table gives starting points. They are engineering reasoning from the sources above, and none reports a result for any product.
| Device situation | Starting material | Check before you commit |
|---|---|---|
| BLE or Wi-Fi tracker, one rigid board, module with its own antenna | Mid or high Tg FR-4, the stack-up from the module maker reference design | Follow the module layout guide for keepout and 50 ohm feed. Keep the board thickness the reference design used. |
| LTE-M or Cat-1bis tracker with GNSS | High Tg FR-4, multilayer | Antenna feed lengths, ground plane size, and whether a short feed on FR-4 is good enough before you pay for an RF laminate. |
| Band or bracelet that curves around the wrist | Rigid FR-4 islands joined by polyimide flex, or rigid-flex | Is the bend static after assembly or dynamic in daily wear? Set the bend radius from the flex thickness and layer count. |
| Ring or very small wearable | Thin rigid-flex or a flex circuit with stiffeners under parts | Panel yield at the fab, assembly fixtures for a curved part, and the bend radius the shell actually allows. |
| Clip, pendant or badge that folds two boards together | Rigid-flex, or two FR-4 boards with a flex jumper | Count the connectors rigid-flex removes. Compare that with the cost and lead time of a rigid-flex prototype. |
| Long RF trace, filter or PCB antenna above a few GHz | Low-loss RF laminate on the RF layers, FR-4 for the rest | Ask the fab whether it runs a mixed stack-up. The Rogers data sheet lists a separate design Dk, so record which value the impedance model used. |
Two habits save rework. Lock the stack-up with the fab before layout starts, since impedance and antenna tuning depend on it. Build the first prototypes from the material the production fab will use, because a board tuned on one laminate may detune on another.
What should you ask your hardware team about PCB material?
Take this list to your electrical lead and to any fab that quotes the board.
- Which laminate and which IPC-4101 slash sheet does the fab note call out, and are equivalents allowed?
- What Tg does the board need, and how many reflow passes will it see, including rework?
- Does the stack-up match the module or chip reference design, including board thickness?
- Which Dk value did the impedance and antenna design use, and at what frequency?
- Where does the board bend, and is that bend static or dynamic?
- What bend radius does the flex stack-up allow, and does the enclosure respect it?
- Are there vias, plated holes or parts within the bend area?
- Would rigid-flex remove connectors, and what does that change in prototype lead time?
Material decisions sit inside the electronics work at the PCB prototype stage. For how that work is organized, see engineering.
Questions about PCB material
What is the most common PCB material?
Is a flex PCB more reliable than FR-4 with connectors?
It depends on the bend. A flex circuit removes connectors, but it can crack if the bend is too tight or if it flexes often. One fabricator guide sets dynamic bends at 100 times the finished thickness (flex design guidelines, as of November 2026). Test the real bend on samples.
Do I need a Rogers or other RF laminate for Bluetooth?
Often not. A 2.4 GHz design on FR-4 can work when it follows the chip or module reference layout. TI advises using the same thickness and type of PCB material as its antenna reference design (AN043, as of November 2026). Consider an RF laminate when RF lines are long or the frequency is high.
Which IPC standards cover PCB materials?
IPC-4101 covers base materials for rigid and multilayer boards. IPC's preview of revision F is dated February 2026 (IPC-4101F preview, as of November 2026). IPC-2223 is the sectional design standard for flexible and rigid-flex boards, and IPC's preview of its revision F is dated May 2026 (IPC-2223F preview, as of November 2026). Both are paywalled, so we name them and quote no thresholds.
How can Duobay help choose a PCB material?
Our Shenzhen engineering team includes electrical and mechanical engineers, so the board stack-up and the enclosure are reviewed together. Gate 0 Feasibility is a paid, fixed-fee study where questions like these get worked through before a prototype board is ordered. We do not publish prices. Tell us about your device.
If you want help picking a stack-up for a wearable or tracker, tell us about your device.
Sources
All pages accessed November 5, 2026. Data sheets and standards are revised, so confirm the current version before you decide.
- Isola, IS400 laminate and prepreg: https://www.isola-group.com/pcb-laminates-prepreg/is400/ (accessed 2026-11-05)
- Isola, 370HR laminate and prepreg: https://www.isola-group.com/pcb-laminates-prepreg/370hr/ (accessed 2026-11-05)
- Rogers Corporation, RO4000 series data sheet (RO4003C and RO4350B): https://www.rogerscorp.com/-/media/project/rogerscorp/documents/advanced-electronics-solutions/english/data-sheets/ro4000-laminates-ro4003c-and-ro4350b---data-sheet.pdf (accessed 2026-11-05)
- Pyralux AP product page: https://www.qnityelectronics.com/pyralux-ap.html (accessed 2026-11-05)
- Sierra Circuits, flex PCB design guidelines: https://www.protoexpress.com/blog/flex-pcb-design-guidelines/ (accessed 2026-11-05)
- Texas Instruments, AN043 Small Size 2.4 GHz PCB Antenna (SWRA117D): https://www.ti.com/lit/an/swra117d/swra117d.pdf (accessed 2026-11-05)
- Espressif, ESP32-S3 hardware design guidelines, PCB layout design: https://docs.espressif.com/projects/esp-hardware-design-guidelines/en/latest/esp32s3/pcb-layout-design.html (accessed 2026-11-05)
- IPC (Global Electronics Association), IPC-4101F preview with cover, contents and scope: https://www.electronics.org/TOC/IPC-4101F-toc.pdf (accessed 2026-11-05)
- IPC (Global Electronics Association), IPC-2223F preview with cover, contents and scope: https://www.electronics.org/TOC/IPC-2223F-toc.pdf (accessed 2026-11-05)
Planning a device like this? Tell us what it needs to do. A Duobay engineer replies within 1 business day. Send a project brief →