A PCB antenna is a copper trace or pattern etched directly onto a printed circuit board that transmits and receives radio frequency electromagnetic waves. It is the cheapest way to give a product wireless connectivity, because it adds no connector, no cable and no bill-of-materials line.
It is also the part of a design most likely to fail for reasons that have nothing to do with antenna theory. In our experience reviewing returned boards, the overwhelming majority of PCB antenna problems are layout problems: copper where there should be none, a ground plane that grew during routing, or a design with no margin left to absorb normal fabrication variation.
This guide covers what actually determines whether a PCB antenna works: the keep-out zone, the substrate, the matching network, and the tolerances the fabrication process is allowed to miss. It is written for the engineer who has been handed a radio module and needs the antenna to work on a specific board.
Key Takeaways – The single highest-leverage rule is a copper-free zone on every layer beneath and around the radiator. Most PCB antenna failures trace back to this one rule being broken, usually by an inner-layer ground pour that is invisible on the outer-layer view most layout engineers work from. – Clearance requirements scale with wavelength. A 433 MHz antenna needs dramatically more board area than a 2.4 GHz one, and this is the constraint most often discovered after the board is routed. – The substrate sets the antenna’s physical size through its dielectric constant and sets how much power is lost as heat through its dissipation factor. FR-4 is genuinely adequate at 2.4 GHz. – Solder mask measurably detunes a PCB antenna. A peer-reviewed measurement at 433 MHz found that removing the mask shifted resonance up by 3.5%, and improved peak gain by 1.2 dB. – Design bandwidth is the budget that absorbs fabrication tolerance. A narrowband design has almost no margin; a wideband 2.4 GHz design absorbs the same variation without noticing.
What Is a PCB Antenna?
A PCB antenna is a conductive copper trace or pattern etched onto a printed circuit board that converts high-frequency current into radiated electromagnetic waves, and converts intercepted electromagnetic waves back into high-frequency current on receive. The board itself is part of the radiating structure.
That last point is what separates a PCB antenna from every other antenna choice. When you buy a chip antenna or an external whip, the radiating element arrives characterised and tested. When you etch a trace, you take responsibility for the geometry and for everything near it. You control the radiator, and you also control every piece of copper, metal and plastic that will detune it.
Three practical consequences follow:
- There is nothing to break off. No connector, no cable, no assembly step. For a product that will be dropped, this matters.
- The cost is board area and layout discipline. You are trading real estate and design attention for a lower unit cost.
- Performance is set by your layout, not by a datasheet. The same trace on two different boards is two different antennas.
The trade is usually worth making. A PCB antenna is the default choice for any connected device where the board has room and the design team is willing to treat the antenna area as protected space rather than as routable area.
PCB antenna vs chip antenna vs external antenna
| Option | Footprint | Relative cost | What you take on |
|---|---|---|---|
| Trace antenna | Largest | Lowest | Layout discipline and tuning time |
| Chip antenna | Small | Low | Little tuning risk, slightly lower efficiency |
| External / FPC antenna | Largest total | Highest | Connector, cable and an assembly step |
Section 9 develops this into a full decision matrix.
PCB Antenna Types and When to Use Each
Five antenna geometries cover almost every PCB antenna application, and the choice is driven by how much board area you can give up rather than by which shape looks best in a reference design.
| Type | Governing dimension | Typical 2.4 GHz footprint | Pattern | Best for |
|---|---|---|---|---|
| Monopole | Quarter-wave over ground | ~23 mm trace (Nordic) | Omnidirectional | Simplest integration, widest bandwidth |
| Meandered inverted-F (MIFA) | Quarter-wave, folded | 7.2 x 11.1 mm | Omnidirectional | Compact connected devices, the workhorse |
| Patch | Half-wave | Large | Directional, high gain | GPS, point-to-point |
| Dipole | Half-wave, two arms | Medium | Balanced omnidirectional | Wi-Fi and LoRa modules |
| Loop / NFC | Inductive | Varies | Near-field | RFID and NFC |
The trade-offs in one line each:
- Monopole. The easiest to tune and the most forgiving, because it has the widest bandwidth. Costs the most length.
- MIFA. Folds electrical length into a small footprint. Costs bandwidth and efficiency for that size saving, which makes it less tolerant of fabrication variation.
- Patch. Buys gain and directionality. Needs a solid ground plane directly beneath and a lot of area.
- Dipole. Balanced and less dependent on the ground plane, but needs a clear keep-out around both arms and symmetric routing.
- Loop and NFC. A different design model entirely. Do not apply a GHz patch model to a near-field inductive loop.
The MIFA dimensions above come from Infineon’s antenna design and RF layout guidelines, which specify a 7.2 mm x 11.1 mm antenna with a 20 mil trace width for 2.4 GHz human-interface applications (Infineon AN91445, document 001-91445).
How a PCB Antenna Radiates
An antenna radiates when its physical length is a specific fraction of the signal’s wavelength, and everything on the board near that conductor changes the effective length.
At 2.45 GHz, the free-space wavelength is 122.4 mm, so a quarter-wave is 30.6 mm. That is the textbook figure. What it does not tell you is how long a real printed trace should be, because the relationship between a formula and a board is weaker than most guides suggest.
Consider the other bound people quote. Dividing the free-space quarter-wave by the square root of the substrate dielectric constant gives 30.6 / √4.3 = 14.8 mm. Neither number describes a working antenna:
- √Dk is the wrong divisor for a trace antenna. The velocity factor for a microstrip line depends on the effective dielectric constant, not the bulk value, and for a trace over FR-4 that effective value lands nearer 3.0 to 3.3 than 4.3.
- A quarter-wave monopole over a ground plane is close to the free-space length, not the substrate length. The ground plane acts as an image plane, and end loading plus finite ground plane size then shorten the trace somewhat.
Nordic Semiconductor’s published design guideline resolves this with a real number: a printed quarter-wave monopole at 2.4 GHz measures about 23 mm long, requiring a minimum 5 mm clearance to the ground plane (Nordic Semiconductor, General PCB design guidelines). That is neither 14.8 mm nor 30.6 mm, and it is 55% longer than the substrate calculation.
The practical lesson: treat the wavelength arithmetic as a sanity check on order of magnitude, and treat a vendor reference design as the actual starting point. Then measure.
One more piece of physics matters for everything that follows. The antenna is a transducer between roughly 50 ohms at the radio and 377 ohms of free space. Every element between those two points, the feed line, the matching network, the substrate, is loss. This is why nearby copper is not a minor concern: metal couples to the radiator, loads it capacitively, and shifts its resonance.
PCB Antenna Layout Rules: Keep-Out, Ground Plane and Placement
The layout rule that decides whether a PCB antenna works is a copper-free zone on every layer beneath and around the radiator, and its size scales with the wavelength you are transmitting on.
Here is what vendor documentation actually specifies, and it is less than you might expect.
| Figure | Source | What it actually measures |
|---|---|---|
| ~23 mm trace length, minimum 5 mm clearance to ground plane | Nordic Semiconductor | Clearance from antenna trace to ground plane edge, at 2.4 GHz |
| L4 shortened to 19.0 mm to move 433-510 MHz to 868-930 MHz | Texas Instruments SWRA730 | Trace length versus operating band, on a 43 x 25 mm antenna |
| Antenna area cannot be used for other routing | Texas Instruments SWRA730 | Qualitative prohibition, single-sided layout |
| ~70 mil keep-out around the RF matching circuit | Silicon Labs AN928.2 | Matching network keep-out, not antenna keep-out |
No silicon or module vendor publishes a per-band keep-out table in millimetres. Every vendor expresses clearance either qualitatively, relative to a specific antenna part’s footprint drawing, or as a single clearance figure at one frequency. If you have seen a table giving a specific millimetre range for each band, it almost certainly traces back to fabrication blogs that attribute it to no vendor document. Treat any such table as unattributed industry rule of thumb, not as guidance.
What the documentation is unambiguous about:
- No copper pour, plane or trace on any layer beneath the radiator. Nordic requires solid unbroken ground under the RF path from the chip pad to the antenna feed, and separately requires an inner-layer keep-out under the matching circuitry. Texas Instruments states that the area underneath the antenna cannot be used for any other routing.
- Clearance scales with wavelength. This follows directly from the physics: a 433 MHz quarter-wave is roughly 173 mm in free space against 30.6 mm at 2.45 GHz. The board area a sub-GHz antenna needs is therefore several times larger, and this is the constraint most often discovered after routing is complete.
- Antenna at a board edge or overhanging the substrate, where the radiator has clear space on at least one side.
- No metal inside the keep-out. Mounting hardware, battery contacts, shield cans and connector shells all reflect radiated energy back into the antenna.
- Freeze the mechanical layout before tuning. Moving an enclosure, a battery or a mounting boss after tuning invalidates the tuning.
Why copper under the antenna detunes it
Any copper beneath or beside the radiator couples to it electromagnetically. The coupling adds parasitic capacitance, which loads the antenna and pulls its resonant frequency down while spoiling the impedance match. This is the mechanism, and it is why the rule is absolute rather than a guideline: a ground pour that looks harmless on the top layer is a capacitor plate on layer three.
The specific risk is that inner-layer pours are invisible on the outer-layer view most layout engineers work in. The fix is to check the keep-out on every layer, not just the one you are drawing on.
PCB Antenna Materials and Stackup
The substrate sets the antenna’s physical size through its dielectric constant and sets how much power is lost as heat through its dissipation factor. FR-4 is genuinely adequate at 2.4 GHz.
Two numbers govern the choice, and they do different jobs. Dk sets size: a higher dielectric constant means a shorter antenna for the same frequency. Df sets loss: a higher loss tangent converts more of your transmit power into heat in the dielectric instead of radiated signal.
| Material | Process Dk | Design Dk | Df @ 10 GHz | Notes |
|---|---|---|---|---|
| Isola 370HR (FR-4) | 4.04 @ 2 GHz | n/a, construction-dependent | 0.0210 @ 2 GHz | Construction-dependent; see below |
| Rogers RO4350B | 3.48 ± 0.05 | 3.66 | 0.0037 | RF circuitry |
| Rogers RO4003C | 3.38 ± 0.05 | 3.55 | 0.0027 | Mid-band RF |
| Rogers RT/duroid 5880 | 2.20 ± 0.02 | 2.20 | 0.0009 | Low-permittivity PTFE |
| Rogers RO3003 | 3.00 ± 0.04 | 3.1629 | 0.0010 | PTFE |
All Rogers values are specified at 10 GHz with 2.5 GHz in parentheses, and each is a typical process value with a stated tolerance (Rogers RO4350B, RO4003C, RT/duroid 5880). The Isola figures come from Isola’s 370HR product page, revision E, dated June 2024, which publishes a construction-dependent sweep: Dk runs 4.24 at 100 MHz, 4.17 at 1 GHz, 4.04 at 2 GHz and 3.92 at 5 GHz and 10 GHz, with Df running 0.0150 to 0.0250 across the same range (Isola 370HR).
Two things in that table deserve emphasis.
There is no universal FR-4 Dk. Isola’s own published data spans roughly 3.54 to 4.44 purely on construction, varying with glass style and resin content. Any sentence of the form “FR-4 has Dk 4.3” is defensible only as a rule of thumb, never as a specification. Specify the actual grade.
Process Dk and design Dk are different numbers, and mixing them up is the most common sourcing error in this topic. RO4350B is 3.48 process and 3.66 design. The 5% gap comes from copper surface roughness and foil treatment in a finished board, and it will visibly move a simulated antenna. Use the design value for simulation and the process value, with its tolerance, for manufacturing. Cite which one you used.
The honest threshold for material choice: FR-4 works at 2.4 GHz. Above roughly 5 GHz, dielectric loss starts costing real range and a low-loss laminate becomes worth specifying. An RF laminate does not rescue a bad layout.
How solder mask shifts your resonant frequency
Solder mask raises the effective dielectric constant around the trace and pulls resonance down. The measured figure is larger than the rule of thumb usually quoted.
A peer-reviewed measurement on a 433 MHz modified inverted-F antenna on 1.6 mm FR-4 found that removing the solder mask layers, with all other parameters unchanged, shifted resonant frequency from 433 MHz to 448 MHz, a 3.5% increase, and improved peak realised gain by 1.2 dB, from -13.8 to -12.6 dBi (Buckley et al., Electronics Letters, Vol. 50 No. 8, 2014).
The 1-2% figure that circulates widely comes from fabrication blogs rather than measurement, and it is roughly half the published value. For a narrowband application, a 3.5% shift is the difference between in-band and out. The fix is a solder mask opening over the radiator in the Gerber when the band is tight enough to need it.
Impedance Matching and Tuning a PCB Antenna
Tuning a PCB antenna means transforming its impedance to 50 ohms at the radio output, and the same in reverse on receive, so that power crosses into the antenna instead of reflecting back.
The acceptance number is return loss of 10 dB or better across the entire band. In practical terms, 10 dB is a power ratio of ten, so one tenth of incident power is reflected and 90% is delivered. Infineon’s antenna design guidelines tabulate the relationship directly: S11 of -10 dB corresponds to 10% reflected and 90% radiated, while -20 dB gives 1% reflected and -3 dB gives 50% reflected (Infineon AN91445).
The practical procedure:
- Measure S11 with a vector network analyser across the full band of interest.
- Read the resonant frequency and the complex impedance at band centre.
- Add or change matching components until return loss clears 10 dB across the whole band, not just at centre.
Two things that are easy to get wrong. First, most module reference designs ship a two or three component matching network with specific part values; those values are starting points, not constants, and they change with your stackup and your ground plane geometry. Second, both directions matter: tune looking into the antenna from the chip, and looking into the radio from the antenna.
Be careful not to invert the return loss relationship. A 10 dB return loss means 90% delivered. Confusing it with 90% reflected would be about 0.46 dB, which is a badly broken antenna, not a working one.
Manufacturability: What Fabrication Tolerances Do to Your Antenna
The fabrication process is allowed to miss your nominal dimensions within a published tolerance. An antenna is the one part of the board where those misses show up as RF performance rather than as a slightly different trace.
The strongest sourced figure here is the laminate dielectric constant tolerance, because Rogers publishes it as a headline datasheet specification rather than as a statistical claim:
| Material | Process Dk tolerance | Relative tolerance | Approx. frequency effect |
|---|---|---|---|
| Rogers RO4350B | ± 0.05 | ± 1.4% | ± 0.7% |
| Rogers RT/duroid 5880 | ± 0.02 | ± 0.9% | ± 0.5% |
| Rogers RO3003 | ± 0.04 | ± 1.3% | ± 0.7% |
The relative tolerances and the frequency effects are derived, not stated by the vendor. The derivation is straightforward: relative Dk tolerance is the absolute band divided by nominal, and resonant frequency scales as 1/√Dk, so a ±1.4% Dk band gives roughly ±0.7% resonant frequency shift.
What else moves the antenna, and in which direction:
- Etch undercut shortens the trace and pulls resonant frequency up. The direction is textbook physics. No primary source quantifies the magnitude, because it is process-dependent. Do not fill in a number here.
- Dielectric thickness variation changes the effective dielectric constant the trace sees, moving both resonance and feed-line impedance.
- Copper thickness variation changes trace width and therefore characteristic impedance.
- Lot-to-lot Dk variation pulls resonance down, as derived above.
On etch tolerance specifically: the widely quoted “±0.0005 inch” figure is not a universal standard value. Most standard subtractive processes quote a percentage rather than an absolute figure, and absolute figures at that scale belong to premium fine-line or laser processes. Likewise, claims that IPC-4101 mandates a specific Dk tolerance trace back to fabrication blogs paraphrasing a paywalled standard, not to the standard itself. Get your fabricator’s actual numbers.
The consequence is the important part. The bandwidth you designed in is the budget that absorbs all of this variation. The 433 MHz antenna in the solder mask study above had a 10 dB return-loss bandwidth of 4.5 MHz, which is about 1% of its centre frequency. A design like that has almost no margin for a ±0.7% Dk shift. A wideband 2.4 GHz design, where Infineon’s worked example holds S11 below -10 dB across 2.33 to 2.56 GHz, about 200 MHz or 8% of centre frequency, absorbs the same variation without noticing.
These are two different antennas at two different frequencies, so read the comparison as a ratio rather than as a like-for-like measurement. The point is that one design has roughly one per cent of its centre frequency available to absorb variation and the other has eight, and that difference is set by the design’s bandwidth, not by its frequency.
Three actions follow: specify controlled impedance, name the laminate grade rather than writing “FR-4”, and ask your fabricator for their actual etch and dielectric tolerances before you freeze the design.
Testing and Measuring a PCB Antenna
A vector network analyser and fifteen minutes on the bench will tell you whether your antenna works. Most of what goes wrong shows up in a single return-loss sweep.
Two tiers of testing exist, and they answer different questions.
| Tier | Instrument | Measures | Who needs it |
|---|---|---|---|
| Bench | Vector network analyser | S11, return loss, resonant frequency, rough efficiency | Almost everyone |
| Chamber | Anechoic chamber | Radiation pattern, gain, TRP, TIS, EIRP | Cellular and certified products |
Tier one gets the most attention here because it is what nearly every reader can actually do. The pass criteria are concrete: return loss of 10 dB or better across the whole band, and resonant frequency centred in the band of interest. If the resonant peak sits at the edge of your band rather than in the middle, the design is marginal even if it passes at centre frequency.
Tier two answers questions about how the antenna radiates into space rather than how it matches. Total radiated power measures total power radiated across a band while transmitting; total isotropic sensitivity measures average receive sensitivity across a band. These are the quantities carrier certification schemes assess for cellular products, which is why they matter commercially rather than just technically.
One rule governs both tiers: measure in the final configuration. The antenna must be measured on the final stackup and in the final enclosure, because that is the only configuration that means anything. A result from a bare board is not a result. This is also why the mechanical layout has to be frozen before tuning began.
Passing the RF measurement is not the same as passing final acceptance. Once the board is assembled, the workmanship criteria that decide whether it ships are a separate question, covered in our guide to IPC-A-610 acceptance criteria.
PCB Antenna vs Chip Antenna vs External Antenna
The choice between a trace antenna, a chip antenna and an external antenna is a trade between board area, schedule risk and range. The right answer depends on which of the three you can least afford.
| Option | Footprint | Relative cost | Relative efficiency | Integration effort | Failure mode |
|---|---|---|---|---|---|
| Trace antenna | Largest board area | Lowest | Best per unit area | High: layout discipline plus tuning | Fails silently if the keep-out is wrong |
| Chip antenna | Small | Low | Slightly lower | Low: minimal tuning | Fails if the keep-out is wrong too |
| External / FPC antenna | Largest total volume | Highest | Best range | Medium: connector and cable | Fails at the connector |
The decision rules:
- Board area is genuinely available and volume justifies the tuning work? Go trace. It is cheapest and performs well, and the tuning effort is a one-time cost.
- Board is small, or the schedule is tight? Go chip. It removes most of the tuning risk for a few cents more, and the keep-out discipline still applies.
- Enclosure is metal, or the range requirement is aggressive? Go external and accept the connector and the cable. There is no good way to radiate from inside a metal case.
Note what the middle column of that table says. A chip antenna is not a way to avoid the keep-out rule. It is a way to avoid tuning a custom geometry, and it fails the same way a trace antenna does when copper ends up where it should not be.
Common PCB Antenna Failures and How to Fix Them
Most PCB antenna problems reduce to five symptoms, and each has a single most likely cause you can check in under an hour.
| Symptom | Most likely cause | The check | The fix |
|---|---|---|---|
| Resonant frequency measured low | Copper beneath or beside the radiator | Inspect the keep-out on every layer, not just the top | Cut the keep-out on all layers, re-measure |
| Resonant frequency measured high | Trace etched short, or smaller than the reference assumed | Compare fabricated dimension against the Gerber | Correct the trace length, or verify against the vendor reference |
| Return loss fine, range poor | Matched but inefficient | Check for metal inside the keep-out; check substrate Df against frequency | Remove the metal; check the loss tangent is appropriate |
| Works on bench, fails in enclosure | Enclosure or plating detuning the radiator | Measure with the case closed | Evaluate case material dielectric properties; move the antenna |
| Behaviour varies between units | Fabrication variation eating design margin | Compare S11 across several boards | Widen bandwidth or tighten the tolerance spec |
The first row is by far the most common, and the check is the one most often skipped. A ground pour added during routing, on a layer you were not looking at, produces exactly this symptom.
The fourth row deserves a note. It is the reason the mechanical layout has to be frozen before tuning. An enclosure change after tuning is not a small perturbation; it can detune the antenna out of band entirely.
Frequently Asked Questions
What is a PCB antenna?
A PCB antenna is a copper trace or pattern etched directly onto a printed circuit board that transmits and receives radio frequency electromagnetic waves. Because the board is part of the radiating structure, its layout determines the antenna’s performance as much as the trace geometry does.
Are external antennas better than internal antennas?
Yes for range, no for cost, size and reliability. An external antenna radiates into free space and typically achieves better range, but it adds a connector, a cable, an assembly step and a failure point. An internal PCB antenna is cheaper and harder to damage but gives up range, and it needs protected board area to work.
How much board space does a PCB antenna need?
It depends almost entirely on frequency, because clearance requirements scale with wavelength. Nordic’s 2.4 GHz reference design uses a roughly 23 mm trace with 5 mm clearance to the ground plane, while a 433 MHz quarter-wave is about 173 mm in free space, so sub-GHz antennas need several times the area.
Can you put a ground plane under a PCB antenna?
No. Copper beneath the radiator couples to it, adds parasitic capacitance and detunes it. The ground plane belongs outside the keep-out boundary, not under the antenna. Nordic requires solid ground under the RF feed path and separately requires a keep-out under the matching circuitry.
Does solder mask affect PCB antenna performance?
Yes. Solder mask raises the effective dielectric constant and pulls resonance down. A peer-reviewed measurement at 433 MHz found that removing the mask shifted resonance from 433 MHz to 448 MHz, a 3.5% increase, and improved peak gain by 1.2 dB. For narrowband designs, create a solder mask opening over the radiator.
How do you tune a PCB antenna?
Measure S11 with a vector network analyser across the full band, read the resonant frequency and impedance at band centre, then adjust the matching network until return loss clears 10 dB across the whole band. Reference design component values are starting points that change with your stackup.
Are PCB antennas hard to design?
The theory is demanding, but the practical failure modes are few and specific, and they are almost all layout problems rather than mathematics problems. If you protect the keep-out zone on every layer, name your laminate grade, and measure before the enclosure is closed, most of the risk goes away.
Do PCB antennas need special PCB materials?
Not at 2.4 GHz, where standard FR-4 performs adequately. Above roughly 5 GHz, dielectric loss starts costing range and a low-loss laminate becomes worth specifying. Specifying an RF laminate does not compensate for a bad layout, and there is no single universal FR-4 dielectric constant to specify against.
Where to Start
Audit your own board against the keep-out rule before touching anything else. Check every layer for copper beneath and beside the radiator, not just the layer you are drawing on, and confirm no metal has migrated inside the clearance boundary during mechanical layout.
Then name your laminate grade rather than writing “FR-4”, and measure S11 before the enclosure is closed. Those three steps, in that order, catch most of what goes wrong.
If your stackup and artwork are already released, we can review the antenna area, the laminate specification and the controlled-impedance requirements before you commit to a build.
Sources
- Rogers Corporation, RO4350B laminates, RO4003C laminates, and RT/duroid 5880 laminates. Process and design dielectric constants with tolerances, and dissipation factors, specified at 10 GHz (2.5 GHz). Retrieved 2026-10-20.
- Isola Group, 370HR laminate and prepreg, revision E, June 2024. Construction-dependent dielectric constant and dissipation factor across 100 MHz to 10 GHz, with IPC-TM-650 test methods cited. Retrieved 2026-10-20.
- Nordic Semiconductor, General PCB design guidelines, for the approximately 23 mm printed quarter-wave monopole length, the 5 mm minimum clearance to the ground plane, and the requirement for solid ground under the RF path with an inner-layer keep-out under the matching circuitry. Retrieved 2026-10-20.
- Infineon Technologies, AN91445 Antenna Design and RF Layout Guidelines, document 001-91445, for the return loss and power-reflected table, the 10 dB sufficiency threshold, the MIFA dimensions of 7.2 x 11.1 mm with 20 mil trace width, and the worked wideband 2.4 GHz example. Retrieved 2026-10-20.
- J. Buckley, D. Gaetano, K. G. McCarthy, L. Loizou, B. O’Flynn and C. O’Mathuna, “Compact 433 MHz antenna for wireless smart system applications”, Electronics Letters, Vol. 50, No. 8, pp. 572-574, 10 April 2014, DOI 10.1049/el.2013.4312, for the measured solder mask resonant frequency shift from 433 MHz to 448 MHz, the 1.2 dB gain change, and the 4.5 MHz return-loss bandwidth.
- Texas Instruments, SWRA730 433 to 930-MHz and 2.4-GHz BOM Tunable PCB Antenna, February 2022, for the 43 x 25 mm antenna dimensions, the L4 trace length of 19.0 mm, and the prohibition on routing beneath the antenna.
- Silicon Labs, AN928.2 EFR32 Series 2 Layout Design Guide, revision 1.5, for the matching-circuit keep-out figures of approximately 70 mil and 37 mil. Note that these apply to the matching network, not to the antenna radiator.
- 47 CFR Part 15, FCC rules for unlicensed transmitters, governing operation in the 902-928 MHz and 2.4-2.5 GHz ISM bands in the United States.
- ETSI EN 300 328, covering wideband transmission systems in the 2.4 GHz ISM band in Europe.
