Continue to Site

Welcome to

Welcome to our site! is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

GPS Module Antenna and RF Layout Design Guidelines

You can eliminate much of the requirement for complex RF design by using a GPS receiver module, but the signal
path from the antenna to the module RF-input is still a critical part of the board design that can have a big impact
on the system performance. A simple RF-signal path is not difficult to design provided you follow some basic
guidelines and use a software design tool for the geometry calculations. The following is intended to summarize
the basic RF design guidelines and give examples for proper layout and antenna-to-module RF signal path design.
Choosing an Antenna
As a general rule of thumb, when the antenna is located within 6” of the Module RF-input, you can use a
passive antenna. When the antenna is located beyond 6” from the module input, you should use an active
antenna to overcome the cable loss and maximize the signal-to-noise ratio. There are many choices of antenna
configurations for GPS; the best choice is often a balance between size, gain, bandwidth, noise, and cost. The
best advice is to test several antennas in the configuration of the final system to determine which provides the
best overall performance.
Antenna Configuration
• Passive Ceramic Patch – A ceramic patch antenna is a great low-cost choice that provides good sensitivity
and good omni-directionality. Its small size allows you to mount it within the same enclosure as the module.
It is also possible to mount the patch antenna on the same PCB as the module, but to reduce the possibility
of digital noise, we recommend that you mount the antenna on the opposite side of the board to the module.
In addition, to improve the performance of the patch, use the largest possible ground plane under the
• External Active Antenna – An active antenna is essentially a passive antenna with a built-in LNA and a coaxial
cable to connect the antenna to the module. It may be located remotely from the module and requires antenna
power, normally provided via the coaxial cable. To attach the coaxial cable to the PCB, a coaxial connecter is
required. The active antenna usually costs more than a passive patch and consumes more power, but
performance in low signal environments is typically much better.
• Helix – The Helix antenna can also be passive or active. The advantage of a Helix antenna is that it is small
and easy to embed and it does not detune in proximity of people, which is why it is used in mobile devices.
Antenna Connections
The connection between the antenna and the RF-input of the module is the most critical part of the PCB design for
GPS. The goal is to provide a perfectly matched 50Ω transmission line environment between a 50Ω antenna and
the module RF-input to ensure maximum power transfer to the RF front-end. Any discontinuities due to unmatched
impedances in the signal trace, excessive vias, poor layout design, or energy coupling because of poor grounding
can reduce the GPS performance significantly or even render it non-functional. To reiterate, this signal path is the
most critical part of the GPS system design. Follow the guidelines below to maximize performance.
PCB Layout – 50Ω Connection
To move the RF signals to the modules, we suggest a 50Ω grounded co-planar waveguide. In general form, this
consists of the RF input signal with RF ground on either side and RF ground below. Theoretically, for a given RF
signal trace width, the surrounding RF grounds should be at least twice as wide. In addition, the gap between
the RF grounds and the RF signal is important. The coplanar waveguide is the lowest loss transmission line
configuration for connecting the antenna to the module. You can use other methods such as microstrip or stripline,
but we believe the coplanar waveguide is the most efficient.


NOTE: While we can provide guidance and an example for your reference on how to construct and layout a coplanar
waveguide, we strongly recommend using transmission-line design software to ensure the design is correct for your
specific PCB type and system design. We suggest you use a freeware program, such as AppCAD.
For a two-layer board design, typically 0.062” thick board made with FR-4 material (Dielectric = 4.6) and 1 oz
copper (1.2-1.4 mils thick), the RF-input should be 30-32mils wide, the gap to the adjacent grounds should be 6
mils, and each of the RF grounds should be at least twice the width of the input signal (60-64mils).
If the board is thinner, such as a 0.031” thickness FR-4, then the RF-input width can be reduced to 25-26 mils and
the RF grounds reduced to 50-52mils wide, still with a 6mil gap between.
If ½ oz copper is used for the RF-input and surrounding grounds, add 3-5 mils in width.

General RF Layout Guidelines:
• Maintain a characteristic impedance of 50Ω throughout the entire RF signal path. Keep the RF signal path
as short as possible, and do not route near noise sources such as digital signals, oscillators, switching power
supplies, or other RF transmitters, such as Bluetooth.
• Do not route the RF signal under or over any other components (including the module) or other signal paths.
• Avoid sharp bends. If a bend is necessary make two 45° bends or a radius bend instead of a single 90 bend.
• Avoid vias whenever possible. Every via adds inductive impedance to the signal path. Vias are acceptable for
coupling the RF grounds between layers.
• Do not route the RF signal path on an inner layer of a multi-layer PCB (if possible) to minimize signal loss and
minimize the need for interlayer vias.


Guidelines for Isolating Digital and RF Grounds
• Give careful consideration to the floor plan of the design. The ideal floor plan will partition digital and RF
circuitry into clearly different regions.
• Keep RF and digital signal paths as short as possible.
• Do not route digital signals long distance across the board as they may pick up or couple noise into/from the
RF circuitry.
• Locate bypass capacitors as close as possible to the supply pin they are bypassing.

  • Like
Reactions: MSadegh


we have produced an OEM GPS product for our customer. Our customer finish all design,like yours. and send us PCB Gerber file and BOM. We do OEM only. but for this kinds of board, test is not easy.Function test equipment is offered by our customer,this equipment often has problem.So,our delivery time is not so quick.

Part and Inventory Search

Blog entry information

Read time
5 min read
Last update

More entries in Uncategorized

More entries from TomTang

Share this entry