asked by
SR4L034 and SR4G008 placement and clearances e.t.c.

We have a board with a SR4L034 antenna as well as a SR4G008, as shown below (early placement, far from final).
0402 passives, Quectel BG95-M3. Board length is 100mm.

1. The datasheet for the SR4L034 gives a rule of thumb for height clearance on components close to the antenna (8 degrees).
That is for the "top" side. What about the back side? Same or different clearance angle?
Reason for asking is that we'd like to place batteries on the back, and getting as close as possible to the antenna.

2. The SR4G008 is not at an optimal location, as it should be in the center of the PCB.
As there will be batteries on the furthest part of the PCB, (about 50mm), the antenna cannot be placed in the middle, but it could be moved quite a bit towards the center, at the cost of a long transmission line (which is now extremely short).
Would the efficiency resulting from the movement towards the center out-balance the use of a longer transmission line?

3. For future products, a PCB that is a lot shorter, is planned. Length about 40mm.
What is the most suitable antenna, similar to the SR4L034, covering the "regular" LTE Cat-M, NB-IoT (and GSM) bands in EU and USA?

4. Any other comments regarding the design are very welcome.


Please log in or register to answer this question.

2 Answers

answered by
edited by anonymous

I have tested SR4G008 extensively and use the antenna in many designs. SR4G008 is a classic loop antenna. The function is explained in my IoT M2M Cookbook. The ground plane/length left and right of the antenna is part of the antenna. "Left" is not a mass. Therefore the antenna will not work well.

SR4G008 will not work on 40 mm ground plane. This is what it says in the IoT M2M Cookbook.

My recommendation: Replace SR4G034-R with SR4G034-L Then the SR4G008 Groudplane will automatically increase in size. Measure the return loss of both antennas even on an empty PCB with housing and battery before you place the other components. As long as the return loss is suitable it makes no sense to place additional components.

Incorrect return loss in cellular antennas usually leads to an error in RED/FCC.

answered by
Hi Jesper,

To answer your 8 degree question; yes, it should be 8 degrees on both sides of the board. Placing the battery underneath the antenna right up to the edge of the ground clearanced area will not only have an affect on the radiation pattern it will load the antenna due to the proximity of the ground of the battery shunting some of the near field radiation to ground. It will be hard to say how much the battery will affect the performance of the antenna but if you could move it back even 5mm that would have a noticeable improvement.

For the SR4L008 antenna, I agree with Harald's answer. Switch to the SR4L034L moving the LTE antenna to the opposite side of the board therefor giving the SR4L008 a longer edge to operate against.

Using a 40mm ground plan will significantly reduce your low band performance and is not recommended unless your device will be plugged into a harness like an PBD2 device. Can you share what your device will be attached to?

Using four or more layers in your board stack up is advisable and keep the top and bottom layers as uninterupted as possible will benefit the antenna performance. Try not to run long traces across the top and bottom layers because they cut up the ground plane the antenna operates against and have the potential of radiating noise that will interfere with the radio's receiver and cause difficulties passing RSE.

Best regards,

Geoff Schulteis
commented by

Thanks, I expected it was the same on both sides with the 8 degree clearance, just wanted to be sure. It's not a problem, we do have the space to move the batteries away on the current design. But in the future, it will be more tight.
The problem of using the SR4L034-L, is that the feed line will be relative long. Also, due to the keepout areas below the antenna, it is impossible to route the feed-line there, without moving the module 10-15mm to the right.
It will in that case be a lot simpler to move the GNSS antenna.

Board is not connected to anything.
This version have a 100x35mm ground plane. Future versions will have a lot less, down to about 40-50mm square.
The antenna might not work well with that, but I'm sure there is other antennas that will work (more or less) with a shorter ground plane.
I mean, there is watches with cellular and gps receivers, so it definitely IS possible.
It would be great if you could suggest some antenna solutions to shorter boards.

I have normally been using coplanar waveguides for feed lines (most often on two-layer boards).
This board was planned to be 4-layouts.
But you are suggesting keeping outer layers as GND and using a stripline instead of coplanar waveguides on the top layer? As this would require at least two vias (perhaps even blind vias) and even 6 layers, assuming inner GND/PWR layers, is this really better / needed? 
I'm not quite sure I understand the "Try not to run long traces across the top and bottom layers because they cut up the ground plane" part.
Normally GND layers will an inner layer + top/bottom (with some cuts), so an unbroken GND is always there (inner).

Alternative module placement, better GNSS antenna placement, but longer transmission lines.


commented by
Hi Jesper,

The placement you show at the bottom of your response does not have unruly length traces. I would go with the longer traces to ensure optimal performance of the antenna. The longer trace lengths would only add less than 0.5dB loss to the input signal from the antenna to the radio versus a poor performing antenna that could be several dB below optimum performance.

The reason I suggested placing the ground on the top and bottom layers is for two reasons. The first is noise likes to radiate off of traces and if those traces are locked between two ground layers they cannot radiate.  The second reason is along the same principal that because these antennas are electrically small they use the ground near the antenna as a counter poise so the currents that flow between the antenna and ground operate best on the surfaces layers. If the antenna counter poise is buried in between signal and power layers it is less likely to radiate and more likely to pick up noise from those layers and reradiate it causing failures in RSE and TIS. The energy that is supposed to radiate away from the antenna would also be absorbed into the signal and power layers because it is not able to radiate away from the antenna.

Antennas in wearables are usually certified under AT&T's small device category that only requires the device to radiate 9 to 12dB instead of 18 to 20dB for TRP. The allows the antenna to only have an efficiency of 15 to 20% in order to pass carrier spec. You should be able to pass this small device spec easily with your 100 by 30mm PCB and will be cutting it very close with the 40 by 50mm PCB.

I hope this is useful information.

Best regards,

Geoff Schulteis
commented by
Thank you Geoff, yes, very useful.
For now, we'll go with a version that is pretty much like my latest pic.
The whole upper edge of the board is free from top-layer traces, so that should keep the noise down. Anyway, we don't have any "busy" high-speed traces on this board.

We'll get back to the smaller board when it's time for that.

Thank you!
commented by
Sounds great!! Best of luck and let me know how I can help in the future!!

Meet the moderators

Yu Kai Yeung

Antenna Engineer at Antenova Yu Kai is an antenna expert with over 10 years of experience in the design and testing of antennas. He has experience helping customers with certification testing, combined with his knowledge of RF measurement procedures.

Raymond Lee

Senior Antenna Engineer at Antenova Raymond has a wealth of experience in RF and antennas across many industry sectors. He has over 20 years of experience in electronics design and manufacturing.


Antennas: The Comparison Guide

Find the perfect antenna for your project