Will this PCB trace GSM antenna be affected by EMI?

Question

I am designing a PCB in which there are 3 SIM800 GSM modules sharing a (commercial) external antenna. The external antenna is connected to the PCB via an antenna connector, and from that connector, the antenna signal is “shared” via PCB traces running to the GSM_ANT port of the GSM modules (please see photo)

The reason I prefer this design is that it is both cheap and convenient. But without in-depth knowledge on antenna design and EMI, my question is Could this be a bad design? Or should there be scenarios that this design does not work reliably?

Just to provide more info, the PCB will be housed inside a steel enclosure, and its main PSU is an AC-DC adapter (good brand) which is already sealed for EMI. The adapter is also inside the steel enclosure. The steel enclosure will be deployed in a residential area where there are no large machineries around.

Thanks in advance! Dave

UPDATES:

Following some of your answers, I update the question as follows: Below is the old design, which uses 3 separate antenna connectors for the 3 GSM modules. However, these 3 antenna cables are combined (soldered) into one (with seal) outside the PCB and go to the external antenna.

The 3 GSM modules are supposed to be sending signal one at a time.

This old design has been tested and worked (though I suspect that signal strength are just around 8/10 of what it should be - good enough for the application though)

Answer 1

I think a more reasonable way would be to use an external three way splitter and the old design to connect your three GSM modules to one antenna.

You don't seem to have the knowledge to do RF PCB designs (not knocking you, I don't either) so it would be safer for you to use an external device that "Just Works."

Three-way splitter:

---

The old design may have been more advanced than you think - proper lengths of coax joined correctly can form an RF splitter. See "Wilkinson power divider" on the Wikipedia power divider page. For the uninformed eye, this would look like somebody just lashed a bunch of coax cables in parallel and hoped for the best - when in reality the lengths and connections were carefully selected to make a proper splitter that isolates the three sources from each other.

Wilkinson divider:

You can also make a Wilkinson divider on your circuit board, though that may take too much space.

Microstrip Wilkinson divider:

Answer 2

Apart from EMI issues, I have a hard time believing that this will work at all. Is there a reference design available for something similar? From what I would guess (I'm not an antenna specialist at all):

• Multiple drivers for one antenna
• No matching network (at least none which could be used if required)
• Your antenna line doesn't have a solid reference but there are traces on the other side.
• If this is a two layer board, I don't think that your trace is 50Ohms impedance
• The two connectors in the middle look like Ethernet. So it's probably metal, directly above your signal line.
• If you remove two of the SIM800, you will have crazy stub lines all around, nowhere terminated.

Answer 3

At the risk of giving a product recommendation you may want to look at an RF power splitter/combiner IC from someone like mini-circuits. Mini-circuits splitters

These will allow you to combine the 3 outputs (and split the returning signal) on the PCB without the impedance mismatches and other nasties caused by your current design.

Answer 4

A has been mentioned before, this is an 'interesting' way to combine the signals. Certainly it is not good, but really I think you're asking if its any worse than your old bodged solution of paralelling the coax.

With the coax, you have a more symetrical circuit (each RF path looks similar, and has the same parasitic connections). You also have a longer transmission line providing a hint of isolation from the joining point (maybe only 0.1-0.2 dB, but it goes both ways, so is not nothing). I feel this design is inferior, but can't quantify it. You will for example be pushing more transmit power directly into the other two modules (but they need isolation for their own Tx, so this should be OK).

I would be tempted to try and lay this out as more of a star, and experiment with series resistors to improve the matching (you have certain losses here, but also better matching, so overall it will probably be better). Mis-matching the antenna pot on the modules might affect the tuning of filters, etc. About 25\$\Omega \$ should be right, I think.

Clearly this is the cheap and ugly option, a proper low loss spliter would be nicer.

Answer 5

This is a horiblle bodge (whether implemented in coax or on the PCB).

Firstly the direct interconnections will create horiblle impedance mismatches which will reduce signal integrity. Some high power RF transmitters can even be damaged by signal reflections.

Secondly whenever any module transmits a substational fraction of the transmit power will feed back into the other modules. This may blind the modules to incoming signals or in extreme cases may even damage them.

A proper impedance matched splitter is a better soloution but reflections from the splitter and antenna may still cause problems as impedance matches are rarely exact.

Answer 6

First of: all of the combiners from the other answers can only work on a single band. You can't use the same combiner for GSM900 as for GSM1900. That is physically impossible.

The fact that GSM devices can use the same antenna for transmit and receive at all is due to the fact that up- age downlink in GSM are on different frequencies, so that you can use a frequency-selective device, called a diplexer to avoid TX signal going into the receiver (and destroying it).

Now, the way a diplexer works is that you basically have at least one filter in the RX branch that blocks out the uplink frequencies and only lets through the downlink. Together with the same principle and a splitter, the TX branch is connected to the antenna. Since this is very cost-, space- and energy-efficient microwave technology, the two filters and the splitter are basically combined into one device.

The problem with that is that it's very hard to achieve perfect impedance matching on both RX and TX at the same time over all frequency bands that GSM exists on (800,900,1800,1900,...).

Since receiving successfully is more important than transmitting at perfect efficiency, typically a mismatch of the TX branch's impedance compared to the nominal antenna impedance is accepted. In the single-transmitter-per-antenna case, that's OK.

This means that quite a bit of the TX energy gets reflected back into the TX amplifier in the single antenna case.

Now, imagine you have two TXing senders A and B connected to a splitter. Not only will a bit of transmitter A's energy be reflected back into A at the diplexer, the remainder that actually goes into the splitter will inevitably at least partially be seen by B's diplexer, where it's going to be partially reflected back, and by the way all directive couplers work, destructively interfere with A's signal at the antenna port.

So, you'd need to build three diplexers, one for each GSM module, build an impedance matching network for the TXes, a three-way splitter (or, while you're at it and have singled out the RX signal, anyway, add an LNA) for RX, and then you'd have a truely better system.

Answer 7

How do you intend to use it? Do you want to use three SIM800 modules at the same time with one antenna? This will not work. First of all, due to impedance split. Secondly, the modules output will affect each other which will disrupt the communication. Just add two additional connections for the antennas. Remember that the antenna trace should be as short as possible.

You are aware of the fact that with an antenna on a PCB you need to certify your device?

One tip: Add a via shielding around the antenna trace. Google -> via shielding.