SIM800L Issue

[Suraj143]

I have programmed a system when I give a call to SIM 800L modules SIM number it detects & if it is a valid number then it activates the buzzer. The design works fine at home. But when I place this design near a factory its not working. In factory there are some different RF panels as well. How to solve my problem?

In the factory when the call is receiving I can hear some interference noise form my buzzer...!

See my diagram.

 

[Diver300]

The RF signal level when the SIM800L is transmitting will depend on how far from the nearest cell tower it is. Even receiving a call will mean that the SIM800L is transmitting, so it could be that you are getting more transmitted power at the factory.

Is the PIC driving the alarm output down when the alarm is not supposed to be on?

When there are strong RF signals, layout is important. Have you got a photo of what the system looks like?

 

[Suraj143]

Thank you for the input.

Here is my PCB layout .Note that I'm not using the PCB relays. I have connected the buzzer to the B+ & B- pads.

 

[rjenkinsgb]

I'm not fully clear on what the problem is? Does it work at all in the factory?

If you are using the antenna connector position on your PCB, that is unlikely to work well; there is no ground plane or transmission line connection to the RF module and the "ground" is via a long track connecting other components. The electrolytic cap near the antenna is unlikely to work well at GSM frequencies.

You could try adding a ceramic cap directly from the module ground pin to the connector ground, on the solder side?

Interference from the switch mode module is also a possibility. If the cellular signal is weak, that could have much more effect than with a strong signal.

The LM338 does not appear to have any input or output stabilising caps?
Electrolytics are good for bulk storage and low frequency coupling, but do little or nothing at very high frequencies; you need such as polyester or ceramic caps for that, and at RF just trace lengths can be extremely critical.

Even the PIC or the output traces from that could be causing some low level interference; again, a ceramic directly across the power pins under the board is worth a try?

 

[Suraj143]

Many thanks for the detailed review.

I'm not fully clear on what the problem is? Does it work at all in the factory?

In factory it didn't work at least one time. Sometimes when I give a ring to the sim module It says it is "switched off".

If you are using the antenna connector position on your PCB, that is unlikely to work well; there is no ground plane or transmission line connection to the RF module and the "ground" is via a long track connecting other components. The electrolytic cap near the antenna is unlikely to work well at GSM frequencies.

I have placed a SMA base connector on PCB. There is a PCB connection line from module to SMA base (transmission pin). Please see the markings on the attachment. Is that ground path to antenna too long from the buck converter?

You could try adding a ceramic cap directly from the module ground pin to the connector ground, on the solder side?

module ground and the SMA connector ground are same. It will short out the ceramic capacitor

 

[rjenkinsgb]

OK, that pad for an antenna is intended only for a directly-soldered wire antenna, not for external connections.

You could try a cap direct from connector ground to the module positive pin, on the basis that is likely to have good RF decoupling - but ideally use the onboard antenna connection rather than external.

Note that a PCB track is only a "transmission line" if it has a constant impedance; that means eg. the correct width and below a ground plane.

The earth tracks do not short out a capacitor at RF, the capacitor bypasses the inductance of a long track.

Any PCB trace can resonate at high enough frequency, unless it is properly impedance matched. You need to use topside ground plane and plenty of VIAs to any grounded underside traces, anywhere near any RF connections.

See the info here:

http://www.disk91.com/2015/technology/hardware/design-a-50ohm-impedance-net-for-rf-signals/

And here:

Simple RF PCB Layout Tips (2.4GHz and 5GHz bands)

Some simple RF PCB layout tips and tricks for properly laying out RF PCB traces in designs with WiFi and Bluetooth or other high speed RF traces.

iot-bits.com

The antenna is the only part of that board that matters for RF rules, so if you can just use the onboard connector and isolate the other PCB, some problems should be eliminated.

 

[Nigel Goodwin]

There's an aerial socket on the top of the SIM800L board - simple remove the spurious pin down to the PCB and plug the aerial in there instead.

There are also decoupling capacitors on the SIM800L board, so you don't need and high frequency decoupling capacitors on the supply to the board.

However, the SIM800L board (like most GSM boards) is extremely sensitive about the power supply feeding it, and drawing large fast current spikes. My boards using them usually have a 1F super capacitor (yes 1 Farad) on the supply rail for that reason.

 

[Diver300]

I have placed a SMA base connector on PCB. There is a PCB connection line from module to SMA base (transmission pin). Please see the markings on the attachment. Is that ground path to antenna too long from the buck converter?

For the antenna connection, the distance from the ground pin to the buck converter do not matter.

The antenna and the antenna ground should follow the same path from the SIM800L. That is why coaxial connectors are used. The SIM800L, not the PCB, the surface mount part, has four grounds connections adjacent to the antenna connection. If you use an antenna with the connector that is on the PCB, there is a ground plane on the PCB that joins the outer of the connector to those four ground connections. The antenna on the surface mount part is a few mm from the antenna connector, so the path is very short and is very close to the path of the ground.

The ground path of your circuit goes all the way round the board and through the buck converter.

The yellow line shows the antenna ground path. It is terrible. It is about as long as is possible on a board that size, and it should be as short as possible. That alone will induce noise in everything on your board.

You should use the connector on the PCB and use coaxial cables and connectors.

As a quick test, you could try joining where I have put a dashed orange line. Scrape the solder resist from the ground track and put a wire link. If that improves things, then you will know that a better board layout will help.

This comes from personal experience. On one board with a GSM module, I had a ground plane, I wired the antenna and its ground directly and I still had problems from the rf signals induced by the signal from the phone when it transmitted. I redesigned the board with more suppressor capacitors, bridges where the ground plane had to make way for a track, suppressor capacitors on all wires that didn't need to run a high frequency and series resistors in tracks to stop them resonating. I had to throw away a few hundred pounds worth of PCBs that were made to the earlier design.

I have also seen a circuit that misbehaves when a phone is near it. The microcontroller had a suppressor capacitor right beside it, with just a few mm from the +ve of the microcontroller to one connection of the capacitor. Unfortunately, the negative of the capacitor connected to a ground that was 100 mm of track length from the -ve of the microcontroller, making the capacitor all but useless at high frequencies.

I've got a few other comments on the circuit board.

The ground should have been linked locally like this:-

but it would be better to have a complete ground plane. You only have a few wires on the top, and it should be covered in copper where possible to make a ground plane.

You don't need a 5 A regulator to feed the relays. In fact you don't really need a regulator at all. If you had a 9 V ac transformer, it would run the 12 V relays and a 12 V buzzer fine. Neither of those needs a regulated supply. The regulator is only needed if you are switching on and off a larger 12 V load.

A lot of tracks are longer than they need to be, and the chamfers on the corners could be a lot larger in places, which will improve the rf performance.

There is no connection to the reset line on the microcontroller. It should be connected to +ve with a resistor, and have a 10 - 100 nF to ground, or you could just connect it straight to +ve.

You don't have programming connection for the microcontroller. Those can be very useful to avoid needing to unplug the microcontroller to reprogram it.

 

[Suraj143]

Many thanks for the support & ideas.

Now I understood my layout have problems.

*Firstly I will try connecting the Antenna ground to the nearest SIM800 module ground.
*Also I will place 104 ceramic caps under direct PICs VDD & vSS & will add some 10uF near power rails near the PIC.
*Also I will try with a socket antenna on plugging direclty to the Module (Disconnect the SMA antenna in my PCB).

It is very hard to make the same environment at home.I have to visit to noisy environmets & do the test.

I will tell the progress Ass soon as I go.

 

[Suraj143]

Hi Again,

I'm about to change my PCB layout. Did some changes. As below.
*Changed the level converter from GSM module to PIC.
*Lowered the PIC supply to 3.3V & connect UART pins directly to GSM module.
*Made ground to GSM module much shorter.
*Also added a top layer ground plane (Blue colour) under the GSM & antenna area.

1) How can I connect the SMA antenna connector to ground ? Shall I connect it o top ground plane?
2) Top layer ground plane still not connected to circuit ground. Where is the best place to connect it?
3) Do I need to add another bottom layer ground plane also?

 

[Diver300]

You should connect the SMA connector to the top ground plane.

You should connect the top ground plane to ground at the module.

A bottom ground layer could be an advantage. It should be connected to the top ground layer at least every 1 cm.

Does the board have through-plated holes? If not, it may be difficult to connect the layers together.

 

[Suraj143]

You should connect the SMA connector to the top ground plane.

You should connect the top ground plane to ground at the module.

A bottom ground layer could be an advantage. It should be connected to the top ground layer at least every 1 cm.

Does the board have through-plated holes? If not, it may be difficult to connect the layers together.

Many Thanks. I did the 1st two changes.

The board have through-plated holes. Regarding the bottom layer. Is it ok if I just copper fill the area? (No nay ground plane just only copper fill).

 

[Diver300]

I think that your connection to the ground plane is about as good as it's possible to have with the module in the circuit board.

There isn't really any difference between a copper fill and a ground plane.

 

[Suraj143]

Thanks.

There isn't really any difference between a copper fill and a ground plane.

I mean like this. There is a copper fill in bottom layer but not connected to any ground. Thats what I mean.Because there is no any way of connecting the copper fill area to modules ground

 

[Diver300]

You can simply put through-plated holes to the top layer. You shouldn't have copper areas unless they are grounded.

You might want to have more chamfers on the tracks to reduce length.