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.