Hi everyone,
I’ve noticed an issue with my RFID module when it is soldered onto my custom made PCB unless I make use of the onboard standoffs as shown in the module images here:
I am aware that the module has an operating frequency of 13.56 MHz but can the interference from the copper layers be preventing my RFID module to function properly??
have attached my custom made PCB images in the SVG files below:
Any insight or tips on this would be greatly appreciated.
Thank you!
Your posted image is not much better than postage stamp size.
Is the module parallel or perpendicular to your pcb?
If parallel is the module pcb likely to be touching your custom board in various places?
If parallel your custom pcb might just be too close to the module so the antennas do not work correctly?
You can right click and open the image in a new tab to open the entire image 
The RFID is connected in parallel to the PCB and the module is close to the custom PCB and is potentially touching the edges of the module.
My question is why does the RFID act this way when the PCB is touching even though there are no noisy traces running under the module ?? The only traces immediately around the module is the traces going into the JST plugs and the two piezo buzzer traces.
Here is an image showing another angle of the bottom of the board:
Your PCB screenshot apparently it has a GND plane over it’s whole area, and this is a common cause for malfunctioning antenna’s.
Hi Paul,
Yes this is a two layer board with a GND plane on both the top and bottom layer. What should I do to fix this?? Should I remove the ground plane for both the top and bottom layer under the module?? Should I have a board cutout in this case??
Why is this interference caused, is it because the return path of the 3.3V power source is very noisy and would require the RF module to be sectioned off from the rest of the board??
Thank you!
When your antenna is close to the GND plane, then the GND plane sort of acts like a faraday cage. There should not be any copper on your PCB near the antenna.
No. It has nothing to do with noise generated by your PCB.
The GND plane distorts the electromagnetic field that the antenna is supposed to pick up, so there is just no (or far too less) signal left for your antenna to pick up.
And on top of that, There is a capacitance between your antenna and the GND plane, and this can also de-tune the antenna so it works at a different (and therefore the wrong) frequency.
What does the module datasheet say about spacing. I have Mifare readers with a dumb antenna PCB spaced about 10mm above a ground plane
I have often opened .png images on this forum. But your svg file does not behave similarly. I was going to say that your method does not work on my machine. The additional tab opens for maybe 100 mSec and then closes. But I see that I downloaded .svg files to the download location on my C drive.
Generally any antenna can be interfered with (shielded or blocked) by nearby conductive surfaces. You want to get the antenna away from metal planes that exceed some minimum size depending on frequency and antenna design.
I just looked at the datasheet, it says nothing about spacing. Found an article (google for “placing RFID antenna close to ground plane”), at https://www.researchgate.net/publication/224652628_The_Effects_of_a_Metal_Ground_Plane_on_RFID_Tag_Antennas
… they investigated the effect of a ground plane… here’s the summary of their results:
Para below that table says:
"The antenna patterns above show that the antenna beamwidths drop when they are placed
close to the metal. Even though the antennas become more directive in the presence of a
ground plane, Table 2 shows that once inside two centimeters the effects of the ground
plane on the radiation cause the antennas to lose 0.1 to 8.6 dB of gain when compared to
free space."
So, expect problems if you put the RFID antenna next to a ground plane!
Copper layers near antenna work as shorted coils - consumes high % of antenna energy and changes it into heat.
Copper layers change antenna inductance detuning it.
In any 13.56 MHz RFID IC application note you can read that you have to tune antenna in final working environment that is including all metal elements that will be around it.
In my opinion the more important is consuming of energy emitted by antenna. RFID tag need some field strength to be powered by it. With too low power it just not works. Crypto tags need more field strength to work than standard tags as they need more energy for calculations they have to do.
Hi Piotr,
I was thinking of implementing this as a solution for the Sunfounder RC522 module:
The ground copper plane is still present on both the top and bottom layer, do you suggest removing any one of the ground planes or will the board cutout be sufficient to fix my issue??
Thanks for your help thus far!
You have to consider what for is the ground plane you use and if it is ‘for nothing’ than near RFID it should be probably removed.
You can also use ferrite to isolate RFID antenna field from nearby ground plane. The field on the back of the antenna closes in the ferrite and not generates eddy currents in ground plane so power is not lost for that currents.
There are some of them made by different producers.
An example:
https://eu.mouser.com/ProductDetail/Laird-Performance-Materials/MSLL12060-000?qs=sGAEpiMZZMua3V2yDfsb6b9Hw1mlUwDoztSbsuStmMk%3D
Have in mind that 13.56MHz antennas have only few coils and the voltage at such antenna can be in a range of 5…20V (because of rezonanse it is higher that voltage powering the circuit) . So in a track at your PCB going like 1/2 of one of antenna coils you can expect 1/8 of that voltage (assuming antenna has 4 coils).
I am only using the GND plane to make the net GND connections for the module and JST connectors, I assumed that having a solid GND plane would be the best method of grounding. I think having a solid GND plane improves signal integrity by providing a return path for the top layer signal traces.
I went ahead and removed the top layer GND plane and kept the bottom layer GND plane. I moved the bottom layer traces to the top layer so my stackup would look something like this:
Where the top layer is the signal and power traces and the bottom layer is the GND plane.
Piotr:
Have in mind that 13.56MHz antennas have only few coils and the voltage at such antenna can be in a range of 5…20V (because of rezonanse it is higher that voltage powering the circuit)
The module functions on 3.3V RFID Module and has passive components built into the module
And you have to compromise between signal integrity and RFID needs. You should have GND plane where return currents travel and you need not GND plane where they don’t travel.
But your tracks can still interlock with the antenna itself and I was writing only about it.
RFID antennas are rather more than less symmetrical. That helps to avoid common mode emissions. If you go with GND track along the symmetry axis you will have the same 0 voltage at both its ends. If some signal track will go from one side along one half of antenna and then on the other side will be referenced to that GND (routed along symmetry axis) you will have there voltage I was writing.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
