Help !!!!! 50 Ohm PCB Antenna tracewidth and airgap ?
For our current design we need to creat 50 ohms tracks for RF Signal,
We are not going to give any reference to this either by a plane or a trace,
How can we get the Tracewidth and airgap of 50 ohms impedance differential signals (2 traces).
Thanks ,
Mobin Mohandas
Hi everyone... Since I'm also working on the same project, I'll explain a bit more on the requirement... We have an RF transceiver chip that sends out RF signals. This will be routed to an RF Switch IC (HRF-SW1030), where it's switched between 6 channels. Each of the 6 channels is connected to an antenna coil (and associated passive components to maintain 50 ohm impedance). Since all the 6 antenna coils are on the same PCB, we have to run traces from the switch IC to each antenna. If we were using different PCBs for each of the six antennas, we could've used a 50ohm cable for each connection. Here, since we are running PCB traces in place of the 50ohm RF cables, it is imperative that the traces should have 50ohm impedance in order to have proper matching. How can this be achieved? Is it wise to have a ground conductor underneath the two traces, so as to provide reference, and hence maintain 50ohm impedance throughout the length of these tracks?
What do you mean with "two traces"?
Do you use a differential line pair for each RF signal?
A transmission line consists of signal and return path. The choice of microstrip (one signal line over ground plane) or differential line pair (signal and return side by side) or some other structure depends on your application.
Two traces = one signal and one return -> here it is quasi differential.
A ground 'plane' is out of question, as the RF radiated by the antenna coil would get absorbed by the ground plane itself. So, how do we maintain a 50ohms impedance as seen by the chip?
I hope I made it clear that we intend to use the traces as an alternative to 50 ohm cables. It must look something like this:
<50 ohm source>===================<50 ohm tuned antenna> [Of course there would be bents and curves on the traces while doing the actual layout]
We are using 13.56MHz RF, for reading tags.
I understand, that the first post is asking for a differential pair design. 50 ohm differential is a rather low impedance and can be best achieved with a ground plane and a thin substrate (differential microstrip). A differential pair without ground plane (e.g. differential coplanar waveguide) would result in rather extreme gap to trace width relations.
The same basically applies to 50 ohm single ended transmission lines. But if you intend to incorporate antennas with your PCB, you should primarly care for the antenna requirements regarding ground planes and PCB substrate. In any case, you can expect, that the individual antennas interact with each other and the common ground plane.
The term "antenna coil" is mostly used for D << λ inductive couplers, that don't have much antenna properties.
P.S.: As expected. In this case, you also don't actually need 50 ohms transmission lines. Instead the trace can be considered as lumped inductance and goes into the dimensioning of the matching network. In may be appropriate to design a low inductance connection anyway, so wide traces above a ground plane seem reasonable. Of course, you can design the connection as 50 line to simplify calculations, but it isn't actually required.
Could you explain a bit more on that? Would greatly appreciate it if you could provide some means of calculating the gap/width requirements.
You are spot on, on the last sentence. Yes, it's an inductive coupler that we are designing, and not a real antenna.
Individual antennas do interact, but in our case, they are quite far apart and their sizes are also considerably less relative to the separation between any two antennas.
The issue we have here is, it's a bit difficult to get the matching circuit right in order to have a working system. In our case, this effort multiplies by six, since we have six antenna coils to take care of. Apart from that, we will have to deal with each antenna system separately, as against the 50 ohm design.
If we can get this transmission line between the switch IC and the antennas right, we are saving a lot of time, expenses and also avoiding potential board-to-board variations.
As FvM correctly stated, the whole concept of controlled impedance transmission lines is NOT useful for lines that are electrically short. If the line is shorter than 1/20 wavelength or so, the "distributed" nature of the line can be ignored and you can calculate the line as a simple RLC network. For 13MHz, the routing on your PCB can be considered lumped elements.
But if you insist to use controlled impedance for your differential line pair, I can calculate the values for you. Please choose a line width or a gap size, and I will calculate the second value for you.
There are various commercial and free tools for calculation of PCB transmission lines. Some have been suggested at edaboard.
Regarding your multi RFID "antenna" design, I see the following basic aspects
- the driver side is 50 ohm single ended. A 50 ohm connection line between driver and impedance matching network would be suggested by the usual cable setup, but isn't necessarily required
- you don't want a ground plane near the coils. But a single ended transmission line effectively requires a ground plane (or at least a ground area of some extent)
- the impedance matching network involves a single ended to differential conversion (a balun), because the coil should be driven balanced
In my opinion, the placement of the impedance matching network and the impedance and type (unbalanced/balanced) of the transmission line are both open for design optimization. If you want the TL without a ground plane, a differential line would be suggested, but involves a balun at the driver side. So one option is to move part or all of matching network to the driver side and connect the coil through a balanced line. A parallel capacitor at the coil side seems reasonable.
Just to confirm that, here is an example:
I simulated your differential pair with 50μm and 100μm gap size, and varied the line width. The resulting line Z0 is shown in the plot below. Line width is in mm. Substrate was 0.5mm FR4.
As you can see, the line impedance is higher than 50 ohm even for very wide lines, which tells us that the line is too inductive and we need more capacitance between the lines. Increasing the capacitance by a smaller gap might cause manufacturing problems, so we need a different approach.
One possible solution is to use broadside coupled lines (i.e. line pair where lines are vertically stacked, instead of side by side on the same layer), but that depends on the thickness of the dielectric between the lines.
So much for the calculation. Note that this controlled line impedance is not a requirement for your application because your lines are short compared to the wavelength.
We already have a matching circuit and balun at the driver side, and it's the signal coming out of the balun that's being fed via the switch IC to these 6 antennas. FYI, each of the 6 antennas are to be identical, hence each one has a matching network comprising a couple of capacitors in parallel and another one in series, along with a small resistance.
Yes, we are planning to run a balanced line, after deliberating on your worthwhile posts, among other things.
EDIT:
sounds interesting, but haven't explored this method yet. Will definitely give it a thought
Do you intend 50 ohm or 50+50=100 ohm balanced line? 50 ohm balanced would be inapparoriate low impedance in my opinion.
Also using a 50 ohm switch (double pole) for a balanced line suggests 100 ohm line impedance.
Like i mentioned earlier, my intention is to use PCB traces in place of a 50 ohm RF cable that is generally used in these kind of applications - RF chip on one board, and the antenna coil positioned at another place. Therefore, i am using a balun transformer to convert ~200ohms impedance as seen by the chip, to 50 ohms on the transmission line, and finally connect to a 50 ohm tuned antenna.
Yes, that's what I understood from your first post. But it doesn't fit a balanced line.
I just gave it a try in the simulator. If we keep the 8mil line width, we would need a FR4 thickness of ~3.2mil between the broadside coupled lines for 50 Ohm line impedance.
If you have something like a thin prepreg layer in your board, these broadside coupled lines might be an option with reasonable dimensions.