Bottom line up front: successful prototype, need help designing a smarter-looking remote control but my RF knowledge isn't up to scratch.
I built a prototype remote control for a project using bog-standard 433 MHz RF Tx. The antenna is a simple 17cm monopole copper wire coming out the back of the Tx ANT pad. Driven by a 9V battery and a Micro plus inputs.
I'd like to now make a better version, using the Atmega as-is and placing it buttons and all on a smart-looking PCB, epoxied and on display. I plan to place the RF Tx flat against the PCB and connect the ANT to a nearby SMA and 1/4L stub antenna via a trace as shown in the pic.
You can wind the antenna wire so it looks like a spring. i.e. wind it round a pencil.
In this way, the antenna is not sticking out by 17cm. So, you could encompass the antenna within the bounds of the project box. However, the performance/reach/distance will be reduced.
You can buy then ready made (made with spring wire so they hold their shape).
And a small point - the antenna should be 17.3cm long.
Hi, thanks. Sorry, I was rounding. 17.3cm is correct (although TBH at the ranges I'm using, it didn't really matter).
The thing is, there isn't really a project box. What I'd like to do is make something that looks good enough that it can be epoxied and all on show. But the antenna, wire-wound or not, is the tackiest bit of the design and my idea was to trace it to an SMA connector.
Hi Pogo, yes that's the sort of thing I'd like to connect to it. I'm using RS Components for my parts list currently.
Question is, how to get the signal off the little RF Tx board and to the SMA without ruining the signal. I know it's to do with impedance matching, and having the trace on the other side of the board...but I'm just trying to figure it all out.
That's the magic bit. I know that there are macros in several PCB design packages that will give you a 50 ohm matched trace, so I'd start there (but I haven't looked in detail, so I can't recommend one). Otherwise, keep it short and away from anything that might become part of the 'circuit' at those frequencies.
Yeah. At magic frequencies, length is relative to wavelength (on the board, where the speed of light is about 0.6c, so short is even shorter). My experience is that less than about 10% is 'short', over that is 'significant'. Keeping impedances matched helps to reduce the losses due to these length mismatches, but there is no perfect, only minimally bad.
Thanks Pogo, this is really helpful. Wavelength of a 433 MHz signal on the board, assuming 0.5c, is ~350 mm. So, a conservative 10% critical length would be 35 mm.
The trace is about 25 mm. The ANT pad on the PCB is about 6 mm along a header pin from the ANT pad on the Tx module. The antenna and SMA are both 50 Ohm impedance.
My understanding therefore is that I'd probably get away with it but it would be better if I matched the 25 mm trace to have 50 Ohm impedance by changing its width. I assume that the header pin is (0.02 wavelength) and any circuits/traces on the Tx module are irrelevant.
I've also seen comments elsewhere about:
Unintentional antennas being created with header pins and the SMA's signal pin
Issues with the 90' bends that would come about
For some reason, it's suggested to have the trace on the underside of the board. Still figuring that one out.
In my experiments, those particular TX modules showed a sensitivity to load, sometimes failed to oscillate. If presented with an actual 50 ohm load, the feedback available to the oscillator is reduced to near the margin of failure. The reason most people don't notice it, the antennas they connect are random and don't load the transmitter output as much. If I had to do that, I would put a modest attenuator pad between the module TX and any properly matched dipole or 50 ohm approximately antenna, for example. I'm not sure if you're planning to do that, or if the SMA is more for convenience. I kind of guessed otherwise from your interest in 50 ohm PCB traces.
Your trace should be over a ground plane, it matters less which side. You should clear away some pour of VCC adjacent to the trace, you should minimize coupling with the power plane.
Also excuse me if it was said and I missed it, but you can make a PCB antenna. Just not a really great one. But it would solve your "looks" issue.
Hello aarg, that's some of the most useful feedback yet. I wouldn't be surprised if the components gave up when presented with an actual impedance. Are there any modules you have had better experience with? Ideally I'm looking for one-pin OOK as I'm pretty maxed out on pins for the receiver.
Your points about VCC and GND plane I'd figured but good to have it repeated. There's no need to have VCC there.
Excuse me being uneducated but I think what you're saying with the attenuator is this. The modules are cheap, the oscillator circuits are not well protected, and any reflected signal (aka feedback) gets to it and messes with it, causing deviation in the carrier signal. We can limit that by placing an attenuator in the transmission line to lower the power in one direction, meaning that if any power was reflected it would be that much lower again after going through the attenuator twice?
Have you got any suggestions on how to construct a PCB antenna? Just a useful web link or calculator would be fine. Would that get us around the issue of reflected power and would it suffice for a few metres' transmission?
If the PCB is 1.6mm thick 2-layer FR4, then use a 3.2mm wide trace over a solid groundplane for approx 50ohm microstrip. Keep other traces 5mm away from the
microstrip trace. There are online calculators for microstrip, using the board material,
and pcb thickness.
The narrow trace you've used is significantly higher impedance I suspect, could be
causing significant power to be reflected/back-scattered.
Hi MarkT, you're right and that's the bit I've figured out. I actually calculate a little narrower as I believe the solder mask can reduce the impedance.
I don't suppose you have any advice on whether the header pin between the Tx module's ANT pad and the main PCB would cause any issues? Especially since it's at right angles? Or, is it small enough given the frequency that it's immaterial?
Hi MarkT, amazing. Thanks also, I admire your other posts on the forum.
OK so I think I'm closing in on the solution.
Move things around so that the total transmission path is as short as physically possible. I reckon I can reduce it to <10mm straight line.
Impedance-match the transmission line on the PCB - 3.2mm (but I'll check the PCB specs)
Transmission line on opposite side from connector, ground plane on same side as connector
Get rid of any other traces or planes in the area
Take care with solder joints - as good as I can get. Perhaps pre-heat the SMA.
I might be overthinking this but the areas I still have doubts over are:
Whether the stubby monopole is any good or whether it will be poor without a ground plane. However, like I say the 17.3cm straight wire was sufficient in the prototype...
Whether I'd be better off with one of these or these or these compared with what I've tried which are these. I see 'superheterodyne' is preferred by many but I know that some operate at lower power. Should it be as simple as checking datasheets and using P = I*V?
Is mounting the Tx Module parallel to the PCB or perpendicular better - or is it immaterial?
Should the GND plane flood inside the footprint of the SMA or just touch the pads on the outside?
The SMA (despite the silkscreen) is a perpendicular one, pointing straight up. Is this better/worse than a right angled one?
Have you a new PCB layout with the microstrip - a picture is worth many words. No need to make the microstrip as short as possible, its a transmission line - just avoid right angle bends, use 45 degree only.
Monopoles work against a groundplane or ground radials. Antenna designs are something you can find online...
Hi MarkT, I've done a new layout. I couldn't actually get the transmission line to 3.2mm and still get it through the GND feet of the SMA but I've made it as wide as possible and as short as possible. I've also cleaned absolutely every trace other than GND off the component side of the PCB and tried to leave a margin for any signal. Finally I've switched out the cheapo ones for one of these.