-
Good evening, in the middle of a project(already asked some questions about it in this forum), its a small sensor "node" with an Atmega256RFR2 and some humidity, light, temperature sensors.
After a ton of code, its working fine, but the suggested SMD antenna gives an awfull small range(about 5-6m with transmit power on full tilt), I will admit my RF knowledge is about zero or maybe even negative, I only followed the datasheet for the recommended balun and antenna from the Atmel datasheets/app notes.
After trying some random caps and inductors to tune the thing with even worse results, I just unsoldered the SMD antenna, cut a patch antenna from a laptop with about 10cm of coax wire, soldered it to the balun and scratched a bit of the solder mask near it for the ground and got a much, much better result of 150m LOS, was baffled by the range with the random laptop antenna.
Now, I'm going for rev 0.2 of the board, and I dont know what to do regarding the antenna :/
SMD antennas with gain are kinda rare from what I could find searching around Mouser, almost all have +/- 0.5dBi of gain, that with my RF skills will net me again some 5m range boards, another option would be so just put an u.FL connector and buy some laptop patch antennas from molex or someone that sells them and just glue the antenna to the box, given that all I have is a couple multimeters and a 100Mhz scope, antenna tunning/matching is more or less impossible for me..
Any ideias about antennas, or maybe it was all fault from my layout?
The parts used are:
balun: 2450BM15A0015
SMD Antenna: 2450AT42B100
Print screen of the pcb:
-
First of all check that your balun is installed in the correct orientation.
In general, your layout looks fine. A better layout will break the ground between balanced and unbalanced parts of the balun.
Have you requested controlled impedance for the board manufacturing? Do you have any reports on that? -
I don't think impedance controlled PCB is necessary for such a short trace. And it doesn't look like anything has the correct impedance unless it is a 4 layer board (50ohm traces on a 2 layer pcb are very wide!).
But you are right, I doubt it is the layout. 5m range is wrong, even for a completely mismatched antenna. It sounds more like no antenna at all. So check if all parts are connected correctly. -
Well, I assume it is a 4 layer board. If this is a standard 2 layer 1.6 mm board, then there is going to be gross impedance mismatch and the board house will not be able to do anything to help it. Whether this mismatch directly related to performance issues - who knows, it is impossible to tell without doing actual measurements.
Also, how do you define and measure range? -
It is sadly a 2 layer board, the design per se doesn't need a 4 layer pcb, not that dense, I tried to stitch the ground planes as much as I could its a battery powered if that changes anything.
I have already checked everything and oh robot jesus
The balun is soldered the wrong way, well, its in fact rotated 180ยบ in the layout
I'm testing outside, with faint/almost no WiFi signals around me, my friends grabs in a board an starts walking, and I stay with another board hooked up to the laptop watching the signal quality value that the rfr2 reports back..
I will see if I can rotate the balun and have it working with the existing pcb layout so I can test it out, but now I'm feeling so dumb..
And how can the laptop antenna give soo much range even with the balun not doing its work?
Literal
for 5 minutes before replying to you guys..
-
And how can the laptop antenna give soo much range even with the balun not doing its work?
Exactly for this reason. You have a huge impedance mismatch, so RF energy, instead of being channeled into the antenna with minimal loses, is radiated by the points of impedance discontinuity.
You can remove your antenna, it is not doing anything in this case. All energy is radiated by the traces and component pins. -
Tomorrow I will rotate one balun and see how the small smd antenna works, it was just soldered the wrong way around, in 4 boards, the board house edited a bit of the silk and the pin 1 marker was removed from one side and looks like a pin 1 marker on the other side, but damm, I must be blind to do the same mistake 4 times.
Thanks ataradov because you just hit the nail. -
Thanks ataradov because you just hit the nail.
That's like number one reason for custom boards not working RF-wise. I don't know what is it about baluns that trips people over. -
Well, turned them around, and the result is the same, around 8 meter line of sight range with the small smd antenna, and around 150 meters with the WiFi patch antenna.
I also have a "base" board that as the rfr2 and a Wiz5500 and in that one I put an SMA connector and used a router WiFi antenna and that one is the worse range/rssi wise.
-
Well, turned them around, and the result is the same, around 8 meter line of sight range with the small smd antenna, and around 150 meters with the WiFi patch antenna.
As expected... Try with piece of 1/4 wavelength long wire instead of pcb antenna. If your sensor node will not move consider directional antenna. And if you need long range why 2,4GHz band was selected?
-
I dont really need long range, its just a "bonus", a stable 150m range is pretty sweet from a chip that uses at most 19mA when transmitting, that and the fact that there is such a difference between a smd antenna and a patch antenna from a laptop.
I choose this chip because:
RF and MCU in one package.
Its an Atmega, I have been using them for years.
Its low power(ish).
LwMesh from Atmel is a decent mesh network stack ready to use, so no need to re-invent the wheel or use a 300kB ZigBee stack.
I also looked into some CC sub Ghz from TI, and some of them have integrated mcu's(8051's but with small rom's so not much room for code), and it is still a possibility that I might jump to another rf interface.
I had also considered the RFM69HW but going for two chips will use a bit more power, but sub Ghz would give me tons more range, and I dont really need a mesh network between my sensors and the base station, but that would involve re-designing everything from scratch and scrapping a ton of code that is kinda dependant on the way the network works. -
Your smd antenna is intended for placement close to ground plane for compact short range (Bluetooth) devices so 8m is perfect range, considering that it is not matched or tuned. On your re-design avoid "dead copper" on pcb. The antenna need more ground to have good efficiency.
Personally, I do not like "combo" (MCU+RF) solutions, because is not clear availability in future. BTW, now Atmel is part of Microchip.
I prefer separate radio that could be selected according to related case. For instance ANSEM (now ON Semi) AX5043 or AX5243 cover range from 27MHz to 1050MHz and can be used worldwide. Lowering frequency increases range and decreases wasted power.
-
That is one interesting chip!
Will save that references.
I might/most probably will re-spin this project with that AX or some CC and a cortex M0 or M3.
I know that Atmel was bought by Microchip..
I followed the recommendations from the antenna datasheet, for now I will go the uFL and a Molex patch antenna(just like the laptop one) and call it a day..
I would prefer doing it the correct day and match a decent antenna, but no VNA or anything that can do 2.4Ghz or even near that, so I will do it a bit half assed
-
With AX, you can use EU 169MHz band that is intended for smart metering and 1/4 wavelength vertical antenna even without matching.
-
Well, turned them around, and the result is the same, around 8 meter line of sight range
There is still something wrong with the antenna, soldering or tuning. I've seen 100+ meters range obstructed (but not directly interrupted) by walls from chip antennas. -
As expected... Try with piece of 1/4 wavelength long wire instead of pcb antenna. If your sensor node will not move consider directional antenna. And if you need long range why 2,4GHz band was selected?
I once did exactly that with an Ackme wifi module on an OSHPARK PCB and got very good results. Starting with a longer wire, about 2 inches long, and cutting it in small increments while monitoring the s/n ratio reported by the module.
-
Why not simply follow the reccomended layout for FR-4?
http://www.atmel.com/Images/Atmel-42131-RF-Layout-with-Microstrip_Application-Note_AT02865.pdf
NO SOLDER MASK over the microstripline and areas < 2 mm close to it. Connect that strip directly to an SMA connector and use small coax for antenna connection, all 50ohm.
-
Why not simply follow the reccomended layout for FR-4?
That layout is for 4 layer board. There is not much you can do on a 2 layer board to do proper impedance matching.
But for the original design, note how grounds are routed under the balun (note the split ground). -
Why not simply follow the reccomended layout for FR-4?
That layout is for 4 layer board. There is not much you can do on a 2 layer board to do proper impedance matching.
But for the original design, note how grounds are routed under the balun (note the split ground).
Yes, but in their layout they only care about layer 2 ground plane:
"Copper pour on Layer-1 with ground stitching vias is a common practice in RF layout. For microstrip designs the copper
pour on layer-1 should be kept away from the transmission line. The underlying Layer-2 ground plane needs to be the
dominant ground reference to minimize variables. A keep-away distance of 4x the dielectric thickness will reduce the
parasitic effects of copper pour to less than 1%. In other words the gap between the microstrip transmission line and
copper pour on layer-1 should be 40 mils or more. "
So I think this design will work for 2 layer FR-4 assuming of course that bottom layer is ground.
-
As expected... Try with piece of 1/4 wavelength long wire instead of pcb antenna. If your sensor node will not move consider directional antenna. And if you need long range why 2,4GHz band was selected?
I once did exactly that with an Ackme wifi module on an OSHPARK PCB and got very good results. Starting with a longer wire, about 2 inches long, and cutting it in small increments while monitoring the s/n ratio reported by the module.
You could also try with two wires instead of one and feed them from the differential lines directly? No balun required.
Also the chip antenna datasheet shows a 1.5uH inductor that doesn't seem to be on your board. -
Yes, but in their layout they only care about layer 2 ground plane:
"Copper pour on Layer-1 with ground stitching vias is a common practice in RF layout. For microstrip designs the copper
pour on layer-1 should be kept away from the transmission line. The underlying Layer-2 ground plane needs to be the
dominant ground reference to minimize variables. A keep-away distance of 4x the dielectric thickness will reduce the
parasitic effects of copper pour to less than 1%. In other words the gap between the microstrip transmission line and
copper pour on layer-1 should be 40 mils or more. "
So I think this design will work for 2 layer FR-4 assuming of course that bottom layer is ground.
The dielectric is much thicker in a two layer board so you need impractically wide traces (and also keep-away distances) to get a good impedance match. -
Yes, but in their layout they only care about layer 2 ground plane:
"Copper pour on Layer-1 with ground stitching vias is a common practice in RF layout. For microstrip designs the copper
pour on layer-1 should be kept away from the transmission line. The underlying Layer-2 ground plane needs to be the
dominant ground reference to minimize variables. A keep-away distance of 4x the dielectric thickness will reduce the
parasitic effects of copper pour to less than 1%. In other words the gap between the microstrip transmission line and
copper pour on layer-1 should be 40 mils or more. "
So I think this design will work for 2 layer FR-4 assuming of course that bottom layer is ground.
The dielectric is much thicker in a two layer board so you need impractically wide traces (and also keep-away distances) to get a good impedance match.
True. I missed that. Looks like the microstrip on picture is about 20 mil, that implies ~0.28 mm thick FR4 (Er=4.80) to the ground. For 0.8 mm FR4 it will have to be 1.4 mm wide strip with 3 mm pull back. Yeah ... whole RF section layout need to be redesigned for 2 layer.
Maybe U.FL connector close to balun is better option in that case?
-
For RF a better option is to go with 4 layer board, even if you don't need that otherwise. And ask manufacturer for controlled impedance.
This helps a lot if you don't have proper equipment to do the tuning. -
I am not sure what senso is going to do after all. Perhaps it make sense to make small 4 layer breakout board and solder it on top of 2 layer if going 4 layer for entire design is not justified.
When people say "popper equipment" I wonder what do they mean specifically in cases like this? Thing is so tiny. Suppose I have 6GHz VNA and want to "tune it". How do I even approach measuring/tuning it? I sometimes solder pieces of RG405 with SMA connectors at other end right to the track, but here even that won't fit well.
Whoever has the "proper equipment" how exactly do you guys do it in cases like this? Please share. Even few photos would mean a lot.
-
I'm in TSA line, so I'll be brief. 6 GHz VNA is good to have, but 3 GHz will work as well.
There are reversible switch connectors. They look like u.FL, but disconnect circuit under test and redirect it to the mating connector.
If you have 2 boards, you can reverse direction if this connector, so you can independently test the antenna and the source.
Connector can be left on the board or replaced by a short for production units.
I don't have the name of this connector right now, but I can look it up later.