holesflow:
That's a neato PCB, Paul! It's like a project board with radio built in, right?
Yes, it is a sensor node using LoRa radio for use on TTN or similar. The prototype area allows the user to choose type of sensor.
PaulRB:
Yes, it is a sensor node using LoRa radio for use on TTN or similar. The prototype area allows the user to choose type of sensor.
Just curious... How does that radio do against others you've tried? I have a few sitting around that i never used. I do know the range/ etc. of tbe nrf24... I need to make similar to get rid of my breadboards scatteted around the house!
With the RFM95 @ 868MHz, I got 20-30m in a building and a few hundred meters to a kilometer outdoors with spring antennas.
Compared to the nrf24, it is a completely different league.
Data packets from my prototype LoRa sensor have been picked up 11Km away. But that was by a proper LoRa multi-channel gateway with a high gain outdoor antenna. The sensor's antenna is just a length of wire. My self-built single-channel "gateway" doesnt seem to be able to pick up signals from the same sensor at more than a few tens of metres, about the same as WiFi. I suspect the antenna I have on my single-channel gateway is rubbish. It was sold as 868MHz and claimed a 3dB gain, but it arrived in a plastic bag with no labels on it and looks identical to the 2.4GHz antennas sold for use with WiFi routers.
PaulRB:
It was sold as 868MHz and claimed a 3dB gain, but it arrived in a plastic bag with no labels on it and looks identical to the 2.4GHz antennas sold for use with WiFi routers.
The 868MHz antennas I got from Aliexpress are much longer than most wifi antennas. They work for my rfm69 MySensors network, with a longer range than Wifi. I use them on the gateway. All the sensors and the test equipment for the rfm95 use spring antennas and it works fine. If I did the calculation correctly, at max power, more than a spring antenna isn't allowed in Europe anyway, at full rfm95 transmission power.
ElCaron:
The 868MHz antennas I got from Aliexpress
Can you post a link please ?
Thanks, I've ordered the sma antenna to try
Don't forget to take care of trace impedance to the SMA connecor.
How? I am trying to keep the PCB track between the LoRa module and the sma socket or wire antenna hole as short as possible. What else should I do?
PaulRB:
Thanks, I've ordered the sma antenna to tryHow? I am trying to keep the PCB track between the LoRa module and the sma socket or wire antenna hole as short as possible. What else should I do?
Set trace width, distance to groundplane to the sides and groundplane on the bottom such that you get a trace impedance of 50Ohm: CPW (grounded) line calculator - Spok Technologies Inc
Use a line of vias on each side to connect he side gp o the boom gp. I usually put a ground fill area with adjusted settings around the trace.
Thanks. So I need to find out the PCB thickness and dialectic constant, and the track height that easyEDA offer, then I can adjust the antenna track width and clearance to get 50R using the calculator on your link.
he side gp o the boom gp
Sorry, you lost me there! Did you mean "the side ground-planes to the bottom ground-plain"? I guess I am trying to form something similar to a coaxial cable using the tracks, vias, ground planes and substrate.
From easyEDA's basic board offer:
Height = 1.6mm = 63mil
Thickness = 1oz = 1.4mil
Substrate = FR4, so I'm assuming dialectic constant ~ 4.5
I get ~50.8R impedance using track width 24mil and clearance of 5 mil.
Am I doing it right? Feels like a very wide track and very narrow clearance!
Co-planar? ie is there an earth plane underneath? And FR4 is normallly Er 4.7 - 4.8. Check with your PCB supplier.
It all makes a difference
Draw us a picture of your transmission line and we'll figure out it's impedance - or there are plenty of calculators on the net. Microwaves101 is an excellent source.
What frequency are you at? above about 5GHz FR4 is rather lossy.
Allan
Thanks Allan, yes, ground plane on underside of board, 868MHz LoRa. I am using the calculator posted by ElCaron in post #43 which suggested FR4 was 4.3-4.8 so I took the mid point.
easyEDA's spec says
2 Layers
FR4,1.6mm,1 oz,HASL,Green Solder Mask,White silkscreen
Here is the topic I started asking for help. @ElCaron @allanhurst would you mind reviewing it? The exported .jpg picture from easyEDA is not the best representation, but you should be able to see what I'm attempting. The antenna connection is bottom right.
All I see is a picture of a via.
You have to reckon this as inductor of 0.2 - 0.5 nH depending on the hole diameter, length and plating thickness. It's bad practice to use them in series with an antenna because of this variability . If you want an earth use many in parallel or eg a fan terrnination over an earth plane.
Keep everything on one layer.
I'll have a look at your link and get back to you.
edit : had a look, and it's irrelevant.. Correction? /edit
You can model this sort of stuff with eg HFSS and Sonnet etc , but the seats aren't cheap. and they're not easy to use.
Allan
For Microstrip - ie a track over an earthplane, FR4 thickness = 1.6mm, Er = 4.7, track thickness = 0.14mm,
the width for 50R impedance is about 2.8mm .
Keep other tracks at least 5mm away from this.
Allan
allanhurst:
All I see is a picture of a via.
That's just an illustration of the construction of the basic board type that easyEDA/jlcPCB offer. They also offer 4 & 6 layer, more expensive, of course, and there are similar illustrations of them on this page.
allanhurst:
I'll have a look at your link and get back to you.edit : had a look, and it's irrelevant.. Correction? /edit
Do you mean because the connection between the ANT pad on the RFM95 module and the hole for the antenna is so short that I don't need to worry about impedance matching?
For Microstrip - ie a track over an earthplane, FR4 thickness = 1.6mm, Er = 4.7, track thickness = 0.14mm,
the width for 50R impedance is about 2.8mm .
because the connection between the ANT pad on the RFM95 module and the hole for the antenna is so short that I don't need to worry about impedance matching?
I've been wondering about that since I got depressing results from impedance calculators for a TI CC3000 board I was thinking of making. The spacing between pins of the module wasn't enough to fit the "correct" trace width, and the actual traces were shorter than the 0805 components that were supposed to go in there (and much shorter than the traces that made up the PCB antenna itself. Did that mean I shouldn't bother, or did it mean that I was doomed (and needed thinner or more exotic PCB materials)?
At those frequencies it won't be too critical. Only when you get to a few GHz+ do things start to get really fussy.
The package of the IC and of other components will alter the impedances, but if you just copy exactly a recommended design these things will have been taken into account.
Even passives aren't what they say on the box at high frequencies - you have to download S-parameters from the manufacturer or measure them yourself. And mounting pads have to be included as well.
If you want to do it from scratch you will need a simulation package such as HFSS and a fair amount of knowledge/experience. RFSIM99 is available free on the net, but it's very limited.
Allan