I know nothing about this area. I need a 50Ohm antenna for 868MHz. My understanding is that the antenna needs to be 86.3mm long. I used the calculator here
Here is what I have so far. I am constrained by the board size. I’ve added a keepout zone around the antenna to both front and back copper layers. Ground copper pour will be outside of this. No other tracks added yet. Where the antenna connects to the SMD pad I have used a thinner track width of 90 mils so that the rounded end of the track doesn’t get too close to SMD pad 2.
When I drew the track KiCAD said that it was 86.2xx mm long. After completing it and selecting it it says it is 88.796mm long. Is that a problem? If so how can I edit the track without deleting the entire thing and starting again?
I plan to add stiching vias along the edges of the ground copper pours that will border the keep out zones.
My design isn’t super-critical in performance. LoRa is supposed to go up to 12km, I need 100ft. However I would like to avoid any unnecessary errors. Many thanks!!
No, that wont work. You’re using microstrip calculator. It assumes ground plane underneath. So field distribution will be different. Also impedance at feed point doesn’t guarantee that it will radiate effectively. If this is all the space you have, I would suggest using ceramic chip antenna.
Not by using tracks. You can create your antenna as a footprint and use pads there or you can use copper zones.
In nightly you can use polygon pads to make your life easier. In stable you could use svg2mod to import your required antenna shape as a polygon (not editable from within the footprint editor of the stable version.)
Absolutely no ground plane copper under the antenna. jcyrax just noticed that you’ve used wrong calculation for the track impedance in this case.
Without proper knowledge/experience and sophisticated tools, you won’t get even close to a reasonable antenna.
Two solutions: ceramic chip as jcyrax suggested, or closely follow one of the working PCB antennas. Keep in mind that the ground plane and antenna surrounding will play a huge role as well.
Some examples: http://www.ti.com/lit/an/swra351a/swra351a.pdf
Just closely follow the antenna mfr recommendations. Also I see that your antenna is tied directly to the radio module, that’s not the right way to do it. Put some components for matching network, which will also make RF measurements easier. Like shunt-series-shunt at a minimum.
It already has the impedence matching network on it and it seems the only part I need to add is a 50Ohm antenna that is 86.3mm long.
In their test they used a piece of wire directly connected to the module and achieved long range comms.
So back to what I originally did, how can I implement an equivalent but using a PCB trace? Or can I follow the layout provided by the ceramic antenna mfr but omit the pi network?
I suggest you use ceramic antenna, but insert PI network. Try to match suggested design as close as possible. Then on first prototype short pi network with resistor or appropriate capacitor. If your range is acceptable then ok. If you have problems measure antenna impedance and add matching.
If you use PCB antenna liek monopole, you can create it in free space length and then trim, but you will need some measurement equipment. Also, you can’t just fold it in small space. Length is not only parameter here.
Actually, a piece of wire of a correct length, assuming proper ground plane exists, makes a pretty good antenna. Folded PCB track will almost surely be poorly performing, the problem is with real compact devices to fit reasonably large antenna with reasonably extensive ground plane. All compact antennas are more or less trade-offs.
Check out e.g. johansson’s ceramic antenna: https://www.johansontechnology.com/datasheets/antennas/0868AT43A0020.pdf
1)The part that is off ground plane should be exactly as in datasheet.
2)Change feed line to grounded coplanar wave guide. You will need it for PI network anyway. Use KiCAD calculator to get gap width.
3)Try to orient module so antenna feed is shorter. Maybe set antenna to right side of PCB.
