I have been using the NFC Inductance | RF Design | eDesignSuite | STMicroelectronics tool to design a rectangular antenna but I still needed those traces in KiCad… so I created a tool to make copper lines that augment a footprint.
KiCad Antenna Line Generator on GitHub
This seemed like the fastest way to develop and implement things. I’ll make a spiral one soon. Enjoy,
cool, but, why not a plugins?
-an
Did you just volunteer to help make that happen? 
Spiral tab is live as well as an inductance estimator… no guarantees on inductance but it serves as a good sanity check.
Did you have a look at what others have done before you? I have seen at least 4 different footprint generators for PCB inductors.
Before I knew of those, I wrote a similar python script myself. Not for PCB’s but for generating G-code for milling circles. In my own code, it does not use a real spiral, but it’s made out of half circles (each 180 degrees) with two different center points and ever increasing diameters.
Python is just one more step, although I did rip off some of nideri’s code: nideri/nfc_antenna_generator: generate nfc antenna module for kicad
Now you can download the footprint from the interface (or copy/paste). Your only dependency is a web browser and that GitHub is up: KiCad Antenna Generator
These generators seem to work directly from the command line. KiCad has several footprint wizards inside the footprint editor. These are also written in python (so you can easily use them as an example for your own.
One of the advantages of this method is that you can see the results directly in the footprint editor while you change parameters. And when you’re content with the result, you can add manual final touches in the footprint editor before you save the footprint.
@Piotr This antenna generator from nideri (or maybe this one fro gaidica) looks like something you are (were?) interested in. Although nideri (Back in KiCad V5 in 2019) had the same problem with pad connections.
@gaidica How did you (if you did) resolve the shorted pad problem? The copper loop of the antenna shorts the pads (not shown (yet?) in your screenshot). The best method I know is to define the footprint as being a net tie. This suppresses DRC messages because of “shorted” pads.
This was just an exploration, I wouldn’t take it too seriously. Making this a footprint wizard seems like a great idea–I was a bit shocked it’s not out there already. Defining a net is how I’ve done it, too.
FYI - I made an Antenna/other generator and built a FreeCAD plugin for it. Then, did it for a Kicad plugin. They worked fine but, there was very little interest so I did not persue further.
That work was inspired by Inkscape and FreeCAD and, given they both have abilty to do some form of that shape (and push out DXF for Kicad use) and, that I don’t need Anntenna’s, I bailed out. Mine included placing Vias along the Track (also inspired by FreeCAD and it’s Parametric-FP plugin).
I use the Parametric-FP plugin for Coil-Footprint Step files in Kicad.
All that aside, below shows Inductance calc for a Spiral track; it’s inductance is pretty accurate (considering how variable inductance can be depending on a host of things). It’s a single track that Kicad breaks up into segments, thus, the quantity of 1024 tracks measured.
No.
At the end of 90s and beginning of 00s I have been doing some experiments with such antennas for RFID 125kHz but we ended with antenna made of wire ordered from coil winding manufacturer. We use one such antenna and need not more.
In app notes about 13.56MHz RFID I have read that antenna should be as symmetrical as possible. It is to minimize common mode electrical emissions which are sources of unwanted disturbances emitted by readers. So my antennas start from both ends with wire at the outermost circle. Then they are crossed at the opposite to its ends place and going back at next inner circle and so on.
With KiCad V5 I made short at schematic with wire looking like antenna coil. Then I made antenna (those time rectangle using standard tracks) directly at PCB.
Last month I found that with V8 I am able to make footprint of antenna defining it as net-tie.
The coil has end pads numbered 1 and 2 and all vias (for crossing) made as THT pads that get number 3. The wires are the graphic arcs (not converted into pad or track). I have defined 2 such antennas - one round and one rectangle with a shape exactly as this one made with V5 at PCB and I replaced it there.
For electric field shield I have added pad 0 but the shield is made later at PCB as filled zone (in footprint I have only graphic lines to follow with filled zone.
On the way I discovered that net-tie pad sets can contain set consisting only one pad number (have to use it when I tried to make electric shield with graphics connected to pad 0).
Here are Rectangular and Circular Antenna Footprint Wizards: Neurotech-Hub/KiCad-Plugins-8.0
Minor pain but I think it’s the right way to do it. Thanks for the good discussion and insights.
It’s been a while since I last looked in the Plugin and Content manager. It’s got 79 plugins (and libraries) now. And two “Coil Generators”.
In my short experiment I could not get the PCB Coil Generator to work, but the KiCAD Coil Generator installs as a few footprint wizards and that one does appear to work in KiCad V8.0.3
I was able to tie nets in the Javascript generator by adding the line: (net_tie_pad_groups “1,2”)
I still can’t get that to work in the Wizard. For now, there is documentation in Neurotech-Hub/KiCad-Plugins-8.0 for doing this for the footprint via Footprint Preferences.
This is my plugin and I really have to release the update. The issue you’re having is because of a paste-hack I implemented that is kind of janky and straight up doesn’t work at all on Linux. It is fixed on GitHub, I just have to push it to the plugin store.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
