I am trying to design my own Business Card with NFC capabitilities following these two tutorials:
Everything is quite simple until they reach a point where they links to a PCB antenna called class 4-5-6 which are given by the manufacturer NXP in this zip file in an Eagle format:
I’m unable to find any way to convert these eagle files to KiCad or find any libraries or png to follow and trace tracks using it as a clutch, and that is why I’m coming here.
Does anyone know any way of easily converting this eagle files? Or can find any dxf file or something to follow with a copper track?
Thanks in advance
I hereby certify that I am not simply asking someone else to design a footprint for me.
This is an auto-generated message that is in place on the “footprints” section of the KiCad.info forum. If I remove it and ask for a footprint to be designed anyway, I understand that I will be subject to forum members telling me to go design my own footprint or referring me to a 3rd party footprint site.
I may not have fully understood your request… But, let’s say you know the dimensions for the antenna’s shape and want to make copper traces of them, there are a handful of ways to do it.
The way you do it will dictate the usefulness of the result and the required next steps.
Others can provide info on Plugins to use Eagle files.
Drawing Options include: #1) Draw the traces in PCBnew #2) Draw shape in PCBnew on a layer such as Silk, Dwg, Eco…etc and convert them to desired Cu layer #3) Draw shape in your favorite drawing program, save as DXF or PNG.
DXF can be imported directly into PCBnew (and Footprint editor). PNG can be loaded into the BMPtool (in Kicad’s main panel), then exported as .MOD (that makes it a Footprint)
The choice of options above dictates the next steps…
Can trace Cu over the DXF or PNG.
Example shows using a screenshot (thus, a PNG) loaded into the BMPtool and exported as .mod. Then, .mod loaded into PCBnew and traced in Cu layer (I did not fuss with trace-width but, you get the idea). I could have converted it to Cu instead of tracing.
If drawing exact geometry in external program and saving as DXF, you can import into PCBnew and convert to Cu layer…
from the zip file you can get the gerber of the antennas… from the gerber with gerbview you can create a kicad_pcb board with traces and drills generated from the gerber themself…
(moreover in the zip there are eagle brd files… if you have eagle or you are in touch with someone can save from eagle bin to eagle text format, you can directly import the brd in kicad).
Note use kicad 5.99 daily with caution
Hi,
I’ve attached three antenna designs which I’ve downloaded from NXP in Eagle format and imported into Pcbnew. I’ve made some minor adjustments to the Class 6 design and used it myself. I’ve also included my own modified footprint.
I’ve used this design together with an NXP NTAG I2C (NT3H2211W0FTT). To get the best performance from the antenna I used a 18 pF capacitor in parallel with the antenna on my board.
Reading your post again (just read it briefly on my phone before) I do realize that this doesn’t really address what you’re asking for.
I believe that I found the exact same files as you did. If I remember correctly, these files are in Eagle binary format. I had to download Eagle (don’t remember if it was a free version or some trial). I then had to open the files and save them to Eagle XML format. These files can be easily imported into Pcbnew.
Ether way, I hope you don’t have to do what I had to do since I attached the files in Kicad format.
Drawing Options include: #1) Draw the traces in PCBnew #2) Draw shape in PCBnew on a layer such as Silk, Dwg, Eco…etc and convert them to desired Cu layer #3) Draw shape in your favorite drawing program, save as DXF or PNG.[/quote]
Thank you in the end I drew them “manually” as you explained in your post, it took me around 5 minutes and the corners weren’t rounded, but it will make ends meet.
Thank you, seems like a very useful python script.
maui:
from the zip file you can get the gerber of the antennas… from the gerber with gerbview you can create a kicad_pcb board with traces and drills generated from the gerber themself…
(moreover in the zip there are eagle brd files… if you have eagle or you are in touch with someone can save from eagle bin to eagle text format, you can directly import the brd in kicad).
Note use kicad 5.99 daily with caution
I’m not sure if you have tried extracting the files from the zip and trying to read them with Gerbview. Every time I tried to import them in gerbview, I was getting errors. Same thing while I tried to read them in PCBNew. Am I missing something?
Albin:
Reading your post again (just read it briefly on my phone before) I do realize that this doesn’t really address what you’re asking for.
I believe that I found the exact same files as you did. If I remember correctly, these files are in Eagle binary format. I had to download Eagle (don’t remember if it was a free version or some trial). I then had to open the files and save them to Eagle XML format. These files can be easily imported into Pcbnew.
Ether way, I hope you don’t have to do what I had to do since I attached the files in Kicad format.
Thank you so much Albin! The files work great and will definitely use them in the v2 of my board.
So you first imported these files in Eagle, converted them to Eagle XML, which KiCad can read. Right? I have tried importing the original zip files into KiCad first and I was running into errors
