nrf24l01+, pcb mifa antenna design

RE: nrf24l01+, pcb mifa antenna design

QuangCN — Tue, 28 May 2024 12:51:53 GMT

Hi there, i'm currently working on the same project as yours. I just wonder if your board can work?

RE: nrf24l01+, pcb mifa antenna design

AmbystomaLabs — Fri, 24 Jan 2020 14:02:07 GMT

Yeah, that is a drag that you got the footprint wrong on the crystal. Always pay close attention to whether the spec's show bottom view or top view for the pins.

That's probably a good place to start with the communications issue. The extra wiring from flipping it over will change the load on the crystal and alter the resonant frequency. You can easily tune it back to nominal but you need some sort of spectrum analyzer to figure out how much the RF carrier is off. There are cheap WiFi module based spectrum analyzers out there. Normally around $100. Alternatively you can output HFCLK/2 through gpio and try to measure its frequency with an o-scope. The problem with this is most o-scopes have lousy oscillators and you need to get the nominal frequency to +/-40ppm for BLE.

Once you get that fixed you should verify the RF power output. Easiest way is RSSI at one meter. Just put it in a link with a smartphone or something and look at the RSSI. If you thumb around on the devzone you should find what people expect it to be for that chip.

RE: nrf24l01+, pcb mifa antenna design

JoE1205 — Fri, 24 Jan 2020 08:13:40 GMT

Hi guys,

so i soldered everything as good as Im able to, anyway the communication with this module is very poor.

For me there are 2 possible reasons:

-----------------------------------------------

1. Crystal:
While soldering I noticed that the wiring for the crystal is wrong, so i had to solder it upside down onto the pcb ( isolated from it so the is no unintended connection between pcb and crystal). Im not sure if this affects the RF connection.

2. My solder skills are to bad. I tried to check every connection direclty after soldering a component. Anyway the size is a big problem, so its hard to be sure that I get in touch with the pins of the components.

-----------------------------------------------

I assume that the design with the fixed crystal is correct, anyway the communication with this module is very poor. I rarely get a full functional connection at all, atleast sometimes its working. Most of the time I dont get a connection. Sometimes just for a millisecond.

RE: nrf24l01+, pcb mifa antenna design

JoE1205 — Wed, 04 Dec 2019 10:19:37 GMT

Oh no, thats just the changed grid.

RE: nrf24l01+, pcb mifa antenna design

AmbystomaLabs — Tue, 19 Nov 2019 15:34:58 GMT

Something funky happened in your app when you removed the copper pour. It looks there are little dots of copper all over maybe even shorting some of the pads. Almost looks like a remnant of a hatch pattern.

RE: nrf24l01+, pcb mifa antenna design

JoE1205 — Mon, 11 Nov 2019 11:06:32 GMT

RE: nrf24l01+, pcb mifa antenna design

AmbystomaLabs — Thu, 07 Nov 2019 14:48:53 GMT

And so JoE1205 is clear on this, you remove the ground pour on just the top layer (not the bottom layer) and only in that little rectangle. You'll have to remove those two ground vias in the rectangle too.

RE: nrf24l01+, pcb mifa antenna design

AmbystomaLabs — Thu, 07 Nov 2019 14:22:58 GMT

Good catch! I had forgotten you did that in the reference design.

RE: nrf24l01+, pcb mifa antenna design

AmbystomaLabs — Thu, 07 Nov 2019 14:15:16 GMT

Actually it's pretty easy if you don't use a soldering iron. Ideally you never ever use a soldering iron with SMT parts. The thermal stresses from the iron can easily cause the parts to crack and this creates some really difficult to find failures.

Easiest approach is just buy a stencil and paste the board, then hand place the parts and use a hot air reflow gun.

You can get the hot air gun for about $150. You need a good set of fine tweezers (digikey or mouser carry these), you need a syringe of type 3 lead free no-clean paste (chipworks on mouser or digikey). I normally preheat the board to 100C on a cast iron hotplate on its lowest setting with a nonstick surface. Then reflow gun with low airflow set to about 320C and just work it till you see everything flow and center.

You can get an inexpensive stencil here: https://www.oshstencils.com/

For this board you can probably do a polyimide stencil, but most of my work is finer pitch so I generally go for the stainless steel stencil. You will have to create the windowpane pattern for the nRF in you ECAD software everything else can probably use the mask or copper pad layer for the stencil pattern.

You can get a very nice reflow gun here: https://www.sra-solder.com/

The Aoyue brand is very reliable.

If your eyes are still good you should be able to place the parts without a microscope. Though an inexpensive stereo microscope on a boom is an invaluable tool for electronics work.

This company has high quality and inexpensive scopes: https://www.amscope.com/

I still hand place all my prototype boards and most of the stuff that has to go through certification. I can easily build up a complicated board in an hour to two vs. a week for a quick turn CM and I do it at a fraction of the cost. Once I prove out a design then I can turn it over to my contract manufacturer.

RE: nrf24l01+, pcb mifa antenna design

ketiljo — Thu, 07 Nov 2019 14:04:26 GMT

Remove some of the ground plane around the matching network components to reduce capacitance to ground, like this (inside the black rectangle)

Then you're good

RE: nrf24l01+, pcb mifa antenna design

JoE1205 — Thu, 07 Nov 2019 10:32:47 GMT

I adjusted the width of all traces to the pads width without spacing violations.

Thank you so much for guiding me through this.
Not really looking forward to solder this since 0402 is really painful.
Anyway I going to give reply when everything is tested and working perfectly obviously.

RE: nrf24l01+, pcb mifa antenna design

AmbystomaLabs — Tue, 05 Nov 2019 17:44:37 GMT

Looks good. The only thing left is the traces between RF components are rather narrow. Now sometimes this is by design or sometimes it is just impossible to have characterized traces between the RF components or sometimes it just doesn't matter since the whole thing gets matched anyway.

On the reference design the traces between the components on the nRF output match look to be about the same as the pad width. This is a pretty standard practice that gives a less inductive trace while still meeting the trace/space spec for the board.

Anyway, if you feel they are close to the reference designs for both the antenna and the nRF then run with it as is, otherwise I would fatten them up to closer to the width of the pad as long as you don't create spacing violations.

After that make sure your DRC rules match your board vendors spec and run with it. Looks fine to me.

RE: nrf24l01+, pcb mifa antenna design

JoE1205 — Tue, 05 Nov 2019 15:47:25 GMT

More stitches and all without thermals, including crystal and nrf pad (managed to include 9 vias.)

RE: nrf24l01+, pcb mifa antenna design

AmbystomaLabs — Tue, 05 Nov 2019 14:22:37 GMT

You need to turn off the thermals on the vias. There should be a selection in your software that says something like "flood over vias". Only plated thru holes for leaded devices get thermals since this makes soldering easier.

You can stitch under the crystal too.

You forgot to put vias under the nRF. Not sure how many you can fit by looking at it. But an X of 5 vias should probably be sufficient. Just make sure the annular rings are well inside of the edge of the pad. Then you let them flood with mask on the bottom layer and that effectively tents them.

I normally also place a via directly behind or next to all shunt RF components. The farther the ground via is away the worse the phase relationship of that part is to an ideal model. If the ground is close by then the matching solution is a little more predictable.

RE: nrf24l01+, pcb mifa antenna design

JoE1205 — Tue, 05 Nov 2019 11:51:09 GMT

Okay, changed the wrong footprint, edited the gap, added alot stitches by hand since I dont know a feature in Eagle for that. Result below.

RE: nrf24l01+, pcb mifa antenna design

AmbystomaLabs — Thu, 17 Oct 2019 14:19:12 GMT

Sorry for the late reply. I saw your initial message then got swamped with work and it kind of got lost.

Your impedance calculations are similar to AppCad. AppCad shows both designs closer to 45 ohms and to get it to 50 just make the gap width 0.14mm ( 5.5 mil). Actually above 5 mil will make your board cheaper since smaller than 5 mil is generally a more expensive process.

It doesn't really matter if you do 4 layer or 2 layer. You have room for the stripline so I would go for 2 layer since it is cheaper. You should stitch your groundplane more. Most eda packages have a utility that will automatically stitch the entire board with vias. Unless you stitch it the analog portions of the chip won't operate correctly.

You have the wrong footprint for the epad of nRF chip.

RE: nrf24l01+, pcb mifa antenna design

JoE1205 — Tue, 08 Oct 2019 09:59:46 GMT

Okay, that coplanar waveguide with ground results into realistic dimensions. Anyway could you please check my following designs regarding the feeding line. Im not sure about the correct positioning of the antenna components and about the calculation of the feeding line width.

I copied the basic desgin from the datasheet of chip antenna Johanson 2450AT18B100

The dimensions are not really very precise since its not clear to which edge of the components or SMD pads the dimensions are referring to. The position of the chip antenna is unclear aswell.

1. Design: 4 layer pcb

As you can see I guessed that the given dimensions referred to the middle of the smd pads. Im not sure if thats right.

Same dimensions for my second design, but different width of feeding line.

2.Design: 2 layer pcb

I calculated the feeding line with this calculator ( can not install new software on this computer since IT is making problems :( )
https://chemandy.com/calculators/coplanar-waveguide-with-ground-calculator.htm

My pcb supplier is giving this pcb dimensions:

This results into following settings:

2 layer pcb:

Dieelectric thickness matches core ("Kern") thickness (1200um)

4 layer pcb:

Dieelectric thicknes matches prepreg (140um) with layer 2-4 used as GND layers.

Do you think that these designs will work out?
By the way: Thank you very much for putting all the time into helping me

RE: nrf24l01+, pcb mifa antenna design

AmbystomaLabs — Tue, 24 Sep 2019 15:17:06 GMT

Generally the approach is to make everything 50 ohm characterized from the nRF to the antenna. On the antenna you follow the placement guidelines for its match components and on the nRF side you follow their placement guidelines for the nRF's match components. In this manner the absolute length of the strip doesn't matter since both ends are ideally matched to 50ohms. So you understand if something is matched to 50 ohms and you put it on a 50 ohm microstrip then it will always look like a 50 ohm device no matter how long that strip is. The only thing that happens with the length is you get a loss of power being transferred through strip. Thus you don't want it unnecessarily long. During transmit this would mean less power radiated out the antenna and during receive less power brought in from the antenna and poorer receive sensitivity.

The most popular microstrip design for small boards is as a coplanar waveguide with ground. Essentially you bring the ground pour as close as you can to the strip it then capacitively loads the strip along with the ground plane below it. Between the two you can get a fairly narrow strip that is characterized. Though I would say that most RF engineers just lay down the most compact design possible and just match the final solution. Characterized lines are not really necessary, but they are convenient when you are just lumping two solutions together.

The most popular app for calculating the CPW is AppCAD. It looks like broadcomm bought it from Avago (now keysight) so you can find it here: https://www.broadcom.com/appcad

RE: nrf24l01+, pcb mifa antenna design

JoE1205 — Tue, 24 Sep 2019 10:06:13 GMT

Okay I will try to design a second version with a chip antenna. Anyway Im going to test both.
Regarding the chip antenna, I still dont understand how to correctly choose the width and lengh for feeding line. When Im using calculators I get width of 3mm, using the parameters mentioned in my initial post. That feels so wrong and is way to big. And in every datasheet is writen that you have to design the feeding line to provied 50 Ohm impedance.

For example: Johanson 2450AT18B100 (www.johansontechnology.com/.../2450AT18B100.pdf)

RE: nrf24l01+, pcb mifa antenna design

AmbystomaLabs — Fri, 13 Sep 2019 14:44:32 GMT

If your goal is 3 meters then you should just use a chip antenna. Both TDK and Johanson have multiple 2.4 GHz antennae that have reference designs to give a 50 ohm input. They will have several versions and each has a different ground plane and feed orientation. Just choose something that looks right with your design. Instead of your massive monopole, a chip antenna might occupy 4mm x 6mm. In this manner suddenly your screws and 10 pin smt aren't an issue since they will be very far away from the antenna.

Regarding your comment above on free ground plane, just increasing the size of a ground plane doesn't necessarily improve an antenna. All antennae are designed with a particular size and orientation of ground plane in mind. The ground plane both serves to load the antenna to get it to match better and also controls the radiation pattern. So if a design shows no ground plane on 3 sides and a 30x40mm ground on the feedpoint side then ideally yours should look the same. What makes most of the chip antennae nice to design around is that many are created for designs that have ground on 3 of 4 sides and the ground size often conforms to many common requirements. On the TDK site they even have a tool that will let you estimate your antenna response when you change the ground shape to accommodate your design needs.

RE: nrf24l01+, pcb mifa antenna design

JoE1205 — Fri, 13 Sep 2019 10:39:54 GMT

I can not move the 10 pin part at the moment. Anyway I could make the ground free plane bigger, so there are only this 4 lines on the left side of the 10 pin SMT part. This should improve the performance right?

Regarding the mounting holes: Im not using metall screws or any metal parts for the housing. I could remove the hole on left, since it is not that important for mounting anyway. By doing this, I could replace the the complete antenna/nrf package and could move it out of the 10 pin part.

Furthermore I only have to transmit data to a receiver within 3 meters range , so I dont need some extraordinary long range connection. I guess this will work out even though the pcb design has some weaknesses.

RE: nrf24l01+, pcb mifa antenna design

AmbystomaLabs — Wed, 11 Sep 2019 14:12:30 GMT

That 10 pin SMT part and its associated components should really be behind the ground plane (ie, picture a vertical line running through the feedpoint of the antenna. Everything to the right of that line will be ground or ground and circuitry to the left should be antenna and nothing else). The SMT part moves the effective ground plane closer to the antenna and will change the antenna radiation characteristics, passband and impedance significantly. Similarly, that hole next to the antenna for a mounting screw is a big concern. If you mount to plastic and use a plastic screw or plastic snap then it will be ok as long as there is no copper on that hole. But you can't have any metal there. Even the plastic will change the tuning a bit.

RE: nrf24l01+, pcb mifa antenna design

JoE1205 — Wed, 11 Sep 2019 13:32:47 GMT

Hi,

i implemented everything in my current project, but I had to do some change since the size of the antenna is quite big related to the rest . Actually Im not sure if this layout is still fine.
So what I did:
-Antenna is on bottom layer
-all components on top layer
-connection of antenna to components via via-in-pad of closest component
-changed the place of the crystal

GND-Plane is not implemented yet

RE: nrf24l01+, pcb mifa antenna design

Øyvind — Thu, 15 Aug 2019 11:05:57 GMT

Hello, and welcome back!

This is starting to look good.

[quote user="JoE1205"] Anyway Im unhappy with this huge empty space on the left. I guess its okay to reduce the size, but Im unsure about the holes. Is it okay to remove them completely and basicly cut everything whats not needed on the left?[/quote]

The open area on the left should be used to add pads and/or GPIO pins for physical connection to flash/program/debug. Ref. the reference design I referred to in this comment, the image shows that there is a connector placed in the left side of the board. The holes which you mention are via-holes and are used to connect and ensure that the GND layers are connected.

I recommend that you remove the vias and finish your layout with components, GND-plane, and traces. Then send the layout to us, and we can help with adding vias. Have a look at this tutorial on Eagle from Sparkfun, and our tutorial on RF design.
Kind regards,
Øyvind

RE: nrf24l01+, pcb mifa antenna design

JoE1205 — Thu, 15 Aug 2019 09:29:19 GMT

Hey guys, Im back 🙂

the current state of me trying to copy the design is the following. I designed it as a design block in EAGLE in order to import it into my project later. Thats why GND-plane is not implemented yet.

Had to find an other crystal which fits the requirements mentioned by AmbystomaLabs.
So far the GND-plane is planned for the dotted area, whereas the antenna is planed to be free of GND or any other signals on top and bottom layer. Anyway Im unhappy with this huge empty space on the left. I guess its okay to reduce the size, but Im unsure about the holes. Is it okay to remove them completely and basicly cut everything whats not needed on the left? By the way: Whats the intention behind placing all the holes? Whats their use? I cant find a clear pattern so for me it looks very random. Do I need some more holes to seperate the antenna from the rest of the pcb, which is not shown in the picture? Still learning about the whole RF design topic and I very appreciate all your advices.

Thank you :)