ESP32 Forum

Hi,

I have developed a custom PCB usingn the esp32 s3.

I have a reference devboard with the same chip, that i tried to copy the antenna design from. Unfortunatly my antenna doesnt seem to work, since i cant detect a wifi signal.On the reference board (LilyGo-T-RGB), the same code works fine and i get a strong signal.
I would like to request help on how to troubleshoot the design and why i am geting absolutly no signal at all.

C5 and C7 are 3.3pF, while L1 is 2.2nH

My crystal is HY40MSMD3225GB1R30 and i have connected it to 12pF (c31,c32) and L2=24nH

Using 3.3V LDO with less then 5mV swing measured

Thank you for your help.

Goes everyone is struggeling with this one.

Generally, RF is hard. The antenna trace is dependent on more than just the shape: the characteristics involve not only the shape, but also the copper thickness, the thickness of the PCB under it, hell, even the direction of the weave of the FR4 plays a role. Normally you'd simulate the PCB to make sure you're getting the correct impedance on a given substrate, then have the pcb manufactured with that particulat substrate and stackup, and finally tweak the capacitors and inductors using some VNA setup. Given all that, I doubt anyone here will be able to just tell you what's wrong. (Also note that that is one reason why we're also selling modules with built-in antennas: that means you don't have to do all that anymore.)

Thank you for the reply and the tips.

I undestand that it is hard, but we are doing it because we need the extra gpio that the chip provides and also the cost sensetivity of the product. Could you provide some help on how to measure the impedance or the rf performance without any specialised tools?

I am basing this design entierly on an existing working dev board where the wifi works but so far no luck.
The pcb thicness is the standard 1.6mm 1oz 2-layer copper from jlcpcb
I can provide all the info anyone needs, but i dont know in what direction i should start troubleshooting this. Who could i turn to for help with designing the wifi part?

This is the scheamtic of the crystal if this helps at all

Please check this below topic. Seems similar to your case.
viewtopic.php?f=12&t=41564

If we assume your antenna has a 50 ohm impedance, then your matching network can be wrong. I think the transmission line isn't exactly 50 ohms. It should be very thick for a 2-layer board. Nevertheless, the length is short, so acceptable. And C5 and C7 should be on top of the transmission line without those stubs. But again the length is short and they are acceptable. So check the values of C5, C7 and L1 first.

Additionally, the left most ground plane is not good for the antenna. Try to place the antenna on the edge of the board. And move the chip along with it.

Maybe, antenna doesn't have a 50 ohm impedance. Usually, it is good to do simulations before ordering the prototypes. You can include the antenna, PCB and the ground planes as geometries and run a simulation with an EM software. I can recommend openEMS since it is an open source software. But iterating the simulations may take time longer than the PCB layout itself.

After having the prototypes, you can use a VNA to measure the impedance of the antenna and optimize the matching circuit.

I don't understand the job of L2.

selcuk wrote: ↑

Thu Sep 05, 2024 7:23 pm

I don't understand the job of L2.

i think it should be a 0R
or if the crystal need impedanz can be a L too , depends on the crystal

i use 0R in one 40MHz test design to test different things ( SPI PSRAM speed .. )

hope this helps

best wishes
rudi

ales.kramzar wrote: ↑

Fri Jul 12, 2024 12:55 pm

I have developed a custom PCB usingn the esp32 s3.

I have a reference devboard with the same chip, that i tried to copy the antenna design from. Unfortunatly my antenna doesnt seem to work, since i cant detect a wifi signal.On the reference board (LilyGo-T-RGB), the same code works fine and i get a strong signal.
I would like to request help on how to troubleshoot the design and why i am geting absolutly no signal at all.

C5 and C7 are 3.3pF, while L1 is 2.2nH

Hi
check this tool
design your PI Networkmatch Design there with your data example taken from your thread


and fill in the Impedanz from your used MCU SoC and check the parameter -
check the Guide for more infos what the impedanz is for diverse MCU SoC
you can also add online there PCB parameters / other parameters and so on
you need to check the 50 Ohm Impedanz from side your design to the feed point,
then you need to check the 50 Ohm Antenna - S11 | S21 you can use for hobby a cheap mini vna
make a note on the PCB design for the PCB manufactur that the feed line is to
meet 50 Ohm transmission line ( 50 Ohm check ) so your traces need also a check
example 0.127 does not meet the 50 Ohm rule - from handfeel you need 0.350 - 0.370 and the right
space to the next GND , you need to calc this.

hope this helps

best wishes
rudi

ales.kramzar wrote: ↑

Thu Sep 05, 2024 9:58 am

Could you provide some help on how to measure the impedance or the rf performance without any specialised tools?

I am basing this design entierly on an existing working dev board where the wifi works but so far no luck.
The pcb thicness is the standard 1.6mm 1oz 2-layer copper from jlcpcb
I can provide all the info anyone needs, but i dont know in what direction i should start troubleshooting this. Who could i turn to for help with designing the wifi part?

This is the scheamtic of the crystal if this helps at all
crystal.png

ESP_Sprite did all say - it's not easy - you need an exactly step by step thing and the manufacturer need
to be inform, what your need is, this can be controlled then in the manufacturer.

But at first you need to check your traces, the space, the cooper free zone and so on
if you have your basics you can check for virtual all things, i will link to my last doing this last days..

- meet the 50 Ohm transmission line from MCU SoC to the feed point your antenna by calc ( smith chart online )

- meet the antenna power / reflection example by software tools **) example step 1 and the next final step 2

example: ( note the 2mm long trace is also a parameter which has 50.7 Ohm and i need for this a trace of ~ 0.380 -not seen on this picture- but the parameter )
thats a virtual calculated 99.99 prozent near perfect antenna. But the reality looks the most time different.
You need after the pcb comes

- check with vna the things what you did want
- if all ok, you can start solder, and check again
- if there is difference, you need to Match the PI network again with the VNA

there can be allways a difference design come and sometime SMT parts are not allways the same, so use
quality L for the feed line - not a nomame.

hope this helps to get closer the thing you have to do for a working ant design,
if you never did this i would prefer to use a ceramic ant by reference from manufacturer
not a printed pcb antenna - like ESP_Sprite tell you, it's not only the shape form, it's also
how this is "stacked" on the PCB and the material.

And yes, sometime you have a bad day - and nothing is working.
I can speak from my own, the SoC Soldering was bad or to hot reflow and so on.
All parts and steps has parameters - they change on every doing anything with them.

But if you have one time the right matching - never touch it again . never ! Never change the SMT Parts with cheaper things
If you get new PCB'S you need to start the procedure from start, when PCB comes to you from manufacturer.

best wishes
rudi

**) this is just a one of many tools you can use.

What is the Impedance Matching Point for the RF pin


viewtopic.php?t=32344
https://esp32.com/viewtopic.php?f=12&t=40874

Guide ESP32-S3 ( side 16 - 18 ) "the chip conjugate point (35+j0)"
https://docs.espressif.com/projects/esp ... sp32s3.pdf

You need to check the used parts -


check this... it's going better near 50 Ohm - you can optimize further by self, hope this helps
3.1pF ( chip side ) 2.3nH 2.7pF ( antenna side )