Schematic review for ADC Eth first STM32 board

[matb]

Hi, First time doing an STM32 based board I would like someone to take a look :

The board will be used in industrial sensors (2mV/V output sensors) and will contain 1 ADC and 1 Ethernet connection (Modbus TCP, etc). 24V DC is the expected power input.

Boards will be manufactured at JLC so the basic parts and I will be soldering some extended components (IIRC it's 20$ + 3$ fee for every reel needed to be inserted ?)

The goal is to have a working board that could hopefully go for FCC & CE lab tests. It's my first time doing a "real product" for real uses and I'm no electronic pro I learned by myself a lot and it's my first steps in the real world

I heavily inspired my design on the https://www.st.com/resource/en/schematic_pack/mb1364-h743zi-c01_schematic.pdf.
The chosen micro is the STM32H723ZGT6, a beast for what the board will do but it's cheap.

I broke the schematic in 4 parts : Power, MCU, Ethernet and ADC


POWER

For power I have a TPS5430DDAR that convert 24V to ~6V3. Then LDO to 3.3V (MCU) and another LDO to 5V (ADC). Dropout voltage is 1.3V so 6.3 should be just enough.
I copied the suggested feedback network Figure 7.11 from the datasheet https://www.ti.com/lit/ds/symlink/tps5430.pdf?ts=1756253486390

I added a jumper in case the power supply doesn't work as I expect it to.

Components selection is where I'm unsure.


MCU

Not much going on in this sheet, a capacitor on every Vcc. I do not use ADC from the MCU. 3 leds for the software team to play and the programming header is a TagConnect.
No external clock but that should work fine ?

ADC

CS5530 was selected, needs a specific crystal the least expensive at JLC is massive should I pay a little more so that everything is closer together ?

ETH

I copied the schematic from ST is it ok ?

Thanks a lot for any feedback you can provide I tried my best with my limited skills.

[pcprogrammer]

Based on your schematics it is clear that you still have lots to learn.

First of all there is no need to spit a simple design like this in multiple sheets. It could all be done on an A3 size sheet. To make a schematic like this more readable for others it is better to use wires to make the connections in stead of a mix of net names and net labels.

Like for instance on the MCU part you have the net names LED1 - LED3 on the left side of the MCU and the actual LED's on the right side of the MCU, while there is plenty of room to have them on the left and connect them with wires. No need for the net names. Same goes for the SWD connector.

Another issue seems to be that you did not connect the ethernet signals to the MCU. In that part of the schematic the use of wires would also improve readability.

The last issue I see in a quick glance, is that the ADC is also not connected to the MCU. On the MCU you use net labels SCK, MISO and MOSI, while on the ADC part you use SCK, SDI and SDO. CS on this part of the schematic is not connected to the MCU.

If you try to make a PCB based on what you have in your schematic it will fail big time.

The choice of the MCU might also be reconsidered with a part that has less pins. Even though you state it to be cheap, I'm sure there will be cheaper ones that can provide similar functionality and easier PCB footprints.

Edit: The STM32H723VET6 is the 100 pins version which is already a couple of bucks cheaper. But you can also ask yourself if the ethernet bit can be done with a wiznet device. Like for instance the W5500. https://docs.wiznet.io/img/products/w5500/W5500_ds_v110e.pdf

It might also be better to first make a prototype based on modules. Depending on the actual software needs it might be possible to do this with even a STM32F103 based bluepill, a STM32F411 based blackpill or a Raspberry PI Pico in combination with a W5500 module. So my advice is to first look into the software side of thing to decide how beefy the MCU has to be and if a full ethernet interface is needed.

[matb]

Thanks for your reply and advices.

Yes I wanted to try the sheet system of Kicad but it ended up confusing me.
I did as you suggested and made one sheet A3.

I think I corrected your recommandations.

We are going to run Zephyr OS hopefully. A prototype board modules already works that step is done.

The modified schematic **has the same BOM.

[fchk]

I usually use RJ45 jacks with integrated magnetics. This makes layout much easier. Separate magnetics and jacks are mostly used on mass-produced boards due to slightly lower costs. I guess your quantiuties are so low that this doesn't matter.

[pcprogrammer]

The schematic is a bit better, but unfortunately the internet brings the most crappy habits in schematic drawing with it. Don't use the dashed lines to make boxes. It adds noting to the design and only causes distraction. Naming the boxes is also a bit redundant, because one look at parts of a schematic tells an engineer what it is.

I do have some more pointers on the design. With small analog signals in a digital environment it is good practices to create separate grounds. This can be achieved with two ferrite beads and a bunch of ceramic capacitors. See how I have done this in one of my designs.

To get a better 5V for your ADC raise the 6.3V to 8V and place the 5V AMS1117 behind L3. This way the switcher noise is reduced before the linear regulator. Giving it a higher input voltage allows the regulator to regulate better and give of a cleaner 5V.

To have the system be more time reliable I would not use the internal clock of the MCU. Add a crystal to derive the clock from. To not increase the bom you can create the needed 25MHz for the ethernet phy with the MCU.

On the PCB make sure to keep separate ground planes and try to keep the analog input as far away from high frequency signals. To reduce some issues it might also be good to add some small series resistors in the SPI lines to the ADC. Something like 22 Ohms. This reduces spikes near the ADC.

[matb]

Hi, thanks for your answers.

@fchk didn't know that such things existed that's really cool.
I selected this part what do you think ? https://jlcpcb.com/api/file/downloadByFileSystemAccessId/8588896660340813824

I'm unsure about the 49.9 pull-ups but ST includes them on their design ?

@pcprogrammer I removed the dashed lines. Thanks for your recommandation I added it to mine. How should I manage the ground after that does every ground becomes agnd for +5V and +3V3V or just ADC side ?
I also raised to 8V as suggested and added 22 ohm resistors on 4 spi lines, should they be closer to ADC or to MCU ?

I will have a look on the MCU clock

[pcprogrammer]

The ground separation is needed between the digital and the analog parts of the system. The ADC is the point where they come together. This means that VA- of the ADC is the analog ground and DGND of the ADC is the digital ground. Somewhere near the ADC IC you have to make the separation between the two ground planes. So everything on the left of the ADC goes to analog ground, while everything on the right goes to the digital ground.

In your system the 3V3 is a supply for the digital sections of the system and the 5V is for the analog parts. So you should not set them up like you did now. In my setup the analog section needs both 5V and 3V3, and that is why I have the two regulators in series. You should only have the 5V behind the ground separation filter.

The 22 Ohm resistors in series with the SPI signals are normally positioned near a connector leaving the board, but here the ADC is on the board and the lines will be short so it does not matter that much where they are placed.

Something else I noticed in your schematic is having the ground pointing up. Best practice is to always have the ground pointing towards the bottom of the sheet and positive supplies pointing up. For negative supplies one could prefer pointing down, but sometimes it fits better having it pointing up.

Attached is the schematic and the top layer of the PCB I made for this. The digital section runs from the connector on the bottom up to the separation filter and covers the digital parts underneath the IC's. The rest is all analog. Due to their different characteristics the 1nF, 10nF and 100nF capacitors filter different parts of the noise spectrum, giving a better suppression than just a single 100nF capacitor.

This board is connected to a processor board, as can be seen in the photo of the two boards. Why the two boards, simply because keeping the boards within 10x10cm is the cheapest option on JLCPCB. 

[matb]

Ok I get it thanks for your images.

So something like this should work, i separated the 5V and 3.3V LDO.

[pcprogrammer]

Yes, that looks better. Depending on the amount of supply noise and the current drawn by the ADC, you could look into ferrite beads with a higher resistance. I use 2200 Ohm at 100MHz 0805 beads that allow 500mA of current. These give a lot more switcher noise suppression. With a 24 bit ADC you want an as clean as possible supply for the ADC.

[Doctorandus_P]

I very much agree that the dashed lines in between sections are detrimental to productivity, while they add nothing to clarity A bit of whitespace is a very good separation method, so do make sure your schematics do not get too crowded.

But I noticed you also removed the block titles. Some text to identify sub sections does help with getting an overview of the schematic. And because it's for the overview, making this text bigger (and maybe fat) makes it better readable when zoomed out.

Separating GND planes is mostly a deprecated methodology. If you do this, then be very careful about how you rote all things. No ("fast") signals should cross the separation. For this design, it's pretty easy, as apart from the ADC, there are only a bunch of passives on the "analog section". Having good quality GND planes is important, especially in a mixed analog/digital design. It's quite common these days to go to a 4 layer PCB, and then assign both internal layers to GND. The outside layers are then used for power and signals. With a 4 layer PCB, coupling between the signals and the GND plane is much better, because there is only a thin layer of prepreg (approx 100um) of separation, instead of the whole PCB thickness (approx 1.5mm). I do agree that you want to keep the analog section very clean for audio. Audio is a bit of a specialized area (combined with other high accuracy test & measurement devices). I would probably add bigger (2u2 or so) film capacitors for dedoupling the power supply for the ADC. There is also not much signal conditioning on the ADC input. Have you looked at datasheets and application notes for this (and similar) IC's?

I don't know if U2 likes it if you poke 5V up it's rear end, especially with the capacitors in front of it. Back charging such capacitors though the IC in the "wrong direction" is not good and usually a diode is put over the IC for this.

You're using mixed stiles for resistor text and placement. I see an 2R2, but also an 2.4k. Somtimes the values are inside the resistors (which I prefer). sometimes they are outside.

Those 22u capacitors, are they ceramic, or polarized / elco's?

And why use a separate Ethernet chip? STM does have (a few) uC's with built in Ethernet. But I have not compared prices and availability.

A bit similar for the Ethernet transformer. Sure those connectors with built in magnetics exist, but what is the price difference and availability? Also, if a jack gets damaged (wich is relatively common with outside facing stuff) just replacing a connector is easier. With a separate transformer it's also easier to implement "power over ethernet"

Have you ran ERC yet?
Resolution of your png's is a bit low and I can't really see whether you are using the "no connect flags" on all those empty uC pins. But also, I would route them out to some connector. You don't have to place the connector, but having the pins easily available makes it easy to repurpose your uC board for other projects.

Your STM32 does not have a crystal. Maybe it's not needed for this application, but putting the parts in the schematic and routing the footprints makes it trivially simple to solder them in later.

The crystal on your ADC does not have a value. Also audio is quite sensitive to short term variations (and noise) in the crystal frequency. Adding a better clock oscillator may be beneficial.

But overall, the schematic looks quite good.

[matb]

22µF are ceramic capacitors : https://jlcpcb.com/parts/componentSearch?searchTxt=C45783

I don't understand the U2 section of your answer, the LDO takes 8V and outputs 5V ?

I won't do PoE so I don't mind simplyfing the design with an all in one connector

I routed out port F as you suggested so I have I2C, Uart and a couple of I/Os.

How could I upload a better quality image ?

[pcprogrammer]

Posting the PDF is good. Provides high resolution one can zoom.

About U2 there is either a possibility that on the ADC connector an external 5V is connected and then feeding back into the AMS1117 while the 24V input is not present or the capacitors at the output drain slower than the ones on the input creating a similar situation. There are linear regulators that do not like this. The datasheet for the AMS1117 states it does not need these protection diodes. See page 4 of the attached datasheet.

Only in special cases a feedback diode is needed.

[matb]

No it's not possible to get fed 5V through the sensor connector

I also added the 25MHz on the MCU side btw

[matb]

Is the power supply part regarding power inductor correct ? I should have calculated it correctly but a second pair of eyes might see something ?

[pcprogrammer]

No it's not possible to get fed 5V through the sensor connector

It is an connector going to the outside world, and it takes only one fool to f... things up, so making your board fool safe is always a good thing.

It is also not the real issue at hand, it is about the need for a feedback diode across the output and input of the voltage regulator. Here it is not needed in my opinion. Doctorandus_P might think differently.

[pcprogrammer]

Is the power supply part regarding power inductor correct ? I should have calculated it correctly but a second pair of eyes might see something ?

Are you inquiring about L1 or L2?

I'm no expert on switching supplies so can't help with that.

[Doctorandus_P]

I don't understand the U2 section of your answer, the LDO takes 8V and outputs 5V ?

Due to the low resolution of the previously posted PNG's I thought that IC1 also had a 5V output, and you had some sort of switch beween different voltage regulator opions. But In the PDF I see that IC1 outputs 8V.

Also: be consistent. both U and IC are in the recommended prefix list for IC's, but you should not mix them in a schematic.

https://en.wikipedia.org/wiki/Reference_designator

[matb]

Hi, I modified so that they all are U no more IC

[jonathanpaton]

The CS553x family is going EOL. You'll need to select another part from another manufacturer.