My very first ESP32 based PCB Projekt [Mosfet control Board]

[dimidiatusc]

Thank you very much for the explanations!

I understand that my circuit is very messy and unprofessional, and I want to change that. My biggest problem is that I don’t know how to use the software properly—I don’t know which label to choose for what, etc. Did I misunderstand something? I thought GND is GND everywhere.

I understand why it might make more sense to connect everything instead of using labels. However, in my opinion, using labels makes things easier (for mee) because it allows me to position components freely and arrange them in a way that makes the most sense visually. But i will try to mix labels and direct wiring instead.

I would like to make some adjustments:

• Implement the MOSFET setup (with resistors, labels, etc.) only once and then duplicate it. Just to clarify—will the labels be automatically numbered? How can I implement this?
• Place each section in a labeled box. Where can I do that?
• Solve the issue with the MOSFETs’ turn-on voltage.
• Add labels to unconnected pins. How can I mark them as not connected?
• Correctly specify the power sources and properly define GND, including differentiating if necessary. I might need an explanation here.

For you, these questions might be obvious, but I struggle to navigate the program, find functions, and fully understand what they do.

I understand if you don’t want to answer all of this. In other areas, I have a lot of expertise and always offer my help, even for absolute beginners. However, what doesn’t work for me is absolute resistance to fact-based advice. I am doing my best to make my circuit easier for you to read, but first, I need to understand how, where, and what… My biggest issue is finding the right buttons—I don’t yet understand the functionality of such software.

I previously tried Eagle, but the program was so buggy that I uninstalled it immediately.

[RaptorUK]

@dimidiatusc

Add labels to unconnected pins. How can I mark them as not connected?

Thats an easy one . . .

Click this and drop an X onto your pin

[jmk]

@dimidiatusc

For you, these questions solutions might be obvious

Only because most of the regular people on this forum use Kicad daily, have been using it for 5+ years and have been designing PCBs for 30+ years or more.

@dimidiatusc

but I struggle to navigate the program, find functions, and fully understand what they do.

Practice makes perfect. The documentation https://docs.kicad.org/ helps. Start with the parts you most need and practice using the functions when you have found them in the Documents.

And here is the link to the documentation for unconnected pins.

@dimidiatusc

Implement the MOSFET setup (with resistors, labels, etc.) only once and then duplicate it. Just to clarify—will the labels be automatically numbered? How can I implement this?

Have you tried to do this?
Highlight all the parts including wires with a diagonal left button down mouse drag (note the difference between L to R and R to L mouse drag), then copy/paste or duplicate (both in right mouse click menu when hovering over highlighted selection) and observe the results. You will find the Refs increase with either function.

[Piotr]

@dimidiatusc

My biggest problem is that I don’t know how to use the software properly

If you use KiCad 1 or 2 days than there is nothing unusual that you don’t know it. It is huge software.
I like to learn slower (like I also read slow but very accurate).
In 2017 before installing KiCad for the first time I have printed all KiCad documentation pdfs and then read them all (with marker in my hand). All means all - including for example Drawing Sheet Editor. After reading I decided that I like KiCad. From all what I have marked I have made cheat sheet and thus armed I installed KiCad V4 to find that all pdfs I have read are practically related to KiCad V3 while V5 will be soon. Nowadays documentation is probably more up to date.
When I then joined forum I found that even not using KiCad yet I know the answers for many questions asked here.
My way was that with KiCad V4 I spend time on making my own libraries (I use only my libraries) waiting for V5 to start designing my PCBs with KiCad. The reason for waiting was that it was said that V5 solves the via-stitching problem (in V4 you had to connect with tracks all GND vias connecting top and bottom GND zones). Most PCBs I have done with V5 who reigned for 3 years. From V6 I use KiCad rarely - practically only when one of my PCBs need new revision.
Don’t get too carried away and take some time to review the KiCad documentation.
“Don’t get too carried away” is from Google translator from “Don’t be bathed in hot water”. I hope meaning is as I expect.

[Piotr]

@jmk

This is our fourth day in a row of over 37° temperature

We have here about -2°C now, but when I was young at this time of year typical was -10…-20. The coldest I remember (I think it was ±1973) was -35°C. If the air were dry, it wouldn’t be a problem, but it wasn’t. My eyes hurt from the cold. I devised a method of closing my eyes alternately every few seconds.

[dimidiatusc]

@jmk

Practice makes perfect. The documentation …helps. Start with the parts you most need and practice using the functions when you have found them in the Documents.

And (…) is the link to the documentation for unconnected pins.

Good advice, that’s how im gonna do it from now on.

@Piotr

If you use KiCad 1 or 2 days than there is nothing unusual that you don’t know it. It is huge software.
I like to learn slower (like I also read slow but very accurate).
In 2017 before installing KiCad for the first time I have printed all KiCad documentation pdfs and then read them all (with marker in my hand).

I like to learn differently—I start my project from one point, see how far I get, and then correct all the mistakes. I need a practical overview.

@jmk

Have you tried to do this?
Highlight all the parts including wires with a diagonal left button down mouse drag (note the difference between L to R and R to L mouse drag), then copy/paste or duplicate (both in right mouse click menu when hovering over highlighted selection) and observe the results. You will find the Refs increase with either function.

Yes, thats how i copy pasted - but i got told, there’s a better way doing it.

@joob

For the screw terminal/pwm-mosfet repeated circuits I believe there are ways in kicad to repeat the layout using a subsheet. In KiCad 9 there are is a new tool you can use for this:
Post-V8 New Features and Development News - #64 by twl

Well, I should have worked on that link, but I still haven’t had time to address these points.

I did some research on JLC regarding pricing and made a quick calculation. The displayed price seems to be much higher than I expected. How much would one fully assembled PCB cost?

[paulvdh]

It’s a bit effort to get started with things like this and you clearly put a lot of time in it, and overall the schematic looks reasonable.

A few differences:
Try to use less labels, and use wires, or at least put the blocks in an order that makes more sense. For example, you have an USB connector in the upper left corner, and the V_USB label goes to the power supply in the lower right corner. I would put those sections next to each other, and use signal direction from left to right, and voltages from top to bottom.

Also, use the RKM_code. It’s pretty much “industry standard”, and when using these codes, the value of resistors fits inside the resistors (which is also pretty much standard), and this saves space. Also, adding the Ohm symbol is awkward to type. RKM also avoids dots, which can get smudged or overlooked on printouts. Adding “Ohm” to resistors, but not “Farad” to capacitors is also inconsistent. For your capacitors, you’ve also used lower case “u” and the greek micro (lower case u is more logical. 0.1u would then become 100n in RKM format. (I guess 0u1 would also be correct, but I never saw it, and it also seems confusing).

I would also use a second hierarchical sheet for the output FET’s and the connectors. This way you just draw one output section, and you insert as many of the sheets as needed (16 in this case). It’s less work to draw and maintain, and on a separate sheet for this, you also don’t have to fight with space to make it all fit together. Another advantage is that there is no way for the circuits to be different.

I would also put the pull down resistors before the series protection resistors. At the moment they are a voltage divider, and you loose about 9% of the gate voltage for the FET’s (Are they logic compatible?) The pull down resistors can also have a much higher value, something like 1M Ohm would probably work too, but to you have to check the impedance of the output pins during the high impedance (probalby reset?) duration.

At the moment you have 3 diodes in series from the USB connector to the LM2596. Even for schottky diodes that is a bit much. USB is not a good 5V supply either, It’s voltage can be 4V5 or even lower. USB is also not sure to provide enough power for an ESP32. It “usually works”, but there are no guarantees. This may be a cause for unreliable data connections (ESP32 draws most power while transmitting over WiFi).

Why did you use labels for GND? the Power symbol for GND already is a label. (That is how it works internally). Using the power symbols makes them more easily recognizable.

What is the use of resistors Rpd17 and Rpd13? Both of their sides are connected to GND.

[nickmBY]

@dimidiatusc

Maybe you could also kindly explain exactly what I did wrong, what effects this has, and how I can do it better?

Use labels wisely is the simple answer.
A schematic represnts some logic. And you should draw it in a way that makes the logic obvious. That means group things to gether that do belong together. And if you are running out of place, just change the sheet size!
The “use labels everywhere”-pandemic seems to slowly take over. My opinnion is, that these people have never seen thought out schematics. Good schematics do have some kind of beauty. And you have to learn that. Otherwise it looks like skribbling and no one - at least me - will have a look at it. Yes, this is prejustice.

For example, have a look at the schematics in “The art of electronics”. They do show how things flow.
Left to right for input to output, top to bottom for power in and ground.

I spend a lot of time to edit my schematics. Move things around, avoid mess, be clear. It is like writing software. Structure!
And if you realize by your own that your schematic lacks structure, you should also realize that your thoughts lack structure. Yes, this takes time, especially for a beginner.

KiCAD (or any EDA) is not TikTok with wires.
Mechanical 3D-CAD is not TikTok with screws.
Software is not TikTok with goto.

[eelik]

@nickmBY

Use labels wisely is the simple answer.

First of all, you don’t need labels for GND. That have had dedicated symbol(s) since copper age. You see some kind of ground symbol used practically in every normal schematic. Power lines also often have specific power symbols, named according their voltage. GND symbols should point downwards. But don’t use GND symbol for every GND pin, try to draw some horizontal wires which connect nearby GND pins together and add a GND symbol for each such wire.

Second, you have used global labels for everything. It’s kind of OK to use global labels even with one page schematic if you use them for naming nets. However, there specific purpose is to be global between all sheets of a multipage schematic. They should be used sparingly, for example when it’s easy to guess where else the same label name would be used in the whole schematic when you see it in one subsheet.

Third, you have use labels for almost the sole means of connecting parts. But a good schematic uses wires to show connections visually. Labels within one sheet (local labels) should be used mostly for naming nets with good functional intuitive names, not for connecting parts/pins. A good rule of thumb good be to use a label for connecting only if drawing a wire would be somehow difficult AND following labels is easy and intuitive.

If you look at your schematic so that you can’t read the label texts you may notice that it’s a total mess, you can’t say at all what is connected to what and what is the function of each part.

There’s no perfect schematic, you can start little by little. Here’s an example (just approximating your design):

Instead of 9 global labels this has three and is certainly easier to understand. Power source is up/left, output right, GND down. Notice how also the label “arrow” directions follow input/output logic.

Some people may prefer not to use wires for GND connections:

What’s this mess?

You can mirror symbols horizontally and vertically to swap up/down and left/right. So, positive voltage up and GND down. A tad easier to read, don’t you think?

Different voltages even have their own power symbols in the KiCad library. And they, as the GND symbol, work also as global labels, so you don’t have to give another name to the net. (This would clash with the style in the regulator screenshot where voltages are just global labels, you should choose one or the other.)

This is of course also totally unnecessary and confusing:

Stick to the universally standard GND symbol.

This is kind of beautiful, especially if you like honey bees and their combs. However, unnecessary repetition is bad for readability. Instead:

You don’t even have to draw more than one wire segment through all the pins, no copying or drawing one by one!

If you see several identically functioning pins labeled like X1, X2, X3…X16 next to each other, you know they are screaming for a bus to drive over them, as somebody already said.

Maybe you have been afraid of wires because there just wouldn’t be room for them in your schematic, they would be even more total mess. But using a bus or two could solve the problem.

Talking about not enough room – maybe you also rotated U3 to save space. Please don’t! Use hierarchical schematic or change to A3 page.

Finally, finding good advice using google may be surprisingly easy. I just tried “good schematics”, and look what I found:

The art of drawing good schematics

[nickmBY]

@eelik

There’s no perfect schematic, you can start little by little. Here’s an example (just approximating your design):

+3V3 is a power symbol by its own. Use it! No need for a label
The regulator even defines pin 3 as power output (and not “label output”).

[dimidiatusc]

That was extremely helpful, thank you very much!

I watched a video and ended up on the wrong path of adding labels everywhere.

Your examples were extremely helpful, now I know how to wire component groups properly, how to make them clear and that there are power symbols. I’ll look for them immediately when I open KiCad again. I’m currently continuing with the Android app.

[erintse]

Hey, welcome to the community!

Your project sounds solid, and it looks like you’ve covered most of the key components. A few things to double-check:

• Make sure your LM2595T-3.3 can handle the current requirements of the ESP32 and peripherals.
• The IRLZ34N is great for low-voltage logic-level switching, but check if it meets your load requirements.
• For high-current screw terminals (10A+), something like WAGO 236 or Phoenix Contact MKDS series could be reliable.
• For the Conn_01x16_Socket, standard 2.54mm pitch headers or IDC connectors might work, depending on how often you plan to swap voltages.
• Consider adding flyback diodes if you’re switching inductive loads.

If you have a schematic, feel free to share, and we can take a closer look!