They look fairly similar?
The mosfet that I recommended is better for 3v3 gate signals, has a minor RDSOn and has a 40V VDS that is fine for your circuit.
The footprint is identical to yours and the pads function is also identical.
It also costs less and maybe you find it on jlcpcb.
From the video I don’t see a use of the shield with a load that absorbs a large current, 5A - 10A
What current do you need on 12V and 28V?
[EDIT]However the shield is designed for arduino uno.
[EDIT]You tested with 3V3 control signals this shield?
[EDIT]What MCU you use to control the card?
I found it on JLC PCB, so that is perfect then they can mount it also. I dont have any SMD mounting gear.
From the video I don’t see a use of the shield with a load that absorbs a large current, 5A - 10A
When I tested it I started test it with a Arduino UNO that it is designed for. But when I tried to get higher resolution on the PWM signal, UNO was not that good. Then I got the tip of ItsyBitsy M0 Express, fastere cpu more PWM port and higher resolution. Smaller footprint, I decided to use that insted. I tested it with the N-Drive Shield and it worked. Each Original Boeing 737 Panel Backlight uses min lightbulbs as backlight, about 2.5A per panel. My dimmer card is supose to work with a hole Forwar Over Head, a friend of mine that have a hole OEM setup told me it draws about 150W of power, about 2.5 A per panel. Then I thought that I can have 3 panels on each chanel. This dimmer card will also be designed so that you can use LED backlight panel if you want. Mix and match what ever back light and voltage you have. And with my initial tests it workt perfect, with the N-Drive Shield.
Main purpes of this PCB is to get it buteful. With out alot of cables.
What current do you need on 12V and 28V?
That is mainly for LED, or if it happens to be any 28V Backligt. So basicly it can be what ever AMP I want. For exampel ther is som “MAP” light that could be 28V, that draws some power.
[EDIT]However the shield is designed for arduino uno.
Yes
[EDIT]You tested with 3V3 control signals this shield?
Yes, thats what you see on the video. But I rather select what is more sutable for 3.3V
Ther is no probem to PWM 7.5A in 5V threw the Mosfet you found?
[EDIT]What MCU you use to control the card?
What does that meen?
Now I have changed most of the things:
Dimmer project4.zip (1.4 MB)
I am still not happy about the designe of the power input, how can I improve this?
How would you have done?
Also the mounting hole placement, is not perfect.
-
I noticed a singular thing, you have no capacitors in the
schematic. You need at least the 100n ones on the logic chips.
I would also put an electrolytic one on the 3V3 near the input connector. 330uF 6v3 Electrolytic polymeric. -
I would put electrolytic capacitors at least at the input of the supply voltages. Since dim-channels work in pwm.
A flying calculation would put at least 1000uF for each power supply, they should be with greater capacity on the lower voltages as the currents increase compared to what you reported in the previous posts. -
I don’t know what you need the D37, D2, D4 diodes for or put those suppressors or put nothing.
-
I’m looking at the GND plan under the mosfets and I can’t understand how it’s done.
I do not like. -
Switch footprint pads do not have the welding mask layer. If you look at the 3d view, the pads are covered with the welding mask and in this way you will not be able to solder the pins.
[EDIT] You have another problem here :
What do you mean by logic chip? How can that help?
- I would put electrolytic capacitors at least at the input of the supply voltages. Since dim-channels work in PWM.
A flying calculation would put at least 1000uF for each power supply, they should be with greater capacity on the lower voltages as the currents increase compared to what you reported in the previous posts.
Why do I need cap, what would they do?
On the relay card they have 2 100uF caps on the input power. Different types what it looks like. Don’t know why? But I guess I have to have some caps.
- I don’t know what you need the D37, D2, D4 diodes for or put those suppressors or put nothing.
The relay card have that on the 5v power input. Don’t know if it is needed.
I imagine I need that if any reverse current feeds + to the minus side so it doesn’t get back to the PSU.
- I’m looking at the GND plan under the mosfets and I can’t understand how it’s done.
I do not like.
I just copied the N-Drive Shield because that looked professional. I don’t know if it’s supposed to be done that way, but a big copper plane under and over, solder mask removed, so you can fill it with solder to have more mass to cool down the Mosfet, or put a heatsink, I don’t know why “Freetronics” have done it that way? Maybe someone else can answer that?
- Switch footprint pads do not have the welding mask layer. If you look at the 3d view, the pads are covered with the welding mask and in this
I used the footprint in the end of this thred : DPDT/SPDT footprints anyone?
How do I change the footprint with solder mask?
Also should I change the return current path? I can’t visualize how the current would flow. I have put visas on several places. But I don’t known if that is enough. It feels like it would be simpler to draw cables from inputs to each Chanel. But that feels like a workaround.
By the way wrote this in bead with iPhone, so have to review it, maybe change some things.
I have looked alot at busbar, but that increes price to unrealistic. That’s why I went away from 80A.
U1, U4 as close as possible to the chip’s power pins.
The electrolytic capacitors on the power supplies.
They are used to stabilize the power supply otherwise you would have very large voltage peaks generating a lot of noise.
It also depends on the length of the input power wires and the type of load.
I understand that the load is resistive and not very inductive. And this is good.
It is a good practice to put capacitors on the inlet in order to reduce noise.
On the 3V3 it is certainly needed since it also feeds analog parts.
There would be another trick on the analog A0 network, an RC network but it must be sized well since I believe you have a fast reading cycle for the potentiometers and if you miss the values of the two components, read incorrect values.
You would have a more stable signal for reading potentiometers, without having to make averages in the software.
For Diodes, read previous posts well.
You would have negative tensions if you were wrong to connect the wires and in that case either burn the diodes or the tracks that connect them.
They are not needed.
On the relay card the diode is on the 5V which is assumed to have a small short circuit current.
And this is true if it comes from Arduino Uno.
It’s not good protection though.
Use copper wires as bridges between GND zones with a large section instead of the BusBar.
It won’t be very nice to see but functional.
It is inexpensive.
Or review the design of the power part, I think there is important room for improvement.
To fix the switch footprint you must open the footprint editor to load the impression and for each pad you must add the welding mask both front and back. (F.Mask, B.Mask)
I had to make the video very quickly for file size reasons for uploading to the forum.
In the 3d view you must see the copper pads not covered by the welding mask :
First of all I am very very grateful for your very informative answers.You realy help! 
I am so sory but I don’t realy understand and don’t know how I would do that? Should I move the chips?
The electrolytic capacitors on the power supplies.
They are used to stabilize the power supply otherwise you would have very large voltage peaks generating a lot of noise.
It also depends on the length of the input power wires and the type of load.
I am planing to use a PSU like this, or similar:
UHP-350R-5 - Switched-Mode Power Supply, Industrial, 300W, 5V, 60A, MEAN WELL
But I don’t know what is good. I guess low “ripple” high efficiency, many different types of protection is good.
I understand that the load is resistive and not very inductive. And this is good.
It will probably be mostly LED, but the chance of it being mixed is high. As said, you should also be able to use it, as a relay card if you want. I would therefore not like to say that it will mostly be resistive load.
It is a good practice to put capacitors on the inlet in order to reduce noise.
I understand. But isn’t this handled by the PSU? Eg what I linked to?
On the 3V3 it is certainly needed since it also feeds analog parts.
There would be another trick on the analog A0 network, an RC network but it must be sized well since I believe you have a fast reading cycle for the potentiometers and if you miss the values of the two components, read incorrect values.
You would have a more stable signal for reading potentiometers, without having to make averages in the software.
Super good that I get an explanation why.
For Diodes, read previous posts well.
You would have negative tensions if you were wrong to connect the wires and in that case either burn the diodes or the tracks that connect them.
They are not needed.
But what I have learned, if you connect an inductive load, such as a solenoid or contactor, relay, on a relay card like the one I linked to. Then you send an EMF back to the PSU which can even cause the protections to trip. (That’s my experience) To solve this I have previously mounted a diode as close to the coil as possible which I learned is the best. But technically there wouldn’t be much difference if I have a diode in parallel with the supply voltage, right? So it can’t hurt in any way except if you connect the + and minus incorrectly, as you describe.
If there is a better way I am naturally open to it?
On the relay card the diode is on the 5V which is assumed to have a small short circuit current.
And this is true if it comes from Arduino Uno.
It’s not good protection though.
Aren’t the diodes on the relay board flyback diodes to take care of the energy that comes from the relay when you turn them off so that it doesn’t spread/comes back into the PSU?
What protection would you recommend otherwise?
That’s how I thought mine should work anyway.
That is, if I connect a solenoid to the board, I should not need a diode across the coil of the solenoid.
Use copper wires as bridges between GND zones with a large section instead of the BusBar.
It won’t be very nice to see but functional.
It is inexpensive.
Or review the design of the power part, I think there is important room for improvement.
If you come up with something that makes it look nicer and that I avoid expensive solutions. Or solder copper wires. I mean with the design of the PCB, I will be very grateful. If I can get close to the 80A I was aiming for from the beginning, that wouldn’t be wrong either.
Is there a program that a home user can use to simulate the current in the circuit board?
To fix the switch footprint you must open the footprint editor to load the impression and for each pad you must add the welding mask both front and back. (F.Mask, B.Mask)
I had to make the video very quickly for file size reasons for uploading to the forum.
In the 3d view you must see the copper pads not covered by the welding mask :
Incredibly helpful video, shouldn’t I be able to update the original footprint, then update the PCB? It’s important to get it right the next time I use the footprint, isn’t it?
[EDIT]
I fixed this. thank you.
That’s what he ment:
You have no ground plane, so connections to GND as short and as solid as possible.
- capacitors on U1, U4
- Electrolytic capacitors on power supplies. You have enough space to assemble even more capacity.
- Suppressants on the feeds may also not be mounted, in this case of dubious efficacy, it depends on the load. They don’t hurt.
- Space is available for welding copper bridges or as I have already suggested you review the design of the power part. In order not to have signal traces that do not allow you to make a good GND plan, you can use copper wire jumpers to be welded.
- Move the Diode D37 and put it near the entrance to the power supply.
I added the components to the scheme and to the PCB but the tracks must be made and you see where to place them but I would be nearby where I placed them.
Dimmer project4_Mod.zip (1.4 MB)
I added the components to your project.
For the 330uF capacitor on the 3V3 I assumed that the power input connector was the D-Sub 15pins
If you can move the tracks of the 5Vs that feed the relays on the B-Cu the ground plane already improves and you should also move the resistances placed on the mosfet gates. R25 for example, which only serve to have an i mosfet off at power on.
You have to move as many tracks as possible on one side of the PCB in order to have more space for GND on the other side.
If you work in that area you can create a correct copper GND area for your project.
GND plan is there. He also positioned vias in positions that are not needed.
[EDIT]
This is perhaps the least suitable example since it connects two areas of GND .
There are many throughout the PCB .
Be aware whenever google translate says ‘plan’ the correct word is ‘plane’.
But it is a 2 layer board so there is no solid GND plane like a 4 layer board has. You made suggestions to have a large GND area, which is good. But it’s no GND plane.
It is called having a large GND area under the power components given the currents involved.
[EDIT] At the top of the board he created two GND areas on both the top and bottom sides of the board and the connection of the bypass capacitors can be made as you suggested with the document you mentioned.
Thanks, I have to be a little more careful what the translator is up to.
The Google translator works better than what I am using now in “Vivaldi” but it has been a while since problems of praivacy and invasiveness I have tried as far as possible not to use google products.
True,
for GND zones it is perhaps better to use “area” or “zona”, “livelli” level is correct for the various layers of the PCB ,
“Planta” no in Italian can refer to trees or the geometry of a house.
It is better that I study technical English so I can make myself understood. 
As said in this thread or another here on the forum with linguages are a donkey, even in mine.
I think it’s called dyslexia, not serious but annoying.
I have difficulty learning a foreign language.
Ah, I deleted my post too late 
. I realized pianta is nonsense and was not sure about livello. And it is ridiculous that I - being A2 maximum in Italian - make Italian suggestions.
I could not open the modifide files with KiCad 6.07
It was possible with the beta 6.99, but then I get a lot of other errors, and all the diodes 3d parts have diapered:
This is how it looks for me.
Ok I will try to change as you sugest.
What does the capner the D-sub do?
Is it for stable pover to 3V3?
For the 330uF capacitor on the 3V3 I assumed that the power input connector was the D-Sub 15pins
No no it comes from ItsyBitsy M0 Express. I hope i feed 5V to VBAT port on the GIPO, that then feds 3v3 to all the signals.
[EDIT]
Apperently I have forgotten to power ItsyBitsy M0 Express.
Also how do you decide size of caps?