I want to create a board ideally using the RP2350 (if they're able to release for industrial and academic purposes by the end of the year) or the RP2040 as a microcontroller for a custom board. I need it to output +5V for the GPIO pins, not +3.3V, and I need to isolate the USB power and input from my main power and ground as I am trying to minimize the chances of any ground loops formed by the computer as I need everything connected to the earth ground. I was just wondering if anyone had any advice right now on how to set this up. I am trying to follow their hardware design document and try to follow along, but I notice that they setup all the IOVDD pins to a +3.3V. Could I just connect the external +5V power to that instead? How would I need to change the capacitor setup if so, and if at all? I also have some questions on the USB isolation, using the ADuM4160 right now to do so. What exactly should I consider if I want to have consistent and fast serial communication without letting there be any grounding interference due to a USB-C connector? Furthermore, any considerations to be had with my overall PCB, whether it be thickness or ground plane? Was going to make it a 4-layer board with the second layer being a ground plane connected to the earth ground.
-
1\$\begingroup\$ who would buy an RP2350 for industrial purposes? That seems very unlikely to pass any certifications! \$\endgroup\$– Marcus MüllerCommented Dec 9 at 23:46
2 Answers
You're putting the horse in front of the cart by deciding on the microcontroller before considering the architecture.
You can either isolate the USB and use a 5V-capable microcontroller, then you'd need one instance of an isolation barrier transporting signal; or you can isolate the N GPIOs and level-shift while you're doing, that, giving you N times the effort.
I'll be honest, that's an easy design decision to make: use a 5V GPIO capable microcontroller, not the RP2040, for GPIO, and put it on the 5V side of your isolation. If you can't find a 5 VIO microcontroller with a USB interface, you can still use the RP2040 to speak to USB and then send commands e.g. via SPI across an optocoupler to the IO microcontroller, if necessary.
Could I just connect the external +5V power to that instead?
No, as specified in the datasheet, that pin cannot be operated at more than a little above 3.3 V.
Furthermore, any considerations to be had with my overall PCB, whether it be thickness or ground plane?
From datasheet
The RP2040 has a rather fatal design flaw: it only has a single ground contact, in the exposed pad in the middle. And to make matters worse, you have to cross the direct path from IO pins to that for the IOVDD pins, which have been evenly spaced around the package. That means you can't put ground next to signals, and even fast-switching signals and the IO VDD are right next to analog pins. You can't really fix that with board design; energy couples to adjacent conductors, and thus, any RP2040 application that makes use of more than half of its GPIO pins will have to deal with the signal integrity issues arising from that. You could probably solve that issue with a 6 layer board with multiple layers across which power is routed (which is ridiculous for a simple microcontroller!), but the RP2040 reference design just gives up and has terrible ground connectivity and supply voltage rails interrupting ground return paths on their 2-layer design.
That honestly kind of disqualifies it for industrial applications due to doubts in design robustness, in my humble opinion.
The RP2350 doubles down on that and puts the analog pins between the digital supply and the IO VDD pin, i.e. in the region in which, in absence of a nearby ground pin, the highest replacement currents flow.
So, if you want to have an honest response on how to design a 4-layer board for some isolated control application: maybe stick with the microcontrollers of an established microcontroller manufacturer. The ST STM32 are popular, and the NXP Kinetis family has some device series with 5V capable IO.
-
\$\begingroup\$ this is awesome, thank you so much! Any ones you think in particular are best suited for limiting noise with fast serial communication? \$\endgroup\$ Commented Dec 10 at 5:18
-
\$\begingroup\$ also, any suggestions as to the best way to determine how to choose the best microcontroller for my purposes? still trying to establish what exactly i need and don't need, and i've been getting a little lost in deciphering what's important and what isn't from the datasheets \$\endgroup\$ Commented Dec 10 at 5:23
-
\$\begingroup\$ I have used high speed link chips capable of 10Gbps per lane for data transmission, with single exposed ground pad on the bottom. Surely a measly 133 MHz MCU will work too. And if doing an industrial application, you would use a 4 layer board with this MCU without any issues. In fact you can't even do USB impedance properly on a 2 layer board. \$\endgroup\$– JustmeCommented Dec 10 at 14:44
-
\$\begingroup\$ @Justme I mean on a diff 10Gbps link your situation is actually nice, because the fields are wellcontained between the traces and the groundplane you put directly below, and it's kind of inherent that you get a current return path. \$\endgroup\$ Commented Dec 10 at 18:10
No, you can't connect 5V to IOVDD. RP2040 has a maximum rating of of 3.63V after which it will damage. So you can't run it with 5v IO, and it needs no changes to any "capacitor setup" due to that. The RP2040 happens to have some pins that are 5V tolerant as inputs. But they tolerate 5.5V only as inputs and when the IOVDD supply is present and at 3.3V level.
Yes, you can use ADuM4160 for isolating the USB link. Only ADuM will connect to USB cable and you can power the MCU side completely independently in an isolated fashion. However, if the PC sits at earth potential and your want the MCU to sit at same earth potential, why bother with isolation at all. Other options include a serial link, where you have an USB to serial UART chipset and isolate the UART link between chips.
Yes if you use USB and want to do it right with correct differential impedance, you practically can't use 2 layers and must use 4 or more layers. And yes you should have a solid ground plane for differential pairs and MCU etc. Connecting the ground reference to earth potential is up to your liking, but we don't if that's a good idea or not depending on what your board does. If you omit the isolation and connect USB to desktop PC, your ground plane will be at earth potential. Assuming the PC is properly connected to proper mains outlet that provides earth.
