I’m designing the circuit with STM microcontroller, and i am facing the small issue with PCB layout. The MCU often has lot of GND and VCC pins, and in reality, these pins are self connected inside integrated circuit of chip, it means that we no need to reconnect it in PCB anymore. However, the MCU components in KiCad are not realized this point, and it affects routing progress a lot. Is there any ways to make these pin self connected as its nature.
Thank you in advance and have nice weekend
I am experienced with power converters and not with microcontrollers, but I suspect that those pins should be externally connected. Can you provide a link to the datasheet?
You really need to connect all of the stm ground pins as well as possible to a good ground (Ideally to an uninterrupted power plane). The same holds true for vcc pins. These should even have decoupling caps very near them (one Tantal 1u and a ceramic 100n). The tantals also need to be well-connected to the ground plane not just to the positive supply pins. See STM application notes.
The internal power connection of an MCU is not “strong” enough to carry even the internal requirements let alone also carry external currents. (This holds true for nearly every device out there. If a chip has the same pin multiple times then there are very good reasons for that.)
If you can afford it go to a 4 layer pcb and use one inner layer just for ground and the other layer for all your positive supply connections. Not that much more expensive but will get you a much better working end result and save you a lot of tinkering time as you do not need to worry about signal return paths.
Thanks your feedback !! Oh i see, interesting. It means that these pins are used for power distribution purpose since MCU isn’t strong enough. And the decoupling caps are encapsulated for 1 of these pins, isn’t it? or should be all ?
Every VCC pin should ideally get its own decoupling cap. The smaller one should really be as close as possible to the VCC pin (It takes care of your “high frequency” decoupling) with a very good ground connection. The positive power connection should also first go into the decoupling caps positive pad and then from there to the MCU pin.
By the way all i state here is massively simplified. If you want the full details then read a book about EMC design guidlines or take a course on a university or other institution that offers such courses.
I think it is rather not a question of being strong enough but of EMC - to have the smallest current loop for any output pin in a case of positive and negative slope.
I am using microcontrollers at 2 layer PCB. I am using all bottom layer for GND and connect IC GND pins by vias. With VCC I go under IC from its corner then connect from inside to each VCC pin. Then to other circuits I go out with VCC through all other corners and through VCC pins. Of course at each VCC/GND pair I give 100n.
It is both. The chip will work if you only connect one such power pin (but will be more susceptible to EMC). But if you use the power pins as a jumper then you might destroy the chip itself as its internal connection is not meant to be used that way.
@nguyenbao9559 please see datasheet paragraph 5.1.5 Figure 10.
Generally speaking power distribution and low impedance at high frequency is critical with almost all new ICs. When manufacturers provide multiple power pins they do so because they expect them to be used. There may be some special exceptions perhaps if you are not using part of the chip. But best to be certain on that.
