I am learning about the STM32F103CBT6 microcontroller and would like to design a simple PCB. I noticed that the pinout diagram shows four pairs of 'VDD' and 'VSS' ports on the chip. Given the importance of a clean power source, I plan to add two capacitors along the ports to filter out noise from both low and high frequencies.
Do I need to add capacitors for each of the four pairs?"
What is the best approach to decoupling capacitors for the VDD and VSS pins on the STM32F103CBT6?
\$\begingroup\$
\$\endgroup\$
2
-
\$\begingroup\$ Yes, you should put decoupling on each VDD. \$\endgroup\$– EeEmDeeCommented 2 days ago
-
1\$\begingroup\$ It's not just the supply pins you need to care about but also reset pin, clock pins, PLL pins if present, analog Vref, test/mode pins and so on. In case of microcontrollers one should always RTFM as well as any app notes regarding hardware recommendations and they will pretty much always give recommendations about cap values and placement. For supplies it is typically 100nF paired with a 10uF and typically low ESR meaning ceramics. \$\endgroup\$– LundinCommented 2 days ago
Add a comment
|
3 Answers
\$\begingroup\$
\$\endgroup\$
2
The Getting started with STM32F10xxx hardware development application note says:
2.2 Power supply schemes
- The VDD pins must be connected to VDD with external decoupling capacitors (one 100 nF ceramic capacitor for each VDD pin, plus one tantalum or ceramic capacitor (min. 4.7 μF, typ.10 μF).
6.4 Decoupling
All power supply and ground pins must be properly connected to the power supplies. These connections, including pads, tracks and vias must have as low an impedance as possible. This is typically achieved with thick track widths and, preferably, the use of dedicated power supply planes in multilayer PCBs.
In addition, each power supply pair must be decoupled with filtering ceramic capacitors C (100 nF) and a chemical capacitor C of about 10 μF connected in parallel on the STM32F10xxx device. These capacitors need to be placed as close as possible to, or below, the appropriate pins on the underside of the PCB. Typical values are 10 nF to 100 nF, but exact values depend on the application needs.
While the 10(0) nF capacitors must be placed near the respective VDD pins, the big capacitor is typically shared by all components on the board and placed at the power supply (or where the power enters the board).
-
\$\begingroup\$ Regarding the big "bulk" cap, usually there's one on the input and one after the voltage regulator, as specified by the voltage regulator - though very big caps can be used there in case of rough environments like mobile/automotive applications. In addition to this you should have a 10uF something as bulk cap for the MCU specifically, and that one is not there to debounce the incoming power but rather the on-board voltage regulator output + any noise picked up along the way from it to the MCU. \$\endgroup\$– LundinCommented 2 days ago
-
\$\begingroup\$ @Lundin That MCU has internal core voltage regulator. So like for any other regulator, it needs the large bulk bypass right at the regulator pin. In this case, datasheet explicitly says the big bulk cap must be on VDD3 pin. \$\endgroup\$– JustmeCommented 2 days ago
\$\begingroup\$
\$\endgroup\$
Yes.
Don't try to outguess the chip designers. Follow what's in the datasheet exactly.
I saw one case where an engineer tried to save $0.05 by leaving one capacitor off. The design was in production, but failure rate in test was high, with "odd" problems. I grabbed a number of failed boards, installed the missing capacitor, and they all worked fine after that.
I don't know what it cost in total to save that $0.05, but it wasn't trivial. Several thousand dollars most likely, plus the aggravation of "odd" problems for no apparent reason.
\$\begingroup\$
\$\endgroup\$
Yes, for best results, the datasheet mandates to have bypass caps of suggested values on all supply pins. Read the datasheet for details, along with the hardware design appnotes, and a practical example for the MCU as it has evaluation board schematics and layout available.
If you are confident that you can design it with less capacitors, feel free to do so, but it is much simpler to put all the recommended capacitors at the recommended pins and it will simply work in all scenarios.
For example, specifically what the other answers seem to not mention, is that the large 4.7uF bulk capacitor must be connected to pin VDD3 for this specific MCU, because that pin is the supply for internal core voltage regulator.
So it's not there for just some generic bypass of whole MCU or an omittable capacitor, unless you have the board 3.3V regulator right near pin VDD3 with large bulk caps.
