Are 10uF tantalum capacitors needed near every chip?

Thread Starter

dl324

Joined Mar 30, 2015
15,458
MOD NOTE:
The following is the essence of the first post of a thread that was deleted for unrelated reasons but that sparked what many might find a useful conversation. The original replies have been moved to this thread.

I want to have some additional space on PCB for more features. Do I really need 10uF tantalum capacitor near every chip?


Here is my current setup:

- 12V from car,

- AMS1117-3.3 with 330nF ceramic, 10uF tantalum at the input and 100nF ceramic and 10uF tantalum at the output,

- STM32L432 with capacitors according to the datasheet,

- 10uH bead for the analog power supply that powers:

- AD8237 with 100nF ceramic and 10uF tantalum,

- LM324 with 100nF ceramic and 10uF tantalum,

- MCP4725 with 100 nf ceramic and 10uF tantalum,

- ADS1015 with 100nF ceramic and 10uF tantalum.

I am not sure whether to remove the last four ones.


Besides, I would like to change MCU into ESP32-C3, adding wireless capabilities, so that it will introduce additional noise.

MOD NOTE: Below is dl324's response to the original post.
Do I really need 10uF tantalum capacitor near every chip?
No. A conservative design guideline is to place a 0.1uF ceramic capacitor on each power pin and to distribute electrolytic capacitors based on how the power grid is designed. Sufficiently high frequency designs would add in some 0.01uF ceramic caps.
 
Last edited by a moderator:

MaxHeadRoom

Joined Jul 18, 2013
26,286
Most IC's, operating with high frequencies especially, use a 0.1μf - 0.01μf decoupling capacitor close to the IC's power terminals.
 

MrChips

Joined Oct 2, 2009
27,686
As a general rule you should have a 100nF ceramic capacitor at every power pin.

You can add 10μF electrolytic capacitors where they can be most effective in reducing lower frequency supply ripple.
 

WBahn

Joined Mar 31, 2012
27,893
I want to have some additional space on PCB for more features. Do I really need 10uF tantalum capacitor near every chip?
In general, no. While different chips have different bypassing needs, the general guideline is to use 0.1 uF ceramic caps at each chip (and each supply pin for that chip) with as short a connection between that power pin and a ground pin for that chip. If the chip is very high speed, or has/needs fast edges, then a 0.01 uF (and possibly a 0.001 uF) cap is also recommended.

Then, to feed these caps locally, put bulk storage caps, such as 10 uF to 100 uF tantalum in the vicinity. How many and where best to place them depends on a number of factors, including the specifics of the chips being bypassed and the power/ground routing of the PCB. I generally would aim for a 10 uF for every five or so chips, trying to keep one within a couple inches of each chip, and then with a 100 uF cap for every three to five smaller caps, but this was really driven more by the power/ground routing. Finally, there should generally be a pretty good size aluminum electrolytic cap right at the power entry point to the board. The size depends on how noisy the power supply is, whether it is coming in from a long distance, especially over small wires, and how quiet I needed it for the circuitry on the board.

I typically tried to group chips into groups based on how low noise I needed the supplies to be and also taking crosstalk into considerations. I then tried to route power from the power-entry point to each group in a star-configuration, if possible with a 100 uF tant (unless some other value seemed warranted) at the point where the star routing entered the local power plane region and, possible, another one on the local plane as far from the entry point as I could get. The I distributed 10 uF caps at points that seemed reasonable based on the number of chips and how the power/ground plane routing looked.

In addition to a solid bypass capacitor strategy, the use of ferrite beads to keep noise from entering the board via the power supply connections can be helpful. Another thing that can cause problems is poor management of image currents in signal lines as they cross power/ground plane regions. The use of stitching capacitors, to tie the planes together near the signal track can drastically cut down on noise problems.
 

Ian0

Joined Aug 7, 2020
6,711
No. Don’t use them at all, the tend to fail and short everything out.
Use 10uF aluminium electrolytic on the output of the voltage regulator, one 100nF ceramic for each IC, and an occasional extra aluminium electrolytic.
 
Top