Hey guys,
Over the past couple of years I have been developing misc. consumer electronics - usually consisting of a microcontroller, some sensors, integrated circuits & daughter boards, and a dc power supply to power everything.

I generally have multiple power rails, for example a 12vdc power adaptor, a 5V and a 3.3V voltage regulator. I have been using the "RECOM R-78E5.0-0.5" a lot, as well as the MCP1700. I also always put decoupling capacitors near the power of each integrated circuit or daughter board (1uF or 0.1uF)

Different device under different circumstances have a different amount of noise on the power rails - sometimes its pretty significant, other times it doesn't matter. I've noticed that this noise still makes it through to a lot of the integrated circuits, sensors, etc. and sometimes causes problems.

What is the correct way to remove this noise so integrated circuits, sensors, etc. operate properly? It seems that decoupling capacitors sometimes are not enough.

I'm confused on if you would build some kind of a filter to go in front of every single integrated circuit/sensor? Can this be done once at the DC power in of the circuit?

How do you decide if it should be a RC filter, LC filter, or something else? I thought these styles of filters were more for signal conditioning and less for actual power conditioning? Is this because a general RC or LC filter is intended for a small amount of current?

Any advice to clear this up would be much appreciated, thanks again!

 

Each problem might need a different solution. If you have little voltage to spare, a nanohenry choke can be installed to help the capacitor do its filtering. If you can get along while losing half a volt or a whole volt, a resistor is cheaper than an inductor.

Noise is caused inside switching chips. The circuit board traces contain nanohenries. Usually, that is enough when you add a small ceramic capacitor. If it isn't enough, you add some nanohenries.

 

My knowledge of electronics is not as deep as that of some members of this forum. But I've designed several circuits in the past involving both analog and digital electronic components in the same PCB. Most of the time in which noise was an issue, it was caused mainly by the switching of digital ICs. I can tell you that I learned the hard way that component placement in a PCB, as well as the way its traces are laid out (and if it's a 2 or 4-layer PCB) , are extremely important factors that contribute to noise transferred to the analog part of the circuit.

Also, grounding paths are critical. It's important to physically separate the analog part from the digital part of the circuit. And to make sure that its ground paths are also separate. A single point to which all grounds are connected is a common PCB layout technique.

Another couple of observations: Never use an ordinary switching power supply to power analog circuitry whose noise you want to minimize. Either use a linear regulator, or a filtered power supply for this purpose. I've also opted for using separate linear regulator ICs to power the analog and digital parts of a circuit separately, even when they both use the same voltage level.

 

This is by far one of my favorite subjects in electrical engineering. It can be incredibly difficult to get low noise on your analog circuits in a mixed signal design. A typical 12-bit A/D converter (ADC) with a 2.5V reference voltage has a resolution of 610uV - meaning that the input of your A/D converter needs to have noise less than about 500uV to achieve good A/D Signal to Noise Ratio (SNR). In fact, this is so important, that if you have 2mV of noise on a ADC like this, then you've essentially paid for a 12-bit A/D, but are only using 10-bits (note: sometimes this is all the marketing guys want - they don't care about the noise floor, they care about putting '12-bit' on the sales sheet).

First, there is no such thing as a 'correct way to remove noise'. There are, however, more effective ways to filter noise. Low impedance ground and power planes are usually the most important aspect of a mixed signal design. For this reason, I usually insist on having a 4-layer board on mixed signal designs - this makes my job so much easier on so many levels. A 4-layer board is about $0.07/sq. in. more than 2-layer boards in high volume and is worth the money. Digital chips can source amps of current in very short periods of time when they switch from one logic state to the other. (Also note that this is one reason solderless breadboards aren't the best tools to use - poor power planes).

Decoupling capacitors are usually the second step towards a very effective power filtering. There's a lot of information on decoupling caps - so I won't go into all of the details here, but think of a decoupling cap as a water heater in a house. Often times, you need a lot of hot water right now.... so you have a small tank that holds a bit of hot water. As you use the hot water in that tank, the city water tank fills your hot water heater but takes a while to do so, and the city has an even larger reservoirs that fill their city tank but much slower - they may even have to call someone to release more water to meet demand. This is how decouple capacitors work.

Finally, physically separating the analog and digital circuitry on the board is one of the most effective ways of ways of limiting noise. There are many, many, many ways to do this. Every engineer seems to have their own secret sauce. Two methods are commonly used: 1) 'Cutting' your ground plans can be effective - if done correctly. You usually want the cut near the ADC. It's VERY important to have only ONE place where the analog and digital grounds meet - and in large boards this can be very difficult to keep track of. Another way that I've designed boards is to 2) have Power to Digital to Analog separation on my boards... in that order. This way the high currents required of the digital circuitry does not go through the analog section (Note: that these high currents are also high frequency, and high frequency (>~1MHz) currents tend to want to take the shortest route where it's going and tends to follow the same route when it's returning - making the shortest route possible - despite any low impedance planes that may be present).

Note that I didn't even mention LC filters. They are usually bulky and expensive - and can have issues with self resonance if not done properly. They usually should not be used in digital power rails.

RC filters can be useful - but I personally try to reserve them for analog signal filtering. They also should not usually be used to filter digital power rails.

I will also respectfully disagree with cmartinez regarding the linear regulators attenuating noise from switching power supplies - if it does, then it's more due to the RLC filter inherent from the traces going to the output of the regulator more so than the regulator itself. This app note: http://cds.linear.com/docs/en/application-note/an101f.pdf by Jim Williams explains more clearly why linear regulators are not effective at removing high frequency content.

Further reading regarding noise filtering can also be found here: (oops looks like Dr. Howard Johnson no longer offers his free letter writing content :-/ ) [edit: Nevermind! Here is is! scroll down to the 'Keywords' section! http://www.sigcon.com/Pubs/Keyword.html]

 

I will also respectfully disagree with cmartinez regarding the linear regulators attenuating noise from switching power supplies

Excellent application note, thanks for posting. Already learning tons of stuff from it.

As I've already said, I'm not exactly proficient in this field (heck, I'm just a mid-level amateur). But every once in a while a question pops up in this place related to a problem that I've had to solve in the past.
That's when I step in and try to help if I can, and give an answer as accurate as possible; hoping that I'm not so off the mark so as to further confuse, or worse yet, misinform the OP.

Learning is a never-ending process.

Thanks again.

 

I would modify this statement,

Never use an ordinary switching power supply to power analog circuitry whose noise you want to minimize.

to read "Never, never, NEVER! use ANY switching power supply to power analog circuitry whose noise you want to minimize."

A couple of other things I've learned over the years (usually the hard way):

• Lay out circuit boards so that traces carrying signals with high dI/dT or dV/dT are kept as far away as possible from sensitive circuit nodes (e.g., op amp inputs) to minimize capacitive and inductive coupling of interference.
• Segregate digital logic circuit from sensitive analog circuits as much as possible.
• Identify all sensitive circuit nodes and lay out the board so these nodes are as physically compact as possible to minimize their susceptibility to interference.
• Pay close attention to ground return current paths for high-current signals and make sure those return currents don't flow through the ground systems of sensitive, low-level portions of your circuit; make them flow around those portions, instead. Ground topology is important.
• Avoid using open-winding inductors that can emit large, high-frequency magnetic fields which can induce noise in nearby circuits. Use pot-core inductors or toroids instead.

And finally, some app notes for light, bedtime reading:

AN-202 An IC Amplifier User’s Guide to Decoupling, Grounding, and Making Things Go Right for a Change
AN-214 Ground Rules for High-Speed Circuits
AN-280 Mixed Signal Circuit Techniques
AN-347 Shielding and Guarding
AN-342 Analog Signal Handling for High Speed and Accuracy
AN-345 Grounding for Low- and High-Frequency Circuits

 

A story from the past which illustrates a truly extreme example of the first principle I listed above, "Lay out circuit boards so that traces carrying signals with high dI/dT or dV/dT are kept as far away as possible from sensitive circuit nodes (e.g., op amp inputs) to minimize capacitive and inductive coupling of interference":

Many years ago we were designing a product that contained an RCA CDP1802 microprocessor, RAM, ROM and some analog I/O. The analog I/O used a CMOS quad op amp (I forget which one) and a bunch of resistors and capacitors; the resistors were huge, ranging from several hundred kΩ to several MΩ, and the capacitors were very small, most just a couple of hundred pF or less. So this circuit, with its outlandishly high impedances, was an interference magnet from the git-go; I don't know whether the engineer chose those component values because he needed to minimize operating current or just because he was clueless, but that circuit was a signal-integrity calamity just waiting to happen.

Back then (early 1980's), our engineers didn't lay out their own circuit boards the way we do now; we had a separate department staffed by board layout "specialists" who, although they were well-schooled on operating the board layout CAD software, knew little else about electronics.

When Layout laid out the board, they plunked the op amp and its associated components right smack-dab in the middle of the board, surrounded by the digital stuff. And they ran the data bus lines from the 1802 right in between the pins on that op amp; EVERY pin on that chip had two data lines running right next to it, one on each side.

So they got some boards in and stuffed them in the lab, and powered them up. Needless to say, the result was a disaster: every one of the op amp inputs showed several hundred millivolts of spiky noise on it, and all four of the op amp output were banging rail-to-rail in time with the input noise. NOTHING worked right.

That's an extreme example, to be sure, but it just goes to show you how much trouble it's possible to get into with poor PCB layout.