• Welcome to our site! Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

Please share your experience on noise reduction in mixed signal circuits

hesam_m

New Member
Hi,

Please share your opinion on noise reduction techniques in mixed-signal circuits, PCBs.

your experience, tips .. etc
 

crutschow

Well-Known Member
Most Helpful Member
Mixed signal boards are not easy, since the digital noise will do it's very best to try and get into the analog signals (and it's often successful ;-).
So you want to keep the digital signal and signal returns as far from the analog circuit as possible.
Very important is to use separate analog and digital power and ground planes.
Assuming there are signals going between the analog and digital sides, the ground planes should be connected at only one spot (single-point) which should be where the analog and digital signals come together, such as a D/A or A/D converter.
There should be no other point where the analog and digital grounds are connected together (such as the power supply) unless there is only one supply for both the analog and digital circuits.
In that case it's likely preferable to run the power common to the digital side, but that may vary with the application.
You may have to try both ways to see which is best if you have a noise problem.

Connecting the two grounds together at the single point with a ferrite bead or surface mount chip can reduce the high-frequency ground digital noise getting into the analog ground.

Also decouple all the digital and analog IC's with 100nF ceramic caps directly from each IC power pin to ground pin, to minimize the noise generated on the supply and ground planes.
Surface mount caps connected close to the pins work best

If both sides must share a common supply voltage then a separate wire should go from the supply to the analog supply plane the digital supply plane.

In general, try to keep all digital signal lines as far away from sensitive analog lines as possible.

That's a few basic things that come to mind.
A search for mixed-signal PCB design came up with a number of references that will likely have additional things to say.
Some suggestions may be different than mine, so you will have to decide which seems better.
 

hesam_m

New Member
Connecting the two grounds together at the single point with a ferrite bead or surface mount chip can reduce the high-frequency ground digital noise getting into the analog ground.
According to the learnemc, making a ground separation (connection at one point) for the most cases is not a good idea

are you agree?
 

crutschow

Well-Known Member
Most Helpful Member
According to the learnemc, making a ground separation (connection at one point) for the most cases is not a good idea

are you agree?
No.
More than one connection point can cause a ground loop path for the digital ground noise current through the analog ground. You always want to control where the digital currents go to keep them away from the analog.

So you'll have to decide which suggestion seems better in your application.
 

dknguyen

Well-Known Member
Most Helpful Member
Get ahold of Henry Ott's book "Electromagnetic Compatibility"

No.
More than one connection point can cause a ground loop path for the digital ground noise current through the analog ground. You always want to control where the digital currents go to keep them away from the analog.

So you'll have to decide which suggestion seems better in your application.
These are loaded questions and loaded statements and I think you're both talking about different things using the same words.

The OP is probably referring to split planes connected at one point versus a single continuous plane with circuit partitioning, not a split plane with multiple connection points (as you seem to be interpreting the question as).

Ground currents can be controlled in a lot of ways including circuit partitioning, split planes, striplines, or simply distancing circuit partitions farther away so the ground current spreading out as it flows doesn't run into other ground currents. It's in Henry Ott's book. It's good and easy to understand. The OP should go read it.
 
Last edited:

crutschow

Well-Known Member
Most Helpful Member
Yes, I should have clarified that I was mainly referring to split power and ground planes for the analog and digital sections.
It's actually not a good idea to run digital and analog power and ground planes over each other as the capacitance between them can transfer noise currents, thus split planes are usually preferred.
Other situations could certainly require different approaches.
 

ronsimpson

Well-Known Member
Most Helpful Member
When sending signals through the noise, (analog or digital) I some times send "data" and "not-data" or "/data". Differential receivers knock out noise.
Some times I have an "analog signal" and I send along with it "analog ground". At the receiver end I can substract out the noise on ground and get back a clean signal referenced to the new ground.

You need to know how current flows, and how it effects other circuits. Then smartly plan your grounds.
OR
Use low resistance grounds so the noise will be small.
So, say that another way; be smart or be strong! (or be both)
 

Latest threads

EE World Online Articles

Loading

 
Top