Author Topic: Mixed signal PCB layout help  (Read 9931 times)

0 Members and 1 Guest are viewing this topic.

Offline gnuarm

  • Super Contributor
  • ***
  • Posts: 2247
  • Country: pr
Re: Mixed signal PCB layout help
« Reply #25 on: July 11, 2023, 11:12:22 pm »

Quote
I haven't reviewed all the posts, but I can't think why anyone would suggest that you use two ground layers.  A solid power layer will have similar signal integrity characteristics.  If you have more than one power rail, you can divide the power layer into "zones" for each power rail.  In some designs, you also need separate ground areas for analog and digital grounds (joined at one point, at an edge of the ground area).  So, one ground layer and one power layer.

With adequate bypassing, the power planes will act the same as the ground plane, establishing the impedance of your signal traces.

Ok well maybe you should read the whole post because what you saying about splitting ground planes causes more harm than good if not done exactly correctly and its a really outdated way of doing it. Watch that video that was recommended its really good.

"if not done exactly correctly"

You seem to be making a statement, but then you completely undercut yourself by saying it will work, but only if the designer is not crap. 

The idea of isolating analog and digital ground planes is sound.  Digital electronics can produce huge ground currents, such as the impulses from a switching power converter.  No matter how well you design that circuit, it will have very large ground currents that will create ground noise, disrupting sensitive analog circuits.  So, the two need separate ground areas, connected at a single point.  Any digital signals that cross between the two areas, should do so as close to the point of connection as possible.

I've used this approach in any number of designs, and it works.

As previously mentioned in the thread you admitted you didn't read, and covered extensively in the very good video Doctorandus_P shared.... High frequency return currents (above audio frequencies) are concentrated in the path of least inductance.  With a track over a solid ground plane, the return currents take the same path as the track except through the ground plane, because that's the path that encloses the smallest loop area.  At best, splitting the ground plane is not effective for controlling high frequency return currents, because with a solid plane they already take the optimal (least impedance) path available.  At worst, splitting the ground plane can cause serious problem with EMI, SI, and basic function by forcing HF return currents to flow around--or even couple across--the gap in the plane, increasing inductance, and spreading fields out further across the board and beyond where they can impact more signals.  As you note, signals should be routed across the junction point to avoid this, but that also forces the signal and its return current closer to the sensitive ADC/DAC--or you have to make that junction area larger, stretching the definition of "single point", to preserve signal separation without tracks spanning the split.  So, bottom line, split planes can work, but they're not going to be better than a single solid plane for high frequencies, and will cause more harm than good if not done exactly correctly. 

Splits/Slots can be effective at controlling lower frequency return currents (in the audio range down to DC), but that's only relevant if you have enough current in those lower frequency ranges to cause meaningful voltages across the DCR of the return path.  "Meaningful" of course depends on the sensitivity of the circuitry involved as well as the magnitude of the currents concerned.

I don't know why you have ignored what I wrote.  Ground planes must be connected.  The signals can be routed over the point of connection between the two areas, to allow the return currents to follow the same path as the traces.  This is easy to do properly.  Just route the "high speed signals" along the path the return currents will follow.  It is seldom required to minimize the length of traces crossing from one area to another.  The signals just have to cross between the planes at the point of connection. 

What the split plane is better at, is limiting the impact of high current, RF spikes, that are created by one circuit, from crossing the split, and impacting another circuit.  A perfect example are the large transients generated by a switching power supply.  By giving this section of the design a separate area of ground plane, the current spikes are limited to that area, preventing the currents from flowing over the other parts of the ground plane, where the IR drops can cause excessive noise. 

If there is a section of analog circuitry that can be disrupted by digital noise, the semi-isolated area prevents noise from entering.  Think of it as an iso-potential ground area. 

If you don't believe this, consult any good reference on designing such switching power circuits, such as an LT (now Analog Devices) data sheet.  They offer very useful design guidance and theory of operation information. 

You are only talking about the propagation of high speed signals across a split in the power plane.  This is not what I am proposing.

If you don't understand what I am describing, say so, and we can stop discussing it now. 
Rick C.  --  Puerto Rico is not a country... It's part of the USA
  - Get 1,000 miles of free Supercharging
  - Tesla referral code - https://ts.la/richard11209
 

Offline ajb

  • Super Contributor
  • ***
  • Posts: 2733
  • Country: us
Re: Mixed signal PCB layout help
« Reply #26 on: July 12, 2023, 04:47:57 am »
What the split plane is better at, is limiting the impact of high current, RF spikes, that are created by one circuit, from crossing the split, and impacting another circuit.

But split planes aren't good at that.  Say you've got a board with a single point connection between analog and digital sections.  We both agree you wouldn't route any high edge rate signals across the split (and if you DON'T have any signals that need to cross that boundary, then you don't have any intrusive return currents to worry about anyway, thus no need to discuss a split), so all of those signals that cross the boundary now have to bunch up into that one crossing point.  That means all of the return currents also cross at that point instead of crashing into the split, great.  Except if all the signals are routed across that one point we don't NEED the split, because the high frequency return currents are simply following the least inductance path through the ground plane directly under their corresponding signal tracks.  So just get rid of the split, and now you can spread those tracks out and away from the sensitive stuff, and their high frequency return currents go away with them.    Splits or slots may be useful in managing the paths of lower frequency return currents down to DC, but in either case lateral separation of potential interferers from their potential interferees--and good placement to keep those signals and power paths in separate areas in the first place--is more effective.  When sufficiently good placement isn't an option is when splits and slots are useful.
 

Offline nigelwright7557

  • Frequent Contributor
  • **
  • Posts: 701
  • Country: gb
    • Electronic controls
Re: Mixed signal PCB layout help
« Reply #27 on: July 12, 2023, 08:04:17 am »
My star ground is usually at the power connector to the pcb.
Or the main smoothing negative terminal.

Mixed signal is fun, I once designed a USB scope and when I tested it it had 10KHz square all over the signal !
I had run analogue signal beneath a TC7660 inverter IC which runs at 10KHz.
I had also run analogue signal through crystal oscillator and got 8MHz all over the signal.

I designed a USB audio mixer.
With inputs shorted I got 1VAC on output !
I hadn't star grounded it and charging impulses into smoothing cap was modulating the ground line.
 

Offline Siwastaja

  • Super Contributor
  • ***
  • Posts: 8822
  • Country: fi
Re: Mixed signal PCB layout help
« Reply #28 on: July 12, 2023, 08:16:47 am »
What the split plane is better at, is limiting the impact of high current, RF spikes, that are created by one circuit, from crossing the split, and impacting another circuit.  A perfect example are the large transients generated by a switching power supply.

You got this exactly the wrong way. HF return currents closely follow the trace anyway, so split placement (of components and traces) is enough; adding a ground split does not add anything. On the other hand, DC and low frequency currents spread in ratios of resistivity so quite far away from the trace. Ground splits are useful and used whenever low-frequency analog accuracy is important, because DC/LF ground shifts in tens-hundreds of uV are hard to avoid by placement alone. For digital signal integrity, such small shifts do not affect the slightest, and they also are not relevant for EMI because not only the amplitude is small, frequency is too.

Switching power supplies are a perfect example of not using ground splits; you never see them, because adding one is likely to cause a fail in EMC qualification, prompting for a redesign.
« Last Edit: July 12, 2023, 08:46:20 am by Siwastaja »
 

Offline gnuarm

  • Super Contributor
  • ***
  • Posts: 2247
  • Country: pr
Re: Mixed signal PCB layout help
« Reply #29 on: July 12, 2023, 08:43:39 am »
What the split plane is better at, is limiting the impact of high current, RF spikes, that are created by one circuit, from crossing the split, and impacting another circuit.

But split planes aren't good at that.  Say you've got a board with a single point connection between analog and digital sections.  We both agree you wouldn't route any high edge rate signals across the split (and if you DON'T have any signals that need to cross that boundary, then you don't have any intrusive return currents to worry about anyway, thus no need to discuss a split), so all of those signals that cross the boundary now have to bunch up into that one crossing point. 

I reject your premise that the split is required by the presence of high speed signals crossing the split.  The split serves to prevent the current from various sources, crossing the ground plane around the sensitive circuitry and creating voltage gradients within.  This can be digital circuits disrupting analog circuits, or as I've said, switching power supplies creating ground currents.  Try as you might, you will never restrict the impact of switching power supply noise by good layout of the power supply.  That certainly helps, but only reduces, not eliminates.


Quote
That means all of the return currents also cross at that point instead of crashing into the split, great.  Except if all the signals are routed across that one point we don't NEED the split, because the high frequency return currents are simply following the least inductance path through the ground plane directly under their corresponding signal tracks. 

But you insist on limiting your thinking to high speed signals running between the two areas.  That's not the entire design.


Quote
So just get rid of the split, and now you can spread those tracks out and away from the sensitive stuff, and their high frequency return currents go away with them.    Splits or slots may be useful in managing the paths of lower frequency return currents down to DC, but in either case lateral separation of potential interferers from their potential interferees--and good placement to keep those signals and power paths in separate areas in the first place--is more effective.  When sufficiently good placement isn't an option is when splits and slots are useful.

When you accept that there is more on a board than the high speed signals running from the aggressor to the sensitive circuits, maybe we will understand one another.
Rick C.  --  Puerto Rico is not a country... It's part of the USA
  - Get 1,000 miles of free Supercharging
  - Tesla referral code - https://ts.la/richard11209
 

Offline gnuarm

  • Super Contributor
  • ***
  • Posts: 2247
  • Country: pr
Re: Mixed signal PCB layout help
« Reply #30 on: July 12, 2023, 08:50:08 am »
What the split plane is better at, is limiting the impact of high current, RF spikes, that are created by one circuit, from crossing the split, and impacting another circuit.  A perfect example are the large transients generated by a switching power supply.

You got this exactly the wrong way. HF return currents closely follow the trace anyway, so split placement (of components and traces) is enough; adding a ground split does not add anything. On the other hand, DC and low frequency currents spread in ratios of resistivity so quite far away from the trace. Ground splits are useful and used whenever low-frequency analog accuracy is important.

You can't seem to understand the difference between signal integrity of high speed signals, and the prevention of noise in a sensitive circuit.  Not the same thing at all.  There doesn't need to be any high speed signals running into the sensitive circuit to introduce noise.


Quote
Switching power supplies are a perfect example of not using ground splits; you never see them, because adding one is likely to cause a fail in EMC qualification, prompting for a redesign.

If you design a switching power supply circuit next to a sensitive circuit, it will inject significant noise into the sensitive circuit.  Isolating the ground plane of the sensitive circuit, with a single connection at a point away from the noise source, will minimize the impact of the noise.

Please explain the EMC failure.  I expect you are picturing something different from what I am.
Rick C.  --  Puerto Rico is not a country... It's part of the USA
  - Get 1,000 miles of free Supercharging
  - Tesla referral code - https://ts.la/richard11209
 

Offline calvinglosterTopic starter

  • Contributor
  • Posts: 27
  • Country: za
Re: Mixed signal PCB layout help
« Reply #31 on: July 17, 2023, 11:05:22 am »
Ok so I've decided on the 4 layer board. Would anyone please be so kind to explain why I should not shouldn't pour ground on the empty space on the top and bottom signal layer?
 

Offline Siwastaja

  • Super Contributor
  • ***
  • Posts: 8822
  • Country: fi
Re: Mixed signal PCB layout help
« Reply #32 on: July 17, 2023, 11:21:37 am »
Ok so I've decided on the 4 layer board. Would anyone please be so kind to explain why I should not shouldn't pour ground on the empty space on the top and bottom signal layer?

Laziness is a good enough reason. If you do pour, you have to carefully via stitch to avoid leaving long unconnected antennas, which is quite some work and in worst case you need to move stuff around in other layers to accommodate space for these vias. Then there will be those narrow spikes between traces where you can't fit vias, so better remove them. Adjusting pour settings carefully, the PCB software does most of this job but you usually need some manual fine tuning (e.g., adding some pour cutout areas here and there).

When done properly, these fills of course do no harm, but improvements are not that big so I understand the reasoning not to do it. I tend to fill.
 
The following users thanked this post: tooki

Offline gnuarm

  • Super Contributor
  • ***
  • Posts: 2247
  • Country: pr
Re: Mixed signal PCB layout help
« Reply #33 on: July 17, 2023, 09:34:01 pm »
Ok so I've decided on the 4 layer board. Would anyone please be so kind to explain why I should not shouldn't pour ground on the empty space on the top and bottom signal layer?

Adding ground plane on the signal layers will only be useful in creating capacitance to power layers.  Do you have power layer(s)?  What is on the two layers in the middle?   
Rick C.  --  Puerto Rico is not a country... It's part of the USA
  - Get 1,000 miles of free Supercharging
  - Tesla referral code - https://ts.la/richard11209
 

Offline calvinglosterTopic starter

  • Contributor
  • Posts: 27
  • Country: za
Re: Mixed signal PCB layout help
« Reply #34 on: July 18, 2023, 02:46:41 am »


Adding ground plane on the signal layers will only be useful in creating capacitance to power layers.  Do you have power layer(s)?  What is on the two layers in the middle?
[/quote]

I used the bottom layer as a power layer however the power is routed with traces because there is so many different voltages, -3v, +3v, -15v, +15v, +5v. The two layers in the middle is ground
 

Offline calvinglosterTopic starter

  • Contributor
  • Posts: 27
  • Country: za
Re: Mixed signal PCB layout help
« Reply #35 on: July 18, 2023, 02:47:29 am »
I used the bottom layer as a power layer however the power is routed with traces because there is so many different voltages, -3v, +3v, -15v, +15v, +5v. The two layers in the middle is ground
[/quote]
 

Offline gnuarm

  • Super Contributor
  • ***
  • Posts: 2247
  • Country: pr
Re: Mixed signal PCB layout help
« Reply #36 on: July 18, 2023, 04:44:15 am »


Quote
Adding ground plane on the signal layers will only be useful in creating capacitance to power layers.  Do you have power layer(s)?  What is on the two layers in the middle?

I used the bottom layer as a power layer however the power is routed with traces because there is so many different voltages, -3v, +3v, -15v, +15v, +5v. The two layers in the middle is ground

Yeah, I already explained to you this is not good.  There's virtually no reason to have two ground planes.  One should be ground and the other should be power.  The power plane(s) should have significant overlap with the ground plane so as to create capacitance with very low inductance and resistance.  This is the most important part of your Power Delivery System (PDS).  Adding capacitors is useful at a range of frequencies, but poops out at the high end as the series inductance of the capacitor itself dominates.  Add the power plane and you have added a very high frequency cap that covers the entire high end. 

A board I designed 14 years ago, and redesigning now, has +3.3V digital, +3.3V analog, +5V, +12V, -12V.  Each of them have an area of the power plane.  This board is less than 1 inch wide and 4.5 inches long.  Yet I found placements to make this work.  Running traces for power is a terrible way to distribute power with adequate decoupling.  Using two planes for ground is simply wasteful unless absolutely essential for impedance control.  Do you have impedance controlled traces?
Rick C.  --  Puerto Rico is not a country... It's part of the USA
  - Get 1,000 miles of free Supercharging
  - Tesla referral code - https://ts.la/richard11209
 

Offline calvinglosterTopic starter

  • Contributor
  • Posts: 27
  • Country: za
Re: Mixed signal PCB layout help
« Reply #37 on: July 18, 2023, 11:00:46 pm »
No I don't have any traces that need impedence controlled. So if I use 4 layers what stackup do you recommend? Signal, ground, power, signal? If I use this then the signal layer at the bottom is not close to a ground plain. Doesn't matter what I do there will always be a compromise in the layout. I can't have everything.
 

Offline gnuarm

  • Super Contributor
  • ***
  • Posts: 2247
  • Country: pr
Re: Mixed signal PCB layout help
« Reply #38 on: July 18, 2023, 11:42:11 pm »
No I don't have any traces that need impedence controlled. So if I use 4 layers what stackup do you recommend? Signal, ground, power, signal? If I use this then the signal layer at the bottom is not close to a ground plain. Doesn't matter what I do there will always be a compromise in the layout. I can't have everything.

As I've said before, the power planes are closely coupled to the ground plane... at least they should be if you want a low noise PDS.  So the signals couple to the power planes just like they do to the ground plane.  You don't need to worry about the breaks between the power planes, because of the close coupling to the ground plane, they act as one plane at high frequencies. 

Yes, S1, P, G, S2 is what I recommend. 

What edge rates do your signals have?  What is in your design that might generate high frequency noise?
Rick C.  --  Puerto Rico is not a country... It's part of the USA
  - Get 1,000 miles of free Supercharging
  - Tesla referral code - https://ts.la/richard11209
 

Offline calvinglosterTopic starter

  • Contributor
  • Posts: 27
  • Country: za
Re: Mixed signal PCB layout help
« Reply #39 on: July 19, 2023, 12:56:54 am »
The ADC I am using (LTC2326) has a fast edge rate, looking through the datasheet I don't see any specs for the rise time but it capable of up to 100mhz SPI speeds. Other than that I have a microcontroller which is the atmega4809 and a  DAC driven by the microcontroller. So fast signals might be SDO lines coming from the ADC and the clock lines for the ADC and DAC.

 

Offline calvinglosterTopic starter

  • Contributor
  • Posts: 27
  • Country: za
Re: Mixed signal PCB layout help
« Reply #40 on: July 19, 2023, 12:59:18 am »
I've attached a picture showing the clock and ado lines from the micro to the ADC. And the micro to the DAC which is routed on the bottom layer.

 

Offline gnuarm

  • Super Contributor
  • ***
  • Posts: 2247
  • Country: pr
Re: Mixed signal PCB layout help
« Reply #41 on: July 19, 2023, 04:04:26 am »
The ADC I am using (LTC2326) has a fast edge rate, looking through the datasheet I don't see any specs for the rise time but it capable of up to 100mhz SPI speeds. Other than that I have a microcontroller which is the atmega4809 and a  DAC driven by the microcontroller. So fast signals might be SDO lines coming from the ADC and the clock lines for the ADC and DAC.

If you are running a 100 MHz clock (I'm not sure what mhz means), you will probably want to control the impedance and add termination.  In SPI, each signal is one way, which means you can use the simplistic termination at the source.  A series resistor to match the output impedance to the line impedance will provide an initial pulse edge of 1/2 the full scale amplitude.  On reaching the high impedance input, the reflection will be positive, bringing the amplitude to full scale and that wave will bounce back to the transmitter. 

Why do you have parts so spread out?  The closer together they are, the less impact any reflections will have.  I get the impression you have little experience in high speed logic board design.  Do you know how to control the impedance of the traces? 
Rick C.  --  Puerto Rico is not a country... It's part of the USA
  - Get 1,000 miles of free Supercharging
  - Tesla referral code - https://ts.la/richard11209
 

Offline Siwastaja

  • Super Contributor
  • ***
  • Posts: 8822
  • Country: fi
Re: Mixed signal PCB layout help
« Reply #42 on: July 19, 2023, 06:17:02 am »
100MHz SPI is indeed quite tricky. Make sure your master/slave chips can handle it, then route the traces somewhat impedance controlled (no need to pay PCB manufacturer premium for this, but use an online calculator for rough approximation, important parameters are trace width and distance to the ground plane (prepreg thickness)). Then approximate the driving CMOS Rds_on, something like 20-30 ohms, and add explicit series R right at the output pin (MOSI, SCK, nCS at master, MISO at slave) to match the transmission line impedance, e.g. for a 70-ohm line a 33-47R would be right. You might need to test on prototypes because the driver R is an unknown parameter (and it will vary with temperature, sadly).

Another option to avoid having to terminate would be minimization of distance, place the SPI devices very close together, like an inch or so.
 

Offline calvinglosterTopic starter

  • Contributor
  • Posts: 27
  • Country: za
Re: Mixed signal PCB layout help
« Reply #43 on: July 19, 2023, 09:37:18 am »
I don't intend to run the clock at that speed I'll most likely do 1 to 2 MHZ. Yes I don't have any high speed design experience at all hence why I'm asking you guys for your input.
« Last Edit: July 19, 2023, 09:41:46 am by calvingloster »
 

Offline calvinglosterTopic starter

  • Contributor
  • Posts: 27
  • Country: za
Re: Mixed signal PCB layout help
« Reply #44 on: July 19, 2023, 12:04:55 pm »
I spaced everything out so much because I initially used a 2 layer board. Now it's 4 layer, so do you recommend I move everything closer even though I'm not running the SPI at 100MHz? I figured the spacing would keep the analog side well away from the digital side.
 

Offline gnuarm

  • Super Contributor
  • ***
  • Posts: 2247
  • Country: pr
Re: Mixed signal PCB layout help
« Reply #45 on: July 19, 2023, 03:33:30 pm »
I spaced everything out so much because I initially used a 2 layer board. Now it's 4 layer, so do you recommend I move everything closer even though I'm not running the SPI at 100MHz? I figured the spacing would keep the analog side well away from the digital side.

What's important in signal integrity is edge rate, not the clock rate.  By edge rate, I mean the rising/falling time of the clock edge.  The other signals are not so important, since they will have setup and hold times that allow them to settle. 

So, series terminate your clock lines or just keep your clock line path length short and you should be ok.  The clock itself must be clean, to prevent multiple edges being generated from the reflections.  If the rising/falling edge of other signals is even as short as 1 ns, but the path length is only a few inches, it will have settled out by the time the clock edge comes along.  It doesn't matter if the other signals have multiple edges, since they are not edge sensitive.

SPI is programmable as to which edge the clock is active on.  Make sure the data is changing on the other edge.
Rick C.  --  Puerto Rico is not a country... It's part of the USA
  - Get 1,000 miles of free Supercharging
  - Tesla referral code - https://ts.la/richard11209
 

Offline calvinglosterTopic starter

  • Contributor
  • Posts: 27
  • Country: za
Re: Mixed signal PCB layout help
« Reply #46 on: July 20, 2023, 03:04:03 am »

What's important in signal integrity is edge rate, not the clock rate.  By edge rate, I mean the rising/falling time of the clock edge.  The other signals are not so important, since they will have setup and hold times that allow them to settle. 

So, series terminate your clock lines or just keep your clock line path length short and you should be ok.  The clock itself must be clean, to prevent multiple edges being generated from the reflections.  If the rising/falling edge of other signals is even as short as 1 ns, but the path length is only a few inches, it will have settled out by the time the clock edge comes along.  It doesn't matter if the other signals have multiple edges, since they are not edge sensitive.

SPI is programmable as to which edge the clock is active on.  Make sure the data is changing on the other edge.

Ok cool thanks. How will these edge rates affect the analog signals?

The ADC will sample a voltage of around 100mV without any SPI comms taking place, and once it has sampled the voltage, the micro can get the info so I am not too concerned with the digital interference here however the DAC will need to maintain a very stable output voltage constantly during this process happening multiple times, so I guess I am concerned with how the Digital side will affect the DACs output voltage?
 

Offline gnuarm

  • Super Contributor
  • ***
  • Posts: 2247
  • Country: pr
Re: Mixed signal PCB layout help
« Reply #47 on: July 20, 2023, 03:14:29 am »

What's important in signal integrity is edge rate, not the clock rate.  By edge rate, I mean the rising/falling time of the clock edge.  The other signals are not so important, since they will have setup and hold times that allow them to settle. 

So, series terminate your clock lines or just keep your clock line path length short and you should be ok.  The clock itself must be clean, to prevent multiple edges being generated from the reflections.  If the rising/falling edge of other signals is even as short as 1 ns, but the path length is only a few inches, it will have settled out by the time the clock edge comes along.  It doesn't matter if the other signals have multiple edges, since they are not edge sensitive.

SPI is programmable as to which edge the clock is active on.  Make sure the data is changing on the other edge.

Ok cool thanks. How will these edge rates affect the analog signals?

It should be no problem because you are going to keep them miles apart. 

I have learned to use a separate ground plane area for analog from the digital, with the tie point under the ADC.  This will prevent the digital noise from affecting the analog signals. 


Quote
The ADC will sample a voltage of around 100mV without any SPI comms taking place, and once it has sampled the voltage, the micro can get the info so I am not too concerned with the digital interference here however the DAC will need to maintain a very stable output voltage constantly during this process happening multiple times, so I guess I am concerned with how the Digital side will affect the DACs output voltage?

I don't remember much about your design, largely because I don't see where you have shared any useful images.  A schematic is essential. 

I assume you have connectors that go off the board for the analog? 
Rick C.  --  Puerto Rico is not a country... It's part of the USA
  - Get 1,000 miles of free Supercharging
  - Tesla referral code - https://ts.la/richard11209
 

Offline calvinglosterTopic starter

  • Contributor
  • Posts: 27
  • Country: za
Re: Mixed signal PCB layout help
« Reply #48 on: July 20, 2023, 05:11:31 am »
Ya sorry I don't have the schematics on me at the moment. The DAC's output voltages are buffered by summing and subtracting OPAMPS at unity gain to output connectors. Wires that control a piezo actuator then get connected to this output with wires. The input signal is also connected to the PCB via wires. I have drawn a diagram to helpfully explain.

 

Offline gnuarm

  • Super Contributor
  • ***
  • Posts: 2247
  • Country: pr
Re: Mixed signal PCB layout help
« Reply #49 on: July 20, 2023, 05:23:45 am »
Differential input for the ADC is good.  That helps a lot with ground noise, what is called common mode.  You still need a good ground between the board and the amp.  I assume the piezo outputs have good grounds as well.  I assume the frequency to the piezo is not so high?  Is this audio? 
Rick C.  --  Puerto Rico is not a country... It's part of the USA
  - Get 1,000 miles of free Supercharging
  - Tesla referral code - https://ts.la/richard11209
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf