PCM4222EVM input circuit PCB

I've got this very nice eval board, and while it measures very well and has a great clock it always seemed to leave something to be desired sonically.

There's a simple little circuit in the PCM4222's  manual using standard op amps in inverted mode, so I build it for one channel on veryboard and had a listen using various op amps. In the end I liked the 5534 best, it seemed closest to the source and measured very well. Sonically the board sounds way more alive this way than with the differential op amp it comes with.

So I made a PCB design (my very first) using TI's circuit, and added proper PSU filtering and dampening, changed the input resistor to make the input less sensitive (it's at 14 dB otherwise) and also added DC offset adjustments.

There are no DC blocking caps, adding diodes for input protection might be added later, too.

Is the grounding all right? I made sure there are no loops.

Entire board

Copper traces

Silkscreen

OK, etched it, drilled it, built it. Works great!  8)

Connectors will be flipped so +/- I/O are next to each other. Adding ground connectors for the input and or output could be done, but are not necessary (ground is provided via the PSU connector).

Having balanced path you care very little about the ground, to the outside world it should be connected to chasis and not to the ground at the PSU, you do need the reference to the converter which would be best to have from the decoupling caps to minimize common mode noise.

Other than that, if it's working fine and you like it, enjoy it!

JS

joaquins said:

Having balanced path you care very little about the ground, to the outside world it should be connected to chasis and not to the ground at the PSU, you do need the reference to the converter which would be best to have from the decoupling caps to minimize common mode noise.

Other than that, if it's working fine and you like it, enjoy it!

JS

Click to expand...

Thanks! Here's the revised layout. Input ground should be connected to chassis where the input connector leaves the chassis, right? Output ground will connect to the analog ground input on the EVM PCB (there are test point connectors the +/- outputs should be soldered to as well as the ground). 0 ohm resistors on the EVM PCB after the original balanced input should be removed.

living sounds said:

joaquins said:

Having balanced path you care very little about the ground, to the outside world it should be connected to chasis and not to the ground at the PSU, you do need the reference to the converter which would be best to have from the decoupling caps to minimize common mode noise.

Other than that, if it's working fine and you like it, enjoy it!

JS

Click to expand...

Thanks! Here's the revised layout. Input ground should be connected to chassis where the input connector leaves the chassis, right? Output ground will connect to the analog ground input on the EVM PCB (there are test point connectors the +/- outputs should be soldered to as well as the ground). 0 ohm resistors on the EVM PCB after the original balanced input should be removed.

Click to expand...

No, two things here I'd change. First do not connect anything to the input ground, the pin 1 at the input goes directly to the chasis and nowhere else.

The other thing is the decoupling and output ground. Decoupling should be from ground to the rail, not from ground to the rail in one side and from rail to rail in the other. Also you should connect all your 8 decoupling caps to a single ground point and from there run it to de output directly without going anywhere else. So you have your general ground, your decoupling caps and your output. Using a 0R jumper from the general ground to the decoupling caps could help when making the layout.

Attached is a picture with parasitic ground resistance in place as it should be, any crossed parasitic grounds would introduce more dirt. The pict is for an unbalanced stage, in your case you don't need to care for the input part of it but you do care for the output. Best practice would be to make some kind of star ground at the decoupling caps, take from there the reference ground, single trace going to the PS input, another to the V/2 reference points and other to the output directly, so let's say you call 0V the decoupling caps ground node, any current to the output only introduces noise to the output, so no noise there, just a bit of signal loss equivalent to having a teeny tiny resistance in series, absolutely nothing to worry about it. To the V/2 reference would be practically no current so would be at 0V as well, for the PS input you'll have your supply current some how smoothed by the decoupling caps and only would be seen as PS dirt and not as signal reference or output dirt, as 5534 has good PSRR is not a problem. You could figure out a different way of connecting those 4 dots (decoupling node, PS input, signal output and V/2 reference) which works fine, this is what I'd do.

If you do it in another way, let's say you take your reference point from PS input instead of the decoupling caps you'll have the dirt introduced by the current draw at your reference, so your reference will be noisier. All this considerations are due to trace impedance, in audio usually we only care about the resistance usually in the mΩ range, in really low current applications usually is not a problem but best practice to have the considerations if you want to squeeze the last few dB of SNR+THD out of your opamps. In your case you want to drive a very capacitive load, so HF currents will be relatively high and introduce some noise to the ground at the decoupling caps.

You have to connect your ground to the chasis at some point, so the input is referenced somehow to the circuit, but this is usually done outside the PCB at the PS ground, at one point the PS ground meets the chassis and this gives all you need.

JS

A more fancy decoupling topology could be used in your fully balanced configurations, but stability considerations should be taken and could make things much harder. As your load is from one output to the other the current would be from +PS of one opamp to -PS of the other opamp, rather than to ground as it would be in a unbalanced output stage. This means what you really need to decouple is the crossed rails from one opamp to the other needing only 2 sets of caps and no risk to introduce dirt at any point to the ground. Having this could potentially affect the stability of the opamps so I don't recommend going that way but I think it's nice to at least think about it as a mental exercise, where you follow the current rather than brute force make all ground points have as close voltage as possible to avoid signal degradation.

Current for negative output voltage is shown, for positive would be around the other cap but I didn't draw it to keep it clean. The reference drawn as ground but could be a divided voltage from one of the rails bypassed to ground with a cap big enough in relation with the resistors.

As I said I wouldn't run this approach as a DIY project since it may have stability issues that are harder to find and deal with without proper equipment.

JS

Thanks joaquins!

joaquins said:

No, two things here I'd change. First do not connect anything to the input ground, the pin 1 at the input goes directly to the chassis and nowhere else.

Click to expand...

So you mean connecting the shield (pin 1) from each input XLR connector to chassis, but don't connect this to ground on my PCB, right ?

The other thing is the decoupling and output ground. Decoupling should be from ground to the rail, not from ground to the rail in one side and from rail to rail in the other.

Click to expand...

Just for clarification: Per op amp, I've got the usual +/- rail to ground electrolytic in parallel with a ceramic here (4 caps). And I've added one rail-to-rail electrolytic. From my experience this is the most stable way to do it.  There is also one ceramic decoupling cap for each of the two +1.95V references.

Also you should connect all your 8 decoupling caps to a single ground point and from there run it to de output directly without going anywhere else. So you have your general ground, your decoupling caps and your output. Using a 0R jumper from the general ground to the decoupling caps could help when making the layout.

Click to expand...

Right, the "dirt ground". I didn't think it was necessary with large ground plains and a very high quality PSU, especially since the whole ground in the original design is a "dirt ground", since with the circuit being fully balanced all it connects to is decoupling caps.

Attached is a picture with parasitic ground resistance in place as it should be, any crossed parasitic grounds would introduce more dirt. The pict is for an unbalanced stage, in your case you don't need to care for the input part of it but you do care for the output. Best practice would be to make some kind of star ground at the decoupling caps, take from there the reference ground, single trace going to the PS input, another to the V/2 reference points and other to the output directly, so let's say you call 0V the decoupling caps ground node, any current to the output only introduces noise to the output, so no noise there, just a bit of signal loss equivalent to having a teeny tiny resistance in series, absolutely nothing to worry about it. To the V/2 reference would be practically no current so would be at 0V as well, for the PS input you'll have your supply current some how smoothed by the decoupling caps and only would be seen as PS dirt and not as signal reference or output dirt, as 5534 has good PSRR is not a problem. You could figure out a different way of connecting those 4 dots (decoupling node, PS input, signal output and V/2 reference) which works fine, this is what I'd do.

If you do it in another way, let's say you take your reference point from PS input instead of the decoupling caps you'll have the dirt introduced by the current draw at your reference, so your reference will be noisier. All this considerations are due to trace impedance, in audio usually we only care about the resistance usually in the mΩ range, in really low current applications usually is not a problem but best practice to have the considerations if you want to squeeze the last few dB of SNR+THD out of your opamps. In your case you want to drive a very capacitive load, so HF currents will be relatively high and introduce some noise to the ground at the decoupling caps.

Click to expand...

Do you mean I should have seperate grounds for decoupling of the V+, the V- and both Vcom lines ?

BTW, would it be a good idea to add 'global' decoupling caps before the 10R dampening resitors?

A more fancy decoupling topology could be used in your fully balanced configurations, but stability considerations should be taken and could make things much harder. As your load is from one output to the other the current would be from +PS of one opamp to -PS of the other opamp, rather than to ground as it would be in a unbalanced output stage. This means what you really need to decouple is the crossed rails from one opamp to the other needing only 2 sets of caps and no risk to introduce dirt at any point to the ground. Having this could potentially affect the stability of the opamps so I don't recommend going that way but I think it's nice to at least think about it as a mental exercise, where you follow the current rather than brute force make all ground points have as close voltage as possible to avoid signal degradation.

Current for negative output voltage is shown, for positive would be around the other cap but I didn't draw it to keep it clean. The reference drawn as ground but could be a divided voltage from one of the rails bypassed to ground with a cap big enough in relation with the resistors.

As I said I wouldn't run this approach as a DIY project since it may have stability issues that are harder to find and deal with without proper equipment.

Click to expand...

The stability issue is why I only use a cheap electrolytic for rail-to-rail decoupling, it's too sluggish to cause oscillation issues.

The stability issue may become with the crossed decoupling as I suggested since one opamp will be affecting the PS of the others, while the electrolytic is not a problem the ceramic, much closer and with effect at HF, together with the capacitive load may be an issue, your implementation about capacitive load is well done anyway.

Using a cap from rail to rail shouldn't be a problem, but usually the decoupling caps to ground are fine, I don't think you need any more capacitance in your circuit for decoupling, I didn't saw the caps from the other rail, my mistake here.

Input pin one only to chasis, yes.

1.95V reference voltage wouldn't be bad to have a electrolytic to avoid LF noise, depending on the resistors value.

There is no dirt ground here, you have currents going around but the decoupling caps are not making a dirty ground but providing a current path for the return current from the load, so load, opamp 1, decoupling cap 1 to PS rail A, decoupling cap 2 to rail B, opamp 2, load. Dirt ground we usually call the ground to drive LEDs, meters, relays or non critical digital stuff on a mixed signal board. You could avoid inserting this current into the ground with the decoupling scheme I advised, from one opamp to the other at the crossed rails, but as I said I'm not sure about stability, I'm not saying it will be a problem but may be. Also look that NE5534 is not stable at gain below 3 or so, which you don't have, so at least leave the place to put the external compensation cap at the PCB in case you need it.

I'm not saying to use separate ground but neither a ground plane, follow the currents in the grounds and run traces, they may be thick, even parcial planes but think of them as traces, not an overall thing. Connecting the grounds from each critical point to the other in the correct order and configuration is critical to archive the best performance from your converters and opamps. You do need a clean ground reference or you will be inserting noise as common mode in your converter. Also you should see that your approach is not making any about CM signals at the input since (I didn't made the math here) it's CMRR is less than one, or it will be amplifying more the CM than the NM signals, usually a 4 opamp approach is better to ensure good CMRR at the driving stage so you don't trust in the CMRR of the ADC and you avoid loosing headroom at the converter because of the CM signal. There are other quite clever approaches around for driving converters, with clever ways of adding the bias and getting best CMRR and all that. For what you are looking I think you are ok with your approach at least by now, is cheap and easy to build, I think you should give it a try as it is but with a bit more care on the ground management.

JS

Thanks again, much obliged!

joaquins said:

1.95V reference voltage wouldn't be bad to have a electrolytic to avoid LF noise, depending on the resistors value.

Click to expand...

I'll add it. It's not on the original board.

I've attached the schematic of the input of one channel of the PCM4222EVM input with my modifications, OPA1632 input op amp and OPA227 reference voltage buffer (not needed with the 5534) removed, zero-ohm resistors removed, all marked red. Output of my PCB goes to the +/- inputs in yellow. There is no connection to the ground, since the PSU has a ground connector that is connected to the audio ground of the EVM4222 as well as to my PCB.

Also look that NE5534 is not stable at gain below 3 or so, which you don't have, so at least leave the place to put the external compensation cap at the PCB in case you need it.

Click to expand...

Sure, that's why the 22pf compensation cap is there.

I'm not saying to use separate ground but neither a ground plane, follow the currents in the grounds and run traces, they may be thick, even parcial planes but think of them as traces, not an overall thing. Connecting the grounds from each critical point to the other in the correct order and configuration is critical to archive the best performance from your converters and opamps. You do need a clean ground reference or you will be inserting noise as common mode in your converter. Also you should see that your approach is not making any about CM signals at the input since (I didn't made the math here) it's CMRR is less than one, or it will be amplifying more the CM than the NM signals, usually a 4 opamp approach is better to ensure good CMRR at the driving stage so you don't trust in the CMRR of the ADC and you avoid loosing headroom at the converter because of the CM signal. There are other quite clever approaches around for driving converters, with clever ways of adding the bias and getting best CMRR and all that. For what you are looking I think you are ok with your approach at least by now, is cheap and easy to build, I think you should give it a try as it is but with a bit more care on the ground management.

JS

Click to expand...

So what is wrong / should be changed as far as grounding in my PCB is concerned? I'm not an EE myself and lack the theoretical background, so I'm following rules of thumb and use what has worked for me in the past or to my knowledge is general practice.

Start the PCB design placing the opamps and decoupling caps all as close as possible (the decoupling caps to the opamps and the decoupling caps with each other). From the ground that ties together all the decoupling caps route in separate traces the ground to the output and PS. The ground to for the reference voltage where your reference divider resistors and cap goes could be tied to the decoulping caps or to the output, depending on philosophy. You could probably make a central island for putting together the decoupling caps ground and route the grounds from there.

I don't see any attachment on your last post, or are you talking  about a previous one?

JS

joaquins said:

Start the PCB design placing the opamps and decoupling caps all as close as possible (the decoupling caps to the opamps and the decoupling caps with each other). From the ground that ties together all the decoupling caps route in separate traces the ground to the output and PS. The ground to for the reference voltage where your reference divider resistors and cap goes could be tied to the decoulping caps or to the output, depending on philosophy. You could probably make a central island for putting together the decoupling caps ground and route the grounds from there.

I don't see any attachment on your last post, or are you talking  about a previous one?

JS

Click to expand...

Thanks. I set the ceramic decoupling caps closests to the op amps and the electrolytic decoupling caps next.

So there should be an output ground "trace" (via the xlr cable's ground) to the EVM PSU?

Forgot to add the attachment, it's here now.

I haven't paid close attention to this thread so sorry if this has already been discussed.  I gather the 270 ohm feedback R and 560 input Rs are to keep thermal noise down. 560 Ohms seems a little low for many legacy products to drive cleanly. In general distortion often tracks with current, so higher current (from driving lower R) means higher distortion.

Since the chip is running from a 4V rail you could probably afford to attenuate more than -6 dB at that input stage to facilitate hotter, easier to drive input signals.  1.2k-2k  input Rs would be easier.

JR

JohnRoberts said:

I haven't paid close attention to this thread so sorry if this has already been discussed.  I gather the 270 ohm feedback R and 560 input Rs are to keep thermal noise down. 560 Ohms seems a little low for many legacy products to drive cleanly. In general distortion often tracks with current, so higher current (from driving lower R) means higher distortion.

Since the chip is running from a 4V rail you could probably afford to attenuate more than -6 dB at that input stage to facilitate hotter, easier to drive input signals.  1.2k-2k  input Rs would be easier.

JR

Click to expand...

Thanks John, I already accounted for this (1k resistor on the circuit board). I am using 1.2k in the one I actually built, works fine.

The converter itself is so good in terms of SNR that staying way below digital maximum won't hurt in real life.

living sounds said:

...
Thanks. I set the ceramic decoupling caps closests to the op amps and the electrolytic decoupling caps next.

So there should be an output ground "trace" (via the xlr cable's ground) to the EVM PSU?

Forgot to add the attachment, it's here now.

Click to expand...

Ok, from XLR pin 1 to chasis as short as possible, I like to use a wire directly to a mounting screw of the connector.
At some point the chasis goes to the PSU ground.
The PSU ground goes to the board, in there goes to the decoupling caps first and from this point you split into the two other points you need to go, the V/2 reference and the output to the ADC.

If you could use the reference voltage from the ADC may be optimal, they know how much voltage they need and they work from there, that's why they provide the connection to the reference voltage.

JS

joaquins said:

living sounds said:

...
Thanks. I set the ceramic decoupling caps closests to the op amps and the electrolytic decoupling caps next.

So there should be an output ground "trace" (via the xlr cable's ground) to the EVM PSU?

Forgot to add the attachment, it's here now.

Click to expand...

Ok, from XLR pin 1 to chasis as short as possible, I like to use a wire directly to a mounting screw of the connector.
At some point the chasis goes to the PSU ground.
The PSU ground goes to the board, in there goes to the decoupling caps first and from this point you split into the two other points you need to go, the V/2 reference and the output to the ADC.

If you could use the reference voltage from the ADC may be optimal, they know how much voltage they need and they work from there, that's why they provide the connection to the reference voltage.

JS

Click to expand...

Be careful, you don't want to load the ADC's reference voltage output. VCOM is the ADC chip output you want to use to bias the differential driver properly.

-a

Final had time to finish this project. I've added 47uf tantalum caps for filtering the reference voltage. The ground from the xlr cable coming in is connected to the chassis right at the input and the PSU ground connects to the chassis as well.

The unit is dead quit now and measures as good as the board did with the differential op amp it came with, so I didn't make any further changes to the grounding etc. But I'm using a high quality regulated PSU and added chokes to further filter all incoming voltages.

Here's the pcb design. If anyone is interested I'll upload silkscreens, copper layer and a bom.

Thanks for all the help!