Still more interested in playing bad semantics than anything else I see.
The only problem that you rightly point is the need to avoid a contamination of the input opamp PS and 0V reference by the noise induced by the lme49600 on the rails. It is however quite easy to reduce that interaction to inconsequential levels.
If this is taken care of (by layout, the PSRR of the input opamps, additionnal decoupling/regulation), then the noise at the output of the amplifier will be not only determined by the PSRR of the buffer but also by the amount of feedback the input opamp applies around the buffer.
The only problem that you rightly point is the need to avoid a contamination of the input opamp PS and 0V reference by the noise induced by the lme49600 on the rails. It is however quite easy to reduce that interaction to inconsequential levels.
If this is taken care of (by layout, the PSRR of the input opamps, additionnal decoupling/regulation), then the noise at the output of the amplifier will be not only determined by the PSRR of the buffer but also by the amount of feedback the input opamp applies around the buffer.
You'll see what you choose to see. Incidentally did you figure out what I was saying about your common-mode noise issue on the project you solicited input on a few days back?
You go ahead then and show to the OP how easy that is on his layout and I'll maintain a watchful eye in case you overlook something.
Frankly ? Not really.
A groundplane is a nice way to get low impedance for your returns but what about the power rails ? With thin tracks, the big decoupling caps far away from the buffer and the input opamps in between those caps and the buffers, the current draw from the buffer will modulate heavily the supply of the opamps. A better way to do it would be to have in order: the PS input, the big decoupling caps, the buffer PS pins, a RC filter, the input opamps PS pins.
Furthermore, your sensitive input and feedback ground nodes are connecting to ground right in the middle of the returning currents of the buffer. Even if the groundplane has a low resistance, it's still not the best way to proceed. Try to place your components in such a way that the input and feedback ground nodes are linked to a groundplane section, the decoupling caps for the buffers to another groundplane section. Those two sections should come together at the output ground pin of your headphones jack.
I'm not shure, if it is wise to interfere in your controversy, so just let me say: I'm thankful for the advice of you both.
@abraxalito: You gave (and hopefully will give) good advice how to optimize the PS as a main reason for bad sound quality (as you pointed out, the raw silicon is by far good enough for compelete transparency).
@00940: You suggested to optimize to optimize the amplifier design to make it more robust against distorsions.
Beside the disagreeing "No." I don't see, how you are contradicting each other and I'm anxious to implement all of your hints.
@00940:
So your advice is:
- reorder components horizontally (as listed)
- seperate signal and power bypass ground
At one point I'm not shure if it is possible to implement:
As (at least for power bypass ground) very short traces are necessairy to avoid too much inductance I need the ground at very spread positions. Should I prefer keeping it a plane and connect signal ground as traces or should I use some comb-like ground structure to reach all positions by both grounds?
@abraxalito: You gave (and hopefully will give) good advice how to optimize the PS as a main reason for bad sound quality (as you pointed out, the raw silicon is by far good enough for compelete transparency).
@00940: You suggested to optimize to optimize the amplifier design to make it more robust against distorsions.
Beside the disagreeing "No." I don't see, how you are contradicting each other and I'm anxious to implement all of your hints.
@00940:
So your advice is:
- reorder components horizontally (as listed)
- seperate signal and power bypass ground
At one point I'm not shure if it is possible to implement:
As (at least for power bypass ground) very short traces are necessairy to avoid too much inductance I need the ground at very spread positions. Should I prefer keeping it a plane and connect signal ground as traces or should I use some comb-like ground structure to reach all positions by both grounds?
I don't believe I pointed out that the silicon that you have there is good enough for subjective transparency. I've gone away from using simple diamond output buffers myself because I've not found them completely transparent subjectively but I'll not suggest you go the same way as I've gone - far too much of a workup for you without any evidence from your own ears that its worth it. I'm content for now to stick within the boundaries you've set down - the opamps and the IC buffer will take you quite a long way towards subjective nirvana with the details of layout (control of noise currents especially) addressed.
Not only do power supply noise currents need addressing carefully but also common-mode currents that'll be flowing (in the 0V connection) between your source equipment and the mains supply you have for this unit. If you're definitely using balanced inputs addressing these becomes very much easier.
I've also noticed you have a fairly lowish input impedance - subjectively I've found that the higher the input impedance the better the SQ so you might wish to address that point too. With opamps its not really difficult to achieve a few hundred kiloohms for input impedance.
sorry for this, it won't happen again. 😱 I'll stick to practical stuff.
What I was trying to point out: you don't need to have two groundplanes. But the signal ground and the power ground shouldn't share the same areas on that plane, as much as possible.
Consider what happens if you put the opamp at the left, the buffer in the middle (as well as the output) and the PS at the right. Keep a groundplane for everything. At the left, the only PS currents circulating are very low (the opamp is lightly loaded) and due to the low impedance of the groundplane won't induce much error voltage. At the right, we have charging currents circulating in between the PS and the buffer's decoupling caps. And in the middle, we have the return current from the headphones, going back to the PS on the right while providing to its left a clean sense point for the input opamp.
As an aside: try to keep the + and - PS rails close to one another. One more restriction, I know...
Alright, so thank you both for your rich feedback!
It will take me some time to implement all of them. (Additionally there are some physical design constraints, f.e. fitting all the 16 channels in one 19" rack width.)
If you have another comment, please don't hesitate to post it, it is very appreciated.
@abraxalito:
Yes, the signal input is fully balanced on both sides. Therefore R10 is inserted, so the ground can be lifted or chocked or whatever is necessairy (as it is only the signal shielding).
The source impedance is 75 ohms (bal.) (i mixed it up in the first post). Currently the input impedance is defined by the balanced to unbalanced conversion. I could buffer the balanced signal by an additional 2-channel opamp. Do you think it is worth the effort?
@00940:
With the physical output I am restricted in the layout (max. 48mm width, output at one of the short sides, no additional interfaces at this side). But I thought about virtually placing it somewhere else by putting some (thick, about 1mm) extra traces from the physical placement to the virtual placement and only there connecting to ground and amp/filter output.
Do you think this will do the job as well? Thus I would get more freedom with the placement of the other components.
@abraxalito:
Just one further question:
When driving the DC servo by a JFET, does it work well? I don't have that much experience with that, therefore I added space for a blocking cap.
But if I don't need it for sure, I could save its space for more freedom in placement.
It's just I want to have PCBs manufactured so I can't add it later on.
When I am finished with the redesign (could take some days as I'm a bit busy in work), I will post the result.
If you don't mind I would appreciate your comments on the result.
It will take me some time to implement all of them. (Additionally there are some physical design constraints, f.e. fitting all the 16 channels in one 19" rack width.)
If you have another comment, please don't hesitate to post it, it is very appreciated.
@abraxalito:
Yes, the signal input is fully balanced on both sides. Therefore R10 is inserted, so the ground can be lifted or chocked or whatever is necessairy (as it is only the signal shielding).
The source impedance is 75 ohms (bal.) (i mixed it up in the first post). Currently the input impedance is defined by the balanced to unbalanced conversion. I could buffer the balanced signal by an additional 2-channel opamp. Do you think it is worth the effort?
@00940:
With the physical output I am restricted in the layout (max. 48mm width, output at one of the short sides, no additional interfaces at this side). But I thought about virtually placing it somewhere else by putting some (thick, about 1mm) extra traces from the physical placement to the virtual placement and only there connecting to ground and amp/filter output.
Do you think this will do the job as well? Thus I would get more freedom with the placement of the other components.
@abraxalito:
Just one further question:
When driving the DC servo by a JFET, does it work well? I don't have that much experience with that, therefore I added space for a blocking cap.
But if I don't need it for sure, I could save its space for more freedom in placement.
It's just I want to have PCBs manufactured so I can't add it later on.
When I am finished with the redesign (could take some days as I'm a bit busy in work), I will post the result.
If you don't mind I would appreciate your comments on the result.
If you think about it, the physical output and the traces leading to it are just an extension of the headphones cable... which means there's no real need for thick traces. The only requirement is to keep the ground and signal wires close to one another.
With only two layers, don't hesitate to make use of wires and jumpers. You could for example have the output jack connected to the amp's outputs (L,R,groundplane) at any point you want with a few cm of twisted wire.
Last edited:
No I don't - it looks to me that you can raise the impedance of the resistor/cap networks that you already have in place.
Presumably here you mean a JFET opamp? No reason it'll work any worse than with a bipolar, except the input bias currents will be much much lower and hence the output offset will be dominated by the opamp's offset voltage rather than its input bias currents.
Most likely a servo's going to take up less space than a blocking cap? For low impedance headphones the cap will want to be into the millifarad range to avoid premature bass roll-off.
Whilst on the subject of caps, I'd avoid SMT types for power rail decoupling as in my experience (measurement of samples) they tend to perform poorer in terms of ESR than leaded ones do. For signal coupling they'll be fine as then ESR isn't an issue.
I quickly checked Mouser and the lowest ESR they're showing for SMT 470uF/25V is 60mohm whereas I found Panasonic FM/FR are at 30mohm (the latter being leaded). Go for the narrower, taller can sizes (hoping you have enough height) rather than shorter, fatter ones for PSU duty.
So I tried to implement all of your advice.
I know, only one channel currently is layed out, but I thought to obtain your feedback before proceeding.
I tried to implement following changes:
- Using TL082 as DC servo
- changed coupling of DC servo to -40 dB
- added alternative assembly for high input impedance (10k -> 100k)
- using leaded caps for PSU bypass
I also thought about tapping the ground for the output connector in the right of the LE49600, because it is much closer to the GND of the PSU and thus its currents have less influence to the GND reference.
But this way it would connect close to the PSU bypass capacitors. Would be the PSU noise be (much more) audible in this config?
Additionally I made some changes to the PSU design:
- move series resistor
- add EMI filter
- (externally) add common mode choke
So what do you think about the project now? Could I achieve the goal of high linear transparent sound?
Shall I proceed with the second channel or should I still revise something?
Thanks for all your effort!
I know, only one channel currently is layed out, but I thought to obtain your feedback before proceeding.
An externally hosted image should be here but it was not working when we last tested it.
An externally hosted image should be here but it was not working when we last tested it.
I tried to implement following changes:
- Using TL082 as DC servo
- changed coupling of DC servo to -40 dB
- added alternative assembly for high input impedance (10k -> 100k)
- using leaded caps for PSU bypass
I also thought about tapping the ground for the output connector in the right of the LE49600, because it is much closer to the GND of the PSU and thus its currents have less influence to the GND reference.
But this way it would connect close to the PSU bypass capacitors. Would be the PSU noise be (much more) audible in this config?
Additionally I made some changes to the PSU design:
- move series resistor
- add EMI filter
- (externally) add common mode choke
An externally hosted image should be here but it was not working when we last tested it.
So what do you think about the project now? Could I achieve the goal of high linear transparent sound?
Shall I proceed with the second channel or should I still revise something?
Thanks for all your effort!
As regards the input impedance changes you've made its not looking like they'll work in practice. Do you know how to use a circuit simulator? Your 0.01% tolerance Rs at the input to the first opamp are still 10k - the one on the -ve input will determine the input impedance. They'll need to be increased to get the higher Zin. One side effect of higher Zin is you can reduce your 2.2uF caps to something around 10X lower which allows you to use relatively cheap NP0 input caps (SMT).
Your output inductor is what part? You'll want to check its a shielded one. TDK have some jolly nice 7mm diameter SMT inductors which might be suitable here.
I'm not sure of the utility of the EMI filter you've added. What's its spec please? The 220nF input caps should have series Rs so they'll introduce damping. I'd also not use a preset pot over its whole range to set the output voltage - decide what range of output voltage you need and include a series R with it. Otherwise with a very wide control range there's the chance of some instability in the setting.
Are you intending to have around 20dB gain from the first stage? Seems to me this is likely to clip.
Your output inductor is what part? You'll want to check its a shielded one. TDK have some jolly nice 7mm diameter SMT inductors which might be suitable here.
I'm not sure of the utility of the EMI filter you've added. What's its spec please? The 220nF input caps should have series Rs so they'll introduce damping. I'd also not use a preset pot over its whole range to set the output voltage - decide what range of output voltage you need and include a series R with it. Otherwise with a very wide control range there's the chance of some instability in the setting.
Are you intending to have around 20dB gain from the first stage? Seems to me this is likely to clip.
The assembly variants are described in the values - seperated by slashes. So the original variant was R11=10k, R1=R2=R3=R4=10k 0.01% - the new variant is R11=n.a., R1=R2=R3=R4=100k 0.1%. The values of R2 und R4 are removed due to the long value text of R1 and R3. (The long text all describes one resistor.)
So: No gain (Av=1), but in the second variant, the input impedance should be 100k.
But I think I still need a film capacitor as 220nF won't be available as NP0 (which goes up to about 1nF). And I guess I want to avoid class 2 ceramic caps because of their non-linearities.
Atm I thought about the DR0608. But I doubt it is shielded. Which one did you refer to? After a quick search in digikey I would guess you meant CLF7045T-100M-CA or SLF7055T-100M2R5-3PF, did you?
http://www.bourns.com/data/global/pdfs/emi_t_series.pdf
It's number 10 in the datasheet (Subtype 103).
As you were worried about the RF I thought blocking the MHz range (which is attenuated by 25 dB here) would be a good idea. Of course I can install a discrete filter, but I think this wouldn't change the filter response very much.
Last edited:
Aha, my mistake in missing that vital slash. If your resistors are all 100k then there's no gain, but the Zin is then going to be lower on the -ve side when driven balanced (from memory about 66k). Incidentally the 220k resistors prior to this appear not to have any function, other than adding loading.
0.01% resistors aren't worth using in practice as most likely your CMRR is going to be limited by the non-zero source impedance. Higher values though should improve the CMRR. If your aim is to get the very best CMRR then look into the ICs from THAT corp which have trimmed resistors and bootstrapping to raise the CM impedance. For myself I doubt its worth it though.
I have plenty of NP0 caps above 1nF - the largest I consider to be cost-effective is 100nF. They do exist higher than this but get expensive pretty rapidly. If you need 220nF I'd use two 100nF in parallel, they're only 1206 size. NP0 is class1, not class2 - TDK?s Guide to MLCC Temperature Characteristics | FAQ | Multilayer Ceramic Chip Capacitors | TDK Product Center
I was thinking SLF7045 but either of those others look fine too.
I'll take a look later on.
I was a bit concerned about putting AC into the filter - coming out of the rectifier there will be edges which might cause this filter to ring. Best to keep all the RF filtering on the DC lines. The larger sized TDK inductors might work OK (above 7mm as the current capability's a bit low in these).
Not a lot of time on hand, just a short comment: you'd have a more compact design by pushing C18, U$2 and all the components at the output in the empty spaces next to the headphones jack. They're out of the feedback loop and in line, so it doesn't matter much where they go. It would however shorten the feedback loop and that would be a good thing.
The 220k resistors on both sides of the cap originally had the purpose to set the DC offset to zero. On the right they are only needed if the voltage is buffered and the right side is floating, so - as you stated - they can be removed in this design.
On the left side I would keep them. (I don't know wether you referred to them, too.) Depending on the design of the source, this side could really be floating in means of common mode (f.e. when using an output transformer in the input source).
Oh yes, there are really nice line receivers, especially the THAT1200. Unfortunately they know it, too, and charge a nice little sum. (about $5 at mouser, nearly as much as the LME49600.)
While dimensioning the resistors R1 to R4 I thought of a source impedance of 75 ohms. If not the most cheapest ones were chosen for the output stage of the input source device, they could be about 1% tolerance, so (a bit less than) about 1 ohm. Therefore I didn't want to further decrease the impedance matching and chose a tolerance of 1 ohm, too.
[The resistance and capacity of a wire <10m should be negligible in this calculation (<< 1R series, >> 1 Meg parallel).]
But if I can relax that to 0.1% it would relax the financial calculations, too. 😀
However I made some calculations about noise (inspired by considerations of approximating the influence of the THAT1200):
As the LME49720 are of bipolar type, they have an noise resistance of about 2k ohms (referring to the datasheet). Thus using 10k input impedance the noise already is dominated by the equivalent input noise current - not the equivalent input noise voltage anymore. If increasing the input impedance to 100k the output noise voltage will raise by nearly 20 dB to about 20uV/-91dBu (typical), which is only 26 dB lower than the PSU noise of about 450uV/-65dBu (which is also the approximate RMS level of the residual 100Hz ripple).
Have I missed something or could I really get some audible noise here?
Fascinating 😱 There are indeed available some NP0 caps up to 470nF - or at least 100nF with usable casing and rated voltage. (And some of them additionally are reasonably priced.)
Sorry for expressing that uncertain: NP0 is class 1, but I don't want to use class 2 (X..., Y..., Z... types) ceramic caps. Not because of the temperature characteristics (varies in seconds, so much slower as the signal itself) but because of the voltage dependencies (modulates signal with itself = distortion).
Alright. But I'm a bit confused at this point. Did you recommend to use them in the signal chain (output) or for the PSU (as indicated in the quote below)?
So you suggest to replace the filter by series inductors at the same position. Did I get this right?
Yes, I thought about this, too. But unfortunately this is impossible in the current design due to physical constraints (I didn't mention - sorry):
The area in the top and in the bottom of the connector is occupied by potis and LEDs (also mounted in the front plane of the case).
To fit all 16 channels in the rack case I have to get along with 5cm width - or in the perspective of the board layout: height - for every 2 channel module.
The only alternative would be to put all connectors off-board. So I can 1) use the whole board area and 2) can place the pcb some cm away from the front panel so I don't have to mess with the front-interface.
But atm I wanted to avoid the 2 downsides: Increasing (unbalanced) signal length and having to connect everything by wires instead of soldering it directly onto the PCB.
But what do you think about ground and supply decoupling in this design. Did it work?
Last edited:
If their purpose is only to keep the offset at zero then keep them but increase the value - let's say 1Mohm. No particular reason for 220k that I can see.
0.1% resistors nowadays are quite affordable - here in China about 1mao (a little more than one Euro cent).
I concur with your noise calculations, that opamp is indeed designed for low source impedances. I suggest swapping it out for a low noise and JFET opamp. Finding one that's JFET and low noise and cheap though is something of a challenge - I looked at TI's newest offerings and they seem to have gone over to MOSFET input types at the low cost end. One I like is the ISL28210 but its not particularly cheap from Mouser in small qtys.
Worries about class 2 seem to me to be overblown, they do a great job at decoupling because of small size (so low ESL) and very low ESRs. The voltage dependency in signal coupling applications can be reduced by oversizing the cap so there's practically no AC voltage generated across it. Easy to oversize when they're so small and cheap. My main concern with them is microphony.
Both - but different current ratings in each - your supply needs 2A or so but no more than 200mA is called for for the headphone out.
I suggest the inductor after the first smoothing cap, not prior to it.
I have looked for some alternatives to the LME49720 in a reasonable priced area.
I haven't found very much, but what do you think about LT1122 or OPA1652 (not ...42)?
(Just one small appendix to the ceramic caps: Of course I only referred to those of them, which are in the signal chain. As you can see, I have used them for decoupling, too.)
I haven't found very much, but what do you think about LT1122 or OPA1652 (not ...42)?
(Just one small appendix to the ceramic caps: Of course I only referred to those of them, which are in the signal chain. As you can see, I have used them for decoupling, too.)
- Status
- Not open for further replies.