This is the current state of the project:
Please note:
- As stated a little earlier, C19 is just a SMD jumper with value 0R or not assembled. I intended to correct this, but forgot to do so before this post.
- For identical blocks, only one of the two channels is shown (for the sake of clarity).
- While moving blocks to do so, I accidentally showed the wrong Opamp-Power-Block (U1_SUP and U3_SUP, but amps U2 and U4 shown) - U2_SUP and U4_SUP is identically.
Again: Please excuse not to place the name labels good readable.
Changes since last update:
- removed DC servo
- removed 2nd AC coupling
- added the possibility for both: assembly with or without buffer
NOTE: the schematics currently only show the configuration for "with buffer" as the configurations "without buffer" didn't change very much since last update
- significantly reduced signal lengths, especially those between output buffer and its driving opamp (although it is still "long")
- reduced signals on 2nd layer (to only 5 short tracks) so GND plane is nearly uninterrupted
- simple power supply distribution (high current: direct, others: RC-buffered through "mid-rail") - V+ and V- always directly together
- shielded SMD output inductor
- make all electrolytic capacitors leaded types
- added weak pull-down for pot output
- moved output RF bypass to output connector
- increased opamp bypass capacitors to 2,2 uF (as easily available for SMD 0603 with 50V voltage rating)
@all: Still some comments left for this part of the Amp?
NOTE: (especially @sgrossklass)
There is a seperate PCB for all "user interfacing" (pots, pre-gain, level indicators), which will be stacked on this PCB.
As the signal has to pass it either way (because of the pot) I want to implement the pre-gain on this "UI-PCB".
Please correct me, if this is a bad idea!
An externally hosted image should be here but it was not working when we last tested it.
Please note:
- As stated a little earlier, C19 is just a SMD jumper with value 0R or not assembled. I intended to correct this, but forgot to do so before this post.
- For identical blocks, only one of the two channels is shown (for the sake of clarity).
- While moving blocks to do so, I accidentally showed the wrong Opamp-Power-Block (U1_SUP and U3_SUP, but amps U2 and U4 shown) - U2_SUP and U4_SUP is identically.
An externally hosted image should be here but it was not working when we last tested it.
Again: Please excuse not to place the name labels good readable.
Changes since last update:
- removed DC servo
- removed 2nd AC coupling
- added the possibility for both: assembly with or without buffer
NOTE: the schematics currently only show the configuration for "with buffer" as the configurations "without buffer" didn't change very much since last update
- significantly reduced signal lengths, especially those between output buffer and its driving opamp (although it is still "long")
- reduced signals on 2nd layer (to only 5 short tracks) so GND plane is nearly uninterrupted
- simple power supply distribution (high current: direct, others: RC-buffered through "mid-rail") - V+ and V- always directly together
- shielded SMD output inductor
- make all electrolytic capacitors leaded types
- added weak pull-down for pot output
- moved output RF bypass to output connector
- increased opamp bypass capacitors to 2,2 uF (as easily available for SMD 0603 with 50V voltage rating)
@all: Still some comments left for this part of the Amp?
NOTE: (especially @sgrossklass)
There is a seperate PCB for all "user interfacing" (pots, pre-gain, level indicators), which will be stacked on this PCB.
As the signal has to pass it either way (because of the pot) I want to implement the pre-gain on this "UI-PCB".
Please correct me, if this is a bad idea!
Last edited:
Out of curiosity, do you have a link or further details on this Midas box?
On your revised schematic, its looking like you have maintained low impedance loading of your opamps. Great for low Johnson noise, not so great for SQ.
On the layout you've moved the input connectors to the opposite end, away from the power connector. So now there's the potential for high frequency common-mode currents to flow through your groundplane between the 0V pins of both (via C13 in the case of the input connector JP2). If you take pin1 of your XLRs direct to chassis, as is recommended practice, also there should be just one link between chassis and the 0V (groundplane) on the PCB - in a system with more than one channel as here that would most likely be at the power input (JP1).
There's a version slightly optimized for live performance and one for fixed installations (or more complex setups):
DL16 | I/O Interfaces | Mixers | Midas | Categories | MUSIC Group
DL153 | I/O Interfaces | Mixers | Midas | Categories | MUSIC Group
Unfortunately I don't have the reviews I read at hand, but I found the link to a technical review of the mixing console where they used the same modules:
http://www.msmsystemsinc.com/storage/blog_pix/M32 Review.pdf
As I mentioned I plan a side by side comparance of the both architectures (low impedance with buffers using LME49720 vs high impedance without buffers using the ISL or OPA). I simply have to connect pin 2 to 3 and 5 to 6 of the buffer opamp pads (without a buffer installed) to use this layout without buffer.
But I'm a bit confused and maybe you could bring some light into the darkness:
Regarding SQ vs Impedance I thought you referred to the input impedance. This is the reason I added the buffers in variant 2. So I can use the full potential of LME49720 by using 2k2 resistors while keeping a very high input impedance by using the buffers. Thus I thought I could achieve both: Low noise and the best possible SQ. (Based on the assumption only the impedance seen by the signal source matters.)
Or did I understand you wrong regarding the correlation between impedance and SQ?
Yes, this layout modification intended to reduce the influence of the power supply and ground currents of the LME49600. But I think I understand what you are pointing out. If there's no smart solution I will simply implement your suggestion by wires as it is only one connection per board. Thanks for the hint.
Right, I noticed you had introduced options. I look forward to hearing of some listening comparisons 🙂
Yes I was referring to the input impedance, but its a general principle that opamp-based circuits tend to sound less dynamic the lower the impedance that they drive. The input (source) typically comes from an opamp-based circuit since they're ubiquitous nowadays. Hence the lighter its load, the better for SQ. Internally if you keep loads very light you'll end up with opamps with their output stages not exiting classA and hence have lower noise on your supply rails. Meaning less spent on fancy low impedance caps - I was also going to add '...and regs' but you've got yours so distant improving their output impedance won't do much.
The load-induced currents are a different matter from externally induced currents - when I spoke of 'common-mode currents' I was speaking of the latter.
It really looks nicer and nicer. A few nitpicking comments though:
- If you use a fet opamp for the buffers, you can have even higher input impedance without penalty.
- It might not be useful to have seperate rc filters for left and right channel opamps' PS. I'd rather use two caps for all the opamps than split them into two rc filters. Crosstalk really isn't much of an issue with headphones unless you get tons of it.
- You can quite easily push the rc further right, move C18 and L1 just to the right of the jack and push all the rest closer to the buffer. That will shorten the feedback again.
- jcx pointed out to me that it was a good idea to use physically larger resistors for the feedback network, to limit thermal modulation. Especially here since you're using low value resistors. I'd consider using 1206.
- I wouldn't worry too much myself about SQ and opamp's loading. Still, I wouldn't go under 2k to 3k if there's no imperious reason for it. Since you're not at microphone level, no need to go extreme wrt noise.
- I might be missing something but... C20 goes to a plane that doesn't appear to connect to anything else.
- As a safety (and even more so if you don't fit the output capacitor), I wouldn't use simple 3 pins connectors to connect to the PS, unless you plan on soldering them. If you want to use connectors so that you can remove cards, I'd use a 6 pins one (two rows), with connections in parallel. That will make the connection much stronger.
- If you use a fet opamp for the buffers, you can have even higher input impedance without penalty.
- It might not be useful to have seperate rc filters for left and right channel opamps' PS. I'd rather use two caps for all the opamps than split them into two rc filters. Crosstalk really isn't much of an issue with headphones unless you get tons of it.
- You can quite easily push the rc further right, move C18 and L1 just to the right of the jack and push all the rest closer to the buffer. That will shorten the feedback again.
- jcx pointed out to me that it was a good idea to use physically larger resistors for the feedback network, to limit thermal modulation. Especially here since you're using low value resistors. I'd consider using 1206.
- I wouldn't worry too much myself about SQ and opamp's loading. Still, I wouldn't go under 2k to 3k if there's no imperious reason for it. Since you're not at microphone level, no need to go extreme wrt noise.
- I might be missing something but... C20 goes to a plane that doesn't appear to connect to anything else.
- As a safety (and even more so if you don't fit the output capacitor), I wouldn't use simple 3 pins connectors to connect to the PS, unless you plan on soldering them. If you want to use connectors so that you can remove cards, I'd use a 6 pins one (two rows), with connections in parallel. That will make the connection much stronger.
First of all: Sorry for the pause. Unhappily I was busy the whole weekend.
Yes, I'm looking forward to them, too. 🙂
Alright, so I got you right concerning, what you spoke about, although I wasn't thinking about it before. I added an additional grounded drill, but I'm not happy about the position. But if I place it at the left side, I have to connect grounds (and use a soldered connection because of too few space).
Do you think it will do its job or should I revise it?
1- As I'm also testing just the OPA1652, I will add a test with OPA1652 as buffer and LME49720 as input stage. Thanks for the tip.
2- Makes things easier, yes.
3- Yeah, we mentioned that already, but sadly the physical space is already occupied by the front-interface. But I revised the connector to the interface-board (stacked on top of this board) and moved the LME49600 10mm to the left. (Also reduced board length from 100mm to 90mm.)
4- Good point!
6- The through hole connection of the output jack is plated and connects the ground plane to the ground signal (on top)
7- Good point, too.
Yes, I'm looking forward to them, too. 🙂
Alright, so I got you right concerning, what you spoke about, although I wasn't thinking about it before. I added an additional grounded drill, but I'm not happy about the position. But if I place it at the left side, I have to connect grounds (and use a soldered connection because of too few space).
Do you think it will do its job or should I revise it?
1- As I'm also testing just the OPA1652, I will add a test with OPA1652 as buffer and LME49720 as input stage. Thanks for the tip.
2- Makes things easier, yes.
3- Yeah, we mentioned that already, but sadly the physical space is already occupied by the front-interface. But I revised the connector to the interface-board (stacked on top of this board) and moved the LME49600 10mm to the left. (Also reduced board length from 100mm to 90mm.)
4- Good point!
6- The through hole connection of the output jack is plated and connects the ground plane to the ground signal (on top)
7- Good point, too.
Not quite. What I suggested earlier was to use the empty space above and below the jack (using the posted image as a reference). What I'm suggesting now is rather to put the output cap/inductor where C10 is and push everything else to the right. But you'll have to see if it makes sense with your add-on board or not.
According to your picture, the groundplane doesn't connect to the through hole connection. Unless there is a thermal relief hidden under the top track? Difficult to see for us 😉
As the schematics didn't change significantly I'm just updating the layout here:
An externally hosted image should be here but it was not working when we last tested it.
Ah ok, sry my fault. But good idea, I will check this.
Yes, that's how it is. (Really hard to see.) Because of the board outline and the drilling only 2 thermal relief remain. If that's not enough, I'll add additional vias.
I just arranged the upper half like you suggested.
What do you think?
For me, I'm unsure which is better. The one on the top is a bit nicer between driving opamp and output buffer, but I like the input stage design of the one on the bottom much more.
Btw: I wasn't sure where to pick up the ground for the output. I didn't want to connect it left of any opamp signal ground, but as there's no (significant) space left between output buffer and opamps I just took the ground from right of the buffer.
What do you think?
For me, I'm unsure which is better. The one on the top is a bit nicer between driving opamp and output buffer, but I like the input stage design of the one on the bottom much more.
An externally hosted image should be here but it was not working when we last tested it.
Btw: I wasn't sure where to pick up the ground for the output. I didn't want to connect it left of any opamp signal ground, but as there's no (significant) space left between output buffer and opamps I just took the ground from right of the buffer.
Last edited:
I'm unclear what the purpose of your grounded drill hole is, would you explain it please?
Incidentally, before finalizing the PCB it'd be a good idea to sketch out the grounding arrangements of the complete system. Just in case there are some hidden 'gotchas' 🙂
As the two drillings on the right are isolated to GND I added the drilling in the middle to get the link between chassis and GND. Or doesn't that work as desired?
I'm concerned that you've said this system is multi-channel. What you definitely do NOT want is multiple connections between your 0V and your chassis - which appears to be what you'll get if you use that GND on all of your PCBs.
My take would be if you want a pillar to connect between 0V and chassis, that should be on the PSU PCB. Because you only have one of those, right?
My take would be if you want a pillar to connect between 0V and chassis, that should be on the PSU PCB. Because you only have one of those, right?
Ahh, ok, so you mean one connection on total (per device), not per PCB.
So I was just right before adding the grounded drilling?
I originally planned to isolate ground from the chassis (isolated spacers for PCB mounting, and plastic output jacks NR-J6HF) and just to connect mains ground/earth wire, chassis and PSU GND at the PSU.
Is this what you suggested?
<edit>Sry, I forgot to answer your question: Yes, one PSU, 8 Amp PCBs, 8 Amp Interface PCBs
So I was just right before adding the grounded drilling?
I originally planned to isolate ground from the chassis (isolated spacers for PCB mounting, and plastic output jacks NR-J6HF) and just to connect mains ground/earth wire, chassis and PSU GND at the PSU.
Is this what you suggested?
<edit>Sry, I forgot to answer your question: Yes, one PSU, 8 Amp PCBs, 8 Amp Interface PCBs
Last edited:
You were right except potentially for the fact that you have 3 pins for your input connectors - where do you intend to connect that third pin (the one that doesn't carry signal)?
Yes, this needs to be changed: Pin 1 of the pin header indeed was originally designed for pin 1 of the XLR input. But if I get you right, you stated that Pin 1 of the XLR should (only) be connected to the chassis.
Btw: Do you suggest AC or DC coupling for Pin 1 to chassis?
Btw: Do you suggest AC or DC coupling for Pin 1 to chassis?
I suggest pin1 at each of the XLRs is connected directly to chassis by the shortest possible wire. Then you have no need for the third pin (or the R,C to it) - saves a little bit of space.
Curious about the tracking of the 0V to the headphone OP - why two tracks, forming a loop?
R19 and R20 - also my curiosity alights on these components. What calculations (if any) lead to choosing 47R for them and why are they not SMT? They do look to me to unnecessarily increase the LF impedance of your opamp rails.
R19 and R20 - also my curiosity alights on these components. What calculations (if any) lead to choosing 47R for them and why are they not SMT? They do look to me to unnecessarily increase the LF impedance of your opamp rails.
I want to pick up GND as close as possible to the signal source (output buffer) to prevent high GND currents through the input stage area. But as both channels' GND currents from the headphone arrive at the GND pin I added GND tracks to both sides.
It's not really nice but I couldn't think of a better solution.
They are intended to decouple the opamp power from the buffer power supply. 47R are just enough to get a cut off frequency below the audible band and not too much to drop the voltage below 14V (from 15V).
SMD resistors just cannot dissipate enough power.
- Status
- Not open for further replies.