pcb layout tips for (yet) another summing bus

Hi folks,

I'm new to the forums and I know that there has been a lot of discussion about summing bus circuits. However, this being my first pcb project I am a little bit nervous about going forward and ordering them before I got some feedback from most of you knowledgable folks out there. So here goes

I'm trying to build 24 channels ito a 2U rack space unit. I'm using THAT 1240 chips for the differential input stange, with a 990 for the summing amp and a JLM audio hybrid opamp as a buffer. I also have a pre fader expand out to daisy chain multiple units (the expand ins connect directly to the summing buss with a THAT1246 -6dB chip to balance out the +6dB for the expand out balanced line driver . The 25 THAT chips fit on two 11" BY 3" PCBs (12 channels and one mono expand in per pcb) and the summing amp and buffers fit on two 5" by 3" pcb (one for left and the other for right).The plan was to stack them up using nylon standoffs.  Custom pcb offers a 11" by 8" 4 layer pcb for $120 so I'm going to go for that for all the pcbs. Using the 4 layer board for the summing amp pcb makes things a whole lot easier and since I have so much extra space I'm going to do the differential input pcb on 4 layers as well.  For the diff input pcb I have a + and - 24V power plane and a ground plane. The THAT 1240 chip reference as well as all the decoupling caps connect to this ground plane. The summing circuit pcb has a segmented ground plane that meets at the local star point on the board. Both pcb's ground connects to the star point on the 2U chassis which ultimately goes to the star point in the external PSU through a 5 pin XLR. The pin 1's on the XLR are terminated directly at the chassis with the option to conect it to the ground plane of the diff input pcb as well for unbalanced connections. The summing buss is a  solid copper 10 gauge wire.

I was looking at the forssell summing buss circuit and I wanted to make room for a ground buss. However I am a bit confused because it requires each channels ground to conect to the ground buss via a 1k resistor which then ties to the non-inverting input of the 990. Since I have one ground plane can I connect this plane to the non-inverting ground of the 990 with just one 1k resistor? In the schematic attached right now, I have a 415ohm resistor to ground on the non-inverting input of the 990 which is the equvalent to the resistance as seen by the inverting input.

I'm posting the schematic and tomorrow I'll be able to post a jpeg of the pcb's too. (I'm using Diptrace). Any comments, suggestions etc would be most welcome. I'm excited about this project as its my first pro audio one; built a lot of tube amps and horns on the past. Once I have he pcb's figured out I can hook them up to the audio precision test setup at work.

The VU buffer and expand outs... Also I noticed that in the summing bus schematic I accedently deleted the wire connecting the post fader buffer dc servo to the OPA2604's inverting input...

and the LCR assign stage with 4.5 dB panning law....

The summing bus pcb. Top signal layer is shown. The second layer is the ground plane followed by the -24V and +24V planes respectively.

Too busy to check the whole thing but from a quick glance the diode connected to - supply in bottom right corner of first schematic (left summing amp) looks like a driver bias string gone seriously wrong...

Has any of this been bread-boarded or are you going to make it work on the fly?

Layout, assuming design is solid, I find it useful to think of ground traces as resistors, and evaluate the current flowing in each trace for significance of voltage drops across those traces.

JR

Summing bus schematic is now updated.....

What output transformer are you using - and are you sure it's up to the job (it looks awfully small)?

You probably don't need the DC-Servo in the circuit driving the output transformer - seems to be overkill.

0.1uf between mixamp and fader is too small - and should definitely not be electrolytic at such small values

Jakob E.

Hey gyraf. thanks for the input; the output transformer is a Cinemag 50% Nickel/Steel core line level transformer with about 28dBu of headroom at 600 ohms nominal. Yea, I figured the dc servo on the buffer stage is overkill but I'll leave it on there just to experiment...Why is 0.1uF too small and why not electrolytic? That was what I was planning to use? I figured that 0.1uF had a low enough pole for audio and anyway if I use the dc servo, I probably will not need it. What do you recommend?

Also I'm a bit concerned about the buffer stage having a Av=2 especially after a pot. Will my noise be affected significantly? I was hoping to get about -75dBu to -85dBu of noise floor. The reason I have the extra gain is I was thinking say, if I daisy chain 3 of these units together, unit one exp out into unit 2 and unit 2 into three, then I will have to calibrate the input channels to avoid clipping unit 3's summing amp. Then the pre fader exp outs on unit 1 and 2 will have a relative low level. But having the 6dB gain through the buffer amp allows me the flexibility to use the main outs of unit 1 and 2 and higher levels. This way, with 3 units I effectively have a 72x6 mixer. Since I know how the gain stages are structured, I can calibrate each output buss to a known digital level without running the risk of clipping. Does this reasoning make sense?

macwanj said:

Custom pcb offers a 11" by 8" 4 layer pcb for $120 so I'm going to go for that for all the pcbs.

Click to expand...

99% of audio equipment is built on two-layer (very often single-layer) PCB; I think you should do it on 2 layer, because it's easy enough to design and prototyping, correcting mistakes with green wire, and so on is much easier. You should save your money for an extra-robust ground bus.

The summing buss is a  solid copper 10 gauge wire.

Click to expand...

There is absolutely no advantage in using VLZ  summing buses, but having as close to zero ground bus is paramount in obtaining low noise, low crosstalk.

I was looking at the forssell summing buss circuit and I wanted to make room for a ground buss.

Click to expand...

This should not be called a ground bus; it is in fact a non-inverting summing bus.

However I am a bit confused because it requires each channels ground to conect to the ground buss via a 1k resistor which then ties to the non-inverting input of the 990. Since I have one ground plane can I connect this plane to the non-inverting ground of the 990 with just one 1k resistor?

Click to expand...

No, the actual Ground bus is still the reference bus (zero volt) and you must create a new bus. [/quote] In the schematic attached right now, I have a 415ohm resistor to ground on the non-inverting input of the 990 which is the equvalent to the resistance as seen by the inverting input. [/quote]If you analyse the circuit, you'll find that the optimum value for the non-inverting bus injection resistors (and the non-inv to ground resistor too) is R/n+1 (R being the inverting injection resistor), but in practice, any value of 100R to 1k is good. The limits are the following: the non-inv bus injection resistor should be >> than the maximum resistance between the two more distant grounds (on aPCB it's a few hundredths of ohm, but on a large desk with ribbon cables, it can be a few tenths of ohm) and should be low enough for the eq resistance presented to the non-inv input brings minor noise contribution. If you use 1k res, this will be ca. 40 ohms, which should be ok.

macwanj said:

Hey gyraf. thanks for the input; the output transformer is a Cinemag 50% Nickel/Steel core line level transformer with about 28dBu of headroom at 600 ohms nominal. Yea, I figured the dc servo on the buffer stage is overkill but I'll leave it on there just to experiment...Why is 0.1uF too small and why not electrolytic?

Click to expand...

0.1uF into 18k (worst case) gives 50 Hz high-pass. Is it what you want? You should use at least 10uF, but considering the low prices of electrolytics, 100uF is a good bet.

That was what I was planning to use? I figured that 0.1uF had a low enough pole for audio and anyway if I use the dc servo, I probably will not need it.

Click to expand...

This cap is necessary to block ANY DC going into the pot, which would make it noisy. The DC servo in the output is there to block DC going into the xfmr.  It is necessary in order to make sure the xfmr does not have any DC bias, which could lead to odd order distortion, premature clipping and possible damage to the output devices.

Also I'm a bit concerned about the buffer stage having a Av=2 especially after a pot. Will my noise be affected significantly? I was hoping to get about -75dBu to -85dBu of noise floor.

Click to expand...

With 6dB gain, output noise should be ca. -100dBu, much less than the summing amp's noise, which should be ca. -80.

The reason I have the extra gain is I was thinking say, if I daisy chain 3 of these units together, unit one exp out into unit 2 and unit 2 into three, then I will have to calibrate the input channels to avoid clipping unit 3's summing amp. Then the pre fader exp outs on unit 1 and 2 will have a relative low level. But having the 6dB gain through the buffer amp allows me the flexibility to use the main outs of unit 1 and 2 and higher levels. This way, with 3 units I effectively have a 72x6 mixer. Since I know how the gain stages are structured, I can calibrate each output buss to a known digital level without running the risk of clipping. Does this reasoning make sense?

Click to expand...

Nothing wrong with that.

macwanj said:

Summing bus schematic is now updated.....

Click to expand...

OK better, but I still don't follow what the two diodes shunted by a singe diode are doing now?

Good luck

JR

Hi JR,

I should have labelled it better but D1 is a led and the idea with the JLM hybrid opamp is that it can be run in class A (with D2 and D3 disconnected with each other) then the led turns on. and provides the bias. In class AB D2 and D3 are connected and the led turns off. I decided to have it permanently in Class AB as it pulls about 30mA in class A and I wanted something with better transient response and anyway most of the coloration will probably come from the output transformer. I guess I can still leave the D1 footprint on the pcb if I change my mind later. But anyways, do you think its a good ides to have a pot before a Av=2 opamp stage? Will the noise floor be compromised?

Also abbey road d enfer, thanks for your valuable input; it all makes some more sense. I was careless in choosing 0.1uF; I forgot to take into account the source and load impedances.... But as far as using a 4 layer board, don't you think having ground and power planes is a good idea? I was thinking that the ground plane in the pcb's were the ground busses which would be tied to a star ground point...I thought that ground buss bar was used in bigger mixers with head amps and eqs, etc.

macwanj said:

Also abbey road d enfer, thanks for your valuable input; it all makes some more sense. I was careless in choosing 0.1uF; I forgot to take into account the source and load impedances.... But as far as using a 4 layer board, don't you think having ground and power planes is a good idea? I was thinking that the ground plane in the pcb's were the ground busses which would be tied to a star ground point...I thought that ground buss bar was used in bigger mixers with head amps and eqs, etc.

Click to expand...

It is a good but expensive idea, and it makes the transition from prototype to finished product more tedious and lengthy. A good experienced draftsman can lay a board of average complexity and have it working the first time, although it may need a couple of gren wires and some track cutting, but I've never seen a 4 layer board be done first time! And if you made a mistake on the inner layers, you can't use your X-Acto and soldering iron! The ground plane in a PCB will never be as efficient in terms of resistance as a single #16 gauge copper wire. In addition, the increased bus-to-ground capacitance may lead to stability problems easily fixed with an inductor at the inverting input of the summing amp and a small cap on the FB resistor (lead-compensation). However a ground plane will provide good shielding, which is almost irrelevant if your project is built in a conductive enclosure. And there is no benefit at all for the power supplies, because you don't necessarily want them to be VLZ, you want the well decoupled, so again a VLZ ground is paramount.

Not to be contrary... but, a 4 layer board should be easier for a given design. That said I agree it is an unnecessary expense for something like a console that can be physically large.. PCB material isn't cheap. I suspect first pass experience relates to complexity and maturity of the design undertaken. By definition more complex designs find themselves on 4 layer boards. Modern CAD tools make it easier to match layout to schematic and meet known design rules, but there are often unanticipated interactions or errors with design/schematic.  A recent post mentioned a library error for a common part... It's always something.

Ground quality and signal integrity is not just about using brute force shielding or fat trace width, but proper consideration of current flows within traces/paths and differential hand off of signals from one local ground to the next (if single ended), or completely differential treatment within a given circuit block where the local ground is common mode and mostly inconsequential. Ground planes and power planes are useful in complex digital designs but less so for relatively straightforward analog stuff. Even then they aren't trivial to apply.

JR

PS: I agree errors on inner layers can be a real PIA. You can always drill out vias but depending on the error it gets complex to tweak.

Since this was my first pcb layout, I was thinking that using a brute force approach with 4 layers would be a good bet to get it right with the least hassles. So abbey road d enfer are you suggesting thick ground and power traces as opposed to planes? You mention that 16awg wire provides less resistance than say a ground plane so are you suggesting that I need to run this wire from each node to the entire chassis' star ground point? My ground plane is segmented and should work like a local star ground and then the local star ground for the pcb will go to the main star ground via a 14awg wire.The actual summing busses will run along on terminal strips with one end connecting to the summing amp pcb, is this going to capacitively couple my summing bus to ground?. The way I have it now is the second layer (the ground plane) has one 2 or 3 non critical traces; traces from the OPA604 trimmer to the OPA in the 990's dc servo, so fixing traces between layers should not be a prolem. The two power layers are mostly uninterrupted planes with thermals connecting to the required pads.  I also generously placed 100uF electrolytics across the board from the power planes to the ground planes. I agree with John that it was easier for me to route everythin on 4 layers since the power and ground traces were now planes.

Even while designing the laying out the ground plane I was asking myself what was the least impedance path for each ground in the schematic and that helped with sectioning the ground plane....Anyways I will have to give this some more thought....