Some LME49600 implementations

[wakibaki]

Thanks. The design doesn't seem to be attracting much interest though. I have a couple of other things I'm working on, a USB DDS signal generator based on an ebay AD9850 module + PIC 18F4550 and another compact headphone amp based on the AD3897. I might get on with writing them up and leave this on the back burner for a while.
 
The digipot is interesting, THD is not as good as the high-end TI and Cirrus chips though, but still probably below the threshold of hearing.  The problem, as I see it though, is that you have to go with the uproc if you want a readout of the setting, in which case you might as well go with the high-end chips. If I could get another decimal place in the THD over the existing chips I'd go for it, because people like the margin of performance, unless they're tube enthusiasts.
 
I had another idea for a simplified protection circuit, I'll write it up in the AD3897 thread I'm going to start.
 
w

 

[wakibaki]

 
Went back and reworked these to give some copper fill to the 49600's and regs for cooling. Should have thought about this earlier. 
 
 
I fiddled with the protection scheme too.
 

 
 
The input voltage needs to be controlled so as not to drop too much voltage across the regs, because they won't dissipate a lot. I could maybe get them a bit more copper area by connecting the 49600's to the bottom with a big hole like I used for the TPA6120's and stealing some of the top from them.
 
The protection circuit:-
 

 
The original layout with modified fills:-
 

 
I did look at the output offsets with the LME49720. They can be pretty horrific. 65mV worst case. Which is higher than I was going to set the offset protection.
 
I think maybe I'll try fitting in single opamps instead of the duals. This would permit the use of say, LME49990 and OPA123 as Avro_Arrow has suggested here and elsewhere. This is probably the thing to do, why spoil the ship for a ha'porth of tar? I can get a bit more room for the amplifier proper if I move the pot and make the front panel layout assymmetrical.
 
Of course there's room on the bottom, but it's pretty much unbroken ground plane for the moment, I don't want to complicate the ground returns. I could go to 100 * 100 mm for the same price board, but it wouldn't fit the O2 enclosure then.
 
Nobody got any input?
 
w

 

[kevin gilmore]

The reference design with the  lme49720 with an lme49600 where one section of the 49720
is used as a servo. It doesn't work, typical outputs are 10+mv. Sounds really good however.
Much better solution is to use lme49710 with the lme49600 and then a very low offset opamp
like tl071 or op27 as the servo.  You can easily get to 200 microvolts offset this way.
Also the gain of the servo is way too high, the 1k resistor should be at least 10k.
And to reduce offsets further replace the 1M resistors with 100k, and the 1uf caps
with 10uf mlcc caps.

 

[wakibaki]

Thanks, Kevin.
 
My calculations of offset due to input bias current were leading me to suspect as much, but in the absence of a first prototype or an example of the National reference board, you can probably understand why I was taking the design from the datasheet at face value.
 
The move to replacing the 1M's in the servo is fairly obvious measure, fiddling with these values and the servo gain are amongst the range of options available subsequent to completing the layout.
 
I have in fact re-laid the board to accommodate 2 single opamps to substitute for the dual 49720, making it possible to build it with a variety of opamps. I'll look at the footprints of 10u MLCCs and make sure that they can be accommodated. Changing the servo authority will have an impact on the gain, what are the symptoms of leaving it as is?
 
Thanks again.
 
The board as it currently stands:-
 

 

 
I'll stew on this now for a few days, there are a couple of things I will probably change, I find that I like to get a board routed even if it's a bit dubious in places, and then come back and improve it. I need to get in some 49600's to verify the footprint, maybe go to 35V electrolytics instead of these 10mm square jobs.
 
w

 

[kevin gilmore]

The servo resistor should be at least a factor of 10 greater than the gain resistor
to ground. Then you can adjust the feedback resistor for the overall gain
you require.

 

[Avro_Arrow]

Here is the board I came up with.
I'm no master but I think it looks OK.
 
The dual op amp position will have a brown bog adapter
with an OPA132 on one side and LME49990 on the other.
 
Power supply is off board.
 

 
And the schematic it was generated from:
 

 
Component value are not final.
Let me know if you see any flaws in my layout.
I tried to make it home etching friendly.
 
Edit:
 
I forgot to mention I was using a BUF634 as I have several in TO-220.
I also have LME49600 so I will do a version for that too.
It will be fun to compare the two.

 

[wakibaki]

Looks good to me, it's certainly suited to a homebrew PCB. You'll need some isolation between the tab and heatsink, or between the heatsink and ground plane.
 
I'd be tempted to put an exclusion zone for the groundplane around the IC pins and tracking to keep stray capacitance to an absolute minimum, but this is arguably unnecessary, unknown in exact effect and subject to discovery since this is a prototype. It's certainly less risky than what I've done, the simplicity minimises the likelihood of any unwanted interactions or feedback. I think you're in love with the Brown Dog idea though, why not make the PCB accept the chips direct?
 
IMO it makes more sense than the one that was being worked up on diyaudio, my approach is to either make an amplifier module to work with some external modules or a complete integrated amplifier with an enclosure in mind.
 
I ordered a couple of these chips, so I guess I'm committed to building some kind of amp using them. 

 
w

 

[sek@]

Hi,
 
I hope nobody minds if I chime in over here too, as I'm also currently fiddling with the BUF634/LME496x0 buffers, but am not particularly happy with how things go over on diyaudio at the moment.
 
Quote:

Here is the board I came up with.

Looks good so far. I have a couple questions/remarks, though.
 
Your circuit of course reminds me of the datasheet application. I assume R5 and R10 differ from the datasheet servo configuration on purpose (i.e. to increase stability)?
 
I don't quite get your grounding yet. You mention the PSU being off board, but some things aren't obvious from the board layout.
 
First off, the circuit differentiates between signal ground and power ground. Why? If it's on purpose, where do they join? How? There's no connector. The solder pad only features signal ground.
 
Secondly, how do you handle signal ground input? You have a single solder pad (per channel) for signal input, but no place to connect the return wire (i.e. cable shield). That would mean you'd have to essentially run a couple of inches of unshielded signal wire from the chassis connectors to the PCB.
 
Have you made your choice regarding chassis input/output connectors and how to handle their insulation/grounding yet?
 
What's with the heat sinks? They look power referenced in the schematic (why actually?), but they're floating on the board. 
 
What's your reason to mix SMD and through-hole components? You've got through-hole capacitors on the board already? I may suggest SMD components throughout.
 
Finally, where's the headphone return wire (ground) connected? Also at the PSU? 
 
 

I forgot to mention I was using a BUF634 as I have several in TO-220.

 
The TO-220 cased variant of the BUF634 has straight legs. There is a library part in Eagle that has the 5-pin device with all holes in a row. That's slightly more difficult to etch at home, but way more gentle on the pins.
 
Cheers,
Sebastian.
 

 

[Avro_Arrow]

Those are all very good observations and questions. Let's see if I can be as good at answering them.
 
It doesn't show up well in the picture, but the heat sink mounting pins and ground plane are isolated.
I tied the pins on the heat sink to V- because the tab on BUF634 is also at V-. I could have just left
them tied to nothing. I may run a jumper from V- to the heat sink pin.
 
The reason I wanted to try the brown bog idea is easier routing. One dip is easier to route than two soic
in this case. There will not be a socket. If I want to "roll", it will involve soldering.
 
The grounding scheme is an off board star ground. The grounding point will probably be at the headphone
jack. The ground connection on the board is to serve the boards ground plane. The ground plane is
split to help isolate left and right.
 
I know lot's of people love PTH components and others love SMD, but I tend to use both whenever
it suits me. I used PTH components because this is a single sided board and they provide convenient
jumpers. 

 
I'll increase the ground exclusion around the input pins on the op amps.
 
 
I have done a board in the past with TO-220 BUF634 using the stock footprint. I found the pad spacing
too close. Even when I zoomed right in, it still looked like the pads were actually touched. When I printed the
transparency my printer could not resolve the fine spacing and I had to use a needle to scratch out
between the pads. I have done TSSOP with my set up but the BUF634 footprint just did not work.
After that I changed the BUF634 footprint from straight legs footprint to staggered. I guess I should
rework the BUF634 straight footprint to have better spacing.
 
I chose this modular approach to give the builder freedom in choosing the case, power supply, etc.
Thats why I also chose not to include a volume control.

 

[Avro_Arrow]

Here is the power supply if you need one:
 

 
And it's schematic:
 

 

[sek@]

Quote:

It doesn't show up well in the picture, but the heat sink mounting pins and ground plane are isolated.

It looked like that in the picture, and it's certainly easier to solder that way.
 
 

The grounding scheme is an off board star ground. The grounding point will probably be at the headphone
jack. The ground connection on the board is to serve the boards ground plane. The ground plane is
split to help isolate left and right.

 
 
Upon closer look I can see that you use the ground plane for joint power and signal grounding. Good.
 
Wouldn't using the output connector as a star point (only) make it difficult to connect the input ground/shield wire? Even if you use a separate connection between input socket and ground star, you could still only incorporate a shielded input wiring by leaving the shield open at least at one end, if at all. What am I missing?
 

I guess I should rework the BUF634 straight footprint to have better spacing.

 
Yes, the original case drawing is unusable, but CadSoft's libraries contain other TO-220-5 cases (i.e. for voltage regulators) that can be borrowed. If all else fails, the pad size and shape can be reduced, i.e. simply made into regular round pads.
 

 
Cheers,
Sebastian.

 

[Avro_Arrow]

I will add a connection at the board for input grounding.
 
I used one of CADSofts "other" TO-220 footprints for my BUF634.
I was thinking of just splaying the legs apart slightly to increase
the spacing. Easier than having to bend the pins for the current
footprint I am using.

 

[Avro_Arrow]

Revised amp board:
 

 
I made the heat sinks a little smaller...I think they were a little too big.
Added mounting holes...duh.
Cut out a little more around op amps.
Heat sink pins now floating, not connected to V-

 

[sek@]

Cut out a little more around op amps.

 
With regard to this I find the concept of guard rings around pins and traces very interesting. Here's an introduction to some ground related issues (from TI).
 
Do you think you can handle a two-sided PCB manufacturing process, with the upper layer being ground plane only? All it takes for this to be effective are a reasonable number of vias (i.e. hand soldered on both sides using resistor wire cuttoffs).
 

Heat sink pins now floating, not connected to V-

 
There's no reason not to ground the heat sink (granted the buffers are mounted in an insulated way), especially if EMI is taken into consideration. OTOH it's not absolutely necessary either.
 
Cheers,
Sebastian.
 
 

 

[sek@]

Quote:

Here is the power supply if you need one:

Just some quick remarks here for now.
 
The heat sinks can be made the same size as on the amplifier boards.
 
Large capacitance is needed more on the input side than on the output side of the regulator. Additionally such large capacitors might benefit from some film or ceramic decoupling capacitors or even snubbers.
 
Seeing that you have the board space available, consider increasing the size of C1 and C2. Up to at least 470uF is a good idea to improve ripple rejection.
 
The very large V+ and V- copper areas form an effective antenna loop, together with the wire between PSUs and amp. A top layer ground plane would solve this issue almost completely (just like I described in my post above).
 
Cheers,
Sebastian.
 
PS: By joining the negative side of the positive supply to the positive side of the negative supply you effectively form a (local) ground star. That's fine, but you could leverage on this by having the screw terminal offer multiple ground point connections. The board space is there.