Here's a first attempt at a PCB for a lm3386 inspired by Cordell's "supergainclone". I kept the input buffer but dropped the dc-servo in favor of the simpler passive DC feedback network Cordell describes in his book. Schematic is attached, the original super gainclone can be found here.
As it is, the PCB is exactly 10x5cm. Decoupling is shown as 4.7uF X7R caps, I plan to stack 2 of these per rail. All small caps (filter, compensation) are 1206 np0. Zobel is 100V MKS4. Big electrolytics are 18mm so one could fit up to 3900uF/35V pana FC but a 1000uF/50V pana FR is probably more than fine.
Now I'll be happy to get any comment or criticism about this pcb but I've a question in particular... I'm not quite sure what to do with the ground end of the zener diodes d1-d2. Where should they connect ? Should I connect the piece of groundplane where they sit to the signal plane ?
Thanks
As it is, the PCB is exactly 10x5cm. Decoupling is shown as 4.7uF X7R caps, I plan to stack 2 of these per rail. All small caps (filter, compensation) are 1206 np0. Zobel is 100V MKS4. Big electrolytics are 18mm so one could fit up to 3900uF/35V pana FC but a 1000uF/50V pana FR is probably more than fine.
Now I'll be happy to get any comment or criticism about this pcb but I've a question in particular... I'm not quite sure what to do with the ground end of the zener diodes d1-d2. Where should they connect ? Should I connect the piece of groundplane where they sit to the signal plane ?
Thanks
Attachments
Pretty nice layout there. You're on the right track with the quiet ground (signal ground) and power ground joining an the output connector.
You could, however, improve performance a bit by flooding the power ground to use all available copper on the left side. Then flood the right side with signal ground. Join the two planes by the output ground terminal, using a top side (red) pour if you have to. The top side signal ground pour should connect to the bottom side (blue) signal ground pour with a field of vias for the lowest impedance (mainly via inductance).
You could probably scoot R10 to the left side of the input connector and shorten up the input traces if you'd want.
Pretty nice, though. I like that you've included the Zobel and Thiele networks as well as the recommended stability components. Excellent.
Tom
You could, however, improve performance a bit by flooding the power ground to use all available copper on the left side. Then flood the right side with signal ground. Join the two planes by the output ground terminal, using a top side (red) pour if you have to. The top side signal ground pour should connect to the bottom side (blue) signal ground pour with a field of vias for the lowest impedance (mainly via inductance).
You could probably scoot R10 to the left side of the input connector and shorten up the input traces if you'd want.
Pretty nice, though. I like that you've included the Zobel and Thiele networks as well as the recommended stability components. Excellent.
Tom
Well, I cannot claim most of the praise here. I've read your webpages about the lm3886 so the grounding was inspired by your experiments/sims. And wrt to the stability components, I just stick to Cordell's schematic.
I tried to redraw the board according to your comments. I hope I understood what you were suggesting.
I'm still a bit unsure about the returns of D1-D2 though...
I tried to redraw the board according to your comments. I hope I understood what you were suggesting.
I'm still a bit unsure about the returns of D1-D2 though...
Attachments
Thanks for the credit. I'm glad you found my Taming the LM3886 pages useful.
Good call. I need to update the Stability section of my Taming the LM3886 page as the stability components you have in your circuit (and I in mine as of MOD86 Rev. 2.0) are actually required.
Good work so far. You could potentially get lower inductance on the decoupling for the LM3886 by rotating the two vias connecting the bypass caps to ground so it's one via atop the other at the end of the capacitor. What you have is fine, but the optimization is free...
You can optimize the input routing further by putting all the traces on the blue layer. Then flood the remaining bit of the board on the right side with signal ground plane. You want a low-impedance (low resistance and low inductance) path to the input ground. Right now you have a fairly long trace (= inductor) on the input ground.
That's a tricky one. The zener current will be modulated by the variations in the raw supply voltage. If you return the zeners via the signal ground plane, you'll get an error term there. If, on the other hand, you return the zeners to the power ground, any ground bounce between the power ground and signal ground will cause a similar bounce in the supply voltages for the opamp.
If you want a more definitive answer, it would be worth setting up a simulation of the two options and see what causes the lowest error on the amp output. You can get a good estimate of the parasitics of your layout by entering the plane/trace dimensions in a trace impedance calculator. Saturn PCB Design is a free tool (sadly Windoze only). If you search for "PCB trace inductance calculator" you'll find some on-line ones as well. I seem to recall the one by TechNick is pretty good.
My best faith estimate is that returning the zeners to the signal ground will provide the lowest error. You can further reduce this error term by biasing the zeners with a CCS rather than a resistor. You can also use low-current zeners. Some zeners will regulate down to a few 10s of uA of reverse current. If the zener current varies, say 10 %, you'll get a much lower error if the zener is operating at 10 uA than the more common 5-10 mA.
Tom
Thanks for the new comments, it really helps. There was a lot of confusing posts about the "optionnal" stability components; glad to read that you're going to post something about it.
As the overall layout was sound, I tidied things up a bit. It was a bit silly to have plenty of smd parts and not take fully advantage of it, so I changed most resistors to 1206. The electrolytics were also a bit excessive, they're now 5mm pitch, 13mm diam (suitable for pana fr 1000uF/35v), which allowed me to move them closer to the IC. As a consequence, the board has shrunk to 8x5cm. The negative consequence is a vertical zobel resistor.
The input network has now its own plane, with a wide connection to the signal plane at the final input filter cap.
The zeners are now fed with a pair of dn2540 ccs. The diodes return is now on the signal plane. I'll probably have to test in situ to have a definitive answer on this.
I've done some housekeeping, keeping the groundplanes away from the opamp inverting's inputs, etc.
Slowly getting there...
As the overall layout was sound, I tidied things up a bit. It was a bit silly to have plenty of smd parts and not take fully advantage of it, so I changed most resistors to 1206. The electrolytics were also a bit excessive, they're now 5mm pitch, 13mm diam (suitable for pana fr 1000uF/35v), which allowed me to move them closer to the IC. As a consequence, the board has shrunk to 8x5cm. The negative consequence is a vertical zobel resistor.
The input network has now its own plane, with a wide connection to the signal plane at the final input filter cap.
The zeners are now fed with a pair of dn2540 ccs. The diodes return is now on the signal plane. I'll probably have to test in situ to have a definitive answer on this.
I've done some housekeeping, keeping the groundplanes away from the opamp inverting's inputs, etc.
Slowly getting there...
Attachments
Last edited:
Why does the input need to be on a separate plane from the signal ground? Would you share your thoughts there?
You may want to do the math on the worst case power dissipation in the DN2540s. They may be able to handle the full power dissipated. Then you can skip R13, R14.
Where's Cmute? (I.e. the cap from the MUTE pin to GND).
Good progress so far, though. Keep it up.
Tom
You may want to do the math on the worst case power dissipation in the DN2540s. They may be able to handle the full power dissipated. Then you can skip R13, R14.
Where's Cmute? (I.e. the cap from the MUTE pin to GND).
Good progress so far, though. Keep it up.
Tom
A couple of points/questions.
First have you calculated the supply impedance to the OPA2134? Given the 1k input impedance to the LM3886 stage you'll get appreciable load modulation of the rails.
Second - you have a single ended input hence common-mode currents will be a potential issue. Looks to me you have them flowing through your ground plane (between input 0V and trafo 0V) - they'll introduce errors which can be eliminated by having the input connector adjacent to the power connector.
First have you calculated the supply impedance to the OPA2134? Given the 1k input impedance to the LM3886 stage you'll get appreciable load modulation of the rails.
Second - you have a single ended input hence common-mode currents will be a potential issue. Looks to me you have them flowing through your ground plane (between input 0V and trafo 0V) - they'll introduce errors which can be eliminated by having the input connector adjacent to the power connector.
Since the input network is an rfi filter, I treat it as a dirty section, connecting it to the rest of the amp only at the terminals of the final filter cap. As currents are low due to the high impedance of the network and since this connection isn't that small anyway, I don't think much is lost in terms of inductance/resistance.
But maybe have I been doing too many digital pcb lately...
Oh, they should be fine and the resistors can be jumpered. With a +/-28V supply, 12V zeners and 20ma, they'll usually see about 320mW, which is fine. But I just prefer to run them at about 200mW.
Gone for a walk ? As I'm using an upc1237 based protection output board, with a delayed start-up and immediate release at power-off, I've ommitted it. But I have space aplenty to put it back in.
I see. I do support the idea of returning the RFI filter ground to the output ground via a separate route for the reasons you mention. That should return to the output ground rather than the signal ground, though. The input ground should refer to the signal ground. After all, it's the difference between the input ground and the input signal that we're looking to amplify.
No, but that does explain why your starting point was quite a bit closer to optimum than that of the typical DIYer.
Fair enough.
You'll still need Cmute. If the MUTE pin voltage wiggles, it'll degrade the THD - at least at the levels I'm achieving in the Modulus-86 and Parallel-86. I'd throw a 100 uF, 6.3 V in there for Cmute.
Tom
What about two stages? The first stage RC returns dirty current to the power ground.
The second stage RZ returns cleaner dirty current to the Signal ground.
There are two resistors there already, just add the C between the two Rs.
Still thinking about this one... Cordell's filter is pretty steep and absolutely requires to be driven from a low impedance. If we move part of the filter in between the input buffer and the inverting one, we gain a lot of flexibility to interface the amp with a simple 10K pot as volume control.
It'd go like this, in order:
isolated rca with 47pF caps going from ground to chassis
twisted wire
10K pot
twisted wire
input connector on the pcb
and then the following schematic:
C4 ground returns by its own track either simply to the input connector or to chassis ground; all the rest sits on the signal gnd plane. It's not perfect but with a jfet input opamp, it should work out ok in practice.
Good point. 100UF/6.3V exists in 1206 X7R, that will be easy to fit underneath the board.
I've thought about it but with the low values of the resistors required by the design, a pair of CCS is more effective. The space needed is similar and the cost isn't much higher either (2 dn2540 vs 2 caps).
Attachments
Two stages would reduce the error term, assuming the dirty ground doesn't couple to the zener through the first cap. Using a CCS would all but eliminate the error term. The performance of the CCS would be limited by its output impedance. It may be beneficial to use an LM317L as a CCS rather than the DN... for that reason as the high-voltage CCSes tend to have lower output impedance. I'd at least look at it as an option.
Tom
Jung has measurements of ccs with lm317 and dn2540 in here.
A simple lm317 is indeed a bit better than a single dn2540 up to 10KHz. Then the mosfet wins. A lm317 cascoded by a dn2540 would be the clear upgrade but I don't have much pcb room left for it and the required stability components.
Well, yeah. You can always choose something to geek out about.
As long as you're using a CCS, you'll at least have some loop gain thrown at the problem, unlike with filtering.
Regarding your question of EMI/RFI filtering, I think you need to up the 100 Ω, 47 pF to something like 1 kΩ, 470 pF for it to provide any meaningful attenuation for RF. Your idea of a filter followed by a buffer is a good one, though.
Tom
Last edited:
I've left the project aside for a while... and managed to somehow delete the eagle files. 
So, back to the drawing board. Here's a new version. It includes pretty much the same things as the one discussed earlier.
The new things:
- provision for up to 4*4.7µF x7r caps near the amplifier.
- more convenient locations for the connectors, use of faston connectors.
- down in size to 6x6.5cm (2.36"x2.56").
- input connector is molex kk (or the cheaper psk stuff from reichelt).
- the nc pins are removed, to clean up the layout.
And now the for the thousand bucks question: where to link the signal ground to the power ground ? The previous design had the link at the output ground connector, which made sense as it was close to the decoupling caps.
Now that the connector has taken a big trip downwards, should I still go join the groundplanes there ? Or should I rather create a bridge near the lm3886, under the feedback resistors crossing the divide ?
Thx for any
thrown in.
So, back to the drawing board. Here's a new version. It includes pretty much the same things as the one discussed earlier.
The new things:
- provision for up to 4*4.7µF x7r caps near the amplifier.
- more convenient locations for the connectors, use of faston connectors.
- down in size to 6x6.5cm (2.36"x2.56").
- input connector is molex kk (or the cheaper psk stuff from reichelt).
- the nc pins are removed, to clean up the layout.
And now the for the thousand bucks question: where to link the signal ground to the power ground ? The previous design had the link at the output ground connector, which made sense as it was close to the decoupling caps.
Now that the connector has taken a big trip downwards, should I still go join the groundplanes there ? Or should I rather create a bridge near the lm3886, under the feedback resistors crossing the divide ?
Thx for any
thrown in. Attachments
- Status
- This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.