Hello all
I'm busy with jet an other chipamp design and i would like some feedback.
I designed a PCB based on an inverting¶lleled LM4780.
Creating a star based signal ground was a challenge. But i think i have found a decent compromise. The ground pins of the chip and the signal return lines are relatively long.
Will this raise a problem?
I created some input - output shield to prevent oscillations. But there is no shielding between V+ ans the input signal. Would that be necessary? Will there be a possible oscillation between the supply and input signal?
The Power is calculated for a 4 Ohm load but the amp will be used for 8 Ohm.
So i left the compensation 'filters' unchanged.
I will mount 2 LM4780 PCB's on one heatsink.
SK568/150/SA SK 568, Standard extruded heatsinks, Heatsinks f.cool, Fischer Elektronik
Which would give me 0.3W/C which seems enough for 4xLM3886 on a 6ohm Load at 25V with a room temp of 35°.
I will reduce the gain later on, to prevent the Chips from reaching max-power.
Based on max output of my Xonar ST.
There will be an extra piece of aluminium between the chips and the heatsink.
aprox. 20mm thick.
And this is how i plan to build the complete 4CH setup
(The left side needs to be mirroed to the right)
As i proceed i will post some pictures of the progress
I'm busy with jet an other chipamp design and i would like some feedback.
I designed a PCB based on an inverting¶lleled LM4780.
An externally hosted image should be here but it was not working when we last tested it.
Creating a star based signal ground was a challenge. But i think i have found a decent compromise. The ground pins of the chip and the signal return lines are relatively long.
Will this raise a problem?
I created some input - output shield to prevent oscillations. But there is no shielding between V+ ans the input signal. Would that be necessary? Will there be a possible oscillation between the supply and input signal?
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.
The Power is calculated for a 4 Ohm load but the amp will be used for 8 Ohm.
So i left the compensation 'filters' unchanged.
I will mount 2 LM4780 PCB's on one heatsink.
SK568/150/SA SK 568, Standard extruded heatsinks, Heatsinks f.cool, Fischer Elektronik
Which would give me 0.3W/C which seems enough for 4xLM3886 on a 6ohm Load at 25V with a room temp of 35°.
I will reduce the gain later on, to prevent the Chips from reaching max-power.
Based on max output of my Xonar ST.
An externally hosted image should be here but it was not working when we last tested it.
There will be an extra piece of aluminium between the chips and the heatsink.
aprox. 20mm thick.
And this is how i plan to build the complete 4CH setup
An externally hosted image should be here but it was not working when we last tested it.
(The left side needs to be mirroed to the right)
As i proceed i will post some pictures of the progress
For paralleling the outputs i plan to use this:
PWR4412-2SCR1000F | Bourns Open Air Shunt Radial Bare Metal Resistor 100mΩ 1% 3W 20ppm/C | Bourns
I had a hard time finding a 0.1 resistor which fitted to my design plan.
Till i found this.
Anybody used this for audio before?
PWR4412-2SCR1000F | Bourns Open Air Shunt Radial Bare Metal Resistor 100mΩ 1% 3W 20ppm/C | Bourns
I had a hard time finding a 0.1 resistor which fitted to my design plan.
Till i found this.
Anybody used this for audio before?
A small update
A softstarter and a DC blocker are build onto a separate PCB:
PCB's are ordered 4 amp boards and 1 mains-utility board!
The utility board is mounted with help from the M8 mounting bolt of the transformer.
The case is getting crowded
A softstarter and a DC blocker are build onto a separate PCB:
PCB's are ordered 4 amp boards and 1 mains-utility board!
The utility board is mounted with help from the M8 mounting bolt of the transformer.
The case is getting crowded
The main concern with pcb layout is the grounding.
Any power grounds should all be routed back to one star ground point.
On my LM3886 amp I routed speaker out back to star ground. I routed zobel back to star ground. Then I routed rest of grounds back to star ground.
Having a separate power supply pcb is good as it keeps its ground separate.
Charging pulses into smoothing capacitors can cause havoc if allowed to modulate audio ground.
Any power grounds should all be routed back to one star ground point.
On my LM3886 amp I routed speaker out back to star ground. I routed zobel back to star ground. Then I routed rest of grounds back to star ground.
Having a separate power supply pcb is good as it keeps its ground separate.
Charging pulses into smoothing capacitors can cause havoc if allowed to modulate audio ground.
So if i understand you correctly
preferably like this:
were the ref point is routed to the supply star
Not like this :
preferably like this:
An externally hosted image should be here but it was not working when we last tested it.
were the ref point is routed to the supply star
Not like this :
An externally hosted image should be here but it was not working when we last tested it.
Tom Christiansen did a lot of research on the LM3886 (the single chip version of the LM4780), I strongly suggest you take the time to read and understand his findings, LOTS of very good info.
Taming the LM3886 Chip Amplifier
Mike
Taming the LM3886 Chip Amplifier
Mike
Last edited:
Read most of it, before, but decided to take a bigger trafo.
300W turns out it is also cheaper then 250W
Thanx 🙂
But i must say he stays very theoretical. That's good but giving a layout for only part of the design is not very practical.
Oversized output filter:
Simplifying things: Finding a 1K//28K resistor
Output filter to scale:
An externally hosted image should be here but it was not working when we last tested it.
Simplifying things: Finding a 1K//28K resistor
An externally hosted image should be here but it was not working when we last tested it.
Output filter to scale:
An externally hosted image should be here but it was not working when we last tested it.
Put the resistor outside the coil.
Some materials affect the way the coil performs.
Some materials are affected by the magnetic field.
Avoid the risk of both.
Some materials affect the way the coil performs.
Some materials are affected by the magnetic field.
Avoid the risk of both.
Yes I understand that would be better. I'm thinking of an output PCB with relais and output filters.
For the relais i'm thinking of the Amplimo LR12/LR24 type.
or are there better suggestions.
For now i'm focussing on a input board.
I need to drive a 500Ohm input and i'm thinking of the THS4031/THS4032
It is unity gain stable (1-2X) but i would like to use with a gain of 0.5X will that kill the performance? Or is that within the 'unity gain' statement?
For the relais i'm thinking of the Amplimo LR12/LR24 type.
or are there better suggestions.
For now i'm focussing on a input board.
I need to drive a 500Ohm input and i'm thinking of the THS4031/THS4032
It is unity gain stable (1-2X) but i would like to use with a gain of 0.5X will that kill the performance? Or is that within the 'unity gain' statement?
THS4031 only come in a smd package.
Damn I like the dip version better because of more easy routing.
Suggestions for a DIP Buffer to drive a 500Ohm load?
Damn I like the dip version better because of more easy routing.
Suggestions for a DIP Buffer to drive a 500Ohm load?
I've dished out tons of advice here on DIY Audio, though. I suggest you re-read the sections of supply decoupling and grounding, specifically the small section titled An Improved Grounding Scheme. Note the first two sentences,
and compare with your choice of a REF ground star. With the circuit you have, I strongly doubt you'll be able to meet the data sheet performance of the LM4780. The THD will rise dramatically above a few hundred Hz due to the ground inductance (routing) in your circuit.
The best way to reduce the ground impedance (= resistance and inductance) is to use as short and wide a conductor as possible. The shortest and widest conductor possible is a plane.
You can see a bunch of data I took on the impact of the grounding scheme here: http://www.diyaudio.com/forums/chip-amps/252436-lm3886-pcb-vs-point-point-data-3.html#post3846783
Tom
Thanx for the reply but
I don't understand it
The whole GND star is just 4mm's away from the Load GND.
The only substantial length is the GND for the in+ resistor but that comes out by the load gnd. How should a load current result in a measuring fault?
I don't see the problem 😕
Well then you didn't fully read or understand what he wrote, Tom goes to great length to explain what's important and why.
I've implemented two of his suggestions in a couple of chip amps that I had designed and built several years ago, and there were palpable improvements to the sound. I followed his recommendations for supply decoupling (what I had implemented was inadequate), changed the "ground" reference of the feedback network from the input side to the output side (that one cleaned up a slight grunge I was hearing in the upper frequencies.)
So I recommend you revisit his "Taming the LM3886" pages and come back with your questions on the parts you don't understand (it took time for me to understand some of it too) ...there's no shame in not understanding something...we all start out ignorant and work our way to enlightenment.
Mike
Since this is germane to this thread and it popped into my head when I was reading through your "Taming the LM3886" grounding page I thought I would post it here.
I have always wondered WHY the speaker return "ground" is tied into the amplifier PCB at all. Thinking of loop area or return path lengths, I suppose that returning the current to the ground pins of the PS caps on the amplifier board makes sense. On the other hand, the currents that are driving the amplifier output devices are coming from the main power supply caps and not just the caps on the amp PCB itself (unless they are the same because of onboard PS). So in a sense you can follow the currents all the way back to the PS by running a separate return wire, which would not at all need to be connected to our routed through the PCB. It would return to the PCB with the positive speaker lead, then separate from it and run above the PCB over to where the PS connections enter the board, at which point it would follow them back to the PS, twisted together with the pos rail, neg rail, and a small signal ground wire. This would seem to eliminate problems with high return currents from the loudspeaker in the PCB, which can corrupt the ground by inducing voltage, etc.
Tom, can you comment on this approach, and if it would create problems talk about what those are? Thanks.
Last edited:
It is where you connect the feedback loop to the load that is important. If you connect the load return to the PSU then any voltage between the PSU ground and the amp ground will produce an error in the feedback loop and at the output.
The load is not in a feedback loop...
The feedback loop is only around the amplifier. I am not recommending eliminating this - but because of the feedback resistor the current is very small and there is no problem due to current.
Perhaps I am not understanding your comment correctly?
Also, regarding your comment "any voltage between the PSU ground and the amp ground": which is worse, voltage drop on a thin PCB trace or voltage drop on some thick wires to/from the PS? Compared to the distance to/from the amp/speaker the amp/PS distance is much smaller and I am advocating using wires to make these connections.
Last edited:
The feedback loop should be parallel to the load. Any additional voltage (current flow between PSU and AMP GND) that you place in the loop will cause an error at the input and output.
Last edited:
CharlieL,
you are right.
The current to the speaker comes from the PSU. That current must return to the PSU.
The route that the Flow and Return follows must be low LOOP AREA.
That requires that the speaker leads be at least close coupled, but preferably twisted, or coaxial.
The current that flows THROUGH the amplifier to the speaker also follows a route. The speaker Return must closely follow that route.
The current from the PSU to the amplifier arrives via two supply leads, The +ve and -ve leads of the PSU to amp triplet.
The speaker return has to be close coupled to the +ve AND -ve leads.
Your description seems to meet all those requirements.
you are right.
The current to the speaker comes from the PSU. That current must return to the PSU.
The route that the Flow and Return follows must be low LOOP AREA.
That requires that the speaker leads be at least close coupled, but preferably twisted, or coaxial.
The current that flows THROUGH the amplifier to the speaker also follows a route. The speaker Return must closely follow that route.
The current from the PSU to the amplifier arrives via two supply leads, The +ve and -ve leads of the PSU to amp triplet.
The speaker return has to be close coupled to the +ve AND -ve leads.
Your description seems to meet all those requirements.
Last edited:
Then I suggest working on gaining understanding. Play with the different grounding scenarios in a circuit simulator. Or build it several ways and measure it. The former is the less expensive and faster option.
The use of a ground star is problem #1. Here's why: You want as little voltage drop across the ground as you can possibly get. To accomplish this, you need the lowest impedance you can possibly get. Recall, impedance is both real (resistive) and imaginary (reactive (inductive/capacitive)). At audio frequencies, the resistance and inductance are the ones that matter the most and you need to drive both of them as close to zero as you can get as this will result in the lowest error voltage. Any error voltage will degrade the THD of the amp, resulting in crappy "chipamp" sound (rising THD versus frequency). The lowest possible impedance you can get is a ground plane, so use a ground plane.
The argument against a ground plane often goes, "but the currents will mix". That's true. They will. However, by designing the ground plane correctly, for example by keeping all the high currents flowing primarily in one end of the plane with the other end being relatively quiet, you can get good separation between currents. That way you can keep the supply/load currents and the feedback currents separate, for example. Both supply/load currents (A) and the feedback currents (mA) are nasty if they get into your reference ground.
To keep the reference/input ground separate, you can either pour a separate plane for it or you can make a moat in your current plane using anti-copper to make an island in the plane. The small input/reference ground plane island should join with the main ground plane at the output ground connection.
Pouring a ground plane in high-end audio is not as simple as just plopping down a rectangle in the CAD tool and calling it done. You have to put some thought into where the currents flow and make sure you keep the large currents away from the sensitive spots, either by careful component placement or by moating. Most likely you'll be using both methods. Do beware that whenever you slice the ground plane, you'll increase its impedance, so you need to think about where to put the input section to avoid excessive hacking of your main ground plane.
The load current creates a voltage drop across your ground connection. With a ground star, you maximize this voltage drop. You then proceed to put it in series with your input signal ground through that 4 mm connection to the load ground. That's the problem; or rather part of it.
Thank you.
Yep. It takes work. The results are well worth it, though.
As I write in the first paragraph of the An Improved Grounding Scheme section (second time I quote it on this thread, by the way):
Maybe I should add a qualifier: This means that GND_SIG should connect to GND_LOAD with a low-impedance connection.
I would also invite you to think about where GND_LOAD should connect. At frequencies above a few hundred Hz the vast majority of the current flows from the local bypass caps, through the IC, through the load, and back to the local bypass caps. At least it does if you follow my suggestions for bypassing on my "Taming the LM3886" pages. This means GND_LOAD should connect to the PCB, preferably as close to the local bypass caps as you can get and tied to them via a ground plane. This means that GND_LOAD and GND_SIG will meet on the PCB as well.
Bingo!
Correct. That current flow is from the main reservoir cap, through a wire to the board, through the local bypass caps, back through a wire to the main reservoir cap. Keep those wires relatively beefy (low impedance) and tightly coupled either with a very tight twist or with zip ties (low loop area).
No, it just moves the problem to the supply wiring and increases the loop area. There is NO problem having the load currents on the PCB if you pay attention to where the current flows, minimize the impedance the currents flows through, and minimize the loop area.
That is 100 % true as long as you keep in mind that the feedback loop has two connections: signal and ground. You are trying to control the voltage across the output of the amp. This means, the input to the feedback loop needs to measure the output of the amp. Connecting the signal part of the feedback loop is easy. Just tap off at the pin of the output connector (or the "inside" pin of the Thiele network, if used). The feedback ground connection is usually the one that causes trouble.
There are two reasons for the trouble. One issue is that with a crappy layout, part of the load or supply current ends up flowing in the feedback ground, adding to the feedback signal. I addressed how to keep the currents separate earlier in this post. The other issue is that the feedback current is pretty nasty. It basically contains the error-correction signal imposed by the loop. You definitely want to keep this away from the input signal.
One way to keep the feedback current separate is to run a long and skinny trace to the ground reference (where the GND_LOAD and GND_SIG join). That will keep the current separate, but it will also drastically increase the inductance of the feedback ground connection. This will result in a degradation in THD+N at frequencies above a few hundred Hz due to the reduction in gain caused by the increasing magnitude of the feedback impedance. Recall the magnitude of the impedance of an inductor rises with frequency. This is why we use a ... wait for it ... ground plane to connect the feedback ground.
The final issue is the input ground. In a single-ended amp, adding a voltage on the input ground adds a voltage directly in series with the input signal. It should go without saying that the input ground should be kept quiet for this very reason. That's why I suggest using a small island in the main ground plane if you can do so without mucking up the main ground plane as I described above.
Tom
- Status
- Not open for further replies.