[转自www.neurochrome.com] Taming the LM3886 Chip Amplifier

90999

[转自www.neurochrome.com]  PS:光看图就能懂。


                        Taming the LM3886 Chip Amplifier                                                                    
NOTE: I consider this page to be a live document. I.e., I will update it when I have new thoughts or findings on the topic. Last update was: July 10th, 2016.
The National Semiconductor (now Texas Instruments) LM3886 chip amp is a pretty nice little chip.

With headline specs touting nearly 70 W of output power at 0.03 % THD and the ability to source over 11 A, what’s not to like?

Well, as with any high-performance IC, it takes some engineering to get the circuit to live up to the data sheet specs.

In particular with power op-amps, such as LM3886, the PCB layout or point-to-point wiring routes make a significant difference in the circuit performance.

Judging by the chatter on the DIY Audio Chip Amps Forum, the main challenges for designers appear to be stability, bypassing, grounding, layout, and thermal design.
My intent with these pages is to explore some of the common pitfalls and provide a design guide to a successful LM3886 design.





                        Stability                                                                 

• Model Validation
• The Influence of Circuit Layout on Stability
• The Zobel Network
• Those Extra “Stability Components”
  

The main source of concern of the DIY crowd appears to be stability.

There are good reasons for this. High frequency instability can cause the amplifier to emit large signals at frequencies well above the audible range for humans.

These signals will dissipate significant power in the speaker tweeters, causing them to fail.
Hence, many amps have been given a bad reputation for being “tweeter eaters”.

This is further exacerbated by the fact that many DIY enthusiasts do not own the tools, such as oscilloscopes and signal generators, to spot the signs of instability before the speakers are connected.
I have identified five main causes of high frequency instability:

• Low phase or gain margin
• Excessive capacitive load
• Excessive parasitic inductance in the feedback network
• Lack of supply decoupling
• Operation without Zobel or Thiele networks
  

To determine the impact of each of these culprits, I rely on circuit simulations validated by laboratory measurements.
Simulations have the beautiful feature that circuit performance under ideal conditions can be compared with circuit performance under real conditions by including the relevant parasitics in the simulation.

Model Validation

For the simulations, I chose to use TINA-TI, a free Spice circuit simulator available from Texas Instruments.
I chose TINA because it is directly compatible with the Spice models found on TI’s website.

Note that TINA uses modern day SI notation for the prefixes. I.e., m = 10-3 = milli and M = 106 = mega, unlike Spice which is not case sensitive and uses “meg” for mega.
The first step with any simulation project is to validate the models used.
In other words, simulation results need to be compared with reality.

As the objective of this project is to determine the stability of an LM3886-based amplifier, the primary point of interest is the open-loop gain/phase curve. This is simulated below.



The challenge with open-loop measurements (and simulations) is that the feedback loop needs to be closed at DC so the circuit can settle at the correct DC operating point, but needs to be opened for the AC part of the measurement or simulation.
In simulation, this is easy. An LC lowpass filter (L1, C1) with an incredibly low cutoff frequency is inserted in the feedback loop.
The cutoff frequency of the filter is lowered until it no longer impacts the gain/phase response within the frequency band of interest.

In this case, an LC filter using L1 = 10 MH and C1 = 10 MF is used. This results in a cutoff frequency of 16 nHz. Gotta love simulation…

The resulting gain/phase plot is compared with the data sheet figure:



Simulation shows a phase margin (PM) of 78 ° for a gain of 20 dB (10x).

The data sheet indicates a PM of about 65 °.
Simulation also shows the unity-gain bandwidth (UGBW) to be about 10 MHz, whereas, the data sheet indicates an UGBW of about 4 MHz.
The simulated DC gain (AVOL(DC)) matches the data sheet figure of 115 dB (TYP).
The skeptics are muttering in the hallway.
“Yeah, yeah… All this simulation is great. What about reality?!”

To address this, I measured the phase margin of an LM3886 amplifier.

The amp was built using a very compact point-to-point layout and loaded by an 8 Ω resistor.
The phase margin was measured using an HP 3577A network analyzer injecting a test signal into the feedback loop using a Tektronix CT-6 current transformer.

The result is shown below. The marker is placed at the unity gain frequency.

The CT-6 is optimized for use at RF, hence has significant roll-off near DC.

This is responsible for the flattening of the gain and phase curves towards 200 kHz in the plot above.

The phase margin measures 67.8 °. This is in very good agreement with the data sheet specs.
The UGBW measures 1.4 MHz, a bit higher still than the simulations and data sheet would indicate.
Conclusion: Overall, the model is slightly optimistic.

The PM and UGBW are slightly higher than the data sheet indicates.

The DC performance, however, is spot on.

I trust the model to provide good information regarding trends and stability mechanisms and I would expect the simulated PM to be about 15~20 ° higher than the measured value.

It is worth noting that the UGBW measures even higher on actual circuits than the simulated value.

The Influence of Circuit Layout on Stability

As noted in the LM3886 data sheet (p. 20), the inductance in the output lead of the amplifier IC greatly impacts stability.

As a rule of thumb, figure that 1 mm of wire or PCB trace has a self-inductance of approx. 1 nH.
Hence, the placement of the feedback resistor will have a big impact on amplifier performance.
The example below shows two common layouts of the LM3886 with resistive feedback.

Only the feedback resistors have been included here. The dimensions marked in green are in mil (1 mil = 0.001″ = 25.4 µm).



As shown, the good layout results in approx. 240 mil (6.1 mm) of trace routing in the feedback network.

Allowing for a little parasitic inductance in resistor R2, the parasitic inductance in the feedback path of the good layout is approx. 10 nH.
The poor layout exhibits 1.04″ (26.4 mm) of trace routing, resulting in a parasitic inductance of roughly 30 nH.
Simulations of the phase margin (PM) and gain margin (GM) were performed for a parasitic inductance, Lout, of 0 nH (ideal case), 10 nH (good layout), and 30 nH (poor layout). The results are plotted below (click for a larger view).



Note that the textbook definition of stability is that PM > 0 ° and GM < 0 dB.
In an actual circuit, I prefer the PM to be greater than 60 ° and the GM below -10 dB.
The impact of the layout is pretty stark.
Note how the poor layout (which really does not look that bad in the layout editor) causes the PM to fall off a cliff once the load capacitance exceeds 200 nF.

The degradation in circuit stability is caused by the resonance of Lout and Cload.

It’s pretty easy to spot the trouble brewing in the loop response.



Note the resonance at 6.5 MHz. Once that peak crosses 0 dB, the circuit will oscillate.
This is a tweeter eater.

The Zobel Network

To combat the phase change caused by the Lout, Cload resonant circuit, a compensation network is added.

Two types of networks are commonly used: an RC series combination from the amp output to ground and an LR parallel combination in series with the output.

The resulting schematic is shown below.

The values used are the ones listed in the LM3886 data sheet.
There is much confusion about the naming conventions of these output filters.

Technically, the RC series network is the Zobel network and LR parallel combination a Thiele network.

Occasionally, the Zobel network is referred to as a Boucherot cell as well.
In the schematic below, it would have been more consistent with the naming convention to use Lt and Rt rather than Lz and Rz2.

As previously stated, there’s much confusion…

I will do my best to limit the confusion from here on.


The Zobel network performs two main functions:

• If selected properly, it aids the stability of the LM3886 feedback loop by adding a pole-zero pair in the feedback loop. The pole-zero pair is the result of the frequency-dependent voltage divider comprised of the open-loop output impedance of the LM3886, Rout, together with Cz and Rz1.
• It provides a low load impedance for the LM3886 output stage at frequencies where the Thiele network has effectively decoupled the external load impedance.
  

The LM3886 has a quasi-complimentary output stage.

When the amplifier output is positive, the output is driven by an emitter follower.

When output is negative, a complimentary feedback pair (CFP) output stage drives the output.
Emitter followers are notorious for oscillating under light load conditions.

This is caused by the rolloff of transistor current gain (β) at HF.

In addition the maximum operating speed of the transistor, ft, decreases at light load.
These two properties cause the output impedance of the emitter follower to be inductive at HF, in particular at light load.
The output inductance forms a resonant circuit with the parasitic and load capacitance, resulting in oscillations.

This is combated effectively by adding a load, Rz1, to the amplifier.
To avoid dissipating significant power at DC, a capacitor, Cz, is in series with the resistor.
CFP output stages contain a local feedback loop with relatively high gain.

This is a common culprit for oscillations as well, which is why the LM3886, under marginal stability conditions, will often oscillate on the negative swing but not the positive.

On the CFP output, the Zobel network, essentially, works as a snubber, dampening the local oscillations.
The main function of the Thiele network is to isolate the external load capacitance, Cload, from the amplifier output at HF.
Rerunning the PM, GM vs Cload simulation with the Zobel and Thiele networks added, the following results are obtained.



The importance of the Zobel and Thiele networks is pretty obvious here… The improvement is mainly due to the Thiele network. Let’s explore that a bit from an intuitive standpoint. There are three main frequency regions of interest:

• Low frequency: Audio frequencies. At these frequencies, the impedance of Cz is significantly greater than that of Rz1. At these frequencies, the Zobel network is not presenting much of a load on the amplifier. Consider it an open circuit. For the Thiele network, at LF, the impedance of Lz is significantly smaller than that of Rz2, so the parallel combination of the two is dominated by Lz. Hence, Lz || Rz2 present practically a short circuit at LF.
• High frequency: At HF, the impedance of Cz is significantly smaller than Rz1, hence, the Zobel network is mostly resistive. It will present a load of Rz1 = 2.7 Ω on the amplifier. The impedance of the Thiele network is dominated by Rz2 as the inductor’s impedance is significantly higher than Rz2 at HF. The total load on the LM3886 will be Rz1 in parallel with Rz2 + Zload. If Zload is mainly capacitive, it will act like a short circuit at HF. Thus, the total load on the LM3886 approaches Rz1 || Rz2 as the frequency approaches infinity.
• The transition region. This is the region where LF transitions to HF. The component values for the Thiele and Zobel networks should be selected to place the transition region well outside the audio band.
  

So what is considered “LF” and “HF”?

Numbers, please! Notice the use of the word ‘significantly’ in sections 1. and 2. above? What is ‘significant’?
In most engineering math, where 1-2 digit precision is the norm and three digits considered a luxury, “significantly greater” means “a factor of ten greater”.

I would go as far as saying that 5~10x is probably close enough.
From 1. and 2. above, the transition region is the frequency range where neither Rz1, Cz or Rz2, Lz dominate over one another.
Recall, the reactance of a capacitor and an inductor are: XC = 1/(2π·f·C) and XL = 2π·f·L, respectively.

The frequency where the reactance of Cz is considered significantly greater than Rz1 can be found by solving this equation: 10·Rz1 = 1/(2π·f·Cz). Solving for f yields: f = 1/(2π·C·10·Rz1).
Similarly for the Thiele network: Rz2 = 10·2π·f·Lz → f = Rz2/(2π·10·Lz).
Plugging in the values from the schematic above yields: 1/(2π·C·10·Rz1) = 58.9 kHz and Rz2/(2π·10·Lz) = 227 kHz respectively.

Hence, the lower bound on the transition region would be 58.9 kHz.
Substituting 0.1 for 10 in the equations above yields the upper bound on the transition band: 1/(2π·C·0.1·Rz1) = 5.89 MHz; Rz2/(2π·0.1·Lz) = 22.7 MHz.
From these calculations, it is determined that frequencies from DC to 59 kHz should be considered “LF”, frequencies above 23 MHz, “HF”, and the range in between, the transition band.
Some designers will use two Zobel networks.

One located close to the IC and one mounted on the speaker output terminals of the amplifier. However, simulation shows minimal impact of the second Zobel network.



The inductance L2 and resistance R4 model the effect of the wire between the amplifier board and the speaker terminals.
I figured 15 cm (150 nH) of wire would be representative of a nice, compact layout.
If you are interested in replicating my results or explore further, feel free to use my TINA circuit file: LM3886-LoopStability.TSC
Note: The power dissipated in Rz1 depends on the capacitance of Cz: P(Rz1) = f·Cz·V².

The voltage V is the RMS output voltage at output frequency f. A few examples are tabulated below.

Rail Voltage	Cz	Rz1	P(Rz1)
±22 V	100 nF	2.7 Ω	416 mW
±28 V	100 nF	2.7 Ω	697 mW
±35 V	100 nF	2.7 Ω	1.12 W
±28 V	56 nF	4.7 Ω	390 mW
±28 V	33 nF	8.2 Ω	230 mW

Above calculations assume a symmetric drop-out voltage of 1.6 V at clipping.

Note that all RC combinations listed form a zero at roughly the same frequency, hence, are equally effective as a Zobel network as far as stability is concerned, however, they may not all be equally effective as an HF load for the LM3886.

For continuous sine wave operation, the resistor Rz1 should be rated for operation at 3~4 times higher power than listed above.

For music signals with crest factors of 3 dB or higher, one can probably get away with specifying a power dissipation rating for Rz1 of 1~2 times the value calculated above.

For the higher rail voltages it is good practice to choose a Cz1 with a lower capacitance such that a resistor with a lower power rating can be used.

Note, however, that power resistors of higher resistances tend to exhibit higher parasitic inductance which will affect the frequency response of the Zobel network.
I suggest limiting Rz1 to 10 Ω to avoid excessive inductance. Alternatively, a thick film resistor type can be chosen.


Those Extra “Stability Components”

Much is read into the various figures in the data sheet.
For example, Rf2, Cf, and Cc in the AC Electrical Test Circuit are often mentioned by DIYers as “required for stability”.

Note that these test circuits are optimized for use on the tester used for final test.

These testers and load boards often exhibit significant parasitics, hence, these circuits should not necessarily be considered “recommended” or “required” configurations.



The circuit works as follows: Rf1 and Ri set the LF gain to +21 V/V. At HF (when the reactance of Cf is small compared to Rf2), the gain is set by (Rf1 || Rf2) and Ri to +11 V/V.
This creates a zero in the loop gain response around 150 kHz followed by a pole at about 300 kHz.
This explains the slight bump around 200 kHz on the gain curve in the simulation below.



Note that the phase margin is actually considerably worse than without those “stability components”.
Here is the circuit without the “stability components”:



And phase/gain margins versus load capacitance:



The degradation in phase/gain margin is primarily caused by Cc.

According to the data sheet (pp. 8, 22), the purpose of Cc is to eliminate quasi oscillation caused by the pickup of EMI from the engagement of the SPiKe over-current protection.
Cc is needed if the output impedance of the source driving the LM3886 is high and long signal traces are used.

It follows that the quasi oscillation issue could just as well be addressed by lowering the source impedance or placing a resistor from the non-inverting input pin to ground on the LM3886.

The EMI filter can then be placed on the non-inverting input of the LM3886, where it does not affect the phase margin.
It should be noted that it is possible that Rf2 and Cf are employed to address effects not included in the model. Stay tuned for lab measurements.

90999

                        Supply Decoupling                                                        

               
Unfortunately the effects of power supply non-idealities are not included in the LM3886 model, hence, not part of the simulation.
It should be relatively obvious, however, that if the supply to the LM3886 is bouncing, the LM3886 may behave in unintended ways.
The most common cause of supply bounce is parasitic inductance.
As mentioned earlier, the self-inductance of a piece of wire or PCB trace is approximately 1 nH/mm.
Hence, excessive trace length between the supply bypass capacitors and the IC will result in significant supply inductance.
This inductance will restrict current flow into the IC.
This may cause the IC to, effectively, brown out on fast current spikes.
This can lead to high frequency instability.
The data sheet is a bit ambiguous on the exact requirements for bypassing.
On page 20, it is mentioned that a 10 µF tantalum capacitor with a 100 nF ceramic cap in parallel from each supply pin to ground is all that is needed.
Then in the following paragraph, it is mentioned that if the supply bypass capacitors are greater than 20 µF, HF instability is only an issue if the supply lead inductance exceeds 1 µH (corresponding to about 1 m of trace length).
The larger tantalum cap is intended to provide a low supply impedance at audio frequencies.
The 100 nF ceramic cap ensures that the supply impedance remains relatively low at RF frequencies beyond the self-resonance frequency of the tantalum capacitor.
In addition to the smaller capacitors by the LM3886 supply pins, larger capacitors are needed by the power entry to the circuit board. National recommends a minimum of 470 µF per supply rail.
As mentioned earlier, the purpose of the supply bypass network is to keep the supply impedance as low as possible throughout as wide a frequency range as possible.
In the 15+ years that have passed since the release of the LM3886, there has been a tremendous development, in particular, in the field of multi-layer ceramic capacitors (MLCC) and electrolytic capacitors. Hence, it seems prudent to explore the limits of the supply bypassing and explore the performance that can be achieved by using more modern components.
The figure below shows the resulting supply impedance for one supply rail, as seen by the LM3886, for the recommended supply bypass network.
The network consists of a 100 nF film cap by the IC pin, then a 10 uF tantalum capacitor, followed by a generic 1000 uF electrolytic can where the power enters the PCB.
I assumed that the board is connected to the power supply by 20 cm (8″) of 0.5 mm2 (AWG 20) wire and that the supply is an ideal supply (Zout = 0 Ω).



The capacitor parasitics used in the simulation were those measured on actual components using an HP 4194A Impedance/Gain-Phase Analyzer.
The supply impedance shows a slight effect of the 1000 µF electrolytic cap around 5 kHz and the resonance of the lead inductance and the 100 nF film cap is apparent at 5 MHz.
The impact of the 10 uF tantalum capacitor is difficult to spot. It may be responsible for the slight change in slope near 100 kHz.
Let’s explore the limitations of the system.
The LM3886 supply pins are rather long.
There is at least 7~8 mm exposed outside the plastic package and probably another 7~8 mm as part of the lead frame inside. Hence, the inductance between the IC die and the first bypass cap is about 15 nH.
This may even be a tad optimistic.
The inductance of the IC supply leads dominates the supply impedance at HF. At 10 MHz, the impedance of the 15 nH inductor is about 1 Ω (at 100 MHz, 10 Ω), hence, this is the lower limit on the supply impedance at HF.
At DC, the limit is set by the resistance of the wires, connectors, and terminal blocks on the supply inlet to the board. Hence, the lowest impedance possible at LF, in this setup, is 20 mΩ, not including the DC resistance of the IC pin itself.
The commonly recommended supply bypassing strategy of small-medium-large capacitors in parallel works by employing the progressively increasing self-resonance frequencies (SRF) of the bypass capacitors.
At frequencies higher than the SRF of the capacitor, the impedance of the capacitor is dominated by the impedance of its parasitic inductance, i.e. the capacitor “has turned inductive”.
The idea behind the traditional bypassing scheme is to ensure that when the large cap “has turned inductive”, the medium cap takes over and dominates the total supply impedance.
Similarly for each of the following caps in the decoupling network.
This strategy is valid as long as the inductance of the IC pin is lower than the inductance of the traces and parasitic inductances of the bypass capacitors.
In cases where the IC pin inductance dominates, the game changes.
For the LM3886, a more appropriate bypassing strategy is to get as much energy storage as close to the IC pin as possible.
With the parts available in present day, it is possible to improve greatly upon the bypassing scheme recommended in the LM3886 data sheet.



Above simulation uses a 4.7 µF X7R ceramic capacitor (TDK P/N: FK20X7R1H475K) and a 22 µF OSCON electrolytic capacitor (Panasonic P/N: 35SEPF22M) along with the same generic 1000 µF electrolytic can from the previous simulation.
The simulation shows a significant improvement in the 100 kHz to 10 MHz frequency range.
The ceramic caps and the OSCON caps needed for proper bypassing of the LM3886 will set you back a grand total of about $3.50 in today’s Digikey prices.
That seems like money well spent.
It is worth noting that increasing the 1000 µF capacitor to 10000 µF has very little impact on the supply impedance.
In fact, reducing the capacitance to around 100 µF is possible without any adverse negative impact.
The data sheet recommendation of 470 µF or larger is very reasonable.
This allows sufficient margin to maintain a good, low supply impedance, even with the relatively large component tolerances found on electrolytic caps.
I recommend 1000 µF as it is commonly available at a reasonable price point.
For the ceramic capacitors, it is worth spending a little extra to get the X5R or X7R dielectric ceramic capacitors rather than the cheaper Y5V ceramic.
The voltage coefficient of Y5V is horrid! At half the rated voltage, expect the capacitance to be about 30 % of the marked value.
It’s down to 20 % of the marked capacitance at the rated voltage for a Y5V cap.
The voltage coefficient of X5R and X7R is not pretty either, but unlike Y5V, you can expect the capacitance to be about 50 % of the marked value at 50 % of the rated voltage.
Therefore, if possible, I also suggest getting capacitors rated for operation at 100 V rather than the commonly used 50 V types.
For additional information on the different dielectrics, see this white paper and Wikipedia.

90999

                        Grounding                                                               

• The Layout is the Circuit
• An Example of Star Grounding
• An Improved Grounding Scheme
• The Mute Circuit
  
  

Casual reading of various audio fora quickly reveals that grounding is a perpetual cause of confusion.
It seems most builders have a reasonably good grasp of how to route the VCC and VEE supplies, but the ground routing ranges from giant spider-like trace routes to a solid ground plane.
This is a bit ironic, as one of the main functions of the ground routing is to provide a return path for the supply currents.

The Layout is the Circuit

The Grounding Conundrum starts at the data sheet with the figure on Page 21 of the LM3886 data sheet (reproduced below).



The bottom schematic is touted as the holy grail and represents the Star Grounding scheme commonly used by DIY enthusiasts, confirmation bias prevails, and this is the topology implemented.
However, in a mono block or small stereo amp configuration, this is not the most optimal layout. In fact, it is a rather poor layout.
The fundamental message that the layout has a big impact on circuit performance is still valid, however.

An Example of Star Grounding

The layout shown below is reasonably tight. The decoupling capacitors (C2, C4) are as close to the IC as possible and the main reservoir caps (C1, C3) are tucked in as well.
This minimizes the supply inductance as discussed above.
This layout is by no means optimal, but represents what a reasonably savvy DIYer could come up with.
The ground trace (bottom layer – red) to the output connector is probably quite a bit shorter than it would be in real life as I have omitted the Thiele and Zobel networks.



I operate with four “grounds”:

• GND: Simulator node 0, textbook ground. This is my reference point.
• GND_PWR: The “ground star” at the local decoupling on the LM3886.
• GND_SIG: Small signal ground. I.e. ground connection for the input connector and feedback connection.
• GND_LOAD: The black speaker terminal, speaker (load) ground.
  

The wide traces are 80 mil (2 mm) wide. The GND_SIG trace from R1 is 40 mil (1 mm) wide.
By most people’s standards, these are pretty fat traces.
I used the Saturn PCB Toolkit to calculate the trace inductance and resistance. Using these parameters,
I simulated the effects of the load return current on circuit performance.



In the simulation, the inputs to the amplifier are grounded to GND_SIG and an AC current is injected into the GND_LOAD net.
This represents the current returning from the speaker load.
The return current results in an error voltage developing across the ground nets, part of which is amplified by the LM3886.
The simulation uses a voltage controlled voltage source (VCVS) with a gain of 1 V/V to measure the resulting error voltage developed across the load.
The resulting error voltage is plotted in dBV. Recall, the goal here is to have as little error voltage developed across the load as possible, as this error will degrade the THD performance of the amplifier.
The simulation shows that for signals below 10 kHz, a 1 A return current will result in about 7.1 mV (-43 dBV) of differential voltage across the load.
This is not very impressive performance.
Another common DIY solution is to use the center point between the local decoupling capacitors as the “star ground”.
That’s not a bad idea, although, it does not improve the performance significantly as shown in the simulation below.



Neither star grounding scheme works well. As the current returns from the load, it develops a voltage drop across the GND_LOAD impedance.
This error voltage is subtracted from the desired voltage across the load, resulting in poor performance.
The GND_SIG reference is taken at the ground star point, hence, any error voltage developed across the GND_LOAD net will remain unaffected by the amplifier’s loop gain as it is outside the feedback loop.
It is possible to reduce the error voltage by optimizing the layout, minimizing the impedance of the GND_LOAD net.
In the layout shown above, this would be trivial to do by swapping the connections to pins 1 and 2 of the output connector and by using a ground plane rather than a trace.
The inductance per unit length of a PCB trace is reduced when the trace width is increased.
A plane or pour is the widest trace possible, hence, a plane has the lowest possible inductance and lowest possible resistance.
The proper use of ground planes and/or pours for high-current routes (supply pins, output pin) greatly improves circuit performance as the trace impedance is minimized.
This will translate directly to improvements in the THD performance of the circuit.
There is more room for improvement, however.
Significant improvement in circuit performance can be obtained by applying the loop gain of the amplifier to reduce this error voltage.

An Improved Grounding Scheme

From a feedback theory point-of-view, it seems apparent that if the voltage across the load is what we intend to control, the feedback voltage should be measured as close to the load as possible.
This means that GND_SIG should connect to GND_LOAD. The resulting circuit is shown below along with the simulation result.



Bingo! Now 1 A of returning load current will result in 100 nV (-140 dBV) of error voltage developed across the load for DC signals.
Even at 10 kHz, the error voltage is only about 56 µV (-85 dBV) – a 40+ dB improvement over the star grounding scheme at 10 kHz and 95 dB improvement near DC.
The only difference between the star ground and the improved grounding scheme is that the GND_SIG trace was routed to the output connector rather than to the star ground.
The layout is the circuit! I keep coming back to this statement as the mantra of precision circuit design.

The Mute Circuit

The final point of confusion is that pesky “GND” pin on the LM3886. Where should it connect?
The short answer is: It doesn’t really matter. Let’s explore the equivalent circuit schematic for the LM3886 shown below.



It may look a bit intimidating at first, but it can be broken down into sub-blocks pretty for ease of understanding.
It turns out the LM3886 has two input stages. The input stage consisting of Q4B, Q5B, along with the two emitter followers connecting to +IN and -IN, is the one used during normal operation.
The second input stage, Q4A, Q5A, is used when the output is muted. Switching between the two stages is done by Q1 and Q2 operating as an analog switch.
Consider the case where Imute = 0 and the amp is muted. Imute = 0 causes Q3 to turn off. Hence, the base of Q1 is pulled high through the two diodes and the 1 kΩ resistor.
The base of Q2 is pulled low by Iref, hence, Q2 conducts the full input stage bias current. Q2 directs the current to the mute input stage, Q4A and Q5A.
This current path is highlighted in red in the figure above. Q5A senses the voltage at the output of the amp. Q4A is biased to GND through a 10 kΩ resistor (matching the 10 kΩ on the base of Q5A).
In this mode, the amplifier will be driven to present the voltage on the GND pin at the output of the amplifier.
As Imute is increased, Q3 will turn on.
When Imute is sufficiently greater than Iref, Q1 and Q2 will switch, and all the input stage bias current now flows into the main input stage (Q4B, Q5B) along the path highlighted in green above.
This enables normal operation of the amplifier.
Examining the equivalent circuit schematic above, it becomes apparent that the voltage present at the GND pin of the IC is only relevant when the amplifier is muted as it is only used by the mute circuit.
Unless you care tremendously about the sound quality when the amplifier is muted, exactly how the GND pin connects to ground does not matter.
I would connect it to the ground by the decoupling caps as that’s usually the closest available ground.

90999

                        Thermal Design                                                               

• Temperature & Length Correction
• Thermal Design Example 1: The Engineering Solution
• Thermal Design Example 2: The Crest Factor
• Thermal Design Example 3: The Duty Cycle
• Thermal Design Example 4: Other Solutions
  
  
  • Thermal Cut-Off Switch
  • Real World Design Example
    
  
  
  

A sticking point for many DIY enthusiasts appears to be thermal design.
This is rather unfortunate, as thermal design is very important in chip amp applications.
The math is as simple as Ohm’s Law, E = I × R, so it appears the challenge is mainly related to the terminology used in thermal design.
For reasons that will become obvious in a bit, an analogy between the thermal domain and the electrical domain can be made.
This analogy allows for the use of “electrical equations”, such as Ohm’s Law, on thermal systems.
The relevant bits of the analogy are tabulated below.

Thermal Property	Symbol	Thermal Unit	Electrical Analogy	Symbol	Electrical Unit
Power	P	W	Current	I	A
Thermal Resistance	θ	W/°K = W/°C	Electrical Resistance	R	Ω
Temperature	T	°C	Voltage	E	V

Note: All equations on this page use SI units except where noted. If in doubt, assume SI units.
The biggest challenge in thermal design is often to obtain the thermal resistances needed for the calculations, in particular the thermal resistance of the heat sink.
If not provided by the manufacturer, I know of two ways to obtain this data:

• Mount a power transistor or power resistor to the heat sink, connect it to a power supply, and operate the circuit at a known power dissipation until the heat sink temperature has fully stabilized. Measure the temperature of the ambient air and the heat sink. The thermal resistance can then be calculated as: θsa = (Theat sink – Tambient)/Pdiss.
• Find an extrusion in Aavid’s catalog that matches your heat sink and use their thermal resistance simulator to calculate its thermal resistance. Aavid: North American Extrusions; European Extrusions. If an exact match is not found, it is usually possible to find an extrusion that is reasonably close in terms of width, breadth, length, fin dimensions, and base thickness.
  

Temperature & Length Correction

Note that heat sink manufacturers tend to specify the thermal resistance of their extrusions for a 3″ (76.2 mm) long section of extrusion operating 75 °C above ambient temperature.
If you operate your heat sink at a different temperature differential or use a length different than 3″, you will need to apply a couple of correction factors.
The thermal performance is measured at a temperature differential of 75 °C, i.e. the heat sink temperature is 75 °C above ambient temperature.
Unless your are planning to operate the LM3886 near or above its thermal limit, you will likely have to reduce the temperature differential.
Sadly, this means the heat sink becomes less efficient.
At a temperature differential of 30 °C, the heat sink has a 25.7 % higher effective thermal resistance (Aavid, temperature correction factors), hence, multiply the specified thermal resistance by 1.257 to obtain the effective thermal resistance at ΔT = 30 °C.
A longer heat sink of a given extrusion profile will have a lower thermal resistance (heat up less for a given power dissipation) than a shorter length of the same extrusion. Unfortunately, the relationship is far from linear.
Again, Aavid comes to the rescue with a table of length correction factors.
For example, a 6″ piece of an extrusion specified for a thermal resistance of 1.0 °C/W at 3″, ΔT = 75 °C will have a thermal resistance of 1.0 * 0.73 = 0.73 °C/W at ΔT = 75 °C.
If both the temperature differential and length are different from the specified values, the two correction factors multiply.
If our example heat sink extrusion (1.0 °C/W @ 3″, ΔT = 75 °C) is cut to 6″ and operated at ΔT = 30 °C, the math works out as follows: 1.0 * 0.73 * 1.257 = 0.92 °C/W @ 6″, ΔT = 30 °C.

Thermal Design Example 1: The Engineering Solution

A well engineered amplifier should be able to handle anything the user throws at it, including sine wave testing at the highest power dissipation.
Hence, the thermal design originates from the power dissipated in the LM3886.
This can be calculated, but the math gets a bit hairy.
Thankfully, National was kind enough to provide graphs for 4 Ω and 8 Ω loads in the data sheet (Figures 35 and 36).
The power dissipated in the LM3886 versus output power and supply voltage is shown below for a 4 Ω load.

For this example, let’s assume a safe and sane supply voltage of ±25 V.
From the graph, the peak power dissipated in the LM3886 is found to be about 32 W.

For the ambient temperature, I normally use 25 °C (just shy of 80 °F).
This jives pretty well with the temperature in a warm living room.
The maximum allowable heat sink temperature is the subject of some debate.
I would consider 50 °C to be comfortable and 60 °C to be the limit for an external heat sink. 50 °C is definitely hot to the touch, but I can touch the heat sink continuously for a few seconds before I have to remove my hand.
60 °C is hot enough that I can only touch the heat sink for a brief moment (maybe half a second) at a time. It’s definitely hot but not hot enough to leave blisters on brief contact.
One can also draw some inspiration from the standards used for kitchen appliances.
For example, according to ANSI/UL 858 and ANSI Z21.1, exterior metal surfaces are allowed to reach 66 °C – metal handles and knobs, 55 °C.
For an internal heat sink, i.e. a heat sink that is inside a closed enclosure, higher temperatures may be considered reasonable, as long as there is ample ventilation in the chassis and the user cannot access the heat sink through the ventilation holes.
Knowing the ambient temperature, Tambient = 25 °C, and the dissipated power, Pdiss = 32 W, the thermal resistance of the heat sink can be calculated: θSA = (Tsink – Tambient)/Pdiss → θSA = (60 – 25)/32 → θSA = 1.1 °C/W.
As noted earlier, manufacturers tend to specify the thermal resistance of the heat sinks at a temperature differential between heat sink and ambient, ΔT, of 75 °C, hence, a temperature correction factor of 1.257 should be applied when selecting a suitable heat sink from the catalog.
I.e. we should choose a heat sink with a specified thermal resistance, θSA, of 1.1/1.257 = 0.88 °C/W as this heat sink will have an effective thermal resistance of 1.1 °C/W at ΔT = 30 °C. An example of such a heat sink is the 10.000″ profile from Heatsink USA.

In addition to the heat sink, there are two additional thermal resistances in the system:

• Device junction to IC package or case (θJC)
• IC package to heat sink (θCS)
  

From the table on page 3 of the data sheet, the thermal resistance of the non-isolated package is found.



Two thermal resistances are listed. θJC is the resistance from the device junction to the case. θJA is the thermal resistance from junction to ambient air.
The latter is only relevant if we were to operate the LM3886 without a heat sink. So: θJC = 1.0 °C/W.
As the package of the IC is connected to the negative supply voltage, a thermal washer or pad is needed between the heat sink and the IC.
These washers are designed to provide reasonable thermal conductivity while maintaining good electrical isolation.
Traditionally, mica washers have been used in combination with thermal compound. If quality materials are used, this results in a thermal resistance of about 0.2~0.3 °C/W.
The more popular (and certainly less messy) silicone washers have a thermal resistance of about 0.4 °C/W for the better ones.
For exact numbers, see the manufacturer’s data sheets. Note that in addition to the thermal washer, an isolating shoulder washer is needed as well.
The ones intended for TO-220 packages work well.
For this example, let’s use a silicone washer: θCS = 0.4 °C/W.
Finally, the junction temperature can be calculated: Tjunction = Tambient + Pdiss * (θJC + θCS + θSA) → Tjunction = 25 + 32 * (1.0 + 0.4 + 1.1) = 105 °C.

The observant readers will notice that this equation is of the same form as Ohm’s Law.
Temperature is analogous to voltage, power to current, and thermal resistance to electrical resistance.
Ohm’s Law, E = I × R, in the electrical domain, is analogous to T = P × θ in the thermal domain.
This means we can simulate this thermal system using an electrical circuit simulator such as TINA-TI.



Power is analogous to current, so Pdiss = 32 W becomes Idiss = 32 A.
Temperatures become voltages, so the 25 °C ambient temperature is now a 25 V voltage source.
The resistances just change units from °C/W or °K/W to Ω.
By plotting the node voltages in the TINA-TI simulation, the temperatures in the thermal system can be determined.
We recognize the temperature of the heat sink (60.2 V = 60.2 °C) and the junction temperature (105 V = 105 °C).
Now let’s see what happens if we use the isolated version of the LM3886 (or LM3886TF to be exact).



With the isolated package, all you need between the package and the heat sink is a thin coat of thermal grease.
The purpose of the grease is to fill in the voids in the surface roughness.
The thermal grease is actually not very thermally conductive, but it’s a lot more conductive than air, hence, a good quality thermal grease applied according to the manufacturer’s specifications can reach a thermal resistance as low as θCS = 0.05 °C/W.
Note that the heat sink remains at the same temperature as with the non-isolated LM3886.
This is expected, as the dissipated power is the same and the heat sink hasn’t changed.
However, note that the junction temperature is significantly higher at 126 °C.
This is caused by the higher thermal resistance from junction to case, θJC.
This thermal resistance is actually not specified in the LM3886 data sheet, but in Application Note AN-1192 (also known as BPA200), it is measured to be about 2 °C/W.
How about a stereo amplifiers with two LM3886 on the same heat sink?
Still assuming ±25 V rails and 4 Ω load, the power dissipated in the heat sink is now twice as high, hence, to maintain the same heat sink temperature, the thermal resistance of the heat sink must be reduced by half, θSA = 0.55 °C/W. The simulation schematic is as follows:



A heat sink with a thermal resistance of 0.55 °C/W at ΔT = 35 °C would have to be specified for 0.55/1.257 = 0.44 °C/W at ΔT = 75 °C. 0.44 °C/W is a rather large heat sink.
I have some older Wakefield heat sinks specified to be 0.4 °C/W.
They measure 300 x 140 x 40 mm. The base thickness is 10 mm and the fin pitch is 10 mm as well. They weigh in at 2.1 kg each.
Most DIY enthusiasts seem to look at the headline specs and aim for those.
Let’s see what happens if we use ±35 V rails, use a 4 Ω load, and crank it to eleven. At an output power of 50 W, we find the highest power dissipation in the LM3886 to be 65 W.
Then the thermals look like this:



The heat sink reaches 77 °C. This is clearly not safe for an external heat sink! In addition, the junction temperature exceeds the ABSMAX by 60 °C.
The amplifier will reach the thermal shutdown limit quickly and the SPiKe protection engage at even moderate output power levels.
This is not a recipe for success or good sound. Thermal design needs to be done using a calculator rather than by guesswork and assumptions.
For more detail on heat sinks, semiconductor packages, thermal interfaces, and mounting techniques than you ever wanted to know,
I suggest reading ON Semiconductor’s Application Note, AN1040/D: “Mounting Considerations for Power Semiconductors“.

Thermal Design Example 2: The Crest Factor

As some people will quickly point out, The Engineering Solution above results in a rather large, heavy, and expensive heat sink.
They will also point out that most audio amplifiers are used for amplifying music signals, which are rather different from pure sine waves.
These are perfectly valid points.
The main difference between music signals and pure sine waves lies in the crest factor.
This factor describes the ratio between the peak amplitude and the RMS value of a signal:

The crest factor is often expressed in dB:
The crest factor of a sine wave is 1.41 (3 dB).
The crest factor of music ranges from about 1.8~2 (5-6 dB) for heavily compressed heavy metal to approximately 10 (20 dB) for well-recorded classical music.
This implies that an amplifier delivering, say, 100 W peak playing well-recorded classical music, only delivers about 1 W RMS.
The same amplifier would deliver 50 W when reproducing a sine wave at the same peak power.
There is a world of difference between the thermal design of an amplifier designed for 1 W RMS and one designed for 50 W RMS.
The burning question is then: Which crest factor should I design for? For an amplifier used in a home stereo to mostly play background music with the occasional use for a loud-ish party, designing for a crest factor around 10-20 dB is probably realistic.
For example, Sound-on-Sound Magazine analyzed the crest factor of 4500 tracks of various types of music.
The article is available on-line: “SOS: Dynamic Range & The Loudness War”.
Their sample collection had an average crest factor of 14 dB.
I will use this number in the design example below.
To perform the thermal design, we need to calculate the amount of power dissipated in the LM3886 for a given output voltage swing.
This requires a bit of arithmetic. You can find the full derivation in textbooks such as Sedra/Smith.
I’ve summarized the highlights below.
It is assumed that the amplifier is driven by a sine wave signal.
The RMS power dissipated in the load can then be calculated as:

PL is the power dissipated in the load, RL is the load resistance, and VOUTpeak is the peak output voltage.
Neglecting the idle dissipation for a minute, the power drawn from the power supply by the output stage can be calculated as:

Where PS is the total power supplied by the power supply and PS+ and PS- are the powers drawn on the VCC and VEE supplies, respectively.
It is assumed that a symmetric power supply is used, i.e. VCC = -VEE. Thankfully, this is normally the case.
The amount of power dissipated in the output stage is the difference between the supplied power and the power delivered to the load, i.e.,

where PD is the power dissipated in the output stage.
As shown above the dissipated power, PD, is a function of the peak voltage of the output swing, VOUTpeak.
The peak output voltage at the maximum power dissipation can be found by taking the derivative of PD(VOUTpeak).
I will spare you the arithmetic and provide the result:

Pugging this value into the equation for PD above, yields the peak power dissipation:

Including the idle dissipation, the peak dissipated power works out to:

Where Ibias is the quiescent current of the output stage. As a sanity check, let’s double-check the numbers from Example 1 above, where RL = 4 Ω, Vsupply = ±25 V, and Ibias = 50 mA (typical spec.).
The peak power dissipation can be calculated as:

This matches the 32 W read from Figure 35 in the data sheet rather well.
The engineers at National Semiconductor may have forgotten to include the idle dissipation, which explains the 2.2 W difference between the calculated number and the one read from the graph.
Now, back to the crest factor…
Using the load impedance and supply voltage from Example 1 (RL = 4 Ω, Vsupply = ±25 V), let’s design the heat sink for a 14 dB crest factor.
First the peak output voltage just before clipping is calculated:

At first glance, Vod is found in the spec table of the data sheet:

However, note that the output dropout voltage is tested with a load current of 100 mA.
To find the dropout voltage at more realistic load currents, we need to dig a bit deeper into the data sheet.

Data sheet figures 14 and 15 show the dropout voltage for 4 Ω and 8 Ω loads, respectively.
There are a couple of noteworthy details here. First off, note that Vod is strongly dependent on the load current, hence, considerably higher when the LM3886 is driving a 4 Ω than an 8 Ω load. Also, note the asymmetrical clipping, i.e. higher Vod when the LM3886 output voltage approaches the negative (VEE) rail than when it approaches the positive (VCC) rail.
The maximum swing without clipping is calculated using Vod = 3.5 V. The resulting peak output power, i.e. the instantaneous power at the crest of the sine wave, can be calculated as:
From the peak power, the RMS power as function of the crest factor in dB can be calculated as:

It follows that the peak output voltage at an RMS output power of PL can be calculated as:

The power dissipated in the LM3886 as function of crest factor may then be calculated from this equation

This time, the quiescent current (or bias current) has been included in the equation.
The dissipated power, including the quiescent dissipation, for a few commonly used crest factors is tabulated below.

Crest Factor (dB)	PL RMS	PL peak	VCC	RL	PD
3 (sine wave)	58.0 W	116 W	±25 V	4 Ω	30.2 W
6 (max. PD)	29.0 W	116 W	±25 V	4 Ω	34.2 W
10	11.6 W	116 W	±25 V	4 Ω	29.2 W
14	4.60 W	116 W	±25 V	4 Ω	22.0 W
20	1.16 W	116 W	±25 V	4 Ω	13.4 W

Readers wanting to tweak the numbers to suit their own application will probably find my Class AB Output Stage Calculator (Excel Sheet) useful.
As shown in the table above, if the amplifier is expected to play music with a relatively high crest factor, the size of the heat sink can be reduced dramatically, as considerably less power is dissipated under these conditions.
This may complicate performance testing using sine wave signals, as the amplifier will overheat if driven continuously at the peak power dissipation if designed to a crest factor above 3 dB.
However, the savings in heat sink weight, bulk, and cost usually outweigh engineering concerns about sine wave testing.

Thermal Design Example 3: The Duty Cycle

An approach similar to using the crest factor is to take advantage of the fact that the amplifier does not dissipate the peak power at all times.
Rather, the amplifier is assumed to be operated at peak power dissipation only for some fraction of the time.
This fraction is called the duty cycle, D = ton / (ton + toff), where ton and toff are the on-time and off-time respectively. In professional audio, a duty cycle of 33 % is commonly assumed.
Using the amplifier specs from Example 2 above (Vsupply = ±25 V, RL = 4 Ω, PDmax = 34.2 W) and a duty cycle of D = 0.33 (33 %), the average dissipated power can be calculated as: PDavg. = D * PDmax → PDavg. = 0.33 * 34.2 = 11.3 W.
For a more conservative estimate, designing for a duty cycle of 50 % might be a more reasonable goal: PDavg. = 0.50 * 34.2 = 17.1 W.
Even with the more conservative 50 % duty cycle, the savings in heat sink size are considerable.

Thermal Design Example 4: Other Solutions

If you have read this far, you have probably realized that my design philosophy is based in solid engineering and science.
This approach is the most likely to produce products that will meet or beat the data sheet performance of the parts.
By now you may have looked at some heat sinks and concluded, “OMG! THOSE THINGS ARE HUGE!!”.
For many DIYers, this reaction is typically followed by denial, “Joe Schmo on The Internet said his amp worked just fine with this itty-bitty heat sink.
See! He has pictures of it. Physics must be wrong!”. Sadly, however, physics is right. Mr. Schmo’s amplifier probably works just fine at normal listening levels where the power dissipation in the LM3886 is barely above the idle dissipation. It may even work well at somewhat high listening levels, as, for most speakers in typical residential settings, this requires less than 1 W delivered to the speakers.
Under these conditions, Mr. Schmo’s amplifier probably works. Probably.
So… Where’s the limit? Given the finite limitations set by physics, what does the design continuum look like and which tradeoffs can be made to reduce the size of the heat sink?
As I see it, there are five reasonable options:

• Reduce the rail voltage, thereby limiting the peak power dissipation.
• Increase the load resistance, i.e. use an 8 Ω speaker rather than a 4 Ω one.
• Use forced air cooling.
• Add a thermal switch on the heat sink to turn the amplifier off before it overheats.
• Design for the needed output power rather than the data sheet headline figures.
  

Reducing the rail voltage will result in an amplifier with a lower max. power output spec.
This may not be palatable to some. Increasing the speaker impedance is also not likely to work for most people. Fans tend to be noisy, or require fan controllers to keep them quiet when the demand for cooling is low. As a result, most readers will likely look at options 4 or 5.
Regardless of how you plan to work around the limitations set by the laws of physics, make sure to do the math to ensure that the implemented amplifier can survive if someone decides to crank the volume knob and run the amp at high power output levels for a while. It may not be able to deliver the high output power indefinitely, but it should at least not self-destruct or endanger the user.

Thermal Cut-Off Switch

For an internal heat sink, the thermal protection circuit in the LM3886 is likely sufficient to protect the IC from melt-down, however, the heat sink and chassis may still get uncomfortably hot under these conditions. For an external heat sink, the heat sink temperature should be limited to 60 ºC for reasons outlined in Example 1 above.
If you are skimping on the size of the heat sink, even if using the methods outlined in Example 2 and 3, I strongly recommend fitting the heat sink with a thermal cut-off switch.
Such switches range from simple bi-metal switches, through thermistors, to semiconductor temperature sensors, such as the LM35.
Regardless of the method of temperature sensing, make sure that once the thermal limit is reached, the amplifier turns off and remains off until turned on by the user.
A little hysteresis, requiring the amplifier to cool down by at least 10 ºC before being allowed to be turned back on, would be a nice touch.

Real World Design Example

A frequently asked question is, “how much power do I need?”
Well. It depends, but probably not as much as you think. For a more detailed answer, a little math is needed.
I will work through the math using my home setup as an example. I encourage the reader to go through the math using the design variables for their setup.
It’s an eye-opening experience. My test speakers are KRK R6 passive studio monitors with a sensitivity of 87 dB (1 W, 1 m).
This is a fairly typical sensitivity for a bookshelf speaker. The listening position is 180 cm (6 feet) away from the speakers.
When I really crank it and play, what I consider to be, loud music, the sound pressure level at the listening position is about 85~90 dB(C),
measured using the SPL Meter App from Studio Six Digital. This leads to the resulting design parameters:



Speaker reference SPL (sensitivity): SPLref = 87 dB
Speaker reference power: Pref = 1 W
Speaker reference distance: Dref = 1 m
Distance to the listening position: Dlisten = 1.8 m
SPL at the listening position: SPLlisten = 90 dB
Number of speakers: N = 2

Addition of powers, including SPLs, can be a little tricky.
This is because the SPL from each speaker should treated as independent random variables.
If the two speakers produce exactly the same signal (i.e. are driven in a two-channel mono configuration), in phase, and are equidistant from the listening position in an anechoic chamber, the math is simple. In this case, for N number of speakers, the correction factor is: Pcorr = 20 * log(N).
If the two speakers produce signals that are completely uncorrelated, the math is also simple: Pcorr = 10 * log(N).
For typical listening environments and typical program material, the actual correction factor falls somewhere between these two extremes.
For a worst case estimate, I suggest using Pcorr = 10 * log(N).
This will slightly overestimate the amount of power required to produce the desired SPL at the listening position.

Pcorr = 10 * log(N) → Pcorr = 10 * log(2) → Pcorr = 3 dB.
Hence, each speaker will need to produce,
SPLspeaker = SPLlisten – Pcorr → SPLspeaker = 90 – 3 → SPLspeaker = 87 dB SPL at the listening position.

The SPL decays by the square of the distance, translating to a 6 dB decrease in SPL for every doubling of the distance between the speaker and the listening position.
To find the change in SPL at any distance, the following equation is used, Adist = 20 * log(Dlisten / Dref), where Adist is the attenuation due to the distance from the speaker.
From the values listed above:

Adist = 20 * log(Dlisten / Dref) → Adist = 20 * log(1.8/1.0) → Adist = 5.1 dB.
Now, the applied power needed is calculated as,
Pspeaker = Pref * 10(SPLspeaker + Adist – SPLref)/10 → Pspeaker = 1 * 10(87 + 5.1 – 87)/10 →Pspeaker = 3.24 W per speaker.

You can also use one of the many on-line SPL calculators to do the math. This Pro-Audio Calculator is quite good.
90 dB SPL is actually pretty loud. It’s loud enough to cause permanent hearing loss by prolonged exposure.
It’s about as loud as a jackhammer three meters away [Wikipedia, compensated for the distance according to Adist = 20 * log(Dlisten / Dref) above].
It certainly is loud enough to make my ears ring for a while. 3.24 W is enough to do that.
Three watt! This is the real reason LM3886-based amplifiers with tiny heat sinks work at all: they don’t ever output much power.
Also note that the SPL I use for critical listening is about 70 dB(C) at the listening position. 32.4 mW applied to each speaker produces this SPL. 70 dB(C) is loud enough to drown out the background noise and allow me to perceive the minute details of the music. For background music,
I turn the volume down another 10 dB, resulting in 3.24 mW delivered to the speakers.
Yes. Milliwatt!
From the 90 dB SPL requirement, the supply voltage for the LM3886 can be calculated. Note that the SPL meter measures the RMS sound pressure level.
To determine the peak power level, the crest factor of the music needs to be taken into account.
Assuming the same 14 dB crest factor as used above, the peak power is calculated as,

Ppeak = PRMS * 1014/10 → Ppeak = 3.24 * 1014/10 → Ppeak = 81.4 W.

The minimum supply voltage required to deliver this peak power can then be calculated as,

VCC = √(Ppeak * Rload) + Vod → VCC = √(81.4 * 4) + 3.5 = 21.5 V.

Rounding up to ±22 V rail voltage, the power dissipation in the LM3886 works out to 14.6 W when delivering 3.24 W RMS to a 4 Ω speaker (calculated from the math above).
14.6 W is considerably easier to manage, thermally, than the 32 W derived in the first section above.

90999

                        Power Supply Design                                                                        

The power supply design appears to be causing some confusion in the DIY community as well.
I figured I’d shed some light on the topic by providing the math needed for the power calculations.
As mentioned on the Thermal Design page, the power drawn from the power supply, including the quiescent current, for a given output swing can be calculated as,



where PS is the total supply power, Ibias is the quiescent or bias current, VOUTpeak is the peak output voltage, RL is the load impedance, and VCC is the supply voltage.
It is assumed that the amplifier operates from a symmetric power supply, i.e. VCC = -VEE. The maximum output swing is determined by the supply voltage and the output dropout voltage of the LM3886, which is found in the data sheet, as excerpted below.



The LM3886 clips asymmetrically with the negative swing being clipped before the positive.
Thus, the peak undistorted swing possible for the LM3886 is 2.5 V less than the supply voltage. Similarly, the quiescent current is found in the data sheet.
I will use the typical number rather than the worst case for this example.



Example: Supply voltage: ±25 V; Load resistance: 4 Ω. The power drawn from the power supply at the full undistorted output power can be calculated as:



The supply power for a range of common supply voltages and load impedances is tabulated below.

VCC	VOUTpeak	RL	PS
±25 V	22.5 V	4 Ω	92.0 W
±25 V	22.5 V	8 Ω	47.3 W
±28 V	25.5 V	4 Ω	116 W
±28 V	25.5 V	8 Ω	59.6 W
±35 V	32.5 V	8 Ω	94.0 W

PS is the total power drawn by the amplifier from the power supply. From this power, the VA rating of the power transformer needs to be determined.
Had the amplifier presented a purely resistive load, this would have been a simple task, however, the load presented by a full-wave rectifier is by no means a “nice” load.
Rather, the current through the rectifier is a pulse train. It is possible to find an analytical solution for this, but the math gets rather involved. For those interested in the math, I suggest consulting Blencowe, who suggests using a conversion factor of 1.5 to convert from resistive power to the VA rating of the transformer. I.e. for the ±25 V, 4 Ω example above, a transformer with a VA rating of 1.5 × 92.0 W = 138 VA should be specified.
To verify this rule of thumb, I simulated the class AB load current using LTspice. The sim sheet is shown below. The power transformer model is an Antek AS-2222 toroidal transformer.



The resulting VA rating of the power transformer can be found as the sum of the reactive power (V-A products) of the two secondary windings.
This is plotted below.



The extreme power at the beginning of the simulation is caused by the current needed to charge the reservoir capacitors to the full supply voltage.
After about 100 ms, the supply voltage is within 90 % of its final value and it has fully settled by 250 ms.
This extreme power is no cause for alarm. It is, however, a good argument for using an in-rush limiter or soft-start circuit, in particular in supplies using high efficiency transformer types, such as toroids.
The VA product is a somewhat distorted, half-wave rectified, sine wave with a peak value of 400 VA.
The average value works out to 141 VA – pretty darn close to the 138 VA obtained by Blencowe’s rule of thumb.
Note that the reactive power does depend on the size of the reservoir capacitor.
The bigger the capacitor, the larger the conversion factor between resistive power (W) and reactive power (VA).
Blencowe’s rule of thumb appears to hold up well for reasonable values of reservoir capacitors of, say, 4700 µF – 22000 µF.

Conclusion: An LM3886 running on a ±25 V supply, delivering the largest possible undistorted sine wave into a 4 Ω load will need a 140 VA transformer. For a stereo amplifier a 280 VA transformer should be used. I would round up to the nearest available standard size, which, typically, is 300 VA.

The Crest Factor, Revisited

Anyone who’s ever taken apart a commercially available amplifier will comment that none of the 65 W rated amplifiers they have looked at have contained transformers capable of supplying 300 VA.
What’s the deal…? It’s the crest factor again (see the thermal design section for a more thorough treatment of the subject).
Assuming the amplifier is to be used for music reproduction rather than the reproduction of sine waves, the power transformer can be undersized quite a bit.
Extremely compressed music, such as some heavy metal, has a crest factor of 5~6 dB.
Classical music, lands at the other end of the spectrum with a crest factor of about 20 dB.
This means the peak power of classical music is 100× higher than the RMS power. In an analysis of 4500 tracks performed by Sound on Sound Magazine, an average crest factor of 14 dB was found.
The supply power and resulting power transformer VA ratings (per LM3886 channel) are tabulated below for a range of common crest factors.

Crest Factor (dB)	PL RMS	PL peak	VCC	RL	PS	Power Transformer VA Rating
3 (sine wave)	63.3 W	127 W	±25 V	4 Ω	92.1 W	138 VA
6	31.8 W	127 W	±25 V	4 Ω	66.0 W	98.9 VA
10	12.7 W	127 W	±25 V	4 Ω	42.5 W	63.8 VA
14	5.04 W	127 W	±25 V	4 Ω	27.8 W	41.6 VA
20	1.27 W	127 W	±25 V	4 Ω	15.2 W	22.7 VA

Readers wanting to tweak the numbers to suit their own application will probably find my Class AB Output Stage Calculator (Excel sheet) useful.
As seen in the table, a 100 VA transformer can actually be specified for a stereo LM3886 amplifier, assuming the crest factor remains around 12~14 dB.
A transformer providing 20~22 V RMS, such as the Antek AS-1220 or AN-1222 would be suitable choices.

90999

基于本文我的实战心得，适用于任何DIY功放：

1. 正确的电路和良好的LAYOUT可以得到最好的结果。
2. 散热至关重要，不要认为把片子拧上散热片或者机箱就好了，除非你的机箱或散热片很大。
3. 电源电压越高，失真越低是真的，但是过高的电压容易带来过多的功耗，而且对声音的提升却不如换电容来得好。
4. 功率储备除了要看你的听音环境需要的功率外，还要看滤波电容音效，有些电容的音效会让你误判电源系统。
5. 长时间在高分贝音量下进兴音乐熏陶会导致耳朵受伤！！！！

rayman_ppx

学习一下。

rifjft

就3886而言，加个运放前级，比升级其它配件的效果更好。即使是几块钱的运放

lyz1900

多图杀猫啊。。。一直没刷出来

fsclub

城会玩。。。

yk28981

见到JP把LM3886做激光刻印机振镜驱动