Anyone actually build one?
Regarding the Slone amp: SPICE analysis and theorizing are fascinating, but I'm curious -- has anyone actually tried to build one? What were the manifestations of instability in real life? What performance problems were observed: oscillations, thermal, distortion etc?
Regarding the Slone amp: SPICE analysis and theorizing are fascinating, but I'm curious -- has anyone actually tried to build one? What were the manifestations of instability in real life? What performance problems were observed: oscillations, thermal, distortion etc?
Hil,
I've also been working on an amp using a similar topology to the one described by Andy_C - I've also read Douglas Self's book and noted the omission of the balanced VAS. The single ended VAS approach looks great but I have not been able to get around the non-symetrical slew rate, or overcome the fact that it is limited to around 40VuS without doing some ******** to improve it.
I've done loads of simulations (LT Spice) over the last month or so on the balanced topology. I had quite some trouble getting the amp stable (phase margin better than 40deg, gain slope at 0db cross over point <8db etc). I am quite pleased with the results.
I'll post my results in a few weeks time - got some other things to attend to in the next few weeks.
bye
(by the way I also discovered that the MJE340 and 350 are bad, bad news - low Ft, base strage problems etc - avoid them!)
I've also been working on an amp using a similar topology to the one described by Andy_C - I've also read Douglas Self's book and noted the omission of the balanced VAS. The single ended VAS approach looks great but I have not been able to get around the non-symetrical slew rate, or overcome the fact that it is limited to around 40VuS without doing some ******** to improve it.
I've done loads of simulations (LT Spice) over the last month or so on the balanced topology. I had quite some trouble getting the amp stable (phase margin better than 40deg, gain slope at 0db cross over point <8db etc). I am quite pleased with the results.
I'll post my results in a few weeks time - got some other things to attend to in the next few weeks.
bye
(by the way I also discovered that the MJE340 and 350 are bad, bad news - low Ft, base strage problems etc - avoid them!)
ACR said:
What did you end up using in their place? I originally started with ZTX857 and ZTX957 for my VAS until I realized I had a thermal problem with running them from +/-90V supplies at the current I needed. When I switched to the MJE340 and MJE350, the simulated distortion dropped by quite a bit.
"I've done loads of simulations (LT Spice) over the last month or so on the balanced topology. I had quite some trouble getting the amp stable (phase margin better than 40deg, gain slope at 0db cross over point <8db etc). I am quite pleased with the results."
I'm a little suspicious of LT-Spice or maybe just Spice in general.
A- I'm run a model of an amp I've built and which has been operating on a daily basis for some time. The sim says it has no phase margin, yet in real-life it is just fine.
B-I have modeled a couple identical circuits with LT-Spice and with Simetrix (free version). LT-spice shows badly increasing THD below 1k which is not a common real-life experience while Simetrix shows it flat which is more like reality.
Maybe if I can stop being such a cheapskate and buy a standard version of BrownBag, I'll be happier. Meanwhile, my activities for the next few months are to take 2 or three amps I've been modelling anf build them to see if there is any relationship to the Spice results.
-------------------------------
"MJE340 and MJE350": I use these for modeling because I can't find models I trust for 2sd669/2sb649. Some were posted here but they seemed to produce results too good to be true. So far I've found that if I can get an acceptable result in a SIM with the MJE340/350's, I can build it with 2sd669/2sb649 and get equivalent or better results.
---------------------------------------
"limited to around 40VuS ": One always prefers more to less, but since you cite Self, did you notice the discussion on slew rate where he cites N.Pass among others suggesting that 40V/uS is more than adequate?
I'm a little suspicious of LT-Spice or maybe just Spice in general.
A- I'm run a model of an amp I've built and which has been operating on a daily basis for some time. The sim says it has no phase margin, yet in real-life it is just fine.
B-I have modeled a couple identical circuits with LT-Spice and with Simetrix (free version). LT-spice shows badly increasing THD below 1k which is not a common real-life experience while Simetrix shows it flat which is more like reality.
Maybe if I can stop being such a cheapskate and buy a standard version of BrownBag, I'll be happier. Meanwhile, my activities for the next few months are to take 2 or three amps I've been modelling anf build them to see if there is any relationship to the Spice results.
-------------------------------
"MJE340 and MJE350": I use these for modeling because I can't find models I trust for 2sd669/2sb649. Some were posted here but they seemed to produce results too good to be true. So far I've found that if I can get an acceptable result in a SIM with the MJE340/350's, I can build it with 2sd669/2sb649 and get equivalent or better results.
---------------------------------------
"limited to around 40VuS ": One always prefers more to less, but since you cite Self, did you notice the discussion on slew rate where he cites N.Pass among others suggesting that 40V/uS is more than adequate?
MJE340/350 low ft: not seeing this problem
Well, ACR's post got me to wondering what's going on. So I came up with a simple circuit to simulate ft for the MJE340 and MJE350. The test circuit for the MJE340 is shown below. I'm running them at 5.2 mA, with about 80V across them. I got the models from OnSemiconductor. I've pasted the models below. I first put a current source of 5.2 mA in the emitter, then did a DC operating point sim to find Vbe. Then I replaced the current source with a voltage source of the Vbe value just obtained. This is to provide the required AC ground to the emitter for determining hfe correctly. I'll show the plot of hfe vs frequency next...
.MODEL Qmje340 npn( IS=1.03431e-13 BF=172.974 NF=0.939811 VAF=27.3487 IKF=0.0260146 ISE=4.48447e-11 NE=1.61605 BR=16.6725 NR=0.796984 VAR=6.11596 IKR=0.10004 ISC=9.99914e-14 NC=1.99995 RB=1.47761 IRB=0.2 RBM=1.47761 RE=0.0001 RC=1.42228 XTB=2.70726 XTI=1 EG=1.206 CJE=1e-11 VJE=0.75 MJE=0.33 TF=1e-09 XTF=1 VTF=10 ITF=0.01 CJC=1e-11 VJC=0.75 MJC=0.33 XCJC=0.9 FC=0.5 CJS=0 VJS=0.75 MJS=0.5 TR=1e-07 PTF=0 KF=0 AF=1 Vceo=300 Icrating=500m mfg=OnSemiconductor)
.MODEL Qmje350 pnp( IS=6.01619e-15 BF=157.387 NF=0.910131 VAF=23.273 IKF=0.0564808 ISE=4.48479e-12 NE=1.58557 BR=0.1 NR=1.03823 VAR=4.14543 IKR=0.0999978 ISC=1.00199e-13 NC=1.98851 RB=0.1 IRB=0.202965 RBM=0.1 RE=0.0710678 RC=0.355339 XTB=1.03638 XTI=3.8424 EG=1.206 CJE=1e-11 VJE=0.75 MJE=0.33 TF=1e-09 XTF=1 VTF=10 ITF=0.01 CJC=1e-11 VJC=0.75 MJC=0.33 XCJC=0.9 FC=0.5 CJS=0 VJS=0.75 MJS=0.5 TR=1e-07 PTF=0 KF=0 AF=1 Vceo=300 Icrating=500m mfg=OnSemiconductor)
Well, ACR's post got me to wondering what's going on. So I came up with a simple circuit to simulate ft for the MJE340 and MJE350. The test circuit for the MJE340 is shown below. I'm running them at 5.2 mA, with about 80V across them. I got the models from OnSemiconductor. I've pasted the models below. I first put a current source of 5.2 mA in the emitter, then did a DC operating point sim to find Vbe. Then I replaced the current source with a voltage source of the Vbe value just obtained. This is to provide the required AC ground to the emitter for determining hfe correctly. I'll show the plot of hfe vs frequency next...
.MODEL Qmje340 npn( IS=1.03431e-13 BF=172.974 NF=0.939811 VAF=27.3487 IKF=0.0260146 ISE=4.48447e-11 NE=1.61605 BR=16.6725 NR=0.796984 VAR=6.11596 IKR=0.10004 ISC=9.99914e-14 NC=1.99995 RB=1.47761 IRB=0.2 RBM=1.47761 RE=0.0001 RC=1.42228 XTB=2.70726 XTI=1 EG=1.206 CJE=1e-11 VJE=0.75 MJE=0.33 TF=1e-09 XTF=1 VTF=10 ITF=0.01 CJC=1e-11 VJC=0.75 MJC=0.33 XCJC=0.9 FC=0.5 CJS=0 VJS=0.75 MJS=0.5 TR=1e-07 PTF=0 KF=0 AF=1 Vceo=300 Icrating=500m mfg=OnSemiconductor)
.MODEL Qmje350 pnp( IS=6.01619e-15 BF=157.387 NF=0.910131 VAF=23.273 IKF=0.0564808 ISE=4.48479e-12 NE=1.58557 BR=0.1 NR=1.03823 VAR=4.14543 IKR=0.0999978 ISC=1.00199e-13 NC=1.98851 RB=0.1 IRB=0.202965 RBM=0.1 RE=0.0710678 RC=0.355339 XTB=1.03638 XTI=3.8424 EG=1.206 CJE=1e-11 VJE=0.75 MJE=0.33 TF=1e-09 XTF=1 VTF=10 ITF=0.01 CJC=1e-11 VJC=0.75 MJC=0.33 XCJC=0.9 FC=0.5 CJS=0 VJS=0.75 MJS=0.5 TR=1e-07 PTF=0 KF=0 AF=1 Vceo=300 Icrating=500m mfg=OnSemiconductor)
Attachments
Okay, here's the plot. ft is defined as the frequency for which the magnitude of hfe extrapolates to unity, assuming a 20 dB/decade slope at the extrapolation point. You can see that the slope is 20 dB/decade all the way out to the 0 dB point, so we can read it straight off the graph. The value of ft is 152 MHz. If anything, this seems optimistic to me. But it's hard to say, since the data sheets seem scientifically designed to say as little about the devices as possible 
. At any rate, I wouldn't call this a problem at all. Perhaps there's some other problem, or ACR used a different model than I did? BTW, I got very similar results with the MJE350.
. At any rate, I wouldn't call this a problem at all. Perhaps there's some other problem, or ACR used a different model than I did? BTW, I got very similar results with the MJE350.Attachments
sam9 said:
Regarding the pessimistic results you're getting, you wouldn't happen to be using the On Semiconductor MJL3281A and MJL1302A models would you? If so, I've found these models to be way out in left field - completely wrong. I'm not sure if the devices were oscillating when they measured them, of if they just don't know how to extract the parameters correctly, or what. If you are using these devices, I can post models for the Toshiba 2SC3281 and 2SA1302 that match up much better with the data sheet and expected theoretical performance. Also, the brand new MJL4281a and MJL4302a have models which are totally wrong. 0.4 Volts VBE for 45 mA Ic? I don't think so!
With SPICE in general, the problem is usually the models, not the simulator. The simulator is really just a big nonlinear equation solving system. I've compared CircuitMaker, PSPICE and LTSPICE using identical models and gotten nearly identical results (within hundredths of a dB), even including FFT stuff. But to get the same results with the FFT, I had to force the time steps to be the same between the different simulators. The CircuitMaker residual distortion is extremely low. They must do some additional processing behind the scenes to get this kind of performance. I'm calling "nearly identical results" with the FFT the values of the signal and harmonics, not the residual noise in between. The only thing I don't like with LTSPICE is that the FFT stuff is extremely fiddly to set up. I wish they'd improve that.
Unfortunately, there's tons of totally wrong models floating around. One of the first things I did with CircuitMaker was to do some DC biasing with a current source that used a 1N4148. I got some really strange results. I put a current source of 1 mA into the diode and found that it gave me a voltage drop of 0.8 Volts. Wrong! Put in the 1N4148 model from LTSPICE and everything was fine.
Bricolo said:
The best way to get started with SPICE is to download the freeware LTSPICE (also called "SwitcherCAD") from Linear Technology and try out the audioamp.asc example they provide. But briefly, use DC operating point to get the quiescent currents and voltages. AC analysis for frequency response and stability plots (loop gain, see the audioamp.asc example). Use transient analysis for things like square wave response and, for regulators, output voltage response to a step of load current. Also use transient analysis with sine waves combined with the FFT to compute distortion.
See these URLs:
http://www.linear.com/about/site.html
http://www.beigebag.com/resources.htm
Re the MJE340 and 350 - I originally used them as the cascode pair and as VAS buffers in a circuit topology very similar to Anthony Holtons topology. I never got good results and could not get rid of HF ringing, especially on the negative halves of the output waveform. If I drove the amp into light clipping, the ringing was really bad. I put it down at the time to output parasitics - just could not tame them. I abandoned that approach and went for a fully balanced complimentary design (not built yet - still simulating and exploring). I used the MJE340 and 350's again in the cascode amp and as the first transisors in the output triple circuit (a la Self). When I simumlate the amp going into light clipping (a useful test to check for good behavior) I got the same ringing and could not get the amp stable. Suspecting the MJE's, I checked them out in a switichng circuit (2 V square wave input to base via 1k resistor, 10K load resistor, 70V rail). The devices are slow and have very significant base storage issues. I then tried a BF470/BF469 pair - little or no storage problems and they switch damn fast. I replaced these in the amp similation - problem gone. What is actually happening here with the MJE's can be seen on a gain/phase plot - the gain is well behaved through the 0db cross over point, but then actually starts increasing again in the 1-2 MHz range by about 8db. I surmise that when you drive the amp into soft clipping, or you put a real world load onto the output, it's easy to get the amp to misbehave - once you are clipping for example, all sorts of quite high level harmonics are being generated and this triggers the ringing. Again, this situation does'nt seem to exist with the BF469/470's.
I've still got quite a bit of work to do on the amp, but hopefully can start a proto board in about 6 weeks or so.
I'd like to hear from anone who has had similar experieces with the MJE's.
I've still got quite a bit of work to do on the amp, but hopefully can start a proto board in about 6 weeks or so.
I'd like to hear from anone who has had similar experieces with the MJE's.
andy_c said:
thanks for the advice
I already know how to do distortion analysis, transiant and things like this.
What I don't know how to do is the ac stability. I'm especially inexperienced with power supplies, and not amps.
I don't know how to test a PS i designed. Have I to load it with a resistance, a ccs, an ac curent source? Feed it with a perfect voltage source, add a small ac signal to the voltage source...
Andy_c,
"Regarding the pessimistic results you're getting, you wouldn't happen to be using the On Semiconductor MJL3281A and MJL1302A models would you? "
Actually I've been using the Fairchild models for the 2sa1943 ans 2sc5200 (note: they replace the "2" with "K" indicating manufacture in Korea) since these are the devices I've actually been using since reports of counterfeit 2sa1301 & 2sc3281's have been circulating.
I also have the MJL models (not used actually used) but can't recall where I got them from (dumb of me). The comment header in the file says "Symmetry Design Systems" who ever they are - subcontractors to ON-Semi?
---------------------------------
BTW: LT-Spice incorporates the .FOUR directive which purports to produce a THD figure out to the 9th harmonic. At the same time, the wave form viewer has a menu item to produce an FFT graphical display. Sometimes these seem consistent for the same transient analysis and sometimes I've seen a rather high THD figure (.1% for example) with a very quiet FFT graphic. I suppose I could just read the harmonic peaks of the FFT plot and stick them in a spreadsheet that does the calcs to get THD but that is a tedious process. I'm aware of the need to get the timestep and start/stop points right and followed directions from threads on the LT-Spice forum. Nonetheless, the qualitative direction of results ("beter" or "worse") when comparing alternatives appears ro be correct in all cases.
In any case my approach has been to first look at stability via the .ac analysis and once I think I've got a good margin there, look at THD, behavior at/near clipping, symetry if it's a non-mirrored VAS, etc.
"Regarding the pessimistic results you're getting, you wouldn't happen to be using the On Semiconductor MJL3281A and MJL1302A models would you? "
Actually I've been using the Fairchild models for the 2sa1943 ans 2sc5200 (note: they replace the "2" with "K" indicating manufacture in Korea) since these are the devices I've actually been using since reports of counterfeit 2sa1301 & 2sc3281's have been circulating.
I also have the MJL models (not used actually used) but can't recall where I got them from (dumb of me). The comment header in the file says "Symmetry Design Systems" who ever they are - subcontractors to ON-Semi?
---------------------------------
BTW: LT-Spice incorporates the .FOUR directive which purports to produce a THD figure out to the 9th harmonic. At the same time, the wave form viewer has a menu item to produce an FFT graphical display. Sometimes these seem consistent for the same transient analysis and sometimes I've seen a rather high THD figure (.1% for example) with a very quiet FFT graphic. I suppose I could just read the harmonic peaks of the FFT plot and stick them in a spreadsheet that does the calcs to get THD but that is a tedious process. I'm aware of the need to get the timestep and start/stop points right and followed directions from threads on the LT-Spice forum. Nonetheless, the qualitative direction of results ("beter" or "worse") when comparing alternatives appears ro be correct in all cases.
In any case my approach has been to first look at stability via the .ac analysis and once I think I've got a good margin there, look at THD, behavior at/near clipping, symetry if it's a non-mirrored VAS, etc.
Bricolo said:
You can do AC stability analysis using the Middlebrook technique. There's two versions of this technique: the exact and approximate. For info about the exact technique, see:
http://www.spectrum-soft.com/news/spring97/loopgain.shtm
http://www.analog-innovations.com/LoopGain.zip
I especially like Jim Thompson's mathematical derivation of the loop gain at the second link above. I've also attached an LTSpice example of using both the approximate and exact Middlebrook techniques. I'm not sure what simulator you're using though.
Some people don't use the AC technique for stability at all - they just do a transient simulation with a square wave or similar and look for ringing on the output. I've done simulations of amps with excellent phase margin but poor gain margin (capacitive loading but with a phase compensation capacitor to help stability) show lots of ringing on transient. I try to completely eliminate any ringing.
I've never done a complete simulation of a power supply including transformer, bridge rectifier, etc. - mainly because I don't have any real-world transformer data. Regarding regulators, see http://www.diyaudio.com/forums/showthread.php?postid=231553#post231553 for some discussion of simulation issues. I'm not sure there are any hard and fast answers as to what to use as a load. I tried to simulate a worst case scenario with transients of load current in the referenced link.
"a transient simulation with a square wave or similar and look for ringing on the output."
I hadn't considered that as an alternative to ac analysis so I tried it just know on one of my sims. No ringing, whew. But a question arose: if I set rise time to zero, the square trace is noticably not vertical but otherwise quite "clean". If I set a posative but small value, say 1-to-100pS the trace looks vertical but there is a significant overshoot. I don't know how either one would compare to the results on a real scope. Any comments regarding what rise time makes sense (or is most useful / meaningful) in a sim? For that matter is the overshoot, but no ringing of any significance?
I hadn't considered that as an alternative to ac analysis so I tried it just know on one of my sims. No ringing, whew. But a question arose: if I set rise time to zero, the square trace is noticably not vertical but otherwise quite "clean". If I set a posative but small value, say 1-to-100pS the trace looks vertical but there is a significant overshoot. I don't know how either one would compare to the results on a real scope. Any comments regarding what rise time makes sense (or is most useful / meaningful) in a sim? For that matter is the overshoot, but no ringing of any significance?
sam9 said:
Hmm, I just set up a pulse test with just a generator and 2 resistors. I set the rise and fall times to 1 nsec. I didn't see any overshoot or ringing on the pulse from the generator. If I understand you correctly, you were seeing this on the source itself? Or was it the amp output? With amps, I've seen what initially looked like a tiny overshoot on the output. With many repeated zoom-ins in the overshoot region, I realized that there was a very high-frequency ringing as well. The overshoot wasn't much - a few tenths of a volt or so. This baffled me for a while until I looked at the diff amp currents. They were spiking to max current right where the overshoot and ringing were occurring. I realized this was the result of the transition from linear operation to slewing. The feedback loop temporarily loses control of the situation, causing the overshoot and ringing. The fix was to place an RC low pass filter at the input of the amp. My design has a closed loop bandwidth of only a little more than 100 kHz without the filter, and I didn't want to lessen it with a filter. But a 1 MHz filter was enough to get rid of it. This filter is usually part of the real amp design as well.
As to how this relates to a scope measurement, I guess you could say it's like having a scope with a nearly infinite bandwidth. If you set your pulse rise time too small, your smallest time step in the sim could get very small and it would take a long time to run. If you set it to zero, it takes on a default non-zero value which may be larger than you want. (This is standard SPICE behavior BTW). I just use 1 ns as a rule of thumb. It hasn't caused me any problem so far.
...can you post the Toshiba 2sc/2sa 3281/1302 models you've refered to...please?
Hi Mike,
Here's the models:
.MODEL Q2SC3281 NPN( IS=10.000E-15 BF=155.65 VAF=100 IKF=9.2028 XTB=1.5 ISE=54.325E-15 NE=1.3056 BR=10.787 VAR=100 IKR=1.8561 ISC=106.69E-15 NC=1.6728 NK=.55624 RC=26.745E-3 CJE=2.0000E-12 CJC=534.41E-12 MJC=.33333 TF=8.0821E-9 XTF=3.1968 VTF=21.461E-3 ITF=169.59 TR=187.91E-9)
.MODEL Q2SA1302 PNP( IS=21.479E-12 BF=136.48 VAF=100 IKF=19.980 ISE=21.504E-12 NE=1.3784 BR=329.48 VAR=100 IKR=19.980 ISC=4.3670E-9 NC=1.4264 NK=.72845 RC=93.301E-3 CJE=755.31E-12 MJE=.33333 CJC=1.1417E-9 MJC=.33333 TF=1.2802E-9 XTF=10 VTF=10 ITF=1 TR=10.000E-9)
Here's the models:
.MODEL Q2SC3281 NPN( IS=10.000E-15 BF=155.65 VAF=100 IKF=9.2028 XTB=1.5 ISE=54.325E-15 NE=1.3056 BR=10.787 VAR=100 IKR=1.8561 ISC=106.69E-15 NC=1.6728 NK=.55624 RC=26.745E-3 CJE=2.0000E-12 CJC=534.41E-12 MJC=.33333 TF=8.0821E-9 XTF=3.1968 VTF=21.461E-3 ITF=169.59 TR=187.91E-9)
.MODEL Q2SA1302 PNP( IS=21.479E-12 BF=136.48 VAF=100 IKF=19.980 ISE=21.504E-12 NE=1.3784 BR=329.48 VAR=100 IKR=19.980 ISC=4.3670E-9 NC=1.4264 NK=.72845 RC=93.301E-3 CJE=755.31E-12 MJE=.33333 CJC=1.1417E-9 MJC=.33333 TF=1.2802E-9 XTF=10 VTF=10 ITF=1 TR=10.000E-9)
A- I'll try using the 1ns rise time. Apart from being somewhat new to SPICE, I'm budget constrained hardware wise so I don't always have a way to check simulated results against actual. At least not in fine detail. Nonetheless, using SPICE has avoided sending a couple of poor ideas up in smoke and flames!
B- Thanks for the Toshiba models. just a quick look tells me that they are different from the MJL's. Begs the question - perhaps both are accurate and the Toshiba and MJL versions are actually different in "real" life.
B- Thanks for the Toshiba models. just a quick look tells me that they are different from the MJL's. Begs the question - perhaps both are accurate and the Toshiba and MJL versions are actually different in "real" life.
sam9 said:
Actually...i have just discovered that the mjl1302 model has been recently updated by on-semi.....
**************************************
* Model Generated by MODPEX *
*Copyright(c) Symmetry Design Systems*
* All Rights Reserved *
* UNPUBLISHED LICENSED SOFTWARE *
* Contains Proprietary Information *
* Which is The Property of *
* SYMMETRY OR ITS LICENSORS *
*Commercial Use or Resale Restricted *
* by Symmetry License Agreement *
**************************************
* Model generated on Jul 20, 03
* MODEL FORMAT: PSpice
.MODEL Qmjl1302a pnp
+IS=3.25053e-12 BF=60.3363 NF=0.992063 VAF=19.8199
+IKF=7.18352 ISE=3.25712e-12 NE=3.42487 BR=5.15499
+NR=1.03617 VAR=2.77936 IKR=9.38159 ISC=2.5e-13
+NC=3.89405 RB=0.776136 IRB=0.0998107 RBM=0.776136
+RE=0.000613663 RC=0.0424163 XTB=1.43773 XTI=1
+EG=1.05 CJE=1.57135e-08 VJE=0.728073 MJE=0.42161
+TF=2.63264e-09 XTF=1000 VTF=4.11586 ITF=266.249
+CJC=1.79861e-09 VJC=0.814822 MJC=0.473271 XCJC=1
+FC=0.8 CJS=0 VJS=0.75 MJS=0.5
+TR=1e-07 PTF=0 KF=0 AF=1
Yes sam9....the two families of devices are rather different...for a start, the mjl's are rated at 200W, while the Toshiba's are 150W...etc..
- Status
- This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.