Hello,
I am a Electronics student, its my first year so i am not that good. I have been experimenting with pSpice trying to design a simple amplifier.
I have made one that seems to work in pSpice but its not that good, linearity is not perfect and efficeny is about 40%.
I dont even know if it works at all.
Anyway here is the schematics, any comments would be nice!
I am a Electronics student, its my first year so i am not that good. I have been experimenting with pSpice trying to design a simple amplifier.
I have made one that seems to work in pSpice but its not that good, linearity is not perfect and efficeny is about 40%.
I dont even know if it works at all.
Anyway here is the schematics, any comments would be nice!
An externally hosted image should be here but it was not working when we last tested it.
Hi Arte
For a start lose R17 completely and lift R16 off pin 1 (output pin) of the IC and instead connect it to the output point of the amp (junction of the MOSFETs).
Your MOSFETs are now in the chip/amp feedback loop which should cut the THD considerably. Of course this is a very simple basic amplifier but instructional. You may get almost 5W from it.
For a start lose R17 completely and lift R16 off pin 1 (output pin) of the IC and instead connect it to the output point of the amp (junction of the MOSFETs).
Your MOSFETs are now in the chip/amp feedback loop which should cut the THD considerably. Of course this is a very simple basic amplifier but instructional. You may get almost 5W from it.
Arte,
power is = Output Voltage (rms) squared/ load impedance
This is very compromised due to limited drive current from the 25K resistors and the Vgs losses of the MOSFETS limiting available swing. You could bootstrap or use current sources and add two drive transistors with inverted MOSFETS to reduce output stage losses. Or just raise the supplies.
power is = Output Voltage (rms) squared/ load impedance
This is very compromised due to limited drive current from the 25K resistors and the Vgs losses of the MOSFETS limiting available swing. You could bootstrap or use current sources and add two drive transistors with inverted MOSFETS to reduce output stage losses. Or just raise the supplies.
Hi arte didnt i tell you it is nice looking basic amp, you mentioned that the
diode drops vary, i didnt put them there buddy you did and you knew that
didnt you, i have invented a super-constant bias technique that varies only
within the range of +-40uV you cant use that with your basic amp can you?
diode drops vary, i didnt put them there buddy you did and you knew that
didnt you, i have invented a super-constant bias technique that varies only
within the range of +-40uV you cant use that with your basic amp can you?
And as far as I know, there is no commonly available OP-amp that works off +-35V power supply.
Do not rely just on the simulator - they most often do not have any limit values to their models (unless the models support failure analysis, which is rare), so when you select a component, you need to read it's data sheet, at least as far as normal operating conditions for the part.
The voltage across the diodes varies with current, as well as temperature. The threshold voltage for the MOSFETs also varies with temperature. All of these parameters vary from one to the other example of real life diodes and MOSFETs even if they are of the same type. Because of this you commonly need a means of adjusting the bias voltage (that which you use your diodes for).
Also, although the MOSFETs need very little current into their gates (practicly zero) under static conditions, it is not so under dynamic conditions because gates have a capacitance, which is not very small either, and is not linear. The simplest way to fix this on your amp is to put a capacitor in parallel with each of the diode strings.
Do not rely just on the simulator - they most often do not have any limit values to their models (unless the models support failure analysis, which is rare), so when you select a component, you need to read it's data sheet, at least as far as normal operating conditions for the part.
The voltage across the diodes varies with current, as well as temperature. The threshold voltage for the MOSFETs also varies with temperature. All of these parameters vary from one to the other example of real life diodes and MOSFETs even if they are of the same type. Because of this you commonly need a means of adjusting the bias voltage (that which you use your diodes for).
Also, although the MOSFETs need very little current into their gates (practicly zero) under static conditions, it is not so under dynamic conditions because gates have a capacitance, which is not very small either, and is not linear. The simplest way to fix this on your amp is to put a capacitor in parallel with each of the diode strings.
> Your sim software should have an idealised current source so replace the 25Ks with these and note any difference!
This (like EVERYthing in SPICE) can be misleading.
We can build real-world "current sources" with a couple parts, even just one JFET. These are really current LIMITERS.
The standard IDC current source in SPICE is a real current SOURCE. Its terminal voltage will rise to ANY level to keep the specified current flowing. In this plan, in the linear range, the IDC sources will kick-up 4 or 5 volts beyond the supply rails. A JFET or BJT-mirror can't do that (not without bootstrapping or extra supply rails).
And when driven non-linear, in some cicuits, SPICE will happily swing the IDC terminal up to 10^23 volts and blow-up on a math-overflow error. You may have to study the OUT file closely to see that this is the problem.
Use the IDC, but remember that it is not a REAL part.
> Is it bad to use an IC instead of tranistors,the circuit gets SO much simpler?
> I am a Electronics student
If it was too easy, your school could not charge you $90,000 for 4-6 years for an EE degree. An idiot like me can look at National's LM-Overture chip-book and steal a working amp design. The idea of you getting an EE degree is so you CAN design things that nobody makes a chip for, so you can do the glory work that fools like me can't do, and get the Engineer paycheck instead of a technician's few thin bucks.
Of course if there IS a chip that meets the assigned specs, at bulk-price, USE IT. If you have a party this weekend, slap-up an LM-3999 chip-amp just like the app-note shows, and party-on. But if your employer needs 127 Watts of 346KHz power at 11 ohms and 87% efficiency, for under a buck, you are going to be fooling around with naked transistors. Messing with discrete audio amps is good practice for some fundamental problems.
> How do can i calculate the Power of the amplifier?
Run a TRAN analysis. Pick a likely voltage for the Vstim source, one that will almost but not quite overload the amp. The PROBE display will tell you if the waveform is badly bent. A FOUR analysis will give a (flawed) estimate of THD. If THD is less than 1%, raise the Vstim input level so it will clip; if over 5%-10% you have too much clipping. When you have "a little" distortion, look at the 1st harmonic voltage: this is the peak output voltage. Times 0.707 to get conventional RMS, then square and divide like any voltage-power problem.
If this case: IF the parts were perfect, the output voltage could swing +35V to -35V. On a Sine wave, that's 24.7V RMS. With 6 ohm load, that is 102 Watts.
Being super-generous: the op-amp, diodes, and 25K resistors might eventually swing to +34V/-34V, the FETs might drop 4V Gate-Source, giving +/-30V output, 76 Watts.
In real life, everything has more losses than you think it will. The "35V" may sag to 25V, the opamp/diode/25K thing might not push the Gates near the supply rails, and even fat MOSFETs have some drop unless you smack them very hard (OK for switchers, not for linear amps). And without feedback around the imperfect buffer, THD may get very bad long before it totally clips.
Oh: with a "real" opamp (finite bandwidth, finite output impedance) driving the big Gate capacitance, you may have a supersonic oscillator instead of an amplifier. That's an advanced topic for an EE freshman. You might find a couple big BJTs easier to drive without distractions.
When you get it "working", have some fun. Put a 0.1 ohm "short" on the output, feed a big signal, and compare FET current and peak-power with datasheet MAXimum Spec numbers. Compare the clean world of SPICE with the rats-nest of wires behind a typical home hifi. Are shorts likely? How long can the amp survive a short? Something they don't tell you: BJTs often "burn-up" to a shorted condition (PN junction turns to jelly and conducts real well). What happens to your "35V batteries" when they have a dead-short, and are really low-bid transformers in a plastic case?
This (like EVERYthing in SPICE) can be misleading.
We can build real-world "current sources" with a couple parts, even just one JFET. These are really current LIMITERS.
The standard IDC current source in SPICE is a real current SOURCE. Its terminal voltage will rise to ANY level to keep the specified current flowing. In this plan, in the linear range, the IDC sources will kick-up 4 or 5 volts beyond the supply rails. A JFET or BJT-mirror can't do that (not without bootstrapping or extra supply rails).
And when driven non-linear, in some cicuits, SPICE will happily swing the IDC terminal up to 10^23 volts and blow-up on a math-overflow error. You may have to study the OUT file closely to see that this is the problem.
Use the IDC, but remember that it is not a REAL part.
> Is it bad to use an IC instead of tranistors,the circuit gets SO much simpler?
> I am a Electronics student
If it was too easy, your school could not charge you $90,000 for 4-6 years for an EE degree. An idiot like me can look at National's LM-Overture chip-book and steal a working amp design. The idea of you getting an EE degree is so you CAN design things that nobody makes a chip for, so you can do the glory work that fools like me can't do, and get the Engineer paycheck instead of a technician's few thin bucks.
Of course if there IS a chip that meets the assigned specs, at bulk-price, USE IT. If you have a party this weekend, slap-up an LM-3999 chip-amp just like the app-note shows, and party-on. But if your employer needs 127 Watts of 346KHz power at 11 ohms and 87% efficiency, for under a buck, you are going to be fooling around with naked transistors. Messing with discrete audio amps is good practice for some fundamental problems.
> How do can i calculate the Power of the amplifier?
Run a TRAN analysis. Pick a likely voltage for the Vstim source, one that will almost but not quite overload the amp. The PROBE display will tell you if the waveform is badly bent. A FOUR analysis will give a (flawed) estimate of THD. If THD is less than 1%, raise the Vstim input level so it will clip; if over 5%-10% you have too much clipping. When you have "a little" distortion, look at the 1st harmonic voltage: this is the peak output voltage. Times 0.707 to get conventional RMS, then square and divide like any voltage-power problem.
If this case: IF the parts were perfect, the output voltage could swing +35V to -35V. On a Sine wave, that's 24.7V RMS. With 6 ohm load, that is 102 Watts.
Being super-generous: the op-amp, diodes, and 25K resistors might eventually swing to +34V/-34V, the FETs might drop 4V Gate-Source, giving +/-30V output, 76 Watts.
In real life, everything has more losses than you think it will. The "35V" may sag to 25V, the opamp/diode/25K thing might not push the Gates near the supply rails, and even fat MOSFETs have some drop unless you smack them very hard (OK for switchers, not for linear amps). And without feedback around the imperfect buffer, THD may get very bad long before it totally clips.
Oh: with a "real" opamp (finite bandwidth, finite output impedance) driving the big Gate capacitance, you may have a supersonic oscillator instead of an amplifier. That's an advanced topic for an EE freshman. You might find a couple big BJTs easier to drive without distractions.
When you get it "working", have some fun. Put a 0.1 ohm "short" on the output, feed a big signal, and compare FET current and peak-power with datasheet MAXimum Spec numbers. Compare the clean world of SPICE with the rats-nest of wires behind a typical home hifi. Are shorts likely? How long can the amp survive a short? Something they don't tell you: BJTs often "burn-up" to a shorted condition (PN junction turns to jelly and conducts real well). What happens to your "35V batteries" when they have a dead-short, and are really low-bid transformers in a plastic case?
prr, thanks for yet another excellent post...
cheers.
http://www.diyaudio.com/forums/showthread.php?postid=409662#post409662
cheers.
http://www.diyaudio.com/forums/showthread.php?postid=409662#post409662
> Hell PRR, We're dealing with EE101 here not sim software limitations - just to put perspective back! We know this but you've likely lost arte a long way back.
They learn quick in EE101.
And they use SPICE a lot. Arte needs to know that SPICE is both a friend and an enemy.
I'll draw a picture on the chalkboard:
Plain 24V battery, several current sources and things for current to flow through.
Q1 shows the expected result. Hfe is about 140, so a 1Meg base resistor drops 7V, collector voltage is 7.6V.
Q2 is the same except the base is shorted to collector. Note: 272,000 Volts! In Arte's plan, with ideal current sources, the MOSFET Gates will kick-up beyond what can be done with any "real world" current source. SPICE will claim the MOSFETs can be bottomed; not going to happen. (OK, a bootstrap will kick-up.)
Beyond the fact that the ideal current source will, quite properly, source (not limit) current, we see that the transistor breakdown is not enforced in this model. This can be convenient, or misleading.
Here is one that really bit me. I "know" that 999 out of 1,000 2N4002 rectifiers will stand-off much more than the rated 100V. My SPICE model doesn't know that (correctly), and enforces a 100.1V breakdown. With resistance: breakdown voltage is higher at 10 Amps than at 1mA. However it does not care that we have 1,004 Watts in a 1-Watt part. (I have seen a simulator that will blink obviously overheated parts; cute.)
For simplicity: a 1K resistor gives the "expected" answer; a 100K resistor shows the voltage kick-up of an ideal current source.
Another bit of SPICE trivia: take almost any op-amp model. Connect all 5 pins to Gnd with 1000Meg resistors. Don't have a battery anywhere on the page. Run DC. With most models, there will be non-zero voltage everywhere: op-amps make power!!!? Some models will even amplify a signal, with no battery in sight. (The excuse is: full modeling of a complex IC would take too long. Boyle proposed a simple model that simulates quick and gives working answers for realistic operating conditions; but don't work outside the envelope or flaws creep out.)
Here's Arte's idea with ideal current sources:
For simplicity I've used a DC analysis so the results show on the schematic. (And I changed the stacks of diodes to Zeners; tempco may be wrong but we are not doing temperature runs yet.)
The analysis is "correct", in the fantasy world of SPICE and my models.
It does correctly show that a LM324 won't pull-up much closer than 1V from its positive rail, even when overdriven a bit. (It ignores the fact that the LM324 is living at almost twice its maximum voltage: rated 36V, here it eats 70V.)
It shows the top MOSFET pulling a 6 ohm load up to within 2V of the supply rail, good performance! 91 Watts of barely-clipped sine power.
And it shows M1's Gate sitting at almost 38V. But the highest battery-voltage is +35V. Those darn Idc current-sources really will SOURCE power.
In real life, we might use a diode-strapped JFET. When I do that, SPICE shows the Gate sitting at +35V, a possible answer, though probably not realistic.
> put perspective back!
SPICE has no perspective. If you don't learn that (yes, even in EE101), it will tell you things that are true only in SPICE's fantasy world. EE students need to learn to sanity-check SPICE before they waste a lot of time in Lab, wondering why the Gates don't pull-up to 38V as "SPICE proved".
They learn quick in EE101.
And they use SPICE a lot. Arte needs to know that SPICE is both a friend and an enemy.
I'll draw a picture on the chalkboard:
An externally hosted image should be here but it was not working when we last tested it.
Plain 24V battery, several current sources and things for current to flow through.
Q1 shows the expected result. Hfe is about 140, so a 1Meg base resistor drops 7V, collector voltage is 7.6V.
Q2 is the same except the base is shorted to collector. Note: 272,000 Volts! In Arte's plan, with ideal current sources, the MOSFET Gates will kick-up beyond what can be done with any "real world" current source. SPICE will claim the MOSFETs can be bottomed; not going to happen. (OK, a bootstrap will kick-up.)
Beyond the fact that the ideal current source will, quite properly, source (not limit) current, we see that the transistor breakdown is not enforced in this model. This can be convenient, or misleading.
Here is one that really bit me. I "know" that 999 out of 1,000 2N4002 rectifiers will stand-off much more than the rated 100V. My SPICE model doesn't know that (correctly), and enforces a 100.1V breakdown. With resistance: breakdown voltage is higher at 10 Amps than at 1mA. However it does not care that we have 1,004 Watts in a 1-Watt part. (I have seen a simulator that will blink obviously overheated parts; cute.)
For simplicity: a 1K resistor gives the "expected" answer; a 100K resistor shows the voltage kick-up of an ideal current source.
Another bit of SPICE trivia: take almost any op-amp model. Connect all 5 pins to Gnd with 1000Meg resistors. Don't have a battery anywhere on the page. Run DC. With most models, there will be non-zero voltage everywhere: op-amps make power!!!? Some models will even amplify a signal, with no battery in sight. (The excuse is: full modeling of a complex IC would take too long. Boyle proposed a simple model that simulates quick and gives working answers for realistic operating conditions; but don't work outside the envelope or flaws creep out.)
Here's Arte's idea with ideal current sources:
An externally hosted image should be here but it was not working when we last tested it.
For simplicity I've used a DC analysis so the results show on the schematic. (And I changed the stacks of diodes to Zeners; tempco may be wrong but we are not doing temperature runs yet.)
The analysis is "correct", in the fantasy world of SPICE and my models.
It does correctly show that a LM324 won't pull-up much closer than 1V from its positive rail, even when overdriven a bit. (It ignores the fact that the LM324 is living at almost twice its maximum voltage: rated 36V, here it eats 70V.)
It shows the top MOSFET pulling a 6 ohm load up to within 2V of the supply rail, good performance! 91 Watts of barely-clipped sine power.
And it shows M1's Gate sitting at almost 38V. But the highest battery-voltage is +35V. Those darn Idc current-sources really will SOURCE power.
In real life, we might use a diode-strapped JFET. When I do that, SPICE shows the Gate sitting at +35V, a possible answer, though probably not realistic.
> put perspective back!
SPICE has no perspective. If you don't learn that (yes, even in EE101), it will tell you things that are true only in SPICE's fantasy world. EE students need to learn to sanity-check SPICE before they waste a lot of time in Lab, wondering why the Gates don't pull-up to 38V as "SPICE proved".
amplifierguru said:
Hehe yeah, i have sent pSpice to very distant garbage can and picked up the sissor.
I have read all your posts alot, i and am very thank full for all the answers i have got. I have learned alot!
However, since my goal is to build my own amplifier i have been looking around for the nearest electronic suplier and what stuff they have. So i will remake the amplifier a bit different not using MOSFETS, instead using a TIP41/TIP42 pair. The voltage gain will be a OPAMP as before.
Since almost every OPAMP is limited to about 30-40V is it possible to use 2? One for 30 <-> 0V and one for 0 <-> -30V?
(btw, my amplifier doesnt have to sound good or anything, i prob wont use it - its for learning).
- Status
- This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.