A simple J310 amlifier.
When I added R4, even the value is 0R, ?the output voltage on R3 is 50mvpp.
When I removed R4, the output voltage on R3 is only 5mvpp, same as the input voltage.
It is strange.
Could anyone tell me why?
Thanks!
|
Re: opamp with offset pins
At this moment, I can't remember seeing a SPICE model for a 741-like op-amp that included those offset voltage pins, but they may exist.? They must be rather uncommon.
But there is a way to do it.? In your LTspice installation, there is an LTspice schematic for a full 741.? Find it on your computer's drive at examples\Educational\LM741.asc.? Near the lower left, the top ends of R1 and R3 come out to the IC pins for adjusting the offset voltage.? Note that the schematic shows the 741 wired-up in a complete circuit; don't forget to remove R11, R12, R14, and the voltage sources to get just the 741.
I would consider that OK as a teaching tool, but might not be good for serious work.? I don't know how accurate the schematic is, compared to a real LM741.? The schematic was literally lifted from the datasheet.? "For informational/educational purposes only."
LTspice doesn't come with a generic symbol for an op-amp with input offset pins, so you would need to make your own, if you want to use a symbol.
Andy
|
Greetings everyone, I need a 741 model or it could be another op amp that has offset correction pins, the need for these pins is because I'm making some circuits for teaching purposes, such as the full wave rectifier precision, these circuits are didactic and reinforcement in nature.
grateful
--
Carlos Delfino Quem sou:?
Keybase (PGP): ORCID:?
Celular: ? ? ?(85)?985-205-490 (OI) - Aquiraz/CE ¡°Para o Triunfo do Mal, s¨® ¨¦ preciso que os homens de bem n?o fa?am nada¡± - Edmund Burke ¡°Ningu¨¦m comete erro maior do que n?o fazer nada porque s¨® pode fazer um pouco¡± - Edmund Burke
Conhe?a o Curso Maker (Arduino Minas): ? Arvore dos Saberes/Tecnologia no Social: ?
|
Re: Al Dutcher's forgotten message
Most 'real' circuits have enough other stuff going on, so that the timestep stays more limited.? A smaller timestep leads to less difference between the unfiltered and filtered node voltages from the Modified Trap's filter.
Sometimes it is the "simple" circuits (the ones that don't actually do anything) that lead to visible artifacts.
Andy
|
Re: Al Dutcher's forgotten message
I tried this with my original ckt and alls well. Btw that ckt is a mosfet motor run relay replacement. Thanx again.
On Wed, May 29, 2024 at 1:20?PM Al Dutcher < alziedood@...> wrote: I tried Gear and Trap and alls well. Mod Trap is a mess.
Didnt need to mess with max time step at all. Wow, Nice, Thanx again! Learn something new every day.
OK, back to my original skizzy.
Hmm, I tried something different, and now I see badly distorted waveforms.? They are nothing like sinewaves, but maybe this is what you were talking about.
One of LTspice's interesting "features" is the "Modified Trap" algorithm.? It does a very good job of removing Trap Ringing when it happens.? But there was a change in about 2019, and since then it is not applied uniformly to all waveforms.? (Grrr!)? A consequence is that SOME differential plots do not look right, when plotting small differential signals in the presence of larger signals.? Yes, it is very much like the common-mode problem.
In this circuit, I think the Modified Trap filter gets applied only to V(N002) but not to V(N001) or V(N003) because they are driven directly by voltage sources.? So,
- If you use Modified Trap, and plot either V(N002,N001) or V(N002,N003), it looks bad.
- If you plot V(N003,N001), it looks good.
- If you plot any signal by itself, it looks normal.
- If you change from Modified Trap to either Trapezoidal or Gear and re-run the simulation, everything looks good.
LTspice's Help page for LTspice? > Integration Methods talks about this.
I almost forgot about this because I stopped using Modified Trap a while ago.? Trap Ringing happens infrequently so I rarely need Modified Trap, and I think I can spot Trap Ringing when it happens and then re-enable Modified Trap.? YMMV.
Andy
--
AC2CL
I do not think there is any thrill that
can go through the human heart like that felt by the inventor as
he sees some creation of the brain unfolding to success...
Such emotions make a man forget food, sleep, friends, love, everything.
- Nikola Tesla
-- AC2CL
I do not think there is any thrill that
can go through the human heart like that felt by the inventor as
he sees some creation of the brain unfolding to success...
Such emotions make a man forget food, sleep, friends, love, everything.
- Nikola Tesla
|
Re: Al Dutcher's forgotten message
I tried Gear and Trap and alls well. Mod Trap is a mess.
Didnt need to mess with max time step at all. Wow, Nice, Thanx again! Learn something new every day.
OK, back to my original skizzy.
Hmm, I tried something different, and now I see badly distorted waveforms.? They are nothing like sinewaves, but maybe this is what you were talking about.
One of LTspice's interesting "features" is the "Modified Trap" algorithm.? It does a very good job of removing Trap Ringing when it happens.? But there was a change in about 2019, and since then it is not applied uniformly to all waveforms.? (Grrr!)? A consequence is that SOME differential plots do not look right, when plotting small differential signals in the presence of larger signals.? Yes, it is very much like the common-mode problem.
In this circuit, I think the Modified Trap filter gets applied only to V(N002) but not to V(N001) or V(N003) because they are driven directly by voltage sources.? So,
- If you use Modified Trap, and plot either V(N002,N001) or V(N002,N003), it looks bad.
- If you plot V(N003,N001), it looks good.
- If you plot any signal by itself, it looks normal.
- If you change from Modified Trap to either Trapezoidal or Gear and re-run the simulation, everything looks good.
LTspice's Help page for LTspice? > Integration Methods talks about this.
I almost forgot about this because I stopped using Modified Trap a while ago.? Trap Ringing happens infrequently so I rarely need Modified Trap, and I think I can spot Trap Ringing when it happens and then re-enable Modified Trap.? YMMV.
Andy
-- AC2CL
I do not think there is any thrill that
can go through the human heart like that felt by the inventor as
he sees some creation of the brain unfolding to success...
Such emotions make a man forget food, sleep, friends, love, everything.
- Nikola Tesla
|
Re: Al Dutcher's forgotten message
Thanx so much Andy and peeps
I will give these a try. Makes a lot of sense. So many places to get trapped. Pun intended.
Al,
By the way, this error is considerably reduced by using a smaller timestep.? There was almost nothing in the simple circuit to force the timestep smaller.? Setting a Maximum Timestep of 10? us essentially eliminates it.
Andy
-- AC2CL
I do not think there is any thrill that
can go through the human heart like that felt by the inventor as
he sees some creation of the brain unfolding to success...
Such emotions make a man forget food, sleep, friends, love, everything.
- Nikola Tesla
|
Re: Al Dutcher's forgotten message
Al,
By the way, this error is considerably reduced by using a smaller timestep.? There was almost nothing in the simple circuit to force the timestep smaller.? Setting a Maximum Timestep of 10? us essentially eliminates it.
Andy
|
Re: Al Dutcher's forgotten message
Hmm, I tried something different, and now I see badly distorted waveforms.? They are nothing like sinewaves, but maybe this is what you were talking about. One of LTspice's interesting "features" is the "Modified Trap" algorithm.? It does a very good job of removing Trap Ringing when it happens.? But there was a change in about 2019, and since then it is not applied uniformly to all waveforms.? (Grrr!)? A consequence is that SOME differential plots do not look right, when plotting small differential signals in the presence of larger signals.? Yes, it is very much like the common-mode problem. In this circuit, I think the Modified Trap filter gets applied only to V(N002) but not to V(N001) or V(N003) because they are driven directly by voltage sources.? So,
- If you use Modified Trap, and plot either V(N002,N001) or V(N002,N003), it looks bad.
- If you plot V(N003,N001), it looks good.
- If you plot any signal by itself, it looks normal.
- If you change from Modified Trap to either Trapezoidal or Gear and re-run the simulation, everything looks good.
LTspice's Help page for LTspice? > Integration Methods talks about this. I almost forgot about this because I stopped using Modified Trap a while ago.? Trap Ringing happens infrequently so I rarely need Modified Trap, and I think I can spot Trap Ringing when it happens and then re-enable Modified Trap.? YMMV. Andy
|
Re: Al Dutcher's forgotten message
Al wrote, "The only place with the square wave is the pulse source."
So if you plot the differential voltage across "the res and BE junction", that is exactly the pulse voltage source.? There is no difference.? They are connected by wires.
re: "The res and jctn have this strange distorted 4V sine wave."
That makes it sound a little like waveform compression.? But your simulation has it turned off.? Anyway, 3 V out of 170 V is not enough to cause much if any visible inaccuracy.? (Small waveforms riding on top of larger signals can suffer from waveform compression, but there has to be a greater difference in their amplitudes.)
Andy
|
Re: Al Dutcher's forgotten message
Hmph! I wonder whats different? You have exactly the same ckt. The only place with the square wave is the pulse source. The res and jctn have this strange distorted 4V sine wave. Its like its having trouble cancelling the common mode voltage Very strange
Al wrote, "If you look differentially across Either the res Or the Vbe jctn alone youll see the 4V"
I do not see 4 V.
Across R1, I see 2.645 V or 0 V (alternating).
Across the Vbe junction, I see 0.655 V or 0 V.
I think you did something wrong, but I can't tell what.
Do you see square waves?
Andy
-- AC2CL
I do not think there is any thrill that
can go through the human heart like that felt by the inventor as
he sees some creation of the brain unfolding to success...
Such emotions make a man forget food, sleep, friends, love, everything.
- Nikola Tesla
|
Re: Al Dutcher's forgotten message
Al wrote, "If you look differentially across Either the res Or the Vbe jctn alone youll see the 4V"
I do not see 4 V.
Across R1, I see 2.645 V or 0 V (alternating).
Across the Vbe junction, I see 0.655 V or 0 V.
I think you did something wrong, but I can't tell what.
Do you see square waves?
Andy
|
Re: Al Dutcher's forgotten message
Didnt see a place to send a message. Uploading generates an announcement. I thought the text included with the upload was the message
I used LTspice 24.
If you look differentially across Either the res Or the Vbe jctn alone youll see the 4V The jctn cant do that in fwd bias! This is a snippet from another project that does use the 120Vrms
I didnt want to confuse the situation with extra stuff
Group member Al Dutcher uploaded a file (PecoCMp.asc) but then he forgot to send any message about it.
Al, please re-read the instructions on the group's main webpage, especially the part that tells you to always send a Message about what you uploaded.
The Description attached to your file is:
Heres a strange one thats making no sense
Its a snippet from something that I m working on
120Vrms with a small ckt on the top
If you use the diff prob,
youll get ~4V across the res and BE junction
from 3V source
especially in fwd bias, huh?!
The current is ok
What am i doing wrong?
Its in Temp
What program did you use to simulate it?? I used LTspice, and the simulated differential voltage V(N003,N001) = the voltage across R1 + the Vbe junction, alternates between 0 and 3.3 V.
I saw no ~4 V.
The source is a square wave with 3.3 V amplitude (not "3V" but close).
So my question is, what were you looking at?? Did you upload the wrong circuit?
There are many problems with your circuit.? The 120 Vrms source does nothing, so I don't know why you mentioned it.
Andy
-- AC2CL
I do not think there is any thrill that
can go through the human heart like that felt by the inventor as
he sees some creation of the brain unfolding to success...
Such emotions make a man forget food, sleep, friends, love, everything.
- Nikola Tesla
|
Re: Oscillator stops oscillating
Tony wrote, "By default, this has a tanh transfer function, ..."
That is true, but only partly so.? The tanh curvature applies only when the op-amp's output would be operating between the supply voltages.? With a more typical Avol and supply voltages, then the transfer curve clips first before the tanh has much effect.? I think you are right that the tanh curve is to mimic the input diff. amp.
Whether it is curved or straight linear, I think the "problem" in this case (Ethan's oscillator) is that the transfer function is idealized and the component does not seem to give feedback to the timestep control algorithm.
Andy
|
Re: Oscillator stops oscillating
On 28/05/2024 22:21, Andy I wrote:
One thing to keep
in mind is that your op-amps and comparators in the simulation are
the ideal "UniversalOpAmp2", which is very linear (until it clips)
and very idealized.? The fact that its core is linear means it
sends few if any "clues" to the timestep control algorithm, to
tell it when to slow down (make the Timestep smaller).? As a
result, it can miss the timing of the falling edge at U2's
output.? By the time it checks in and sees that U2's output is
low, the result is a simulated fall-time of about 250 us instead
of 20 us.? It's not a huge difference, but that makes the dv/dt
too slow to pass through the AC-coupling.
It is not actually true that UniversalOpamps are idealised linear.
At the heart of the UniversalOpamp is the LTspice OTA device. By
default, this has a tanh transfer function, which is similar to that
obtained from a long-tailed pair differential amplifier. The OTA can
be made linear by the inclusion of the "linear" flag in the instance
definition, but isn't in the UniversalOpamp series - see /g/LTspice/files/Temp/UniversalOpamp_TF.zip.
--
Regards,
Tony
|
Re: Oscillator stops oscillating
Folks, no need for anyone to spend more time on this. I came up with a better, much simpler way to do what I want, and it works. There is one small issue which I might raise here, but for now I'm all set. Thanks VERY MUCH for the expert help from all of you.
|
Re: step recovery diode in LTspice
On 28/05/2024 21:00, Andy I wrote:
It is ironic that
the figure calls it a "linear NLTL" which I assume means "linear
non-linear transmission line".? (I assume that use of the two
"linears" refer to different things, one to nonlinear diodes, the
other to uniformity along its length?)
"NLTL" or non-linear transmission line refers to an integrated
technique whereby transmission lines are loaded by an array of shunt
varactor diodes distributed along the length of a transmission line.
This contrivance makes the velocity factor of the transmission line
dependent upon the voltage on the line to ground, viz.:
??????????????? 1
VF = ?????
???? c0.¡Ì(³¢.°ä)
..wherein the symbols have their usual meaning, i.e.:? c0=velocity of light
in vacuo, L & C=inductance and capacitance per unit length.
As the capacitance decreases, so the VF increases. Therefore,
assuming the varactors are connected cathodes to line, anodes to
ground, a rising edge can be made sharper. This is a cunning
technique for making picosecond pulses (from already pretty fast
transitions). Note, that this really only works when the varactors
are effectively spaced at <¦Ë/16, if you can get your head around
that. (Of course, the falling edges are also made slower - think
about it... no free lunch!)
--
Regards,
Tony
|
Re: step recovery diode in LTspice
I wrote that choke design depends on frequency.
abid wrote, "Could you please explain the frequency dependency for a frequency value of 10 MHz?"
No, that is something you need to work on.? As I said already, questions about how to make an inductor are off-topic for the LTspice group.? You should read and study that.
For the inductors, if the signal source in V1 is 10 MHz, you have frequencies at 10 MHz, 20 MHz, 30 MHz, ..., 510 MHz, 520 MHz ...? extending up depending on the diodes.? It is not just a 10 MHz problem.
re: "Also for the C1 choice."
Reactance Xc = 1/(2*pi*frequency*C)
Knowing the frequency and Xc, you can calculate C.
It looks like the current through C1 is sinusoidal, so harmonics are not involved.? I don't know if C1 and L1 should resonate.? If they are, then use:
frequency = 1/(2*pi*SQRT(L*C)).
Andy
|
Re: Oscillator stops oscillating
Thanks for all that wisdom Andy. I really appreciate it. I made C2 smaller because it was limiting how quickly I could dump the main C1 cap. The longer I keep C1 low, the longer it extends each cycle a fixed amount making the control voltage to output frequency non-linear.
I realized that at 2n2 the C1 dump time was longer than needed, so I shortened it as low as I could go. Without C2 the circuit doesn't work at all. I can try a different type of timer that doesn't stay low if it's input stays low. I also was worried that the circuit might not work as hardware. There's no easy way to set an .ic in hardware. In the mean time I came up with an alternate version that works on a different principle. It charges C1 up then down rather than up with a fast discharge. But that one too halts early in some cases!
|
Al Dutcher's forgotten message
Group member Al Dutcher uploaded a file (PecoCMp.asc) but then he forgot to send any message about it. Al, please re-read the instructions on the group's main webpage, especially the part that tells you to always send a Message about what you uploaded. The Description attached to your file is:
Heres a strange one thats making no sense
Its a snippet from something that I m working on
120Vrms with a small ckt on the top
If you use the diff prob,
youll get ~4V across the res and BE junction
from 3V source
especially in fwd bias, huh?!
The current is ok
What am i doing wrong?
Its in Temp
What program did you use to simulate it?? I used LTspice, and the simulated differential voltage V(N003,N001) = the voltage across R1 + the Vbe junction, alternates between 0 and 3.3 V. I saw no ~4 V. The source is a square wave with 3.3 V amplitude (not "3V" but close). So my question is, what were you looking at?? Did you upload the wrong circuit? There are many problems with your circuit.? The 120 Vrms source does nothing, so I don't know why you mentioned it. Andy
|
Tony Casey
Ethan Winer