Re: Simulation runs very slowly: test.asc
I was considering the 15 V unbalance, not the
absolute values. But it was just a guess. A generic model would
probably not show that, or not work at all.
On 2025-03-31 13:31, Andy I via
groups.io wrote:
On Mon, Mar 31, 2025 at 05:13 AM, John Woodgate wrote:
It might not be so good
with +20V and -5V rails. I doubt that is tested.
I noticed that the generic SPICE macromodel for the ADA4084
states that it was tested only with 30V (+/-15V) supplies.
?
The built-in LTspice model does not say.? But I would hope
that it works ALMOST the same with 25 V as it does with 30 V
rails.? The part's datasheet has extensive data for 3, 10, and
30 V rails.
?
?
--
OOO - Own Opinions only
If something is true:
* as far as we know - it's science
*for certain - it's mathematics
*unquestionably - it's religion
|
On Sat, Mar 29, 2025 at 09:38 PM, Jim Wagner wrote:
I think I have the circuit you need. It is circa-1965 and uses 3-4 bipolar transistors, a zener diode, and a handful of resistors. ...
Jim,
?
Your schematic in the photo you uploaded shows two NPN transistors, but the description that accompanies it mentions "2N3904/6" which implies that one of them is a PNP.? I have not tried (nor studied the circuit in detail), but I wondered if Q2 is supposed to operate in reverse breakdown mode so it is an NPN, or if it was supposed to be a PNP. ?
Did you draw that schematic, or was it originally drawn with two NPNs, and is one of them wrong?
?
Andy
?
|
Re: creating PNP caracteristicsby sweeping plot in LTspice from a circuit I built
Sorry, I also should have said this:? Ground the Emitter and connect the negative collector voltage source to the transistor's collector.
?
Obviously, the graph you uploaded needs to be inverted (or plotted with negative voltages going right and negative currents going up) when using a PNP.
?
Andy
?
|
Re: creating PNP caracteristicsby sweeping plot in LTspice from a circuit I built
On Mon, Mar 31, 2025 at 07:27 AM, john23 wrote:
Is a there a way by clever type of sweep to recreate the basic characteristics plot of the attached PNP plot?
Sweep the collector voltage.
?
Sweep the base current over a number of steps.
?
Do not do this as a .TRAN simulation.
?
In your circuit, remove R1, R2, and R3.? Replace V1 with a current source.
?
Use one .DC command that specifies two sources.? If I remember correctly, the "1st Source" should be the collector voltage, and the "2nd Source" should be the base current.? Sweep the collector voltage with fine increments (0.1 V or smaller), and sweep the base current over a smaller number of steps (0.2 uA increments).
?
Andy
?
|
Re: Simulation runs very slowly: test.asc
Andy, ? Thanks again for all your help and suggestions. And yes, test.asc is just that – a schematic for testing the circuit in another schematic. The schematic I didn’t post was the one I was commenting on. ? Sorry, busy day.
toggle quoted message
Show quoted text
From: [email protected] <[email protected]> On Behalf Of Andy I via groups.io
Sent: Monday, March 31, 2025 12:43 AM
To: [email protected]
Subject: Re: [LTspice] Simulation runs very slowly: test.asc? Analog Devices has another SPICE model for the ADA4084, downloadable from the part's webpage.? The model that comes with LTspice has elements that require LTspice.? The downloadable model is generic SPICE.? They were likely created by different people at ADI. I tried it in your circuit. It seems to "work" with either Solver, with or without a 10K pulldown resistor at the output.? However, it is rather slow using the Normal Solver.? It's not nearly as slow as your circuit was.? It makes slow but steady progress.? Also there are glitches, so something (an oscillation?) seems to be going on. With the Alternate Solver, it takes a few seconds to find the initial operating point, but then it simulates the rest in the blink of an eye, and I see no glitches in the waveform. These are interesting results, but puzzling.
|
Re: Simulation runs very slowly: test.asc
On Mon, Mar 31, 2025 at 05:13 AM, John Woodgate wrote:
It might not be so good with +20V and -5V rails. I doubt that is tested.
I noticed that the generic SPICE macromodel for the ADA4084 states that it was tested only with 30V (+/-15V) supplies.
?
The built-in LTspice model does not say.? But I would hope that it works ALMOST the same with 25 V as it does with 30 V rails.? The part's datasheet has extensive data for 3, 10, and 30 V rails.
?
?
|
On Mon, Mar 31, 2025 at 03:26 AM, jacfev wrote:
I tried to simulate a negative resistance using btdeboi's netlist, but I can't complete the schematic.
Can you help me complete it ?
See Negative Conductance.asc
Compared to the netlist in btdeboi's?message, there is one omission in your schematic.? Change the formula of the B-source B1, from this:
I = V(Vi,Vo)/R
to this:
I = V(Vi,Vo)/V(Vr)
That's all I can tell you because it is missing a SPICE simulation command (.OP or .DC or .AC or .TRAN?) and I don't know where/why it works.? I guess you need to work that out.
?
If you sweep the voltage source V1 (.DC V1 ...), the current through B1 and Rmeas linearly decreases as V(Vi) increases.
?
Andy
?
?
|
creating PNP caracteristicsby sweeping plot in LTspice from a circuit I built
Hello , in the attacehd zipped file I have created a basic PNP biasing circuit . The simultion is in time domain , I added plots of different ports.
Is a there a way by clever type of sweep to recreate the basic characteristics plot of the attached PNP plot?
Current vs Vce plot.
Thanks.
/g/LTspice/files/Temp/03_01_25.zip
|
Re: Simulation runs very slowly: test.asc
It might not be so good with +20V and -5V
rails. I doubt that is tested.
On 2025-03-31 01:57, Christopher Paul
via groups.io wrote:
Would you
suggest contacting Analog Devices about this? The datasheet says
unity gain operation is acceptable.
--
OOO - Own Opinions only
If something is true:
* as far as we know - it's science
*for certain - it's mathematics
*unquestionably - it's religion
|
Re: Simulation runs very slowly: test.asc
Yes, I know that was Mike's argument, and of
course he is notoriously unbiddable. So I suggest it could be an
option in the symbol creating page, 'Do not add full path to the
model file'. Or the opposite.
On 2025-03-30 23:56, Andy I via
groups.io wrote:
On Sun, Mar 30, 2025 at 06:46 PM, John Woodgate wrote:
Yes, it can be fixed, but
wouldn't it be better if it didn't happen? Should we ask
for it to be changed to only show the model filename?
It is actually this way quite intentionally.? I had a discussion
with Mike Engelhardt about it several years ago.
?
Auto-generating symbols makes it as easy as possible for
anyone to make a symbol without trying.? As such, it needs to
encode where the model file lives, on the assumption that it
might not already be located in a place where LTspice looks to
find model files.? Thus, it saves the whole filespec to the
model file, in the symbol.
?
Shortening that to just the filename SHOULD (in my opinion)
be done, manually, by any LTspice user who wants to have a hand
in the simulation process.? But it would break it for other
LTspice users who don't care or don't want to understand
anything about "what's under the hood".? It would be bad (in my
opinion) to change LTspice in a way that makes the Automatic
Symbol Generation step fail for many users, especially the
newbies.
?
?
--
OOO - Own Opinions only
If something is true:
* as far as we know - it's science
*for certain - it's mathematics
*unquestionably - it's religion
|
Re: PTC model with internal temperature rise
On Sat, Mar 29, 2025 at 03:37 PM, Andy I wrote:
It is currently in the Temp folder at the group's website.
Hello Andy,
it's ok now, I move it to the good folder.
|
Re: Simulation runs very slowly: test.asc
This is what happens if you don't start a new thread: Email
threads. Changing the subject doesn't affect how they are
listed in a threaded display. It just confuses things.
People use threads in (news)groups in order to see which message is
a direct reply to another, and which messages are not. Threads may
contain hundreds of messages, all laid out logically.
--
Regards,
Tony
On 30/03/2025 23:45, Christopher Paul
via groups.io wrote:
toggle quoted message
Show quoted text
I’m
sorry.
?
I
count one email with a definitely wrong subject: RE: [LTspice]
Model of BF970
?
The
others have different subject files which I have emailed, but
they are each my own:
test.asc
test.asc
and ADA4084-2.zip
test_2.zip.
?
I
see now that I should have kept one email title for all of
these, which were the results of problems that Andy requested
I fix.
?
I
use gmail. So:
?
???????????????
In the future, I should continue to post my schematic files in
the temp folder. All emails related to my topic should have a
unique one and only subject. Correct?
?
In
spite of my mistakes, is there something that I can do now to
request help?
?
Apologies,
|
I tried to simulate a negative resistance using btdeboi's netlist, but I can't complete the schematic.
Can you help me complete it ?
See Negative Conductance.asc
|
Re: Simulation runs very slowly: test.asc
Chris,
?
Analog Devices has another SPICE model for the ADA4084, downloadable from the part's webpage.? The model that comes with LTspice has elements that require LTspice.? The downloadable model is generic SPICE.? They were likely created by different people at ADI.
?
I tried it in your circuit.
?
It seems to "work" with either Solver, with or without a 10K pulldown resistor at the output.? However, it is rather slow using the Normal Solver.? It's not nearly as slow as your circuit was.? It makes slow but steady progress.? Also there are glitches, so something (an oscillation?) seems to be going on.
?
With the Alternate Solver, it takes a few seconds to find the initial operating point, but then it simulates the rest in the blink of an eye, and I see no glitches in the waveform.
?
These are interesting results, but puzzling.
?
Andy
?
?
|
Re: Simulation runs very slowly: test.asc
Chris,
?
Here is another thing that seems to help:? Add a pull-up or pull-down resistor between the output of the op-amp and its V+ or V- supply.? I used a 10K resistor and that seemed to do a nice job with LTspice's Normal Solver.? In fact, using the 10K pulldown to V- also makes LTspice find the initial operating point much faster.? (Source Stepping succeeds, but failed without it.)
?
I was noticing the fact that the ADA4084's output pin seems to be the junction of two collectors, so its open-loop Zout might be rather large, and I wondered what were the consequences of that when driving nothing more than a MOSFET gate.? So I added a resistor there to maybe dampen and lower the impedance, and for whatever reason, it seems to quench whatever goes wrong in the simulation.? No guarantees.
?
I don't know if this translates to the need for something similar in actual hardware.
?
The datasheet mentions that the ADA4084 open-loop voltage gain depends on the load connected to the output.
?
Andy
?
|
Re: Simulation runs very slowly: test.asc
On Sun, Mar 30, 2025 at 08:35 PM, Christopher Paul wrote:
... Only one of the _IN, V_Supply and _OUT supplies is active at a time. When active, they test the circuits’ transfer, supply noise suppression, and output impedances over frequency at DC currents of 10, 100 and 1000mA.
What are the _IN and _OUT supplies?? I'm guessing they are on schematics you have but did not upload?
?
?
|
Re: Simulation runs very slowly: test.asc
Chris,
?
These kinds of internal "oscillations" are more mathematical, not real.? Has nothing to do with being unity-gain stable.? I just want to suggest the possibility of some sort of numerical instability, perhaps in the sub-femtosecond range.
?
It's hard to say if their model alone is at fault.? Might be interaction between devices.
?
Andy
|
Re: Simulation runs very slowly: test.asc
Hi Andy, ? ??????????????? Thank you for all your help. ? I had wondered if oscillations were the cause the problem, and were associated with the ADA4084-2 model since replacing it with opamp.sub made things run normally. ? ??????????????? Would you suggest contacting Analog Devices about this? The datasheet says unity gain operation is acceptable. ? Thanks and Regards, ? Chris ?
toggle quoted message
Show quoted text
From: [email protected] <[email protected]> On Behalf Of Andy I via groups.io
Sent: Sunday, March 30, 2025 8:14 PM
To: [email protected]
Subject: Re: [LTspice] Simulation runs very slowly: test.asc? I changed the Subject line of this topic from "test.asc" to "Simulation runs very slowly: test.asc", because "test.asc" by itself was meaningless. It won't affect most of you, and it does not change the problem that it hijacked another topic.? Sorry to you Thunderbird email users, but we are stuck with that.
|
Simulation runs very slowly: test.asc
Hi Andy and John, ? ??????????????? To answer John’s question: ? ??????????????? Both the LM317 circuit and the ?“M1” circuits are voltage-controlled current sources whose loads are the 0V DC voltage sources whose names terminate in _OUT. The LM317 is a standard linear voltage regulator ? The point is to compare the operations of the two circuits. Only one of the _IN, V_Supply and _OUT supplies is active at a time. When active, they test the circuits’ transfer, supply noise suppression, and output impedances over frequency at DC currents of 10, 100 and 1000mA. ? ??????????????? Thanks for the 6 diodes trick, but the schematic is also meant to describe the circuits to non-spice users, as you surmised. ? - Chris. I don't understand you circuits. What are they supposed to do? Where is the output? I can see it might be the top ends of the diode stacks, but that doesn't work for the circuit that doesn't have a diode stack.
I am not sure but I figured the LM317 might be some sort of current limiter or regulator?? I'm guessing the "output" of those sections is the current through the diodes and current-sensing voltage source at the bottom of each stack. The one section without the diode stack doesn't have the LM317 either.? I think it just tests that the current sink (MOSFET + op-amp) below the LM317 does the right thing.? That part of the circuit appears in each of the other three sections. I can't run your sims because your LM317 symbol has the full path to its model which is on your computer only.
That is "easily" fixed and by now I have gotten accustomed to doing that after group members upload their schematics.? It is an unfortunate consequence of letting LTspice auto-generate symbols.? I can't blame the LTspice user for having that.? (Although I think it is quite unnecessary to auto-generate symbols.) Not that it matters, but SPICE gives you a short-cut for having multiple diodes in series.? It is the N=<value> instance parameter.? By adding "n=6" to a diode element, it turns it into effectively six individual diodes in series.? With LTspice, you can do that using either of these: - Right-click on the text "1N4007" and change it to "1N4007 N=6"; or
- Ctrl-right-click on the diode symbol and add "N=6" (without quotes) in the Value2 line, and optionally add an X in the Vis. column.
Doing so does not actually change anything (to any significant degree), but it makes the schematic more compact, as well as the circuit matrix.? You might or might not want to "simplify" your schematic this way because seeing six diodes in series conveys meaning.
|
Re: Simulation runs very slowly: test.asc
I changed the Subject line of this topic from "test.asc" to "Simulation runs very slowly: test.asc", because "test.asc" by itself was meaningless.
?
It won't affect most of you, and it does not change the problem that it hijacked another topic.? Sorry to you Thunderbird email users, but we are stuck with that.
?
Andy
?
|
John Woodgate
Tony Casey
jacfev