|
Hello everyone,
Why is it that I can't view anything smaller then 94ps? I tried confining the simulation run time to the waveform I wish to view and decreased the time step thinking that would give me more data, but no it didn't work.
|
On 01/12/2024 03:33, Richard Andrews
via groups.io wrote:
Why is it that
I can't view anything smaller then 94ps? I tried confining the
simulation run time to the waveform I wish to view and decreased
the time step thinking that would give me more data, but no it
didn't work.
It's just a guess, given that you have disclosed nothing about your
schematic: did you disable waveform compression?
If you want more suggestions, you'll have to upload your schematic,
or at least tell us more about it, for example, what did you
decrease the maximum time step to? May be LTspice doesn't have any
finer data points because there isn't any information to be had.
What are you looking at that requires finer resolution than 94ps?
--
Regards,
Tony
|
On Sat, Nov 30, 2024 at 09:33 PM, Richard Andrews wrote:
Why is it that I can't view anything smaller then 94ps? I tried confining the simulation run time to the waveform I wish to view and decreased the time step thinking that would give me more data, but no it didn't work.
That's difficult to say without knowing more about your simulation and what you tried.
Changing the time-step can affect the data saved, but has no effect on changing the plot's limits. It's unclear why you suggested that. But do make sure that you have also disabled waveform compression, and use View > Mark Data Points so you can see where the simulated (and saved) datapoints actually are. It's 'pointless' to zoom in to limits smaller than the space between simulated AND SAVED time points. LTspice lets you, but by doing so you would be viewing interpolated data which is never as good as real data.
But getting to the matter of the waveform viewer's time-axis limits:
LTspice's waveform viewer does limit how much you can expand the time-axis so that it spans a smaller time interval.
It seems to limit the time span relative to the absolute time values. For example (but these are just numbers out of my head), if you try to make the plot show waveforms from 1.000000000000 to 1.000000000001 seconds (= 1 s + 1 ps), it will not do that. (There is probably a math resolution issue with that.) But if you plot from 0.000000000 to 0.000000000001 second (= 0 to 1 ps), it will, and it can go much much smaller than that. It can be smaller than 0.001 fs at least, and probably much smaller.
There is a "trick" you can use to overcome this when you want to see what's going on between, let's say, 1 s and 1 s + 1 ps. Right-click on the time axis and change the "Quantity plotted" from "time" to "time-1", which has the effect of shifting the entire time axis left by 1 second. (Use your own offset, not my 1 second example.) Now you can zoom in to much smaller limits, because you are zooming-in in the vicinity of 0 in the shifted time-domain.
When doing this, make sure to use View > Mark Data Points periodically to see if you are looking at real data or if it is interpolated.
Andy
|
I am only guessing here --
But LTspice might use single-precision floating point numbers and math in its waveform viewer's axes. If so, numbers and math would be resolution-limited to about 7 digits.
Andy
|
Thank you Andy, I will try your suggestions.
|
I've uploaded my file emp.zip, because I am a quitter and give trying to view the pulse width on this circuit. Maybe there is something that can be done.
|
Missing model for TIP41C.
|
On Mon, Dec 2, 2024 at 05:41 PM, Richard Andrews wrote:
I've uploaded my file emp.zip, because I am a quitter and give trying to view the pulse width on this circuit. Maybe there is something that can be done.
Can you explain exactly what you want to do with it?
Probe what signals? When? Is the question related to the plot's time-axis? When (in time) do you wish to make that observation? There is a huge difference between probing near time=0 and near time=18000000 us.
Earlier you wrote that you "can't view anything smaller then 94ps". Is that still true, and when (in the 18 second simulation) are you trying to or are unable to see things smaller than 94 ps? This helps us zero in on what you want to look for.
Andy
|
I suspect he’s trying to see an expanded waveform pulse of the power in L3, ‘round about 16.000534s
But maybe the timescale is so huge, relative to the pulse width, that it cannot be resolved in the plot.
I tried, even with waveform compression turned off, and it’s too narrow to expand.
переключити цитоване повідомлення
Показати цитований текст
From: LTspice@groups.io <LTspice@groups.io> On Behalf Of
Andy I via groups.io
Sent: Monday, December 02, 2024 4:17 PM
To: LTspice@groups.io
Subject: EXTERNAL: Re: [LTspice] X axis limits.
On Mon, Dec 2, 2024 at 05:41 PM, Richard Andrews wrote:
I've uploaded my file emp.zip, because I am a quitter and give trying to view the pulse width on this circuit. Maybe there is something that can be done.
Can you explain exactly what you want to do with it?
Probe what signals? When? Is the question related to the plot's time-axis? When (in time) do you wish to make that observation? There is a huge difference between probing near time=0 and near time=18000000 us.
Earlier you wrote that you "can't view anything smaller then 94ps". Is that still true, and when (in the 18 second simulation) are you
trying to or are unable to see things smaller than 94 ps? This helps us zero in on what you want to look for.
|
On Mon, Dec 2, 2024 at 07:27 PM, Bell, Dave wrote:
I suspect he’s trying to see an expanded waveform pulse of the power in L3, ‘round about 16.000534s
Um, that simulation does not make sense. Several things seem "off".
(1) In my simulation, L3 has no pulse around 16 s. There is nothing meaningful to see or plot!
(2) V2 switches on and then off from 16.00 to 16.02 s, but its voltage never goes high enough to cross the threshold (Vt=1.0) of S2, so S2 never closes. The "B" input pin of U3 stays low forever. U3 never toggles. U4 never toggles. Its "Y" output = V(N011) stays low forever. S1 never turns ON, and there is no pulse in L3.
(3) Diode D5 between U4 and S1 is puzzling. Diodes work only if there is current through them, but the current through D5 should be zero. The control inputs of S1 have infinite input resistance (well, it might be 1/Gmin) and zero capacitance. Also, why use a zener where it can't ever have a reverse bias voltage?
(4) The schematic suggests that S1 represents a "138ohm" relay. But there is no 138 ohms. If it was supposed to be in the coil, the resistor needed is missing.
(5) Why do both switches (S1 and S2) have Vser=0.6 volts? I think it is probably wrong.
Back to the question about time resolution. Let's say that you wanted to examine something happening at about 16 seconds. As it happens, the smallest increment (the numerical resolution) there is about 1 us, meaning that you can zoom in from 16.0 to 16.000001 seconds, but that's as tight as you can make the plot window. Anything smaller can't be displayed, when you are looking at 16 s.
The easy workaround is this:
- Right-click on the X-axis.
- Change "Quantity Plotted" from "time" to "time-16".
- Click "OK".
That shifts everything to the left by 16 seconds. Now you have lots of available time resolution in the vicinity of 0 on the plot = 16 s in actual time. For example, set the left limit to "0" (representing 16 seconds), and set the right limit to "1fs", which represents 16.000000000000001 seconds = 16 s + 1 femtosecond. You can even change the right limit to 1e-24, which is 1 pico-picosecond.
After doing that, it is easy to zoom in on extraordinarily narrow events. All you need to do is remember that "0" on the plot really means 16 seconds in the simulation.
Andy
|
Can you say "yoctosecond"?
Sent: Monday, December 02, 2024 at 10:22 PM
From: "Andy I via groups.io" <AI.egrps+io@...>
To: LTspice@groups.io
Subject: Re: [LTspice] X axis limits.
On Mon, Dec 2, 2024 at 07:27 PM, Bell, Dave wrote:
I suspect he’s trying to see an expanded waveform pulse of the power in L3, ‘round about 16.000534s
Um, that simulation does not make sense. Several things seem "off".
(1) In my simulation, L3 has no pulse around 16 s. There is nothing meaningful to see or plot!
(2) V2 switches on and then off from 16.00 to 16.02 s, but its voltage never goes high enough to cross the threshold (Vt=1.0) of S2, so S2 never closes. The "B" input pin of U3 stays low forever. U3 never toggles. U4 never toggles. Its "Y" output = V(N011) stays low forever. S1 never turns ON, and there is no pulse in L3.
(3) Diode D5 between U4 and S1 is puzzling. Diodes work only if there is current through them, but the current through D5 should be zero. The control inputs of S1 have infinite input resistance (well, it might be 1/Gmin) and zero capacitance. Also, why use a zener where it can't ever have a reverse bias voltage?
(4) The schematic suggests that S1 represents a "138ohm" relay. But there is no 138 ohms. If it was supposed to be in the coil, the resistor needed is missing.
(5) Why do both switches (S1 and S2) have Vser=0.6 volts? I think it is probably wrong.
Back to the question about time resolution. Let's say that you wanted to examine something happening at about 16 seconds. As it happens, the smallest increment (the numerical resolution) there is about 1 us, meaning that you can zoom in from 16.0 to 16.000001 seconds, but that's as tight as you can make the plot window. Anything smaller can't be displayed, when you are looking at 16 s.
The easy workaround is this:
- Right-click on the X-axis.
- Change "Quantity Plotted" from "time" to "time-16".
- Click "OK".
That shifts everything to the left by 16 seconds. Now you have lots of available time resolution in the vicinity of 0 on the plot = 16 s in actual time. For example, set the left limit to "0" (representing 16 seconds), and set the right limit to "1fs", which represents 16.000000000000001 seconds = 16 s + 1 femtosecond. You can even change the right limit to 1e-24, which is 1 pico-picosecond.
After doing that, it is easy to zoom in on extraordinarily narrow events. All you need to do is remember that "0" on the plot really means 16 seconds in the simulation.
Andy
|
Ah! Clever!
-
Change "Quantity Plotted" from "time" to "time-16".
Interesting. It runs OK for me, *but* I’m still running XVII, and I just OK’ed the missing component warnings.
I see a gigantic 8.2GGW (negative) spike of Power in L3, about 16ps wide.
I set the tran start time to 16s, and specified a very narrow X axis span.
Dave
переключити цитоване повідомлення
Показати цитований текст
From: LTspice@groups.io <LTspice@groups.io> On Behalf Of
Andy I via groups.io
Sent: Monday, December 02, 2024 7:22 PM
To: LTspice@groups.io
Subject: EXTERNAL: Re: [LTspice] X axis limits.
On Mon, Dec 2, 2024 at 07:27 PM, Bell, Dave wrote:
I suspect he’s trying to see an expanded waveform pulse of the power in L3, ‘round about 16.000534s
Um, that simulation does not make sense. Several things seem "off".
(1) In my simulation, L3 has no pulse around 16 s. There is nothing meaningful to see or plot!
(2) V2 switches on and then off from 16.00 to 16.02 s, but its voltage never goes high enough to cross the threshold (Vt=1.0) of S2, so S2 never closes. The "B" input pin of U3 stays low forever. U3 never toggles. U4 never toggles.
Its "Y" output = V(N011) stays low forever. S1 never turns ON, and there is no pulse in L3.
(3) Diode D5 between U4 and S1 is puzzling. Diodes work only if there is current through them, but the current through D5 should be zero. The control inputs of S1 have infinite input resistance (well, it might be 1/Gmin) and zero capacitance.
Also, why use a zener where it can't ever have a reverse bias voltage?
(4) The schematic suggests that S1 represents a "138ohm" relay. But there is no 138 ohms. If it was supposed to be in the coil, the resistor needed is missing.
(5) Why do both switches (S1 and S2) have Vser=0.6 volts? I think it is probably wrong.
Back to the question about time resolution. Let's say that you wanted to examine something happening at about 16 seconds. As it happens, the smallest increment (the numerical resolution) there is about 1 us, meaning that you can zoom
in from 16.0 to 16.000001 seconds, but that's as tight as you can make the plot window. Anything smaller can't be displayed, when you are looking at 16 s.
The easy workaround is this:
-
Right-click on the X-axis.
-
Change "Quantity Plotted" from "time" to "time-16".
-
Click "OK".
That shifts everything to the left by 16 seconds. Now you have lots of available time resolution in the vicinity of 0 on the plot = 16 s in actual time. For example, set the left limit to "0" (representing 16 seconds), and set the right
limit to "1fs", which represents 16.000000000000001 seconds = 16 s + 1 femtosecond. You can even change the right limit to 1e-24, which is 1 pico-picosecond.
After doing that, it is easy to zoom in on extraordinarily narrow events. All you need to do is remember that "0" on the plot really means 16 seconds in the simulation.
|
Since my sim seems to work:
- At 16s, S2 closes, initiating an ~87us pulse from the dashed one-shot
- That pulse closes S1, allowing C5 to discharge into L3
- When the 87us pulse ends, S1 opens (to15e15 ohms)
- The field around L3 collapses and the transferred energy is dissipated in 17ps
Dave
|
Isn't it similar to stting .tran 16 16.000000000000001?
I must say under this form it's easy to forget or add an unwanted
zero...
Le 03/12/2024 à 04:22, Andy I via
groups.io a écrit :
переключити цитоване повідомлення
Показати цитований текст
On Mon, Dec 2, 2024 at 07:27 PM, Bell, Dave wrote:
I suspect
he’s trying to see an expanded waveform pulse of the power
in L3, ‘round about 16.000534s
Um, that simulation does not make sense. Several things seem
"off".
(1) In my simulation, L3 has no pulse around 16 s. There is
nothing meaningful to see or plot!
(2) V2 switches on and then off from 16.00 to 16.02 s, but
its voltage never goes high enough to cross the threshold
(Vt=1.0) of S2, so S2 never closes. The "B" input pin of U3
stays low forever. U3 never toggles. U4 never toggles. Its
"Y" output = V(N011) stays low forever. S1 never turns ON, and
there is no pulse in L3.
(3) Diode D5 between U4 and S1 is puzzling. Diodes work
only if there is current through them, but the current through
D5 should be zero. The control inputs of S1 have infinite input
resistance (well, it might be 1/Gmin) and zero capacitance.
Also, why use a zener where it can't ever have a reverse bias
voltage?
(4) The schematic suggests that S1 represents a "138ohm"
relay. But there is no 138 ohms. If it was supposed to be in
the coil, the resistor needed is missing.
(5) Why do both switches (S1 and S2) have Vser=0.6 volts? I
think it is probably wrong.
Back to the question about time resolution. Let's say that
you wanted to examine something happening at about 16 seconds.
As it happens, the smallest increment (the numerical
resolution) there is about 1 us, meaning that you can zoom in
from 16.0 to 16.000001 seconds, but that's as tight as you can
make the plot window. Anything smaller can't be displayed, when
you are looking at 16 s.
The easy workaround is this:
- Right-click on the X-axis.
- Change "Quantity Plotted" from "time" to "time-16".
- Click "OK".
That shifts everything to the left by 16 seconds. Now you
have lots of available time resolution in the vicinity of 0 on
the plot = 16 s in actual time. For example, set the left limit
to "0" (representing 16 seconds), and set the right limit to
"1fs", which represents 16.000000000000001 seconds = 16 s + 1
femtosecond. You can even change the right limit to 1e-24,
which is 1 pico-picosecond.
After doing that, it is easy to zoom in on extraordinarily
narrow events. All you need to do is remember that "0" on the
plot really means 16 seconds in the simulation.
Andy
|
On Tue, Dec 3, 2024 at 01:25 AM, Jerry Lee Marcel wrote:
Isn't it similar to stting .tran 16 16.000000000000001?
It is! If you are not interested in seeing the first 16 seconds.
(Actually, I think that would be ".tran 0 16 16.000000000000001" (OOPS! Correction:) ".tran 0 16.000000000000001 16" because of that funny SPICE quirk about the extra first parameter whenever there are more than one.)
I must say under this form it's easy to forget or add an unwanted zero...
I believe you can write ".tran 0 16 {16+1f}" (OOPS! Correction:) ".tran 0 {16+1f} 16"and avoid counting zeros.
Andy
|
Dave, you measured 16ps, thank you. I can not for some reason measure anything that small and I don't know why.
|
Sorry I overlooked that, I assumed many would have such a popular component.
|
Thanks Dave, I will try this.
|
Dave, can you be a little more specific as to what you did to get a measurable plot?
|
First, get rid of the lead-in:
.tran 0 16.01 16.0 startup uic
I suggest going to Tools/Control Panel/Compression and set Window Size to 0.
For this, you want all of the data points spice can give you…
Run the simulation.
In the plot window, set the X axis to 0 to 1ms with 100us ticks.
Plot Power in L3, and you should get a line sitting around 0MW, with a negative-going spike right about 100is.
Click-drag and zoom in to the spike.
Now, Andy found that the sim just failed to work for him.
I’m not certain, but nut it may be a slight difference in how different version of LTspice detech the trigger threshold in a SWitch.
Your trigger pulse for S2 runs from 0 to 1.000000V, and the model for S2 switches ON at exactly 1V or higher.
Mine switches, under version XVII, but I believe Andy is running version 24.x
Change the pulse spec to:
PULSE(0.00 1.1 16 10u 10u 20m)
OR, change the SW model to:
.model SW SW(Ron=.1 Roff=200Meg Vt=0.95)
You don’t need all of the suggested parameters, such as “Vh=0 Lser=10n Vser=.6”
Unless you really want the series inductance, for example.
Dave
переключити цитоване повідомлення
Показати цитований текст
From: LTspice@groups.io <LTspice@groups.io> On Behalf Of
Richard Andrews via groups.io
Sent: Tuesday, December 03, 2024 2:14 PM
To: LTspice@groups.io
Subject: EXTERNAL: Re: [LTspice] X axis limits.
Dave, can you be a little more specific as to what you did to get a measurable plot?
|
Tony Casey
Bell, Dave
eewiz