开云体育

Can I remove it from the rectangle and load the symbol for a comparator from a library?

No, the symbol editor lacks many of the features of the schematic editor. You cannot drag items from one symbol into another, like you can with schematics.

--
Regard,
Tony

开云体育

Thanks for answering
That's what I'd like to do..
Find a symbol that looks more like a comparator.
My question is, where do I look for it??' within Ltspice??
And if I find one, how can I associate the appropriate PINS to my comparator?

If your comparator has 5 pins, you can start with the LTspice opamp2 symbol.

The most important thing is for the symbol pin order to match to the order in the .subckt line. The pin names do not have to match. If they match, then you only have to change the opamp2 symbol's value to match the .subckt name, and you're good to go.

But, honestly, if you can draw schematics, you can also draw symbols. It's not hard, and once you have had a little practice, you will never use auto-generated symbols again, and we will all be glad.

Did you look in:

Help > Schematic Capture > Creating New Symbols ?

--
Regards,
Tony

开云体育

I have 136GB free space on the drive where the .RAW file grows.

I did have Mark Data Points turned on which makes the plot window render many times slower.

?

Also, I can crash the plot window, taking LTspice 24.0.12 along with it, whenever I wish.

See

Close a window that overlays the plot window, as the plot window is rendering, and poof, there goes LTspice.

The plot window crashing is nothing new to me.

?

I agree also that increasing numdgts was not the cause of the crash.

Ah, OK. I seem to remember this issue might also be dependent on the graphics card/driver. There are also message threads from many years ago, before V24, that certain (Intel) CPUs were more susceptible to crashes. Helmut documented which types were most problematic, but I can't find that right now.

--
Regards,
Tony

开云体育

Good morning, I have a question about symbols.

Could a symbol be automatically generated from a (.lib) or (.sub) file??..
In this case it would be a comparator.

?

If so, how could I generate it?

Yes, symbols can be automatically generated from any text file containing a valid .subckt. It doesn't matter what the name of the file is. It can be a .lib or .sub file, but it doesn't have to be.

The procedure is simple.

1. Open the file in LTspice. this most easily done by dragging the file from Explorer into LTspice.
2. Right-click with the mouse on the .subckt line.
3. From the drop-down menu, choose Create Symbol.
4. Save.

Whether this is a good idea, or not, is another matter. You will get a rectangular box with the correct pin names, but not necessarily in appropriate places. Nobody will know for sure what kind of component it is. You could delete the box and draw a proper comparator outline, for example, and re-arrange the pin positions. But many people don't bother, and it is often difficult to figure out what a schematic does that uses them.

So, here are some alternatives:

1. Look for an LTspice standard symbol that is appropriate for the type of component.
2. If it also has the correct pin configuration, use it with modification.
3. If it doesn't you can make a copy of the standard symbol, and edit it to have the correct pin configuration.
4. Draw a new symbol from scratch.

--
Regards,
Tony

开云体育

After adding .option measdgt=15:

LTspice 24.0.12 for Windows
Circuit: * C:\users\tony\Desktop\LTspice\_Temp\Eewiz\MEAS_example.asc
Start Time: Tue Feb 25 10:10:33 2025
solver = Normal
Maximum thread count: 32
tnom = 27
temp = 27
method = modified trap
Direct Newton iteration for .op point succeeded.

t1: v(test)=0 AT 0.500500582598

Total elapsed time: 0.044 seconds.

Note, that the correct time value for this is actually 0.5005005005005... The problem was deliberately set so the answer was an irrational number.

--

开云体育

I suppose the OP posted more than one version of the .ASC. I don't think it's worth pursuing any further, but the fact that it runs OK with the simple opamp suggests that there is a problem with the AD757 model.

On Mon, Feb 24, 2025 at 12:38 PM, John Woodgate wrote:

I don't know what's going on here. U1 isn't open-loop. Are we looking at the same .ASC, PID_section_united_AC_separate?

We are.

?

U1 is the integrator with C1 in its feedback path.? For DC, C1 is an open circuit so it is open-loop at DC.

?

?U3 is open-loop at DC. U1 and U2 have unity gain, U4 has 100 times gain at DC.

Wow.? You got quite different component markers than I did, from the same schematic!? Since those numbers are embedded within the schemeatic file itself, I don't know how that would have happened.

In such a circuit, I would not expect a TSTS? error

One never expects Timestep Too Small errors.? They only happen when the simulator runs into great difficulty in the right way.

?

Did I also mention that I never saw a Timestep Too Small error when I tried that simulation?? It was something "john23" had in his Error Log listing.? ?In my simulation it just ran very very slowly but did not abort.

?

Andy

?

开云体育

Yes, I agree.

Rather than assume such was true, I sought to prove that in my case there actually was no 2.0000000000 volts.

In general, it is usually impossible to prove the non-existence of something.

Therefore the effect, however it may be accomplished, is to print the time at which the next sample found is LESS-THAN 2 volts.

?

Wouldn't it be a phenomnal waste of processor time to interpolate between points, following the resultant curve, to find a point on that curve that is exactly 2.0000000000 volts when simply looking for the first value of data less-than 2 volts provides the same result.

Hardly a phenomenal waste of processor power. Linear interpolation between two points is a trivially simple operation. The .MEAS already finds the last data point before, and the first data point after the target is reached. Interpolation means you always get a more accurate answer even when not using very small values of maximum timestep, with very little overhead.

?

Regardless of how it is accomplished, the end result of using FALL=1 is to print the time at which the first data value less-than 2 is found.

This is obviously not true. The end result of using FALL=1 is to print out the interpolated value.

The reason why you found that apparently two points at the same time had two different voltages is due the printed precision of the time points. The time points are printed in single precision in the logfile. You can get double precision by adding .option measdgt=15. This is true whether or not you also use .option numdgt=15.

For example, to find the first falling value of 0, I added:

.MEAS T1 when V(test)=0 fall=1

..when analysing a 0.999Hz sine wave with .TRAN 1.1. By default the logfile was:

LTspice 24.0.12 for Windows
Circuit: * C:\users\tony\Desktop\LTspice\_Temp\Eewiz\MEAS_example.asc
Start Time: Tue Feb 25 10:09:09 2025
solver = Normal
Maximum thread count: 32
tnom = 27
temp = 27
method = modified trap
Direct Newton iteration for .op point succeeded.

t1: v(test)=0 AT 0.500501

Total elapsed time: 0.054 seconds.

After adding .option measdgt=15:

LTspice 24.0.12 for Windows
Circuit: * C:\users\tony\Desktop\LTspice\_Temp\Eewiz\MEAS_example.asc
Start Time: Tue Feb 25 10:10:33 2025
solver = Normal
Maximum thread count: 32
tnom = 27
temp = 27
method = modified trap
Direct Newton iteration for .op point succeeded.

t1: v(test)=0 AT 0.500500582598

Total elapsed time: 0.044 seconds.

Note: this option is sticky. It remains active for the session (until you close and restart LTspice), even if it is removed. Whether this is intended or not is not known. AFAIK, it is not documented.

开云体育

On Mon, Feb 24, 2025 at 05:38 PM, Tony Casey wrote:

By default, the .raw file is written with single precision; this option enables double precision (and approximately doubles the .raw file size).

Although that is true for voltages and currents, time values are always saved to the .raw file with double precision.? Time is special in that way.

?

What probably happened here is that the Waveform Cursor pop-up window itself displays the numbers with less precision than they are saved in the .raw file.

This is also true with .MEAS. The time points are printed in single precision in the logfile, by default. You can get double precision by adding .option measdgt=15. This is true whether or not you also use .option numdgt=15.

For example, to find the first falling value of 0, I added:

.MEAS T1 when V(test)=0 fall=1

..when analysing a 0.999Hz sine wave with .TRAN 1.1. By default the logfile was:

LTspice 24.0.12 for Windows
Circuit: * C:\users\tony\Desktop\LTspice\_Temp\Eewiz\MEAS_example.asc
Start Time: Tue Feb 25 10:09:09 2025
solver = Normal
Maximum thread count: 32
tnom = 27
temp = 27
method = modified trap
Direct Newton iteration for .op point succeeded.

t1: v(test)=0 AT 0.500501

Total elapsed time: 0.054 seconds.

After adding .option measdgt=15:

LTspice 24.0.12 for Windows
Circuit: * C:\users\tony\Desktop\LTspice\_Temp\Eewiz\MEAS_example.asc
Start Time: Tue Feb 25 10:10:33 2025
solver = Normal
Maximum thread count: 32
tnom = 27
temp = 27
method = modified trap
Direct Newton iteration for .op point succeeded.

t1: v(test)=0 AT 0.500500582598

Total elapsed time: 0.044 seconds.

Note: this option is sticky. It remains active for the session (until you close and restart LTspice), even if it is removed. Whether this is intended or not is not known. AFAIK, it is not documented.

开云体育

.options numdgt=15. caused the plot window to crash at the end of simulation as it was rendering.

That plot window crash took LTspice 24.0.12 down with it.

I will restart and try again.

?

On the next try the .meas result was:

.meas TooLow1 FIND V(XSW11:X1:Qc,XSW11:X1:Qe) WHEN V(XSW11:X1:Qc,XSW11:X1:Qe)=2 FALL=1

toolow1: v(xsw11:x1:qc,xsw11:x1:qe)=2 at 0.00804695

AND

.meas TooLow2 FIND V(XSW12:X1:Qc,XSW12:X1:Qe) WHEN V(XSW12:X1:Qc,XSW12:X1:Qe)=2 FALL=1

Measurement "toolow2" FAIL'ed

?

TooLow2 saw no point that fell below 2V on the XSW12 signal, so it reported "Measurement "toolow2" FAIL'ed".

Both syntax error and, failure to find the measurement specified, produce the same "Measurement "toolow2" FAIL'ed" error message.

Isn't that a fine kettle of fish.

?

Subtracting 8ms from the start and stop values on the abscissa saw the plot window simply stop rendering in mid-redraw.

I am not going to burn any more time divining how LTspice works.

I will now move on to more productive efforts.

?

In my case ".options numdgt=15" broke 24.0.12.

The .raw file for the run is 11.5GB.

This suggests that LTspice might have crashed because you ran out of disk space. I have never seen crashes upon invoking double precision, but I have when running out of disk space.

--