I believe that nodes (or nets) can be user-named, and that curves on an LTSpice plot can also be user-named, but sometimes it would be simplest to use the node numbers assigned by the software during the building of a schematic. Is there a way to cause those node numbers to be displayed on the schematic. Thanks, Chris.

开云体育

Those run-time node and net numbers can vary from run to run, especially after adding a component. AFIK, they are not known until the sim runs.

开云体育

Well, except for net 0, common or ground. That is known as the schematic is built.

You can lable the nets with numbers or letters.? As for them showing up as you mentioned I am not sure about that.

开云体育

You always should label nodes if they are being referenced in an equation or within a measure statement. Otherwise, they WILL change. leaving the reference invalid. Those labels are visible on the schematic until they are deleted.

开云体育

No, you can see what the node names before simulation are by:

View > SPICE Netlist

As you say, though, the net names are dynamic unless you explicitly name them. Only explicitly named nets are visible on the schematic.

--

Chris,

You can not display the automatically generated node names on the schematic.? But you can see what they are when viewing the schematic.? Hover your mouse over any node (net).? The node name is shown in the lower left corner.

And as everyone advises you, you really should add your own node names (or numbers) as much as possible, and then they are visible too.

I don't understand what you said about naming curves on a plot.? I do not think you can do that (except by defining functions in the waveform viewer).? But whatever node names you used on the schematic will show in the plot window.

Andy

开云体育

On 18/07/2023 03:33, Andy I wrote:

I don't understand what you said about naming curves on a plot.? I do not think you can do that (except by defining functions in the waveform viewer).? But whatever node names you used on the schematic will show in the plot window.

That's not quite true. As you say, you can define functions and save them in plot.defs.

So, for example:

.func hFE() {Ic(Q1)/Ib(Q1)}

..allows you to label a plot hFE() - useful in device testjigs.

Another useful one is:

.func NF(R,T) {10*log10(V(inoise)*V(inoise)/(4*k*(T+273.15)*R))}

..which allows the label NF(1k,25) to be used as the circuit's noise figure as a function of source resistance and temperature (in °颁).

Using:

.noise V(out) V1 list 1k

..and stepping a parameter Rsrc as the source resistance, you can plot the noise figure vs. source resistance at 1kHz:

NF({Rsrc},25)

Tony,

That is exactly what I was saying (or meant).

Andy

Automatically assigned node numbers are ephemeral between runs, unless you label them.
Giving the same label to different nets, shorts those nets together. I use it often.

Giving more than one label to one net, confuses LTspice. I get no specific warning.
A short wire with label A at one end, and label B at the other, does NOT connect other nets A and B elsewhere on the schematic. It seems LTspice ignores some labels when another label has been found earlier on that net.

What was the need for it, perhaps an alternative can be found. I think mousing over them is all you can do.

Many thanks, guys.

On Mon, Jul 17, 2023 at 02:33 PM, Andy I wrote:

I do not think you can do that (except by defining functions in the waveform viewer).?

Is it possible to use parameters and functions defined on the schematic (not in plot.defs) in the waveform viewer?
Related, is it possible to use such parameters / functions in measurements, even when directly on a .raw file with
a .meas script?

I think this can be done with a dynamically adjusted plot.defs file, but currently that might need restarting the GUI.

-marcel

I can answer my own question: editing the plot.defs file *immediately* has effect.
(I reran the simulation before trying but did not restart LTspice.)

Why don't they document these useful enhancements? Is it in any of the LTspice
books or tutorials? I'm almost certain I tried this before with LTspiceIV and
it didn't work.

-marcel

开云体育

You're right. Changes to plot.defs are now immediately effective in 17.1.9. When this happened - I don't know, either.

The lack of a mention in the ChangeLog is maybe because hardly anyone even knows about plot.defs, let alone uses it. I guess they have a threshold for whether things are documented there, or not.

Thanks for spotting this!

marcel asked, "Is it possible to use parameters and functions defined on the schematic (not in plot.defs) in the waveform viewer?"

I do not believe you can.? If there is some ability to do that, it is limited.

I almost never use a plot.defs file.? At some point I had one, but then I realized that the whole point of plot.defs is to make one's LTspice work differently than everyone else's, which is something I did not want to do.? But that's me.

If they (ADI?) changed how or when the plot.defs file was read (e.g., when making a plot vs. only when starting LTspice, or reading it again when saving it), it might have been an inadvertent change that they thought didn't need an announcement.? That is, if it changed at all.? It's also possible that it always behaved this way, and nobody noticed or cared since so few people use a plot.defs file.? Since you guys have more experience with plot.defs files, I guess you would know if it changed.

Also I think it would make sense that LTspice knows immediately about changes that you make to the plot.defs file, if you made them from within LTspice's plot.defs editor (via the "Edit Plot.Defs File" tool).? But if you edit your plot.defs with an external editor, LTspice would not know about it unless it opens the file again.? That is consistent with editing the standard.xxx files -- LTspice knows the changes if you made them from within LTspice's editor and you don't need to restart LTspice.? But if edited in an external editor, LTspice doesn't know until it is restarted.

Andy

On Tue, Jul 18, 2023 at 11:25 PM, Andy I wrote:

That is consistent with editing the standard.xxx files -- LTspice knows the
changes if you made them from within LTspice's editor and you don't need to
restart LTspice.? But if edited in an external editor, LTspice doesn't know
until it is restarted.

You have the mind of an ADI engineer. Indeed, it does not work when using an external editor :--)

-marcel

开云体育

On 19/07/2023 12:25, Andy I wrote:

marcel asked, "Is it possible to use parameters and functions defined on the schematic (not in plot.defs) in the waveform viewer?"

I do not believe you can.? If there is some ability to do that, it is limited.

Functions defined in the schematic cannot be used in the waveform viewer. Similarly, parameters cannot be used either, unless they are stepped, then they can be accessed through the same syntax as in the schematic, by wrapping them in braces.

In addition, special parameters and constants that the waveform viewer understands, like Freq(uency), Omega, Q and K are not understood in the schematic. Pi is an exception, but not E (Euler's number).

I almost never use a plot.defs file.? At some point I had one, but then I realized that the whole point of plot.defs is to make one's LTspice work differently than everyone else's, which is something I did not want to do.? But that's me.

If they (ADI?) changed how or when the plot.defs file was read (e.g., when making a plot vs. only when starting LTspice, or reading it again when saving it), it might have been an inadvertent change that they thought didn't need an announcement.? That is, if it changed at all.? It's also possible that it always behaved this way, and nobody noticed or cared since so few people use a plot.defs file.? Since you guys have more experience with plot.defs files, I guess you would know if it changed.

Also I think it would make sense that LTspice knows immediately about changes that you make to the plot.defs file, if you made them from within LTspice's plot.defs editor (via the "Edit Plot.Defs File" tool).? But if you edit your plot.defs with an external editor, LTspice would not know about it unless it opens the file again.? That is consistent with editing the standard.xxx files -- LTspice knows the changes if you made them from within LTspice's editor and you don't need to restart LTspice.? But if edited in an external editor, LTspice doesn't know until it is restarted.

LTspice definitely used to only read plot.defs when it was started, and changes were not active until LTspice was restarted. This is also true for library folders. If you add a folder (outside of LTspice) in LTspice's library tree while LTspice is running, it is also not available until after a restart.

I just checked again with 17.1.9, and found that you still have restart LTspice for changes in plot.defs to be available. I could have sworn that you now didn't, so my earlier comment doesn't stand.

The other thing I have found is that if you edit plot.defs within LTspice when the waveform viewer contains a trace that uses one of its function, LTspice reliably crashes. If you delete the offending trace before editing, it doesn't crash. This is while using Wine. It might be different in Windows. The behaviour is the same for 17.0.36 and 17.1.9.

Perhaps someone can check this behaviour in Windows, before I submit a bug report?

开云体育

On 19/07/2023 15:16, Tony Casey wrote:

Functions defined in the schematic cannot be used in the waveform viewer. Similarly, parameters cannot be used either, unless they are stepped, then they can be accessed through the same syntax as in the schematic, by wrapping them in braces.

Although wrapping parameters in braces works, it's actually not necessary - NF(Rsrc) works as well as NF({Rsrc}), in my example. I guess this is because Rsrc appears in the list of waveforms available to plot.