On Thu, May 1, 2025 at 12:09 PM, <ba@...> wrote:
I use currently the FFT of single voltage or current and I would like to do the same with expressions like :
V(n001)-V(n007)
or other valid numerical expressions for instance in a current instance.
The easiest way to do that, is this:
- Start with the FFT menu (View > FFT).
- Highlight all of the node voltages or element currents that you wish to be used in your FFT formula.? (Hint: Use Ctrl-click to select, or Shift-Click to select a range.? These use the normal MS-Windows selection rules.)
- In your example, highlight both V(n001) and V(n007).
- Click OK.
- A second pop-up window follows, asking you to select which waveforms to actually plot.
- As instructed there, now use Alt-Double-Click to enter an expression.? At this point, it doesn't matter which one is now highlighted.
- Type the expression you desire.? You may use only the node voltages and element currents that were previously selected in the first FFT menu.
- Click OK.
Done.
?
Once you get your FFT plot, you can further edit the formula if you desire, by right-clicking on the formula at the top of the plot.? Again, it can include only the voltages and currents that you had selected in the first FFT menu, so the important thing is to first select (highlight) all those voltages and currents which you might want to include in the expression.? Doing that instructs LTspice to find the FFT components of each of those individual voltages and currents - which you can then put into an editable formula.
?
Alternatively, you could generate a separate signal on your schematic that represents your formula, and then simulate with it.? But I like doing it the other way, even if it is more steps to remember.
?
Andy
?
