Hello,

I'm currently simulating several Foster thermal networks (circuit file: thermal simulation.cir). However, when I enable the option to save subcircuit device currents, the simulation results differ from those with this option disabled(Simulation results). Has anyone encountered a similar issue or could offer insights into why this might be happening?

Any advice would be greatly appreciated!

Turn off waveform compression.

On Fri, Oct 25, 2024 at 04:18 AM, Androidbaby wrote:

Hello,

I'm currently simulating several Foster thermal networks (circuit file: thermal simulation.cir). However, when I enable the option to save subcircuit device currents, the simulation results differ from those with this option disabled(Simulation results). Has anyone encountered a similar issue or could offer insights into why this might be happening?

Any advice would be greatly appreciated!

Long explanation:

 

Make the plots have the same time-axis.  By displaying one waveform that starts at 1 ns and another that starts at 20 ns us, they are not fair comparisons.

 

Enable displaying the actual simulated and saved datapoints: View > Mark Data Points.  This will show you where the saved datapoints were, and - more importantly - where they were not.  Notice the lack of saved datapoints between 1 ns and 20 ms us, in the simulation without saving subcircuit currents.

 

So why is this happening?  Because you are looking "down in the mud" (or "down in the noise") at rather small relative changes in node voltages, but larger changes in subcircuit currents.  Mathias Born's reply is spot-on (correct).

 

With subccircuit currents NOT saved:  Between 1 ns and about 20 ms us, although the simulated voltage did slowly change following a curve, that curvature was moderately small and LTspice found it sufficient to say that it was linear and the intervening simulated points could be discarded with "waveform compression".  Remember, LTspice compresses the saved data to remove datapoints that are not needed to draw a reasonable waveform on your screen.  To see what I mean, add this waveform "0V" to the same plot (right-click in the plot > Add Traces > type "0V" as the "Expression to add" > OK).

 

With subcircuit currents saved:  Between 1 ns and 20 ms us, LTspice saw enough activity happening with the saved currents, to not compress the datapoints nearly as much between 1 ns and 20 ms us.

 

How to avoid this:  Turn off waveform compression.  Add this line: ".options plotwinsize=0" to your schematic, or to the netlist (outside of any subcircuit but between the Title line and the .END line).  That command prevents the saved points from being compressed.

 

By plotting a voltage that had relatively little RELATIVE change (relative to its own magnitude), and by using a logarithmic time axis, your plots exaggerated the effect.

 

Andy

 

 

I made several typos in my reply, writing numbers like "20 ns" or "20 ms" that should have been "20 us".  I think I've corrected them now.

 

Andy

 

 

Thank you both for your insights!

I get the issue now, and turning off waveform compression works perfectly. Really appreciate your help!