Whats the best way to show output impedance with LTSpice?

[cbdb]

I have searched DIY audio for a while and only found answers that aren't right.
If anyone can point me to a good solution that would be great.

Failing that:
I came up with my own method using the Delta Vout / Delta Iout technique, but its clunky. It needs 2 identical ccts, one with no load, the other with a a 1ua ac current source load. Do an AC sweep, then plot delta v/delta i or (V(vout1)-V(out2))/1ua. Seems to work well, but doubling the cct is a pain. Want to step the current load. Does anyone no how to plot the difference between the two stepped vouts (vout sep1 minus vout step2 )?? I will keep looking.

[Andrew Eckhardt]

You can use a voltage controlled switch driven by a pulse train to get your step load. I don't think you can set switch resistance to Zero, but maybe really small.

[cbdb]

Found it. (V(vout)@2-V(vout)@1)/1ua

Cool!

[cbdb]

You can use a voltage controlled switch driven by a pulse train to get your step load. I don't think you can set switch resistance to Zero, but maybe really small.

I run 2 sims (.step). First one current source =0a second time 1ua (could be anythig as long as it dosnt over load the cct.) i had trouble finding the @ sign which specifies the step.

[jcx]

AC sources in .AC analysis never "load the circuit" - there is no "sim" going on, the cirucit is linearized around the DC operating point claclulation's output DC bias points

after that the Laplace transfer function is evaluated - you can put in Meg A and other than the scale there is no difference in the FR curves

so just use 1 A, V in AC sources to simplify reading the plots

you can also check at spot frequencies, or .step frequency of test sources in .TRAN - then you do need to pay attention to ciruit limits - but the same (sine) source can have an AC value of 1 A

[cbdb]

Thanks I get it now. I made it more complicated than necesssary.

[Wombaticus]

For LTSpice newbs, the full description of my easy way is this:

Connect a current source with current flowing from ground to the node of interest . Right click on advanced for the current source and set AC amplitude to one in the box for small signal AC analysis.

Then run an AC analysis, and click on the node of interest. The default display shows a value in decibels. But go over and click on the Y axis, then select "linear". It will now show a frequency plot in volts. But because you're injecting current to the node, each volt you see here corresponds to one ohm of output impedance. Done.

[gootee]

Originally Posted by Wombaticus

For LTSpice newbs, the full description of my easy way is this:

Connect a current source with current flowing from ground to the node of interest . Right click on advanced for the current source and set AC amplitude to one in the box for small signal AC analysis.

Then run an AC analysis, and click on the node of interest. The default display shows a value in decibels. But go over and click on the Y axis, then select "linear". It will now show a frequency plot in volts. But because you're injecting current to the node, each volt you see here corresponds to one ohm of output impedance. Done.

THEN, right-click on the voltage's heading at the top of the plot and add /I(I1) , with whatever your current source's name is in place of I1, and the vertical axis will display OHMS, with actual Ω symbols.

Cheers,

Tom