# NGspice Questions: Finding V at time t? Adding a Volt Meter? Freq Counter?

When simulating a circuit … say an OpAmp integrator… or whatever …
1 - Is there anyway to measure the V at time “t” of a particular Plot?
2 - Is there a way to add a cursor to a particular simulation Plot to check a the value at a particular point time?
3 - Is there a way to add a Volt Meter to the circuit?
4 - Is there a way to add a Counter to the circuit to display the frequency of an oscillator or input signal to the circuit?
Thanks for any help.

I avoid the Simulator in Kicad, preferring LTspice for it’s power and user-friendliness.

That said, in Kicad’s simulator, you can Cursor-Drag on the Scale and/or Window-Box-Zoom anywhere… etc and use the Mouse-Wheel to Zoom in/out

1. Use the meas(ure) command in ngspice: Add a net label to the node to be measured: `out`. Add a .control section to your circuit by opening a text box T, assuming we have a transient simulation with e.g.
`.tran 10n 5m`
``````.control
set controlswait         ;  waits until simulation is done
meas tran outsignal find v(/out) at=2m  ; net label prepends a /, we measure at 2ms
.endc
``````
1. Simulator window: right click on signal to be analyzed in Box Signals → Show cursor

2. There is no immediate solution, back annotation is not yet available

3. add another measure line to the text box, somewhat more complex:

``````.control
* waits until simulation is done
set controlswait
* net label prepends a /, we measure at 2ms
meas tran outsignal find v(/out) at=2m
* measure the time period when v(/out) after a delay of 2ms crosses 0 V
* for the second time while rising up to v(/out) crosses 0 V for the third time
* while rising (difference is 1 period)
meas tran period trig v(/out) td=2m val=0 rise=2 targ v(/out) td=2m val=0 rise=3
* calculate the inverse
let freq = 1/period
* print the result
echo frequency = \$&freq Hz
.endc
``````

You will get the period, the frequency is the inverse.