Electronic – How to take Time Measurements using LT Spice

capacitancecircuitsltspicemeasurementsimulation

I've been fooling around with LT spice .MEAS feature for a while now and I just can't seem to determine how to take the time measurements I need for an assignment.

I can look at the time values on the waveform viewer and determine an estimated time, however given that LT spice is equipped with a measurement feature I'd like to be precise.

I have a simple circuit of a voltage source in series with a resistor and capacitor and I need to find the time that the voltage at the capacitor reaches 63% of the Voltage input. I think this is called Rise Time?

the command I've been trying is:

.MEAS Tran res1 FIND time WHEN V(Vout)=0.63(Vin) cross=5 TD=1m

essentially I need to find the time that it takes Vout to reach 3.15v (63% 5V(Vin))

Thanks

My circuit and .meas command

Best Answer

You labeled the nodes Vin and Vout, and you are using the output node correctly (V(Vout)), but not the input node ((Vin) instead of V(Vin)).

You also forgot the asterisk for multiplication: 0.63*V(Vin). If you need to be more precise, use (1-exp(-1))*V(Vin), impose a small timestep (1m of total time, or less), and, optional, add .opt plotwinsize=0 to disable waveform compression. It doesn't look like you need it, though.

Finally, you use cross=5 but you only have four rise/fall edges. Instead, use rise=1 for the first rising edge, rise=2 for the 2nd, etc. You don't need td here.

The new command should look like this:

.meas TRAN res1 FIND time WHEN V(Vout)=(1-exp(-1))*V(Vin) RISE=1

As a minor addition, you could use a bit sharper rise/fall edges on your source, to avoid wrong readings. 1u would do just fine, without sacrificing decimals.

A little bit of attention can go a long way. This also implies no haste.

Related Topic