I am analyzing the voltage and currents of driving a helical coil with a RF generator through a matching network. The coil is modeled as RLC elements with winding resistance and self inductance and capacitance. The generator is an ideal voltage source with a 50 Ohm resistive source impedance. The matching network is a shunt C then series C viewing from the input side of the matching network.
I have determined the matching network component values and verified it on a online Smith chart tool. The reflection coefficient is <0.01 magnitude. Then I verified the impedance match in LTspice by performing AC analysis and plotting V(t)/I(t) at port 1 of the matching network. Zooming into the operating frequency, the impedance is approx. 50 Ohm magnitude and <1 deg phase, i.e. 50 Ohm real and very small reactive.
However, when I perform transient analysis, I find the voltage and currents are not in phase at all, on this one particular run current lag the voltage by 158 degrees. Can anyone explain why the voltage and current are not near in phase?
In my investigation, I learnt that LTSpice even the simple RLC elements are polarized or orientation specific. The direction of current is opposite if you flip the component 180 degrees. I have double checked that the component orientations are what I believe is the direction of current flow.
Hi, Thank you to all that viewed my question post. Since no one has replied as of yet, I thought I add more info that may stimulate a reply. 1st attachment is the schematic. 2nd is a frequency domain plot of the Z at port 1. The 3rd are time domain plots V, I, & P at port 1. Your solution or comments are definitely welcome. Thanks.
Sorry for the late response.
LTspice and any other SPICE will require a small time step compared to the period time of the signal, if the circuit has a small bandwidth like in your case.
.tran 0 2m 0 10n
When you simulate now, you will get 180° phase difference. You have to rotate the capacitor by 180° to get the "right" direction of the current - watch the current probe symbol.
I also turned off data compression which is used by default in the .tran simulation. I mostly do this when I simulate analog circuits with the transient simulation.
LTspice assumes a default series resistor of 1m Ohm in the inductors. I have set it 0 Ohm.
I have added the plot settings file. You can reload the plot settings after the simulation when you press the spacebar.
I added the changes as you indicated and I get the expected result. My faith is restored. Thank you, Helmut.