you post a new thread to ask again
is there any feedback caused this negative real part resistance?
Z11 is measured at Vin/Iin when Iout is zero, which means you should open the output. did you keep the output open?
i think the "negative" is just due to the way you are measuring. depends on the test current flowing in or out of the test voltage source you have defined.
Cgd of FET forms feedback.is there any feedback caused this negative real part resistance?
Surely read all links I showed in your another post.I checked waveforms of all nodes and didn't see any oscillation. Don't know why.
I can't understand a meaning of this sentences at all.I use port1 and port2 as input and output terminal,
if you call that as open?
If let the output open, how can I use port2 to measure ZM1 and ZM2?
Cgd of FET forms feedback.
And if effective load of FET is inductive, it could cause negative real part of Zin.
Surely read all links I showed in your another post.
The Designer's Guide Community Forum - Oscillation in PA
Try to run Transient Analysis without input signal.
I can't understand a meaning of this sentences at all.
What do you want to mean ?
Using port1 and port2 at same time like your schematic, you can evaluate all quantities such as Zin, Zout, {Z11,Z12,Z21,Z22}.
And describe ZM(1) and ZM(2) not ZM1 and ZM2.
ZM1 and ZM2 are not available in Post Processing Enviornment of Cadence Spectre.
Surely read https://www.edaboard.com/threads/166900/
Again surely read my append in your another post.
I can't understand a meaning of this sentences at all.
What do you want to mean ?
Surely read The Designer's Guide Community Forum - Oscillation in PASo if the LC tank has to appear inductive,
then the input impedance of the output stage has to be negative, right?
Then I am wondering how I should deal with negative real part when I calculate interstage impedance.
I got it.Regarding ZM1 or ZM(1), I call it this just because the function name in SP. See the picture below.
Is this right?
Completely wrong.However I am using port1 and port2 so I think port2 will be set open automatically
when I do SP analysis to get Zin by ZM(1).
Still you can't understand difference between Zin and Z11.
Zin=ZM(1) is input impedance when output load's value is resistance value of port2.
Z11=ZP(1,1) is Z-parameter which is input impedance when output load's value is infinite.
Strictly speaking, not correct.I see. So for Zin=ZM(1), since source type of the port2 is set as DC (0V) and resistance is 50 ohms.
So ZM(1) just takes the load (port2) as 50 ohms. Right?
Strictly speaking, not correct.For Z11=ZP(1,1), it takes the output port as open circuit, right?
Right.So Zin=ZM(1) is what I should use for measuring input and output impedance for my case.
Cgd of FET forms feedback.
And if effective load of FET is inductive, it could cause negative real part of Zin.
Still you can't understand my append at all.To get positive input impedance of the output stage,
I have to remove the excess inductance.
To get the correct waveform, I need to add the excess inductance.
Wrong.for the negative real part impedance, can it be explained in the following way?
due to feedback of Cgd,
Rin=Rin@DC/(1+Loopgain)=Rin@DC/(1+gm*jwL*jwCgd)=Rin@DC/(1-gmLCgdw^2).
when gmLCgdw^2>1 at the certain frequency range, you get negative value.
Still you can't understand my append at all.
Class-F and Class-E amplifiers are highly nonlinear amplifier.
On the other hand, your analysis is small signal analysis.
So your analysis is not useful for Class-F or Class-E operation at all.
But if there is no input signal, there could be oscillation.
Again surely read The Designer's Guide Community Forum - Oscillation in PA
Again, this is third times of same comment, anyway try to run Transient Analysis without input signal.
Is there an oscillation ?
Did you set Vdd as step signal which will be cause of oscillation ?1. I run the Transient Analysis without RF input signal by setting amplitude of sinusoid signal as 0 volt.
I run it for 2usec.
I checked the drain waveform of the MOSFET.
It is just a DC voltage, no oscillation at all.
Is there anywhere I can check to see if it is oscillating?
If you prefer Cadence Spectre, invoke PSS/PAC or PSS/PSP.2. I think I am not quite sure which analysis is for nonlinear amplifier.
Could you please tell me what analysis I should use for nonlinear amplifier?
Did you set Vdd as step signal which will be cause of oscillation ?
If not, set Vdd as step signal. And run transient analysis with sweeping input signal from zero to large.
If you prefer Cadence Spectre, invoke PSS/PAC or PSS/PSP.
https://www.edaboard.com/threads/169169/
Next try run LSSP.
I can't obserbe any symptom of oscillation.Do you think it is oscillating?
Retry with setting period as 2sec and pulse width as 1sec.I set the step signal period as 50ns and pulse width as 25ns.
You can evaluate any of Zin,Zout,{Z11,Z12,Z21,Z22} by PSS/PAC.Someone said I can plot Z11 from PSS+PAC.
There is no function for Direct Plot Form in PSS/PAC.However, I couldn't find anything related to Z11.
See the picture below,
what function should I use for measuring input impedance?
I can't obserbe any symptom of oscillation.
Retry with setting period as 2sec and pulse width as 1sec.
And set more sharp edge, e.g. trise=tfall=0.1nsec.
In highly nonlinear amplifier, generally you don't have to worry about oscillation in large drive condition which is enough for Class-C,D,E,F operation.
Rather you have to care about possibility of oscillation in small drive condition or no signal condition.
You can evaluate any of Zin,Zout,{Z11,Z12,Z21,Z22} by PSS/PAC.
PSS/PSP is also useful for your case.
The Designer's Guide Community Forum - Mixer Simulation under Matched Conditions
There is no function for Direct Plot Form in PSS/PAC.
You have to calculate necessary quantity based on definition you like.
This is basically same as conventional AC analysis although PAC uses pacmag parameter in "port" or "vsource".
Here you have to use OCEAN function, "getData()" and "harmonic()", etc.
Youy can calculate any quantity by using "Voltage" and "Current".
The Designer's Guide Community Forum - s-parameter calculation using ac analysis
The Designer's Guide Community Forum - PAE obtained from PSS simulation exceeds 150 % - How come ?
Show me your netlist regarding analysis statements and signal source and load definition.
First of all, you have to understand PSS/PAC.Is there a step-to-step tutorial about using PSS+PAC that I can follow myself to measure/calculate the input/output impedance?[/U]
Basically yes.Or is this the only way I can measure input/output impedance of my nonlinear PA?
We use cookies and similar technologies for the following purposes:
Do you accept cookies and these technologies?
We use cookies and similar technologies for the following purposes:
Do you accept cookies and these technologies?