negative real part of input impedance of a switched mode power amplifier?

[sharethewell]

I am designing a class E power amplifier working at 433MHz. It is a nonlinear power amplifier since the transistor works in nonlinear region (cutoff and triode).

I used ZM1 of SP analysis in Cadence to measure the input impedance of the PA and I got a negative value for real part. Is it normal for a nonlinear PA? Does it mean it's oscillating? I checked waveforms of all nodes and didn't see any oscillation. Don't know why.

 

[prcken]

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.

 

[sharethewell]

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.

Here is how I set it up the output stage:
**broken link removed**

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?

 

[pancho_hideboo]

is there any feedback caused this negative real part resistance?

Cgd of FET forms feedback.
And if effective load of FET is inductive, it could cause negative real part of Zin.

I checked waveforms of all nodes and didn't see any oscillation. Don't know why.

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 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?

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.

 

[sharethewell]

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.

Thanks. regarding inductive load of FET, the load of the CMOS does appear inductive since the series LC tank in the circuit is off tuned on purpose so that it appears inductive for higher Power Efficiency. So maybe that's why the input impedance of the output stage is negative. I simulated it again without excess inductance which means the LC tank is tuned at 433MHz. The Zin is positive now. So 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.

Regarding ZM1 or ZM(1), I call it this just because the function name in SP. See the picture below. Is this right?
**broken link removed**

---------- Post added at 07:05 ---------- Previous post was at 06:59 ----------

I can't understand a meaning of this sentences at all.
What do you want to mean ?

I mean I was suggested that I should set up the circuit so that the output terminal is open. 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). Otherwise, I don't know how to set the output end open while using port2 at the same time. Does it make sense?

 

[pancho_hideboo]

So 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.

Surely read The Designer's Guide Community Forum - Oscillation in PA

Anyway try to run Transient Analysis without input signal.

Regarding ZM1 or ZM(1), I call it this just because the function name in SP. See the picture below.
Is this right?

I got it.
But you have to understand that it uses OCEAN function "zm()" actually.

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).

Completely wrong.

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.

 

[sharethewell]

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.

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?

For Z11=ZP(1,1), it takes the output port as open circuit, right?

So Zin=ZM(1) is what I should use for measuring input and output impedance for my case.

 

[pancho_hideboo]

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?

Strictly speaking, not correct.

So Zin=ZM(1) is what I should use for measuring input and output impedance for my case.

Right.

Do you understand linear network parameters such as Z-parameters, Y-parameters, H-parameters and S-parameters ?

You don't seem to understand SP-analysis at all.
In SP-analysis, we have to define power port.
Here port1 is treated as signal source and port2 is treated as load generally.

Even if you set type of port1 and port2 as any type such as "sine" or "pulse" etc.,
SP-analysis is done with port1 as source resistance and port2 as load resistance.

SP-analysis calcluate S-parameters.
Z-parameters are calculated as post processing by using OCEAN function "zp()" in Cadence Spectre's Post Processing Environment.

Zin and Zout are also calculated as post processing by using OCEAN function "zm()" in Cadence Spectre's Post Processing Environment.

See the followings.
Impedance parameters - Wikipedia, the free encyclopedia
RF Cafe - S to h T Y Z Parameter Conversion

Again surely read basic text book on circuit theory.

The followings are general notes for you.

- Always describe correct tool's name and vendor's name which you use as tool or simulator.
- Don't do multiple posts which are same content.
- Don't request source code or behavioral model without any efforts.
- There are many simulators which have analyses called as PSS, PAC and Pnoise.
- Describe in detail with using correct terminologies.
- Warnigns are different from Errors.
- ADS is not name of simulator.
- There is no tool which name is Cadence.
- Don't use Direct Plot of Cadence ADE blindly without knowing definition.
- All gains in Direct Plot of Cadence ADE are "right", "true" and "practical" voltage gain.
- Don't mix up Simulation with Post Processing. They are completely different phase.
- MATLAB are different from Simulink.
- Learn measurements using actual instruments. Not "EDA Tool Play

 

[sharethewell]

Cgd of FET forms feedback.
And if effective load of FET is inductive, it could cause negative real part of Zin.

Thanks for all the information. It's very helpful.

As to the effective load of FET, it does appear inductive. This is needed for higher efficiency of the PA. Otherwise, the transient output waveform appears distorted in the excess inductance is removed. So here is the problem. 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. Do you know what I should do? Thanks again for your help.

 

[pancho_hideboo]

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.

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 ?

 

[prcken]

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.
but i think you do get positive value at certain lower frequency range.

 

[pancho_hideboo]

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.

Wrong.

See basic text book on RF amplifier.

Re[Yin]=gm*omega*Cgd*(Bload+omega*Cgd)/{Gload**2+(omega*Cgd+Bload)**2}

If Bload < -omega*Cgd, Re[Yin] will be negative.

Here Yload=Gload + j*Bload is effective load of FET.

 

[sharethewell]

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 ?

Thanks for the reply.

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?

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? How about Kr, B1f, NF and SP? Does it mean I can't use ZM(1) and ZM(2) of SP to measure input impedance of the nonlinear PA?

 

[pancho_hideboo]

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?

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.

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?

If you prefer Cadence Spectre, invoke PSS/PAC or PSS/PSP.
https://www.edaboard.com/threads/169169/

Next try to run LSSP.

 

[sharethewell]

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 setup the testbench as you said. I used Vpulse instead of Vdc as source in the schematic. I set the step signal period as 50ns and pulse width as 25ns. I used parametric sweep to sweep Amplitude of RF signal source from 0 to 2 Volts. The drain wave form of the transistor is shown below. Do you think it is oscillating? (It just shows the sweep from 0 to 1.1 V, the rest is about the same in waveform)
**broken link removed**

You suggested PSS+PAC to measure input impedance of the driver stage of the circuit. I took a look at the link you attached. Someone said I can plot Z11 from PSS+PAC. However, I couldn't find anything related to Z11. See the picture below, what function should I use for measuring input impedance? To be honest, I found little info about doing this over internet and very limited info from your link. Could you please give more details about measuring input impedance by using PSS+PAC? Thanks a lot.
**broken link removed**

 

[pancho_hideboo]

Do you think it is oscillating?

I can't obserbe any symptom of oscillation.

I set the step signal period as 50ns and pulse width as 25ns.

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.

Someone said I can plot Z11 from PSS+PAC.

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

However, I couldn't find anything related to Z11.
See the picture below,
what function should I use for measuring input impedance?

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.

The followings are general notes for you.

- Always describe correct tool's name and vendor's name which you use as tool or simulator.
- Don't do multiple posts which are same content.
- Don't request source code or behavioral model without any efforts.
- There are many simulators which have analyses called as PSS, PAC and Pnoise.
- Describe in detail with using correct terminologies.
- Warnigns are different from Errors.
- ADS is not name of simulator.
- There is no tool which name is Cadence.
- Don't use Direct Plot of Cadence ADE blindly without knowing definition.
- All gains in Direct Plot of Cadence ADE are "right", "true" and "practical" voltage gain.
- Don't mix up Simulation with Post Processing. They are completely different phase.
- MATLAB are different from Simulink.
- Learn measurements using actual instruments. Not "EDA Tool Play

 

[sharethewell]

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.

I tried with setting period as 2sec and pulse width as 1sec. For no signal condition, at the drain of the transistor, I got a square wave which is not oscillation. I tried to simulate it with Vpk =100mV (input signal) for 8 sec. It just took forever, so I stopped it in the middle, so as far as what I got, I didn't see oscillation. If you think I should wait that long to see the full result, I can do it.

Here is the netlist of the simulation when input signal is 0.
// Generated for: spectre
// Generated on: Oct 12 11:00:29 2010
// Design library name: RFPA
// Design cell name: PA3impedance
// Design view name: schematic
simulator lang=spectre
global 0 sub!
parameters Vpk=0 Cpal=2.1p C=7p f=433M

// Library name: RFPA
// Cell name: PA3impedance
// View name: schematic
T0 (net049 net028 0 sub!) dgnfet_rf l=240.0n w=800.0000u nf=50 m=1 par=1 \
ngcon=2 ad=1.76e-10 as=1.8816e-10 pd=822.000000u ps=855.52u \
nrd=0.0003 nrs=0.0003 rf_rsub=1 plnest=-1 plorient=-1 pld200=-1 \
pwd100=-1 lstis=1 lnws=0 rgatemod=3 rbodymod=1 gtab=1 ring=2 \
cwire=1 panw1=0p panw2=0p panw3=0p panw4=0p panw5=0p panw6=0p \
panw7=0p panw8=0p panw9=0p panw10=0p sa=6e-07 sb=6e-07 sd=4.4e-07 \
dtemp=0
VDD (net012 net013) vsource dc=1.2 type=dc
V0 (net022 0) vsource type=pulse val0=0 val1=1.2 period=2 delay=0 \
rise=0.1nsec fall=0.1nsec width=1
PORT1 (net011 0) port r=50 num=2 dc=0 type=dc
PORT0 (net028 0) port r=50 num=1 dc=558m type=sine freq=f ampl=Vpk \
pacmag=1 fundname="fund1"
I11 (net049 net022 0) inds x=300.0000u w=10u wu=15.0u s=5u n=15 bp=8 \
tlev1=3 tlev2=2 dtemp=0
I12 (net011 net041 0) inds x=290.00000u w=9.6u wu=15.0u s=5u n=15 bp=8 \
tlev1=3 tlev2=2 dtemp=0
CM10 (0 net011 sub!) dualmimcap l=8.5u w=149.51u c=9.000045p m=1 par=1 \
est=1 tlev1=3 tlev2=2 bp=3 setind=-2 rsx=50 dtemp=0
CM11 (0 net049 sub!) dualmimcap l=8.5u w=-500m c=Cpal m=1 par=1 est=1 \
tlev1=3 tlev2=2 bp=3 setind=-2 rsx=50 dtemp=0
CM9 (net049 net041 sub!) dualmimcap l=8.5u w=-500m c=C m=1 par=1 est=1 \
tlev1=3 tlev2=2 bp=3 setind=-2 rsx=50 dtemp=0
simulatorOptions options reltol=1e-3 vabstol=1e-6 iabstol=1e-12 temp=25.0 \
tnom=27 scalem=1.0 scale=1.0 gmin=1e-12 rforce=1 maxnotes=5 maxwarns=5 \
digits=5 cols=80 pivrel=1e-3 sensfile="../psf/sens.output" \
dochecklimit=no checklimitdest=psf
tran tran stop=8 errpreset=moderate write="spectre.ic" \
writefinal="spectre.fc" annotate=status maxiters=5
finalTimeOP info what=oppoint where=rawfile
modelParameter info what=models where=rawfile
element info what=inst where=rawfile
outputParameter info what=output where=rawfile
designParamVals info what=parameters where=rawfile
primitives info what=primitives where=rawfile
subckts info what=subckts where=rawfile
save PORT1 PORT0 VDD
saveOptions options save=allpub

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.

To be honest, I am not familiar with OCEAN script at all and never used it. Since my project is due soon so I don't know how much time it will take me to understand the script. Is there a step-to-step tutorial about using PSS+PAC that I can follow myself to measure/calculate the input/output impedance? Or is this the only way I can measure input/output impedance of my nonlinear PA?

 

[pancho_hideboo]

Is there a step-to-step tutorial about using PSS+PAC that I can follow myself to measure/calculate the input/output impedance?[/U]

First of all, you have to understand PSS/PAC.
So read document of PSS/PAC. You can see many documens in directory where Cadence Spectre is installed.

Or is this the only way I can measure input/output impedance of my nonlinear PA?

Basically yes.
Or use PSS/PSP.

Direct Plot Form of Cadence ADE is not useful and valuable for RF expert.
If you know Agilent ADS, you can easily understand this.

I can modify your netlist for Zin measurement using PSS/PAC.
But you have to calculate Zin by using calculator without using Direct Plot Form.