How to simulate output impedance of cascode ckt in HSPICE

[Julian18]

Hi, there
I know some guy suggested to use .AC statement, what if i just want to see the the change of ro with respect to the change of other quantities, say, output voltage. how could i write my spice commmand..

TIA

Julian .

 

[yschuang]

Re: How to simulate output impedance of cascode ckt in HSPIC

Try TF analysis.

The .TF statement gives the small signal characteristics (gain, input impedance, output impedance) between a source and node. As an example:

.TF v(vout) Vin

would calculate the voltage gain, input impedance, and output impedance between the node vout and the source Vin

 

[CDRCDR]

Use a voltage source, sweep the voltage source in DC,and measure the current, you can get it

 

[Julian18]

Re: How to simulate output impedance of cascode ckt in HSPIC

Try TF analysis.

The .TF statement gives the small signal characteristics (gain, input impedance, output impedance) between a source and node. As an example:

.TF v(vout) Vin

would calculate the voltage gain, input impedance, and output impedance between the node vout and the source Vin

Thank you yschuang.
i did the .TF simulation, but i got 0 of output impedance, it seems that HSPICE just sweep every DC point and then calculate the DC output impedance of the ckt which is not what i want, I just want the small signal output resistance..

BTB, can i use some calculus calculation in my hspice deck?

 

[CDRCDR]

Re: How to simulate output impedance of cascode ckt in HSPIC

delta(Vds)/delta(Ids) will give you the output resistance,you can use some calculus or cadence caculator to get the small signal resistance

 

[Julian18]

Re: How to simulate output impedance of cascode ckt in HSPIC

delta(Vds)/delta(Ids) will give you the output resistance,you can use some calculus or cadence caculator to get the small signal resistance

Hi, CDRCDR:
u mean typing 'delta' directly in hspice file? i tried but seems hspice doesn't know 'delta', can u give me a piece of hspice deck so that i can see the usage of 'delta' function??

Thanks

 

[yschuang]

Re: How to simulate output impedance of cascode ckt in HSPIC

I guess CDRCDR tried to express delta(Vds)/delta(Ids) as derivative(Vds)/derivative(Ids)

 

[Julian18]

Re: How to simulate output impedance of cascode ckt in HSPIC

I guess CDRCDR tried to express delta(Vds)/delta(Ids) as derivative(Vds)/derivative(Ids)

Hi yschuang:
I tried to use "derivative", the result is the same as delta, no definition for "derivative" in spice...

 

[RDRyan]

Hi Julian18

In HSPICE, there isn't have dY/dx operator. so when you use derivative or delta in spice, it will go error.

CDRCDR means that you can display the output wave in some wavedisplay tools, then use the function of the tools to do calculation. In some tools like CosMosScope, it has many math operator which you can use.
In Cadence toolkit, it also has this similar functions.

 

[ch1k0]

Re: How to simulate output impedance of cascode ckt in HSPIC

.tf works, it give output and input small signal *resistance* , at operating point of DC analysis. Inductor is short, capacitor is open.

Output *impedance* is AC analysis. Put current src AC 1A in ouput cascode, do .ac , look at IM , IP of current src, you have frequency dependent output impedance.

 

[shobha89]

hai this is shobha.
i am doing my project "Designing Cascode differential amplifier".i need schematic diagram of cascode differential amplifier with length and width.presently i am using 0.18u technology in virtuoso.but whatever length and width which i gave ,was not getting output.i want to find gain.
the gain vs frequency curve should be as low-pass filter curve.pls can anybody help me.

 

[xwcwc1234]

Re: How to simulate output impedance of cascode ckt in HSPIC

hi ch1k0,
Can you provide a Spice file as example ?

 

[n1cm0c]

Re: How to simulate output impedance of cascode ckt in HSPIC

Use something like this to do the measurement,

itst 0 out DC 0 AC 1
.ac dec 10 1 1G
.param twopi = 2*3.14159265358979

then measure the small-signal (ac) voltage, and compute:
Ceff = imag(1/vac(out)) / (twopi* freq)

where "freq" is any frequency of the measured ac voltage.

This is because I = Y V, where the admittance Y is the parallel combination of the effective conductance and capacitance:
Y = Geff + j w Ceff
I = 1 (AC magnitude 1 on source itst)
Thus, Y = 1/V, and imag(1/V) = imag(Y) = w Ceff, so
Ceff = imag(1/V) *1/ (2 * pi * freq)

Apply a unit current, measure the voltage developed, the imaginary component is the reactance component. The output curve shows directly the output impedance over frequency.

freq can be the -3db frequency, or the frequency where the phase delay is -45 degrees, for example.