Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

how to get imput impedence waveform from Cadence

Status
Not open for further replies.
E

ethan

Member level 3
Member level 3
Joined
Jul 7, 2004
Messages
67
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,286
Activity points
942
I simulated a single NMOS transistor and got the waveforms from transient and AC analyses. But I am not sure how can I get input/output impedence waveforms from Cadence by using calculator.
say for common-gate topology,
use VF(source)/IF(source)? but it seems Cadence complains that IF(source) is not a waveform object.

or use VT(source)/IT(source)? But this is not small-signal analysis?

Many thanks.
 

Why don't you try S-Parameter simulation? Or Z , Y parameter simulation?

You may also try to connect a ammeter at the input of your circuit and then you can simulate input or output impedance of your circuit??

There is also a calculator and you can divide your results in that..
 

It seems you didn't save AC terminal currents
In Analog Design Enviroment window click
Otput -> Save all -> Select AC terminal currents (userprobes) ->"yes"
After that you can plot VF/IF.
 

u need to connect 2 "psin" ports to the input and one to the output and do a s-paramter analysis. read it up in the manual..its easy to do it.

then after simu plot s11 and s22 in the smith chart form alone!!!

then u can move ur pointer along the curve of s11 and s22 and get

Zin/50 and Zout/50...but please be cautioned that ur Zin/Zout is the impedance calculated with a 50ohm load connected at the output/input respectively.....
 

An easy way to do it, if you're not familiar with s parameters and you have problems with calculator expression, is to put an ac current source with AC=1 at the pin you want to measure the impedance and perform an ac simulation over your interesting frequency range, then plot the voltage at input pin (as mag and/or phase). Being Z=V/I with I=1, Z=V.
Just be aware of the current flow, if wrong you'll get opposite phase results.
That's all.
Mazz
 
Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top