Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronic 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 simulate the output resistance of op-amp by hspice?

Status
Not open for further replies.

cqmyg5

Advanced Member level 4
Joined
Oct 21, 2003
Messages
118
Helped
3
Reputation
6
Reaction score
2
Trophy points
1,298
Activity points
963
Hello All,

I want to know the output resistance of a cascode op-amp, I need this output resistance for farther active filter design. How to get it by hspice simulation?

I tried the ".tf" command, it gave me a very small value, about 0.01.
 

flushrat

Full Member level 3
Joined
Jan 25, 2005
Messages
180
Helped
23
Reputation
46
Reaction score
8
Trophy points
1,298
Activity points
1,532
Re: How to simulte the output resistance of op-amp by hspice

Add ac source at the output, then run ac analysis

out_____||(C1)___+ (Vsource)

gnd_____________-

rout=v(out)/i(c1)
 

surianova

Advanced Member level 1
Joined
Sep 1, 2004
Messages
411
Helped
30
Reputation
60
Reaction score
8
Trophy points
1,298
Location
ASIA
Activity points
3,276
Re: How to simulte the output resistance of op-amp by hspice

cqmyg5 said:
Hello All,

I want to know the output resistance of a cascode op-amp, I need this output resistance for farther active filter design. How to get it by hspice simulation?

I tried the ".tf" command, it gave me a very small value, about 0.01.

1. you put a current source at the output ( from the output to gnd) and put AC=1.
2. Run AC analysis across frequecy.
3. Plot graph v(out) vs frequecy. You will be able to get output impedance.
 

muldersun

Member level 1
Joined
Dec 3, 2003
Messages
40
Helped
4
Reputation
8
Reaction score
2
Trophy points
1,288
Activity points
356
How to simulte the output resistance of op-amp by hspice?

I have tried this method, I think it's right. You can reference:
1. Connecting your OPAMP to buffer structure.
Run .TF, you can find the output impedance.
It's very small, because it's close loop output impedance.
2. Changing structure to run AC simulation.
You can get low frequency gain.
3. So, your open loop output impedance is:
Ro_closeloop*Avdc
You also can run .OP to prove this method.
I think it is right.
 

holddreams

Full Member level 6
Joined
Aug 2, 2005
Messages
351
Helped
15
Reputation
30
Reaction score
7
Trophy points
1,298
Location
Shanghai
Activity points
4,243
Re: How to simulte the output resistance of op-amp by hspice

In allen's book ,chapter 6,open-loop configuration, table 6.6-2, in the .lis file ,there is a "output impedance",

Then ,what's the relationship between this value and that others have discussed?

thx.
 

Status
Not open for further replies.
Toggle Sidebar

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top