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

about fully differential opamp simulation in hspice

Status
Not open for further replies.
L

lhlbluesky

Banned
Joined
Mar 30, 2007
Messages
558
Helped
5
Reputation
10
Reaction score
5
Trophy points
1,298
Location
china
Activity points
0
differential op amp

how to simulate the fully differential opamp in hspice? how to write the input stimilus in netlist?

i write:(vdd=3.3)
V1 vin+ 0 1.65 ac 1
V2 vin- 0 1.65 ac -1

it is wrong.

and i use vcvs to couple two ac small signal to the two inputs,
the result is wrong,too.

i want to know, how to write the right stimilus in the netlist?

can anyone help me, or give me some advice, thanks.
 

hspice fully differential

i think if you want to perform ac analysis, you can use of these sources as inputs:
V1 Vin+ 0 dc 1.65 ac 1
V2 Vin- 0 dc 1.65 ac 0
what's your mean about couple two ac small signal?both of Vin+ and Vin- are inputs of your circuit(you must define inputs of dif. opamp i.e gates of transistors with Vin+ and Vin-) thus vcvs is useless!
Good luck
 
fully differential op amp ac simulation

Hi,

A vcvs should actually work.

As an example, consider this

e+ 1 10 0 7 0.5
e- 2 10 7 0 0.5
vic 10 0 dc 0.9v

here 1 and 2 are connected to 2 input nodes i,e (gate of mosfets where differential input is applied)

All the best
 

phase margin opamp hspice differential fully

i haveused the following two methods:

V1 Vin+ 0 dc 1.65 ac 1
V2 Vin- 0 dc 1.65 ac 0

and

e+ 1 10 0 7 0.5
e- 2 10 7 0 0.5
vic 10 0 dc 0.9v
vac 7 0 dc 0 ac 1

but when i check the waveform of vout+ and vout-, i find their amplitude (at low frequency) is different, one is about 80dB, and the other is only 10dB or so, then why, or i was wrong, pls help me again. thanks.
 

full differential hspice

Dear lhlbluesky, i think standard form for ac analysis is first format and i used to this and i think results of these inputs are reliable.
 
fully differential ac simulation hspice

if i used the following inputs:

V1 Vin+ 0 dc 1.65 ac 1
V2 Vin- 0 dc 1.65 ac 0

then, when i check the output results, should i observe the waveform of vout+, vout-,
or (vout+ - vout-), pls?
 

hspice differential op

if you want to watch the differential output, you can use of .param as follows:
.param Vout=par('V(vout+)-V(vout-)').
for example if you want to find UGBW, you can use of Vout+ merely, then find a frequency that Vout+=0.5 or use of differential output and find a frequency that Vout=1.
besides you can use of these commands too:
.MEAS AC PM FIND VP(Vout+) WHEN VM(Vout+)=.5
.MEAS AC FU WHEN VM(Vout+)=0.5
.MEAS AC Gain max v(Vout+)
fist syntax is for phase margin(but you must plus PM with 180) .
second is for UGBW.
third is for gain.
 
fully diff amp need and some .options

if not set it
probe Vout+ and Vout- will =0

.options acout=0

default acount=1
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top