hspice dc simulation problem

[homejack]

I want a dc simulation with Iin , but there are two nodes conneted to Iin.
Iin=-35ua~35ua, I0=20ua, In and Id are the outputs
how can I use dc simulation.
Any ideal ???
thank you!!

 

[hr_rezaee]

Hi
use better pic and explain more !!!
regards

 

[heyram123]

hey was a gud one... thnx

 

[hr_rezaee]

Hi
I don't understand your queation completely.
you want change Iin from .35u to 35u and then measure In and Id?
you have two Iin in your circuit.
ok
.param Iin=0
Iin1 0 nin1 Iin
Iin2 0 nin2 Iin
.dc Iin -35u 35u 1u

I think it will work.
regards

 

[homejack]

thanks !! i try it

 

[homejack]

this is the error
**error** element 0:iin has been
referenced but not defined
any ideal to solve it ??

Added after 2 minutes:

this is my sp file
*******typical library mode********
.protect
.lib 'c:\hspice work\rf018.l' tt
.unprotect
***********************************
.global vdd gnd
.temp 25
.param iin=0ua
*******voltage-current source******
vdd1 vdd gnd dc 1.8v
vxx vx gnd dc 0.9v
i0 vbias gnd dc 20ua
iin1 5 gnd iin
iin2 55 gnd iin
.dc iin -35ua 35ua 1ua
*************main circuit***********************
*************(+exp)csc**************************
mpp1 vbias vbias vdd vdd pch w=8u l=1u
mpp2 5 vbias vdd vdd pch w=17.75u l=1u
mpp3 2 vbias vdd vdd pch w=8.1u l=1u
mpp4 3 vbias vdd vdd pch w=12.75u l=1u

mpp5 3 3 vdd vdd pch w=8u l=1u
mpp6 6 3 vdd vdd pch w=8u l=1u

mnp1 2 2 4 4 nch w=25u l=5u
mnp2 4 4 gnd gnd nch w=25u l=5u
mnp3 3 2 5 5 nch w=20u l=5u
mnp4 5 5 gnd gnd nch w=50u l=10u
mnp5 3 5 gnd gnd nch w=50u l=10u
****************divider*************************
md1 11 vx gnd gnd nch w=43.5u l=10u
md2 6 66 gnd gnd nch w=43.5u l=10u
md3 12 13 11 11 nch w=32u l=4u
md4 13 13 6 6 nch w=32u l=4u
md5 12 12 vdd vdd pch w=31u l=4u
md6 13 12 vdd vdd pch w=31u l=4u
md7 66 66 vdd vdd pch w=10u l=5u
md8 gnd gnd 66 66 pch w=10u l=5u
*************(-exp)csc**************************
mp1 66 3 vdd vdd pch w=8u l=1u

mn1 66 55 vdd vdd pch w=48u l=10u
mn2 55 55 vdd vdd pch w=40u l=10u
mn3 66 55 gnd gnd nch w=48u l=10u
mn4 55 55 gnd gnd nch w=40u l=10u
************************************************
***********output-file-type*********************
.option post=binary
*******analysis type****************************
.op

.print dc vds(md2) id=par('is(md8)-id(md7)') id(mpp6)
.probe vds(md2) id(mp1) id(mpp6) id(md7) is(md8)
.probe id=par('is(md8)-id(md7)')
.probe vout=par('vds(md2)') voutdb=par('20*log10(vout)')
***********************************************
************************************************
.end

 

[evence]

.dc var1 .....
var1 should be name of current source (iin1 or iin2)
you may need a current control current source to creat another current input.

 

[homejack]

current control current source ??
how can i use it ?
please help me !! thanl you

 

[hr_rezaee]

Hi
yes it is true
another way:
use Current Controlled Current Source (CCCS)
http://www.ece.uci.edu/docs/hspice/hspice_2001_2-209.html
http://www.gnu.org/software/gnucap/man/node65.html
i think it will work.
regards

 

[homejack]

.option post = 2
*******typical library mode********
***********************************
.global vdd gnd
.temp 25
.param iin=0ua
*******voltage-current source******
v1 vdd gnd dc 1.8v
v2 vx gnd dc 0.9v
i0 vbias gnd dc 20ua
i1 nf1 gnd iin
f1 5 gnd nf1 gnd 1

**error** voltage source not found on above line

f2 55 gnd nf1 gnd 1

**error** voltage source not found on above line

.dc i1 -35ua 35ua 1ua

>error ***difficulty in reading input

there are 3 errors ?? Is "nf1" flooting??
any ideal to slove it
thank you!!

 

[hr_rezaee]

Hi
I'm sorry.
that was syntax of VCVS.
I corrected the previous post.
please read the above links.
I'm not sure
but check this:

i1 nf1 gnd iin
vdummy nf1 gnd 0

f1 5 gnd vdummy 1
f2 55 gnd vdummy 1


regards

 

[homejack]

That's OK !!!
thank you very much !!