(Hspice)How to slove this problem?

slove the problem

Today,I have simulated a single-ended differential amplifier with hspice.
I use one netlist file(i.e. one *.sp file) to multi-analysis ,so i make use of the "alter " sentence.
the netlist is as follows:

*differential single-ended amplifier test
.lib "E:\Hspice\model_csmc6\H06MIXDDCT02V21.LIB" TT


.subckt damp p n vdd vss vbias d2
m1 d1 p s1 s1 nmos l=1u w=2u
m2 d2 n s1 s1 nmos l=1u w=2u
m3 d1 d1 vdd vdd pmos l=1u w=2u
m4 d2 d1 vdd vdd pmos l=1u w=2u
m5 s1 vbias vss vss nmos l=1u w=2u
.ends

x1 p n vdd 0 vb out damp


*source
vdd vdd 0 5v
vb vb 0 1.5v

.alter
.connect p n
vdc p 0 2.5v
.dc vdc 0 5 1m

.alter
vsin p n dc=1 sin(0 10mv 1k 0 0 0)
vdc n 0 2.5v
.tran 1u 2m
.dc vsin -5 5 1m

.probe v(out)

.end

But i can not get the right curves.The analysis of the two .alter blocks affect each other,i think.because i got one tran and three dc analysis results.Moreover,the curves is not right in the results.
Are there syntax errores when i use the .alter ?
If i use one of the two .alter blocks separately,i will get the right results.

who can solve this problem??
thanks!!!!

hspice initialization problem

Try to put .probe statement before the last .alter statement.

lmax/lmin hspice

add the folowing massage:
.option post

and use awave or other wave tools

hspice alter site:edaboard.com

To pit1000:
"Try to put .probe statement before the last .alter statement. "


I have tried what you said,but it still have the problem.Nothing changed.

Seem that the dc analysis implements twice.
Is the ".connect p n" statement affect the simulation results?

the output *.lis file is as follows:

.alter
1 ****** HSPICE X-2005.09 (20050729) 18:51:42 10/25/2006 pcnt
******
*differential single-ended amplifier test
****** circuit name directory
******
circuit number to circuit name directory
number circuitname definition multiplier
0 main circuit
1 x1. damp 1.00
1 ****** HSPICE X-2005.09 (20050729) 18:51:42 10/25/2006 pcnt
******
*differential single-ended amplifier test
****** mos model parameters tnom= 25.000 temp= 25.000
******
***************************************************************************
*** model parameters model name: 0:nmos model type:nmos ***
***************************************************************************

*** general parameters ***
deriv= 0.
....................................................

1 ****** HSPICE X-2005.09 (20050729) 18:51:42 10/25/2006 pcnt
******

****** alter processing listing tnom= 25.000 temp= 25.000
******
.connect p n
vdc p 0 2.5v
.dc vdc 0 5 1m



.alter
$ alter processing continues $

**warning** model nmos
device geometries will not be checked against the limits set by
lmin, lmax, wmin and wmax. To enable this check, add a period(.)
to the model name(i.e. enable model selector).


**warning** model pmos
device geometries will not be checked against the limits set by
lmin, lmax, wmin and wmax. To enable this check, add a period(.)
to the model name(i.e. enable model selector).

1 ****** HSPICE X-2005.09 (20050729) 18:51:42 10/25/2006 pcnt
******
*differential single-ended amplifier test
****** circuit name directory
******
circuit number to circuit name directory
number circuitname definition multiplier
0 main circuit
1 x1. damp 1.00
1 ****** HSPICE X-2005.09 (20050729) 18:51:42 10/25/2006 pcnt
******
*differential single-ended amplifier test
****** mos model parameters tnom= 25.000 temp= 25.000
******
***************************************************************************
*** model parameters model name: 0:nmos model type:nmos ***
***************************************************************************

*** general parameters ***
deriv= 0.

*** level 49 model parameters ***
.............................................
Opening plot unit= 79
file=e:\hspice\differential_one.pa1

Opening plot unit= 79
file=e:\hspice\differential_one.sw0


***** job concluded
1 ****** HSPICE X-2005.09 (20050729) 18:51:42 10/25/2006 pcnt
******
*differential single-ended amplifier test
****** job statistics summary tnom= 25.000 temp= 25.000
******

total memory used 250 kbytes

# nodes = 7 # elements= 8
# diodes= 0 # bjts = 0 # jfets = 0 # mosfets = 5 # va device = 0

analysis time # points tot. iter conv.iter

op point 0.00 1 0
dc sweep 0.89 5001 10033
readin 0.06
errchk 0.03
setup 0.03
output 0.00
total cpu time 1.08 seconds
job started at 18:51:42 10/25/2006
job ended at 18:51:44 10/25/2006


1 ****** HSPICE X-2005.09 (20050729) 18:51:42 10/25/2006 pcnt
******

****** alter processing listing tnom= 25.000 temp= 25.000
******
vsin p n dc=1 sin(0 10mv 1k 0 0 0)
vdc n 0 2.5v
.tran 1u 2m

**warning** the above command card is not an acceptable alter card
if it is duplicate in comparison to previous input data.

.dc vsin -5 5 1m


.end
$ end of alter processing $

**warning** both nodes of source 0:vsin
are connected together

Opening plot unit= 79
file=e:\hspice\differential_one.pa2

Opening plot unit= 79
file=e:\hspice\differential_one.sw1

Opening plot unit= 79
file=e:\hspice\differential_one.sw2

1 ****** HSPICE X-2005.09 (20050729) 18:51:42 10/25/2006 pcnt
******
*differential single-ended amplifier test
****** operating point information tnom= 25.000 temp= 25.000
******
***** operating point status is voltage simulation time is 0.
node =voltage node =voltage node =voltage

+0ut = 3.6191 0 = 2.5000 0:vb = 1.0000
+0:vdd = 5.0000 1:d1 = 3.6191 1:s1 = 1.5860

Opening plot unit= 79
file=e:\hspice\differential_one.tr0


***** job concluded
1 ****** HSPICE X-2005.09 (20050729) 18:51:42 10/25/2006 pcnt
******
*differential single-ended amplifier test
****** job statistics summary tnom= 25.000 temp= 25.000
******

total memory used 410 kbytes

# nodes = 7 # elements= 8
# diodes= 0 # bjts = 0 # jfets = 0 # mosfets = 5 # va device = 0

analysis time # points tot. iter conv.iter

op point 0.03 1 12
dc sweep 2.50 5001 30045
transient 0.15 2001 806 403 rev= 0
readin 0.03
errchk 0.03
setup 0.03
output 0.00
total cpu time 2.89 seconds
job started at 18:51:42 10/25/2006
job ended at 18:51:47 10/25/2006


Init: hspice initialization file: C:\synopsys\Hspice_X-2005.09\hspice.ini
lic: Release hspice token(s)

opening plot unit hspice

Analysis statements can not be "altered"

redefine subckt +hspice

put .alter statements just before .end

hspice enable model selector

The reason in .connect can be valid. As far as I remember each following .alter uses input netlist from previous, instead of from head. Then in the last .alter nodes p and n shorted. It is possible to check up it, having rearranged both .alter places.

tot. iter in lis file in hspice

To pit1000:
Thanks for your help!As you said,each following .alter uses input netlist from previous, instead of from head.I also find similar statements in the hspice manual.But how to prevent the preview .alter statement change the netlist?Maybe it cann't,does have any other ways can implement multi-analysis in one *.sp file?

hspice .connect within .subckt

Probably only having refused use .connect, that is having refused change of nodes in the circuit. It is possible to try to simulate connection of units having connected them through very small resistance, and separation - through very big. Certainly all depends on specificity of the circuit.

hspice visual basic

dont use .connect
try to use a resister as
R1 n1 n2 0.01

and after .alter, redefine R1 as
R1 n1 n2 100meg

hspice dc analysis statement is duplicate

Thanks everyone,i will try to do what you said!