How to use HSPICE trans input file

[lordfire]

hspice .trans

such as a trans source

v1 1 0 ac 1 pwlfile ******


.tran 0.01n 30n


i don't know the accurate syntax

 

[Hughes]

V1 1 0 ac 1 pwl time1 val1
+ time2 val2
+ time3 val3
...
+ [R=timeX]
.tran timeStep stopTime [start=startTime]

Anything in the brackets means optional.

 

[wmlaketahoe]

it's seem OK to me

 

[lordfire]

i have witten a vector file
i want to introduce it to the simulate source
but it still seems WRONG

v1 1 0 ac pwl file='d:\lib\simsource.txt'

.tran 0.01n 30n

 

[Hughes]

i have witten a vector file
i want to introduce it to the simulate source
but it still seems WRONG

v1 1 0 ac pwl file='d:\lib\simsource.txt'

.tran 0.01n 30n

You may use data-driven PWL.

V1 1 0 AC 1 0 PWL (time, vol)

With a data statement as,

.DATA vector MER
FILE='vecfile' time=1 vol=2
.ENDDATA

The vector file 'vecfile' may look like:

1.0e-9  0.0
2.0e-9  0.0
2.1e-9  2.5
3.0e-9  2.5
3.1e-9  0.0
...

The transient analysis statement is

.TRAN DATA=vector

Another way is to modify the vector file to comply with the hspice pwl source sytax -- Add a line 'V1 1 0 AC 1 0 PWL' at the beginning; and add a plus sign(+) at the beginning of each line which defines time/value pair. Then including the modified vector file to the simulation netlist using hspice '.INCLUDE' statement.