How to use HSPICE trans input file

Status
Not open for further replies.
L

lordfire

Member level 1
Joined
Oct 19, 2004
Messages
36
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,286
Activity points
253
hspice .trans

such as a trans source

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


.tran 0.01n 30n


i don't know the accurate syntax
 

Code: 
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.
 

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
 

lordfire said:
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
Click to expand...

You may use data-driven PWL.
Code: 
V1 1 0 AC 1 0 PWL (time, vol)
With a data statement as,
Code: 
.DATA vector MER
FILE='vecfile' time=1 vol=2
.ENDDATA
The vector file 'vecfile' may look like:
Code: 
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
Code: 
.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.
 

Status
Not open for further replies.

Similar threads

Menu
Log in
Register
Cookies are required to use this site. You must accept them to continue using the site. Learn more…