Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronic 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.

Problem about hspice simulation

Status
Not open for further replies.

winsonpku

Advanced Member level 4
Joined
Jul 7, 2005
Messages
119
Helped
6
Reputation
12
Reaction score
0
Trophy points
1,296
Activity points
2,351
Dear all:
Who can tell me how to save all the nodes's volatage in the circuit at one specified time when do the tran simulation?
For example,i do a tran analysis,".tran 2n 1u "then i want to konw the voltage of all the nodes in the circuit at 1.5u?

Best Regards
winson
 

Lantis

Junior Member level 3
Joined
Dec 29, 2003
Messages
31
Helped
3
Reputation
6
Reaction score
2
Trophy points
1,288
Activity points
298
try .op 1.5u
 

    winsonpku

    Points: 2
    Helpful Answer Positive Rating

flushrat

Full Member level 3
Joined
Jan 25, 2005
Messages
180
Helped
23
Reputation
46
Reaction score
8
Trophy points
1,298
Activity points
1,532
.op 1.5u
or
.save time=1.5u type=.nodeset/.ic file=xxx.ic level=all/top/none
 

    winsonpku

    Points: 2
    Helpful Answer Positive Rating

jluhzw

Member level 5
Joined
Nov 15, 2004
Messages
94
Helped
17
Reputation
34
Reaction score
4
Trophy points
1,288
Location
Hangzhou China
Activity points
759
hi flushrat is right
for more things about you can refer the hspice manual in "initializing dc/operating points point analysis"
there following is the about SAVE command.

.SAVE Statement
The .SAVE statement in HSPICE stores the operating point of a
circuit, in a file that you specify. For quick DC convergence in
subsequent simulations, use the .LOAD statement to input the
contents of this file. HSPICE saves the operating point by default,
even if the HSPICE input file does not contain a .SAVE statement. To
not save the operating point, specify .SAVE LEVEL = NONE.
You can save the operating point data as either an .IC or
a .NODESET statement.

SYNTAX:
.SAVE <TYPE = type_keyword> <FILE = save_file>
+ <LEVEL = level_keyword> <TIME = save_time>

Parameter Description
type_keyword Storage method, for saving the operating point. The type can be one of the
following. Default is NODESET.
• .NODESET: Stores the operating point as a .NODESET statement. Later
simulations initialize all node voltages to these values, if you use
the .LOAD statement. If circuit conditions change incrementally, DC
converges within a few iterations.
• .IC: Stores the operating point as a .IC statement. Later simulations
initialize node voltages to these values if the netlist includes the .LOAD
statements.
save_file Name of the file that stores DC operating point data. The file name format is
<design>.ic#. Default is <design>.ic0.
level_keyword Circuit level, at which you save the operating point. The level can be one of
the following.
• ALL (default): Saves all nodes, from the top to the lowest circuit level. This
option offers the greatest improvement in simulation time.
• TOP: Saves only nodes in the top-level design. Does not save subcircuit
nodes.
• NONE: Does not save the operating point.
save_time Time during transient analysis, when HSPICE saves the operating point.
HSPICE requires a valid transient analysis statement, to save a DC operating point. Default = 0.
 

    winsonpku

    Points: 2
    Helpful Answer Positive Rating
Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top