Welcome to EDAboard.com

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

spectre using hspice netlist

Status
Not open for further replies.

mitgrace

Full Member level 6
Joined
May 8, 2004
Messages
370
Helped
6
Reputation
12
Reaction score
2
Trophy points
1,298
Activity points
2,538
statement is not in spectre format

Dear All:

Does anyone know how to using spectre artisn to run Hspice netlist. Now I use the calibre to extraction the circuit, The output format is hspice netlist. I want to cosim using spectre, Does anyone know this flow ? How do I do it ? Thanks.
Anydocument or example.


mitgrace
 

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
you can extract spectre format netlist by calibre
 

Manoochehr

Junior Member level 3
Joined
Oct 11, 2001
Messages
27
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
160
I supose that you are looking for a way to simulate an SPICE netlist with spectre.
If this is the case, you should tranlate the spice netlist to spectre netlist with "spp" program that comes with spectre. This is spice pre processor of spectre, since spectre accepts spice netlist as well as spectre netlist. This program will generate an spectre netlist but you should fully check the worinings and errors.

Maybe you had to make some minor corrections on spice netlist to have good specre netlist.

I also recomend to fully verify the erros/warnings when you run specre on this netlist.
 

mitgrace

Full Member level 6
Joined
May 8, 2004
Messages
370
Helped
6
Reputation
12
Reaction score
2
Trophy points
1,298
Activity points
2,538
Dear Sir:

I use IC5141. This version can cosim with hsoice and spectre. It don't need to transfer the hspice to spectre. But I don't find any document with the feature. Does anyone have know the feature or document with IC5141 ? Thanks
 

nkchenliy

Junior Member level 3
Joined
Feb 11, 2004
Messages
26
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
149
You could write the statement of "simulator lang=spice" in the front of the model file with hspice, which change the simulator from Spectre to Hspice. But you must write "simulator lang=spectre" after the statements of ".include model_file", which change simulator back to Spectre again. Do you understand me?
 

hltong

Newbie level 5
Joined
Apr 29, 2006
Messages
9
Helped
1
Reputation
2
Reaction score
0
Trophy points
1,281
Activity points
1,332
You should add +spp option when simulation .
 

mitgrace

Full Member level 6
Joined
May 8, 2004
Messages
370
Helped
6
Reputation
12
Reaction score
2
Trophy points
1,298
Activity points
2,538
Dear nkchenliy :

Actually, I don't know what do u mean. can u said more detail or Can u give e the doc or exapmle . Thanks
 

Hughes

Advanced Member level 3
Joined
Jun 10, 2003
Messages
717
Helped
113
Reputation
226
Reaction score
25
Trophy points
1,298
Activity points
5,984
mitgrace said:
Dear Sir:

I use IC5141. This version can cosim with hsoice and spectre. It don't need to transfer the hspice to spectre. But I don't find any document with the feature. Does anyone have know the feature or document with IC5141 ?
1. You can use spp to convert the spice netlist to native spectre format; or
2. You can use spectrespp command to simulate the spice netlist: spectrespp yourdesign.sp

The "simulator lang=spectre" statement is not needed if the spice netlist file's extension is ".sp" (actually, any thing other than ".scs")

The document is "Virtuoso Spectre Circuit Simulator User Guide".
 

Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top