The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> Circuit Simulators >> spectre simulation error
https://designers-guide.org/forum/YaBB.pl?num=1166597796

Message started by xwcwc1234 on Dec 19^th, 2006, 10:56pm

Title: spectre simulation error
Post by xwcwc1234 on Dec 19^th, 2006, 10:56pm

Hi ,
I try to use Spectre to run a circuit and got the following messages:

Error found by spectre during circuit read-in.
"test.sp" 1: Syntax error in specification of `Fatal'.
Fatal error found by spectre during circuit read-in.
"test.sp" 2: SPICE Reader failure; see SPICE Reader
log file: "test.spplog"

Anyone knows what 's the problem of my spice file ?
Note : I mixed spice and Spectre netlist in one file , and use Bsim2v3 spice model file.

Title: Re: spectre simulation error
Post by Geoffrey_Coram on Dec 20^th, 2006, 4:45am

That error message seems to indicate that the first line of test.sp starts with "Fatal"

I think Berkeley Spice (and some commercial tools) treat the first line as a comment, even if it doesn't start with "*". You could try putting a * at the beginning of the first line. But you should also make sure that your netlist looks right -- maybe the program you used to generate the netlist had a Fatal error, and test.sp contains only the error notice rather than the netlist??

Also, I'm not sure you can mix Spice and Spectre in the same file -- I think you have to split the file and use an include command so you can specify the simulator lang= appropriately for each piece.

Title: Re: spectre simulation error
Post by Ken Kundert on Dec 21^st, 2006, 9:45am

Cadence provides a Spice to Spectre translator called spp that is called automatically by spectre when it sees a Spice netlist. I believe the Spice translator is generating a fatal error message that is some how getting into the netlist it is sending to Spectre, and then Spectre is treating the error message as a netlist statement. You might want to run spp stand alone on your netlist and use it to clean up the original Spice netlist. Once it is clean and generates no errors, you can run it through Spectre directly.

-Ken

Title: Re: spectre simulation error
Post by Andrew Beckett on Jan 12^th, 2007, 6:06am

In fact I'd recommend a newer spectre version (MMSIM60 or MMSIM61) which can natively read SPICE syntax without needing to go through the spp preprocessor. This is both quicker, has better error reporting, and more thorough.

In IC5141, you can add the +csfe command line switch, and it will invoke the new front-end parser (it was introduced in IC5141, but not made the default).

Regards,

Andrew.