Fatal error: Illegal library definition found in netlist

I

irun2

Guest
Hi everyone! The model library is from my teacher, mix025_1.scs. When
I use for simulation, the spectre.out window show the info as below.
Can someone be kindly point out the reason why this happens? I've
google it but still I can't find the solution.

Command line:
/eda/cadence/tools.lnx86/spectre/bin/32bit/spectre -env
artist5.1.0 \
+escchars +log ../psf/spectre.out +inter=mpsc \
+mpssession=spectre2_1008_9 -format sst2 -raw ../psf
+lqtimeout \
900 input.scs
spectre pid = 1653

Loading /eda/cadence/tools.lnx86/cmi/lib/4.0/libinfineon_sh.so ...
Loading /eda/cadence/tools.lnx86/cmi/lib/4.0/libnortel_sh.so ...
Loading /eda/cadence/tools.lnx86/cmi/lib/4.0/libphilips_sh.so ...
Loading /eda/cadence/tools.lnx86/cmi/lib/4.0/libsparam_sh.so ...
Loading /eda/cadence/tools.lnx86/cmi/lib/4.0/libstmodels_sh.so ...
spectre (ver. 5.10.41_USR4.081106 -- 11 Aug 2006).
Includes RSA BSAFE(R) Cryptographic or Security Protocol Software from
RSA
Security, Inc.

Simulating `input.scs' on irun at 10:03:10 PM, Tue Apr 22, 2008.

Error found by spectre during circuit read-in.
"/home/milk/adelabic5/Models/mix025_1.scs" 54: Illegal library
definition
found in netlist

spectre terminated prematurely due to fatal error.
 
irun2 wrote:
Hi everyone! The model library is from my teacher, mix025_1.scs. When
I use for simulation, the spectre.out window show the info as below.
Can someone be kindly point out the reason why this happens?
Click to expand...
yep ...


Error found by spectre during circuit read-in.
"/home/milk/adelabic5/Models/mix025_1.scs" 54: Illegal library
definition found in netlist
Click to expand...
Line 54 in Teacher's mix025_1.scs ;)
 
On Apr 23, 4:14 pm, prime_number <prime_num...@yahoo.com> wrote:
irun2 wrote:
Hi everyone! The model library is from my teacher, mix025_1.scs. When
I use for simulation, the spectre.out window show the info as below.
Can someone be kindly point out the reason why this happens?

yep ...

Error found by spectre during circuit read-in.
    "/home/milk/adelabic5/Models/mix025_1.scs" 54: Illegal library
definition found in netlist

Line 54 in Teacher's mix025_1.scs ;)
Click to expand...
hi, I checked the mix025_1.scs and found that there's one line
written :library tsmclib. How can I solve it? Thanks a lot!
 
hi, I checked the mix025_1.scs and found that there's one line
written :library tsmclib. How can I solve it? Thanks a lot!
Click to expand...
Complain to your teacher ;)
 
Oh Yes, You've to blame your teacher, that's the best ever
occasion ;-)
More seriously ...

Check that your main TSMC model file is consistent, your file should
look something like :

simulator lang=spectre
library tsmclib
// Some data
section tt // This is an example
// Parameters ...?
// Models ... ?
// Subckts ... ?
// Statistics ... ?
// Include file/section ... ?
// Whatever else ... ?
endsection tt
endlibrary tsmclib

You have to ensure that :
'library' keyword is closed by 'endlibrary'
'section' by 'endsection'
'subckt' by 'ends'

A bit of perl/awk/skill_regEx/what ever else can easily do the check
for you.I'm perl-oriented myself ...

Enjoy !

Riad.
 
Hi, Riad. Thanks so much for your kindly and detailed reply!
I talked with my teacher and he suggested to find another model file
on the Internet! But you know that's so impossible! (the file it's
used for my graduate design)
I read that mix025_1.scs again and it has the same description as you
said, like endlibrary and ends etc.
I post it here hope it'll bring more info to you to help. Thanks!
Click to expand...
The file you just posted is technology data from a foundry which has most certainly be made
available to you and your organization under a non-disclosure agreement, which means that you
shouldn't disclose the data.

You seem to have no clue of what you are doing, and sadly the same goes for your teacher... I don't
understand why he seems to be leaving you in such a state of ignorance, it's like giving a car to
someone who can't drive, and not even tell him to avoid killing anyone.

It's not impossible to find model files on the net, (see http://www.eas.asu.edu/~ptm/,
http://pdk.cadence.com), but it's clear that whatever you will find on the net is not real foundry
data (except probably for what you just posted here) and will not allow you to get your circuit
fabricated.


Now coming back to your problem, my guess is that you're including the model file in the wrong way.
Please describe your setup (using ADE or spectre command-line ? How do you include the model file ? )


Stéphane
 
S. Badel wrote:
Hi, Riad. Thanks so much for your kindly and detailed reply!
I talked with my teacher and he suggested to find another model file
on the Internet! But you know that's so impossible! (the file it's
used for my graduate design)
I read that mix025_1.scs again and it has the same description as you
said, like endlibrary and ends etc.
I post it here hope it'll bring more info to you to help. Thanks!

The file you just posted is technology data from a foundry which has most certainly be made
available to you and your organization under a non-disclosure agreement, which means that you
shouldn't disclose the data.

You seem to have no clue of what you are doing, and sadly the same goes for your teacher... I don't
understand why he seems to be leaving you in such a state of ignorance, it's like giving a car to
someone who can't drive, and not even tell him to avoid killing anyone.

It's not impossible to find model files on the net, (see http://www.eas.asu.edu/~ptm/,
http://pdk.cadence.com), but it's clear that whatever you will find on the net is not real foundry
data (except probably for what you just posted here) and will not allow you to get your circuit
fabricated.


Now coming back to your problem, my guess is that you're including the model file in the wrong way.
Please describe your setup (using ADE or spectre command-line ? How do you include the model file ? )


St�phane
Click to expand...
Hi, I feel guilty after reading you reply. Yes, I'd not have posted
the .scs file in the group. The message is deleted now.
Back to your question, I just want to use the file for simulation of
my design! I launched the ADE and in Setup menu I chose the Design
then the Model Library..., I clicked browse and selected mix025_1.scs
and pressed OK. After the aftermath work was done( I mean the
Analyses, and the output to plot, etc), I started the simulation and I
got the "Fatal error"! Illegal library definition found in netlist !
 
Hi, I feel guilty after reading you reply. Yes, I'd not have posted
the .scs file in the group. The message is deleted now.
Back to your question, I just want to use the file for simulation of
my design! I launched the ADE and in Setup menu I chose the Design
then the Model Library..., I clicked browse and selected mix025_1.scs
and pressed OK. After the aftermath work was done( I mean the
Analyses, and the output to plot, etc), I started the simulation and I
got the "Fatal error"! Illegal library definition found in netlist !
Click to expand...
In setup model library, did you specify the section name (TT,SS or FF). ?

I think that's the problem...

StĂŠphane
 
Hi,

Y're learning the hard way ... Just be careful with the data provided
by the founderies ... Hope TSMC will not hunt you down for a 7 years
old model file that nobody care about nowadays ...
I'm rather blaming your teacher than yourself actually ... Anyway, Il
n'y a pas mort d'hommes (That's a French proverb ... Google if you
want ;-) )

Well, when you include inculde your file into your simulation
environment using : ADE -> Setup -> Model Libraries, you have to :
1. fill the "Model library file" field with the path to your .scs
file
2. In your case since you've many sections in your file, you have to
put the target section into the 'Section (opt.)' filed at the right as
mentioned by Stéphane.

The same subckts/models are defined in the different sections but with
different technology sets.
the naming convention for your sections is :
T = Typical
F = Fast
S = Slow

A section 'FF' means the date put into it are measured in the
conditions of a 'Fast' NMOS and 'Fast' PMOS.

If you want to MANUALLY run multiple simulation with TT, then FF, then
SS, then whatever section ..., one way to it is then :
. Include your .scs and specify TT as the desired section and then
click the 'add', this will insert a new line
Back to your section name and replace TT by FF, click add ... And so
on. You will then have as many lines as sections.
The last step, is to make only one 'ACTIVE' by selecting the line you
want and click the Enable/Disable buttons on the right hand side.
A '#' sign is added in front of each disabled line. Ensure than one
section only is enabled. You can than switch vack and forth between
your sections as your work evolves.
That's the manual way to do it ...

Enjoy yourself and please do mind the data you post on the net for the
futur ;-)
 
On Apr 27, 2:05 am, "S. Badel" <stephane.ba...@REMOVETHISepfl.ch>
wrote:
Hi, I feel guilty after reading you reply. Yes, I'd not have posted
the .scs file in the group. The message is deleted now.
Back to your question, I just want to use the file for simulation of
my design! I launched the ADE and in Setup menu I chose the Design
then the Model Library..., I clicked browse and selected mix025_1.scs
and pressed OK. After the aftermath work was done( I mean the
Analyses, and the output to plot, etc), I started the simulation and I
got the "Fatal error"! Illegal library definition found in netlist !

In setup model library, did you specify the section name (TT,SS or FF). ?

I think that's the problem...

Stéphane
Click to expand...
Yes, It's that causes the error! Thanks again!
 
On Apr 27, 5:32 am, Riad KACED <riad.ka...@gmail.com> wrote:
Hi,

Y're learning the hard way ... Just be careful with the data provided
by the founderies ... Hope TSMC will not hunt you down for a 7 years
old model file that nobody care about nowadays ...
I'm rather blaming your teacher than yourself actually ... Anyway, Il
n'y a pas mort d'hommes (That's a French proverb ... Google if you
want ;-) )

Well, when you include inculde your file into your simulation
environment using : ADE -> Setup -> Model Libraries, you have to :
1. fill the "Model library file" field with the path to your .scs
file
2. In your case since you've many sections in your file, you have to
put the target section into the 'Section (opt.)' filed at the right as
mentioned by Stéphane.

The same subckts/models are defined in the different sections but with
different technology sets.
the naming convention for your sections is :
T = Typical
F = Fast
S = Slow

A section 'FF' means the date put into it are measured in the
conditions of a 'Fast' NMOS and 'Fast' PMOS.

If you want to MANUALLY run multiple simulation with TT, then FF, then
SS, then whatever section ..., one way to it is then :
. Include your .scs and specify TT as the desired section and then
click the 'add', this will insert a new line
Back to your section name and replace TT by FF, click add ... And so
on. You will then have as many lines as sections.
The last step, is to make only one 'ACTIVE' by selecting the line you
want and click the Enable/Disable buttons on the right hand side.
A '#' sign is added in front of each disabled line. Ensure than one
section only is enabled. You can than switch vack and forth between
your sections as your work evolves.
That's the manual way to do it ...

Enjoy yourself and please do mind the data you post on the net for the
futur ;-)
Click to expand...
I've fixed the error using the method introduced by S. Badel. Thanks
for your comments!
I realized how serious it was to post the technology info here! I
won't do it again.
 
On Saturday, April 26, 2008 4:32:40 PM UTC-5, Riad KACED wrote:
Hi,

Y're learning the hard way ... Just be careful with the data provided
by the founderies ... Hope TSMC will not hunt you down for a 7 years
old model file that nobody care about nowadays ...
I'm rather blaming your teacher than yourself actually ... Anyway, Il
n'y a pas mort d'hommes (That's a French proverb ... Google if you
want ;-) )

Well, when you include inculde your file into your simulation
environment using : ADE -> Setup -> Model Libraries, you have to :
1. fill the "Model library file" field with the path to your .scs
file
2. In your case since you've many sections in your file, you have to
put the target section into the 'Section (opt.)' filed at the right as
mentioned by Stéphane.

The same subckts/models are defined in the different sections but with
different technology sets.
the naming convention for your sections is :
T = Typical
F = Fast
S = Slow

A section 'FF' means the date put into it are measured in the
conditions of a 'Fast' NMOS and 'Fast' PMOS.

If you want to MANUALLY run multiple simulation with TT, then FF, then
SS, then whatever section ..., one way to it is then :
. Include your .scs and specify TT as the desired section and then
click the 'add', this will insert a new line
Back to your section name and replace TT by FF, click add ... And so
on. You will then have as many lines as sections.
The last step, is to make only one 'ACTIVE' by selecting the line you
want and click the Enable/Disable buttons on the right hand side.
A '#' sign is added in front of each disabled line. Ensure than one
section only is enabled. You can than switch vack and forth between
your sections as your work evolves.
That's the manual way to do it ...

Enjoy yourself and please do mind the data you post on the net for the
futur ;-)
Click to expand...

Hi, I know this is an old discussion.

But can you tell me the Automatic way to cover all the process variations?
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top