Stats

  • Locked Locked
  • Replies 18
  • Subscribers 125
  • Views 21945
  • Members are here 0
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

ERROR [SFE-874]:'Unexpected end of line' while running a .scs file generated using ADE L, cadence Virtuoso v6.1.4 with spectre

Chandu D

Hi, 

I am trying to simulate a basic inverter circuit using spectre. I have generated a netlist file. when I run it, I am getting the following error

ERROR (SFE-874): "/home/eslam/ADETutorial_1/cds.lib" 2: Unexpected end of line. Expected equals sign, numeric value or string value.

For your referrence, I am posting the files 'cds.lib', 'input.scs' and 'spectre.out' here. Can someone help me out. Thanks in advance

*************cds.lib********************

#Following defined by Chandrasekhar DVS
DEFINE analogLib /usr/local/IC614/tools/dfII/etc/cdslib/artist/analogLib
DEFINE US_8ths /usr/local/IC614/tools/dfII/etc/cdslib/sheets/US_8ths
DEFINE basic /usr/local/IC614/tools/dfII/etc/cdslib/basic
DEFINE cdsDefTechLib /usr/local/IC614/tools/dfII/etc/cdsDefTechLib
DEFINE NCSU_TechLib_FreePDK15 $PDK_DIR/cdslib/NCSU_TechLib_FreePDK15
DEFINE ADETutorial /home/eslam/ADETutorial_1/ADETutorial
DEFINE SPECTRE_TUTORIAL /home/eslam/ADETutorial_1/SPECTRE_TUTORIAL
#DEFINE analogLib $CDS/IC/tools/dfII/etc/cdslib/artist/analogLib
#DEFINE US_8ths $CDS/IC/tools/dfII/etc/cdslib/sheets/US_8ths
#DEFINE basic $CDS/IC/tools/dfII/etc/cdslib/basic
#DEFINE cdsDefTechLib $CDS/IC/tools/dfII/etc/cdsDefTechLib

*****************************************

************* input.scs****************

// Generated for: spectre
// Generated on: Apr 21 11:31:37 2019
// Design library name: SPECTRE_TUTORIAL
// Design cell name: myInverterTB
// Design view name: schematic
simulator lang=spectre
global 0 vdd!
parameters VDD_VAL=0.8
include "/home/eslam/ADETutorial_1/cds.lib"

// Library name: SPECTRE_TUTORIAL
// Cell name: myInverter
// View name: schematic
subckt myInverter I O inh_bulk_n inh_bulk_p
I2 (O I inh_bulk_p inh_bulk_p) pmos
I6 (O I inh_bulk_n inh_bulk_n) nmos
ends myInverter
// End of subcircuit definition.

// Library name: SPECTRE_TUTORIAL
// Cell name: myInverterTB
// View name: schematic
I5 (IN OUT 0 vdd!) myInverter
V0 (vdd! 0) vsource dc=VDD_VAL type=dc
V1 (IN 0) vsource type=pulse val0=0 val1=VDD_VAL period=20p delay=0 \
rise=1p fall=1p width=9p
C0 (OUT 0) capacitor c=1f
simulatorOptions options reltol=1e-3 vabstol=1e-6 iabstol=1e-12 temp=27 \
tnom=27 scalem=1.0 scale=1.0 gmin=1e-12 rforce=1 maxnotes=5 maxwarns=5 \
digits=5 cols=80 pivrel=1e-3 sensfile="../psf/sens.output" \
checklimitdest=psf
tran tran stop=40p write="spectre.ic" writefinal="spectre.fc" \
annotate=status maxiters=5
finalTimeOP info what=oppoint where=rawfile
modelParameter info what=models where=rawfile
element info what=inst where=rawfile
outputParameter info what=output where=rawfile
designParamVals info what=parameters where=rawfile
primitives info what=primitives where=rawfile
subckts info what=subckts where=rawfile
save IN OUT
saveOptions options save=allpub

**********************************************************

***************spectre.out************


Cadence (R) Virtuoso (R) Spectre (R) Circuit Simulator
Version 7.1.1.187.isr11 32bit -- 18 Aug 2009
Copyright (C) 1989-2009 Cadence Design Systems, Inc. All rights reserved worldwide. Cadence, Virtuoso and Spectre are registered trademarks of Cadence Design Systems, Inc. All others are the property of their respective holders.

Protected by U.S. Patents:
5,610,847; 5,790,436; 5,812,431; 5,859,785; 5,949,992; 5,987,238;
6,088,523; 6,101,323; 6,151,698; 6,181,754; 6,260,176; 6,278,964;
6,349,272; 6,374,390; 6,493,849; 6,504,885; 6,618,837; 6,636,839;
6,778,025; 6,832,358; 6,851,097; 6,928,626; 7,024,652; 7,035,782;
7,085,700; 7,143,021; 7,493,240.

Includes RSA BSAFE(R) Cryptographic or Security Protocol Software from RSA Security, Inc.

User: root Host: localhost.localdomain HostID: 7F0100 PID: 5290
Memory available: 1.0215 GB physical: 1.9854 GB
CPU(1 of 2): CPU 0 Intel(R) Core(TM)2 Duo CPU T6600 @ 2.20GHz 2200.000MHz

Simulating `input.scs' on localhost.localdomain at 11:40:05 AM, Sun Apr 21, 2019 (process id: 5290).
Environment variable:
SPECTRE_DEFAULTS=-E
Command line:
/usr/local/IC614/MMSIM/tools.lnx86/spectre/bin/32bit/spectre \
input.scs +escchars +log ../psf/spectre.out +inter=mpsc \
+mpssession=spectre0_3079_6 -format sst2 -raw ../psf +lqtimeout \
900 -maxw 5 -maxn 5
spectre pid = 5290

Loading /usr/local/IC614/MMSIM/tools.lnx86/cmi/lib/5.0/libinfineon_sh.so ...
Loading /usr/local/IC614/MMSIM/tools.lnx86/cmi/lib/5.0/libphilips_sh.so ...
Loading /usr/local/IC614/MMSIM/tools.lnx86/cmi/lib/5.0/libsparam_sh.so ...
Loading /usr/local/IC614/MMSIM/tools.lnx86/cmi/lib/5.0/libstmodels_sh.so ...

Error found by spectre during circuit read-in.
ERROR (SFE-874): "/home/eslam/ADETutorial_1/cds.lib" 2: Unexpected end of line. Expected equals sign, numeric value or string value.
ERROR (SFE-874): "/home/eslam/ADETutorial_1/cds.lib" 3: Unexpected end of line. Expected equals sign, numeric value or string value.
ERROR (SFE-874): "/home/eslam/ADETutorial_1/cds.lib" 4: Unexpected end of line. Expected equals sign, numeric value or string value.
ERROR (SFE-874): "/home/eslam/ADETutorial_1/cds.lib" 5: Unexpected end of line. Expected equals sign, numeric value or string value.
ERROR (SFE-874): "/home/eslam/ADETutorial_1/cds.lib" 6: Unexpected end of line. Expected equals sign, numeric value or string value.
ERROR (SFE-874): "/home/eslam/ADETutorial_1/cds.lib" 7: Unexpected end of line. Expected equals sign, numeric value or string value.
ERROR (SFE-874): "/home/eslam/ADETutorial_1/cds.lib" 8: Unexpected end of line. Expected equals sign, numeric value or string value.
ERROR (SFE-874): "/home/eslam/ADETutorial_1/cds.lib" 9: Unexpected end of line. Expected equals sign, numeric value or string value.
ERROR (SFE-874): "/home/eslam/ADETutorial_1/cds.lib" 10: Unexpected end of line. Expected equals sign, numeric value or string value.
ERROR (SFE-874): "/home/eslam/ADETutorial_1/cds.lib" 11: Unexpected end of line. Expected equals sign, numeric value or string value.
ERROR (SFE-874): "/home/eslam/ADETutorial_1/cds.lib" 13: Unexpected end of file. Expected equals sign, numeric value or string value.

Time for parsing: CPU = 195.97 ms, elapsed = 347.244 ms.
Time accumulated: CPU = 243.962 ms, elapsed = 348.989 ms.
Peak virtual memory used = 552 Mbytes.


Aggregate audit (11:40:06 AM, Sun Apr 21, 2019):
Time used: CPU = 245 ms, elapsed = 350 ms, util. = 69.9%.
Time spent in licensing: elapsed = 177 ms, percentage of total = 50.5%.
Virtual memory used = 552 Mbytes.
spectre completes with 11 errors, 0 warnings, and 0 notices.
spectre terminated prematurely due to fatal error.

*********************************************************

  • Andrew Beckett

    By the way, your post went into moderation because it contained lots of repeated text, which is often a sign of spam. As soon as I'd reviewed it (after your feedback) I let it through.

    Two things here:

    1. You appear to be referencing the cds.lib in the Setup->Model Libraries in ADE. That makes no sense, because the cds.lib does not contain the definitions of the Spectre models, but instead is the definition of the library names used by Virtuoso for schematics, layouts etc. You need instead to reference the transistor models (which define the models for nmos, pmos etc). These probably will be in the PDK setup somewhere and have a .scs suffix, and if you look in the file will contain either "model nmos" or "subckt nmos" lines.
    2. You're using very old versions of the tools. Spectre 7.1 is from 10 years ago, and Virtuoso IC614 is probably a similar age (I can't remember off the top of my head, but we've had 4 major IC versions since then, and 10 major versions of Spectre). Why are you using such ancient versions? That's a little bizarre - even for a university. 

    Regards,

    Andrew

  • Chandu D
    in reply to Andrew Beckett

    Thank you Andrew. The input.scs files correspoding to models nmos and pmos are not present in the NCSU_TechLib_FreePDK15 folder I downloaded from the site. is there anyway to generate one by myself? The following are the pictures that show the files present in the pmos and nmos directories.

    Also about the software version, our institute does not have one. We had to go out of state and are working via VMware, accessing cadence virtuoso.

    Thanks in advance.

  • Andrew Beckett
    in reply to Chandu D

    It appears that this kit only comes with HSPICE models - not necessarily a problem though - these can be used for Spectre as well. The models are not within the library itself, but in a directory above the place the library is located.

    The HSPICE models are at $PDK_DIR/hspice/models/fet.inc . However, the models are called pfet and nfet not pmos and nmos, so the first thing you'd have to do is edit the properties of your transistors and change the model name:

    (the same would have been true if you'd been using hspice as the simulator - this seems to be an inconsistency in the PDK). 

    Then in ADE you can set this in the Setup->Model Libraries form:

    Ensure you pick "CMG" as the model section as that is the name of the library in the file. 

    Having done that, I can run a simulation with the nmos and pmos components from the library. 

    Regards,

    Andrew

  • Chandu D
    in reply to Andrew Beckett

    Thanks Andrew. All the previous errors disappeared but a new one appeared. It is as follows.

  • Andrew Beckett
    in reply to Chandu D

    Your spectre version is too old. Level 72 corresponds to bsimcmg, which didn't appear until MMSIM72 (2009) - the version after the one you're using. Expecting to simulate a FinFET design with 10 year old simulator technology is a bit optimistic...

    Mapping it to something else is not going to be that easy, since the number of fins is a parameter of this technology - so making up your own model is not going to work very well (nor is terribly realistic).

    You should contact whoever looks after the software installations you're using and ask them to install something more recent.

    Andrew.

  • Andrew Beckett
    in reply to Chandu D

    You posted earlier today about having found a new version, but that post seems to have vanished (did you delete it?).

    Anyway, to answer your question about how to sort out the UNIX path. First of all in the terminal window type:

    echo $0

    This will tell you the name of the shell you're running - it might be csh, bash, sh or ksh.

    If you know the full directory path to the SPECTRE or MMSIM installation, you can do:

    If csh:

    set path = (/path/to/MMSIM111/tools.lnx86/bin $path)

    or if sh/bash/ksh

    PATH=/path/to/MMSIM111/tools.lnx86/bin:$PATH

    You should then have spectre in your path - try typing "spectre -W" to check the subversion. Having done that, you can then run virtuoso and it would pick up the version of spectre you have.

    Regards,

    Andrew.

  • Chandu D
    in reply to Andrew Beckett

    Hello Andrew. I did delete it (sorry for that) but it was because we found a way to install it. After doing so, we again tried the simulation of inverter with NCSU pmos and nmos instances. However, the following happened.

  • Andrew Beckett
    in reply to Chandu D

    The warnings about ad, as etc are to be expected as the symbol doesn't really match up with the model (you'd have to take that up with the NCSU FreePDK group, if there is a group maintaining it...)

    I presume you edited the model file to change the names from nfet/pfet to nmos/pmos - but other than that, did you make any other changes? I'm presuming you did that because the error message is referring to instances of nmos.

    Please post your input.scs (it must be different from the one you posted originally, because that has the transistor instance lines not correctly defined). My simple inverter simulated fine with no convergence issues.

    Regards,

    Andrew

  • Chandu D
    in reply to Andrew Beckett

    We did not make any changes other than changing nfet/pfet to nmos/pmos. The following is the input.scs

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.