Error with jre when loading corners tool
spectrallypure
seems to work well up to simple schematic simulations. However, when I
try to load the corners tool (Tools->Corners... in ADE) to test the
related models, I get the following error in the CIW:
sevCornersTool('sevSession3)
*Error* The jre process is not running; Unable to find the jre
executable.
The corner tool works fine however with other design kit (AMS 0.35).
Searching in the forum I found something related to corner analysis
and jre, and tried setting the following variable:
envSetVal("asimenv" "loadCorners" 'boolean nil)
But the problem persists and I get the same error message. Could
anybody please tell me what's going wrong here?
Thanks in advance for any help/ideas/etc.
Regards,
Jorge.
Andrew Beckett
What IC version are you running, and what OS are you running on? (including
version)?
What happens if you do this (don't start ADE):
1. In CIW type:
corCornersExport()
2. In CIW type:
sh("xterm &")
3. In the resulting terminal, check that CDS_MPS_SESSION is set:
env | grep CDS_MPS_SESSION
4. In the terminal that popped up, type:
cdsCorners showDialog blah
Does it give any errors about jre? Or do you get a splash screen, and then the
corners UI (if so, just exit it, because it won't work properly).
Regards,
Andrew.
spectrallypure
corners tool not loading seems to have disappeared; I believe I was
(mistakenly) testing the design kit with an account that had the
environment variables not properly defined. Today I tried again from a
fresh session and the corners tool loaded fine. I also tried the
commands you specified:
> 1. In CIW type: corCornersExport() (the CIW output is: t)
> 2. In CIW type: sh("xterm &") (a terminal window pops up)
> 3. In the resulting terminal, check that CDS_MPS_SESSION is set: env | grep CDS_MPS_SESSION (the ouput is:CDS_MPS_SESSION=icfb24191)
> 4. In the terminal that popped up, type: cdsCorners showDialog blah (the "loading corners information" window appears for a little while, and then the corners tool UI opens).
The problem now is that I get a lot of errors when trying to run the
corner simulation itself. This is what I am doing:
1. I have a simple cell with only one nmos transistor, with supply and
excitation included. The transistor used is "nmos2v" from the tsmc
library "tsmc18rf" (according to this component's CDF, the associated
model is "nch").
2. I start ADE and do a simple transient simulation. In the model
libraries setup I am just including the following file:
"/usr/local/software/tsmc/tsmc18rf_pdk_v13d/1P6M/tsmc18rf//../models/
spectre/rf018.scs", section "tt"
Everything works fine and I get the expected waveform at the output.
In the spectre output log I get no errors.
3. From the same ADE window of Step #2 I start the corners tool UI. It
starts without errors, and from it I load a PCF file with the
following contents (I created it from a sample file I found in the
design kit directories):
corAddProcess( "TSMC18MSRF" "./models/spectre" "multipleModelLib" )
corAddModelFileAndSectionChoices( "TSMC18MSRF" "rf018.scs" '("ff" "fs"
"sf" "ss" "tt" ) )
corAddCorner( "TSMC18MSRF" "typ" )
corSetCornerGroupVariant( "TSMC18MSRF" "typ" "rf018.scs" "tt" )
corSetCornerRunTempVal( "TSMC18MSRF" "typ" 25 )
The corners tool seems to be loading this PCF correctly, as I get no
errors in the procedure. A single corner column "typ" appears, with
the variables "rf018.scs" and "temp" set to "tt" and "25",
respectively. In the upper part of the UI, I read "Process:
TSMC18MSRF" and "Base Directory: ./models/spectre" (please note that
"./models" is a local link that points to the design kit's spice
models directory, and the "rf018.scs" file can be successfully
accessed under "./models/spectre/").
4. I use the option Simulation->Run to run start the corner
simulation. The errors I get change very slightly depending on the
version of Spectre I use. With version 5.1.0 I get the following
errors in the output log:
*******[start of output log - Spectre 5.1.0]*******
Command line: /usr/local/software/cadence/ic/tools.lnx86/spectre/bin/
32bit/spectre \
-env artist5.1.0 +escchars +log ../psf/spectre.out -format
sst2 \
-raw ../psf +lqtimeout 900 +param \
/usr/local/software/ams/dk_3.70/ams_v3.70/spectre/
ams_range.lmts \
+inter=skill input.scs
Loading /usr/local/software/cadence/ic/tools.lnx86/cmi/lib/4.0/
libinfineon_sh.so
Loading /usr/local/software/cadence/ic/tools.lnx86/cmi/lib/4.0/
libnortel_sh.so
Loading /usr/local/software/cadence/ic/tools.lnx86/cmi/lib/4.0/
libphilips_sh.so
Loading /usr/local/software/cadence/ic/tools.lnx86/cmi/lib/4.0/
libsparam_sh.so
Loading /usr/local/software/cadence/ic/tools.lnx86/cmi/lib/4.0/
libstmodels_sh.so
...
spectre (ver. 5.10.41.062906 -- 29 Jun 2006).
Simulating `input.scs' on uemcsrv.polito.it at 3:56:28 PM, Wed Feb 4,
2009.
Error found by spectre in `typ', during circuit read-in.
"/usr/local/software/tsmc/tsmc18rf_pdk_v13d/1P6M/models/spectre/
rf018.scs"
5087: Bad (or unacceptable) statement in the body of a alter.
"/usr/local/software/tsmc/tsmc18rf_pdk_v13d/1P6M/models/spectre/
rf018.scs"
5088: Syntax error in specification of `mismatch'.
"/usr/local/software/tsmc/tsmc18rf_pdk_v13d/1P6M/models/spectre/
rf018.scs"
5089: Bad (or unacceptable) statement in the body of a alter.
(...)
(...a lot more of these same errors...)
(...)
Error found by spectre during circuit read-in.
"/usr/local/software/tsmc/tsmc18rf_pdk_v13d/1P6M/models/spectre/
rf018.scs"
5098: Syntax error. Statement ignored.
"input.scs" 37: Syntax error. Statement ignored.
spectre terminated prematurely due to fatal error.
*******[end of output log - Spectre 5.1.0]*******
On the other hand, with Spectre 6.0.2 I get the following output:
*******[start of output log - Spectre 6.0.2]*******
Command line: spectre -env artist5.1.0 +escchars +log ../psf/
spectre.out -format \
sst2 -raw ../psf +lqtimeout 900 -maxw 5 -maxn 5 +param \
/usr/local/software/ams/dk_3.70/ams_v3.70/spectre/
ams_range.lmts \
+inter=skill input.scs
Loading /home/lagos/cds/tests/MMSIM_6.0/tools.lnx86/cmi/lib/64bit/4.0/
libinfineon_sh.so ...
Loading /home/lagos/cds/tests/MMSIM_6.0/tools.lnx86/cmi/lib/64bit/4.0/
libnortel_sh.so ...
Loading /home/lagos/cds/tests/MMSIM_6.0/tools.lnx86/cmi/lib/64bit/4.0/
libphilips_sh.so ...
Loading /home/lagos/cds/tests/MMSIM_6.0/tools.lnx86/cmi/lib/64bit/4.0/
libsparam_sh.so ...
Loading /home/lagos/cds/tests/MMSIM_6.0/tools.lnx86/cmi/lib/64bit/4.0/
libstmodels_sh.so ...
spectre (ver. 6.0.2.290 -- 27 Jun 2006).
Simulating `input.scs' on uemcsrv.polito.it at 4:12:35 PM, Wed Feb 4,
2009.
Using new Spectre Parser.
Error found by spectre during circuit read-in.
"/usr/local/software/tsmc/tsmc18rf_pdk_v13d/1P6M/models/spectre/
rf018.scs" 5087: Unexpected keyword "statistics".
"/usr/local/software/tsmc/tsmc18rf_pdk_v13d/1P6M/models/spectre/
rf018.scs" 5089: No master specified for instance `vthnmis'.
"/usr/local/software/tsmc/tsmc18rf_pdk_v13d/1P6M/models/spectre/
rf018.scs" 5090: Unexpected keyword "vary".
"/usr/local/software/tsmc/tsmc18rf_pdk_v13d/1P6M/models/spectre/
rf018.scs" 5090: No master specified for instance `dlnmis'.
"/usr/local/software/tsmc/tsmc18rf_pdk_v13d/1P6M/models/spectre/
rf018.scs" 5091: Unexpected keyword "vary".
"/usr/local/software/tsmc/tsmc18rf_pdk_v13d/1P6M/models/spectre/
rf018.scs" 5091: No master specified for instance `dwnmis'.
(...)
(...more of these same errors...)
(...)
"/usr/local/software/tsmc/tsmc18rf_pdk_v13d/1P6M/models/spectre/
rf018.scs" 5098: Unexpected end of block statement "}".
spectre terminated prematurely due to fatal error.
*******[end of output log - Spectre 6.0.2]*******
For both cases, the associated content of the file "rf018.scs" is as
follows (these lines belong to the section "tt"):
[*******...line 5086...*******]
statistics {
mismatch {
vary vthnmis dist=gauss std=1/1
vary dlnmis dist=gauss std=1/1
vary dwnmis dist=gauss std=1/1
vary toxnmis dist=gauss std=1/1
vary vthpmis dist=gauss std=1/1
vary dlpmis dist=gauss std=1/1
vary dwpmis dist=gauss std=1/1
vary toxpmis dist=gauss std=1/1
}
}
[*******...line 5099...*******]
Of course, the fact that the corner simulations fail puzzles me since
I am specifying the same model library and section that I used for the
simple transient simulation of Step #2. What could be going wrong? BTW
I am using icfb 5.1.0 on RHEL4.
Thanks again for any further help!
Regards,
Jorge.
P.S. I almos forgot. I have noticed that in the Spectre output logs
(look at the first lines) there is a reference to a file that does not
correspond to the TSMC design kit, but to AMS' design kit:
+param /usr/local/software/ams/dk_3.70/ams_v3.70/spectre/
ams_range.lmts
I don't know where this comes from nor if it has something to do with
the errors. It would be nice to know how could I correct my
environment definitions in order to correct this erroneous reference,
though!
Andrew Beckett
Hi Jorge,
Using spectre from IC5141 is probably asking for trouble - particularly with
model files that are expected to work with a newer version of spectre. Even
6.0.2 is pretty old, so I'd suggest using something more recent (MMSIM70 or
MMSIM71).
The front-end (the netlist parser/elaborator) in spectre changed between IC5141
and MMSIM60 (you could enable the new parser in IC5141, but by default it was
off), and that would explain the changes in errors.
With the TSMC model files, they have a statistics block in a model file section
which is switched out using a spectre capability called "altergroup" - a way of
altering a bunch of things at once. Currently switching statistics blocks via
altergroups is not supported.
The workaround is to set the following cdsenv setting:
spectre.envOpts useAltergroup boolean nil
or from your .cdsinit:
envSetVal("spectre.envOpts" "useAltergroup" 'boolean nil)
this effectively tells the corners tool to start a fresh simulation for each
point in the sweep, rather than trying to do it via an altergroup. This may even
fix it for the IC5141 case, but I'd probably stick to a newer MMSIM version if
you can.
As for the +param command line argument, you probably have:
spectre.envOpts paramRangeCheckFile string
"/usr/local/software/ams/dk_3.70/ams_v3.70/spectre/ams_range.lmts"
in a .cdsenv file somewhere. This ends up in the UI under Setup->Environment in ADE.
Hope that helps you hunt it down!
Regards,
Andrew.
--
Andrew Beckett
Senior Solution Architect - Cadence Design Systems Ltd (UK)
spectrallypure
Seriously, thanks for solving both problems!
Regards,
Jorge.
zg19...@gmail.com
I got some error infomation when start the corners tools in ADE.
And I tried the commands you specified ,at four step,it show me the
error information:
Exception in thread "main" java.lang.UnsatisfiedLinkError: /tools/IC5141USR5/tools.lnx86/jre1.42/lib/i386/libawt.so: /usr/lib/libXp.so.6: undefined symbol: _XEatDataWords
at java.lang.ClassLoader$NativeLibrary.load(Native Method)
at java.lang.ClassLoader.loadLibrary0(Unknown Source)
at java.lang.ClassLoader.loadLibrary(Unknown Source)
at java.lang.Runtime.loadLibrary0(Unknown Source)
at java.lang.System.loadLibrary(Unknown Source)
at sun.security.action.LoadLibraryAction.run(Unknown Source)
at java.security.AccessController.doPrivileged(Native Method)
at java.awt.Toolkit.loadLibraries(Unknown Source)
at java.awt.Toolkit.<clinit>(Unknown Source)
at java.awt.Dimension.<clinit>(Unknown Source)
at COM.cadence.seaStars.corners.Constants.initConstants(Constants.java:75)
at COM.cadence.seaStars.corners.Corners.main(Corners.java:37)
So,what's the problem? What should i do?
Thank you
Gong
yen...@gmail.com
Downgrade libXp version to libXp-1.0.0-15.1.el6
Download old libXp packages from Centor 6.3
#rpm -e libXp-1.0.2-2.1.el6.i686.rpm
#yum install libXp-1.0.0-15.1.el6.i686.rpm
#yum install libXp-devel-1.0.0-15.1.el6.i686.rpm