Interfacing Spectre Output to MATLAB

Search in the MMSIM documentation (cdnshelp) for "Matlab Toolbox". It's in the  Virtuoso Spectre Circuit Simulator RF Theory manual.

Also there are app notes in <MMSIMinstDir>/tools/spectre/examples/SpectreRF_workshop/ which explain how to use this.

Andrew.

 Thnaks Andrew

Dear Andrew,

I went through the documents. 

But I am NOT able to configure the MATLAB tool-box.

MATLAB is unable to recognise the Spectre-Matlab ToolBOX command.

Can you please tell me what I should to do.

Thanks

Which version of MMSIM (spectre -W) are you using, and which version of Matlab? Which platform are you running on?

In my case, I ensure that I have spectre in my path, and do this (for csh; for bash you'd use "export MATLABPATH=...")

setenv MATLABPATH `cds_root spectre`/tools/spectre/matlab/64bit
setenv LD_LIBRARY_PATH `cds_root spectre`/tools/dfII/lib:`cds_root spectre`/tools/lib/64bit:$LD_LIBRARY_PATH

I'm running a 64-bit Linux OS, and running 64 bit Matlab, so as you can see I've ensured that I'm pointing at the 64 bit versions of the shared libraries.

That's all I need to do. 

Note that there was a problem in the early MMSIM10.1 versions (it was fixed in MMSIM10.1 ISR5) where there was a compiler incompatibility as described in solution 11699006

Regards,

Andrew.

Dear Andrew,

Thanks for your reply.

I did spectre  -W

I Got:-

sub-version 10.1.1.017

----------------------------------------

MATLAB Version we are using 7.12.0

Platform- RHEL5.5

In my "cadence.cshrc" file  the following is :-

-------------------------------------------------------------------------------------------------------------------------------------

setenv INSTALL_DIR /home/....../srv/install

setenv CADENCE_DIR $INSTALL_DIR/cadence

setenv MMSIM $CADENCE_DIR/mmsim10

setenv CDS_INST_DIR $CADENCE_DIR/IC5141

setenv LD_LIBRARY_PATH

set  LD_LIBRARY_PATH=($CDS_INST_DIR/tools/lib $LD_LIBRARY_PATH)

setenv MATLABPATH /home/....../srv/install/cadence/mmsim10/tools/spectre/matlab

setenv SPECTRE_FEATURE_FILE $MMSIM/tools/spectre/etc/files/spectre.dat

set path=($MMSIM/tools/spectre/bin $path)

----------------------------------------------------------------------------------------------------------------------------------

The issue I suspect is that MATLAB is not recognising the spectre commands like 'cds_srr' ..etc.

So how matlab can know about spectre. ?

I am confused...

Is there anything more to be added to the above .cshrc file ?

Thanks

 We are using 32-bit paltform

 The error I am getting while 'cds_srr' command in MATLAB window is:-

 ??? Invalid MEX-file '/home/manas/Cadence_install/srv/install/cadence/mmsim10/tools/spectre/matlab/cds_innersrr.mexglx': libvirtuos_sh.so: cannot open
shared object file: No such file or directory

Error in ==> cds_srr at 16
    sig = cds_innersrr(dirname);

That version (MMSIM10.1 Update release) is older than ISR5, and MMSIM10.1 versions prior to ISR5 had the problem you describe, due to the fact that the matlab toolbox was built using the Cadence supported compiler version, which was unfortunately incompatible with the supported compiler version for Matlab.

So you need to use a newer hotfix of the MMSIM10.1 release (or MMSIM11.1). From doing some tests, the newer toolbox no longer requires LD_LIBRARY_PATH to be set to the <MMSIM>/tools/lib dir - because it doesn't use those shared libraries (they would also have compiler incompatibility) - it doesn't do any harm if it's set, but it isn't required.

Regards,

Andrew.

 Thanks Andrew.

It did work with MMSIM11.1.

But the RF workshop documents you have referred is all baout RF plot .

But in my case I did simple ac analysis.  and I want to plot some ac signal in MATLAB.

 When I did signals = cds_srr(resdir,'ac-ac') in matlab, most of the AC signals are not being shown.

When I did :-

cds_plotsig(V4:p, '', '', db20)
??? Undefined function or variable 'V4'.

Can you tell me or refer to some document which actually gives some example for plotting/processing AC signals..

The <MMSIMinstDir>/tools/spectre/examples/SpectreRF_workshop/MatlabAN.pdf is less RF-centric (the toolbox was developed by the SpectreRF team, hence the RF focus of many of the examples).

To access AC results, you can do this:

% access the info about all the signals in the results
signals=cds_srr(resdir,'ac-ac')
% show the Voltage signal names
signals.V
% show the Current signal names
signals.I
% get the V4:p signal
V4_p=cds_srr(resdir,'ac-ac','V4:p')
% look at the details
V4_p.I
V4_p.freq
% plot the signal
cds_plotsig(V4_p,'','freq','db20')

for example.

I suspect that when you did the signals=cds_srr(...) it did list all the signals, but note that you probably got a horizontal scrollbar and may not have seen then all. However, looking at signals.I and signals.V should show everything. You certainly should see the same signals that you'd see in the results browser in ADE - and if they're missing there it would be because you didn't save the signals from the simulator.

Note that you could also plot the waveform directly yourself using:

plot(V4_p.freq,abs(V4_p.I))

this is the equivalent of using 'mag' instead of 'db20' in the cds_plotsig, except it doesn't label the axes and so on.

Hope that helps!

Regards,

Andrew.