how to direct Virtuoso Visualization and Analysis XL to display all signals in single window/Strip?

This is something that (all being well) will be possible in IC618 (in ADE Explorer and Assembler) with waveform templates.

With OCEAN you should be able to control creation of new windows (using newWindow() ) and sub windows (using addSubwindow() ) by adding appropriate function calls. However, bear in mind that only signals with the same units will be plotted on the same axes, so you may need to add:

envSetVal("viva.depAxis" "flexible" 'string "true")
envSetVal("viva.indepAxis" "flexible" 'string "true")

Regards,

Andrew.

Thanks Andrew,

so when will IC618 be available? 

also as you mention about Ocean Script, I got problem with netlisting so haven't really rely on it yet. can you point me how can do re-netlisting from Ocean script? the Ocean script saved from ADE-L would rely on existing netlist which is not that self sustaining then.

thanks a lot,

David

Hi David,

It's currently scheduled for the end of Q3 this year. For the OCEAN script, you can change the design("/path/to/netlist") to design("libName" "cellName" "viewName" "r") to get it to netlist based on the lib/cell/view - and will renetlist if the design changes. The "r" is for read mode - can be omitted if you don't mind it opening the schematic (or config view) in edit mode.

Regards,

Andrew.

thanks Andrew,

now the Ocean script is re-netlisting and showing both digital and analog signals in single waveform all together. glad I asked and really appreciate your quick help.

thanks,

David

hi Andrew,

as mentioned upon, the ocean script does netlisting and "display" digital/analog signals in same waveform. but .... it's actually not quite displaying the right waveform yet and it prompts following error if run from CIW or not even run if from "ocean" prompt directly. but if I run same test from ADE (the ocean script was actually exported from ADE)  such signals plotted well. I guess there must be some setting missed from the ocean script. do you have comments or suggestions? p.s., attached my ocean scripts bellow as well.

thanks a lot,

David

--------------------------------error from CIW (If I haven't ever open up any schematic from fresh CIW, the same error from ocean prompt happens) -------------

*Error* Evaluating expression (getData("/test/abc")).
ERROR (WIA-1006): Unable to plot expression <getData("/test/abc")>
because it does not evaluate to an object that can be plotted, like a waveform or
parametric wave. See the Visualization & Analysis Tool documentation for information
about the types of objects that can be plotted in Visualization & Analysis Tool. Only
the expressions that evaluate to those objects can be plotted.

--------------------------------error from ocean prompt-------------

Loading simui.cxt
WARNING (OCN-6005): You do not have the required cellviews or properties open for this session.
You may have purged the data from virtual memory or the schematic data
has been closed. Type: simulator('simulatorName) to reset the
session or quit the application that you are using.
ERROR (ADE-5750): Unable to Simulate, either session is invalid or design is not specified.

---------------------------------------ocean script------------------------------------------------

simulator( 'spectre )
design( "demo" "test" "schematic" "r")

resultsDir( "~/simulation/test/spectre/config" )
modelFile(
'("/home/cad/libdists/p18/TSMC/...../models/spectre/cmn018_gp2a_5v_v1d4_usage.scs" "tt_lib")
)
analysis('tran ?stop "2u" )
desVar( "vio" 5 )
desVar( "vdd" 5 )

envOption(
'analysisOrder list("tran")
)
temp( 27 )
run()
selectResult( 'tran )
plot( v("/outp") )
plot( v("/outn") )
plot( getData("/test/abc")

a2d_test\.abc = awvAnalog2Digital(v("/test/abc" ?result "tran") nil nil 2.5 nil "centre")
plot( a2d_test\.abc ?expr '( "a2d_test.abc" ) )

I think I got a little clue here. there a few problems for me:

1. the error of "not have the required cellviews or properties open for this session" from fresh Ocean or CIW is because I haven't load the top level schematic yet so it doesn't know where to start with. I found some SKILL code (like dbOpenCellViewByType) to load the schematic and it'll be able to proceed. 

2. then additional problem is, I'm still at behavioral level yet (not all at schematic view based blocks) so I need the config to be loaded before the simulator knows which one to be netlisted with. w/o doing anything else beside design("libName" "cellName" "viewName" "r") would netlisting from all schematic views, not any other behavioral models like VerilogA blocks. so the simulation runs weird to me at the first glance. 

so, now my question is how I can guide Ocean to netlist according to the "config" view, not assuming all from schematic (only the very last stage regression might be all schematics)?

thanks a lot,

David

Hi David,

You really should not need to open the schematic first - this seems very strange to me and I don't recall ever seeing that as a problem before. Which subversion are you using? (what does getVersion(t) return in the CIW?)

To netlist using the config, you'd use:

design("libName" "cellName" "config")

i.e. the view name is the config you're using. Since the config knows the top level schematic, you don't need to tell it that as well (this is how ADE works too - the design is the config).

Regards,

Andrew.

hi Andrew,

yes, design("libName" "cellName" "config")  does the job. it's working now as standalone script by "ocean -replay top.ocn" from any linux terminal. 

w/o dbOpenCellViewByType( "Lib" "cell" "schematic" ), I would just get the following error which requires the top cell view available from memory. again I'd prefer it be able to run by standalone script so I don't even have to bring CIW up.  

WARNING (OCN-6005): You do not have the required cellviews or properties open for this session.
You may have purged the data from virtual memory or the schematic data
has been closed. Type: simulator('simulatorName) to reset the
session or quit the application that you are using.
ERROR (ADE-5750): Unable to Simulate, either session is invalid or design is not specified.

I saw you mentioned in your other forum discussion about this: 

https://groups.google.com/forum/#!topic/comp.cad.cadence/ZrAL85x2dMA

thanks,

David

That post just showed that I couldn't reproduce it without forcibly purging all the cellViews after the design() call and before creating a netlist. 

I did find a question CCR which turned out to be related to using a design management tool (don't know which) and using design in append mode  (i.e. not giving the "r" argument); that was (presumably - there was very little detail) presumably it causing the design to be checked out and replacing the version in memory - or something odd. I found only four references to this warning code in all cases and CCRs, and nothing recent.

There was one related to licensing - are you getting any licensing warnings when you're running the OCEAN script? Also, does it work OK if you use "ocean -restore top.ocn" instead of -replay? (I tend to recommend using -restore rather than -replay for various reasons).

Regards,

Andrew.

hi Andrew,

yes, -restore does the trick, again. I didn't have license or other problem. what's the difference between -restore and -replay?

although, if I load the same script from ocean prompt, such error is still there. should I use some other command there as well?

% ocean

ocean> load("top_sim.ocn")

WARNING (OCN-6005): You do not have the required cellviews or properties open for this session.
You may have purged the data from virtual memory or the schematic data
has been closed. Type: simulator('simulatorName) to reset the
session or quit the application that you are using.
ERROR (ADE-5750): Unable to Simulate, either session is invalid or design is not specified.

thanks,

David