System stimulus data in Cadence

[nxing]

Hello everybody,

I am using verilogA to generate some sort of analog waveform as the stimulus for my system. However, only the output of stimulus block after some time (since there is delay the very beginning and running the whole system is very time-consuming) are useful and I am thinking to write the stimulus data to a file and then use the data to generate the waveform I want. Is it possible? If yes, how?

Thanks!

 

[hoangthanhtung]

using vpwlf in cadence

I think that cadence tool supports writting the stimulus data to a file and then use the data to generate the waveform. However, depend your version of Cadense software, full version A/D PSPICE or custom version. This is my opinion, you can search in help document of ORCAD to find more information. Good luck

 

[santhoshv78]

ipwlf cadence

yes..You can do that..
One way to accomplish this is by printing the values of the waveform
into a file using the calculator's printvs button. This button will print
out a waveform, as an x/y pair. You can then use this file as the input
to a vpwlf/ipwlf (Piece-wise linear voltage/current source from file)
device in analogLib.

Here are the specific steps required:

1) Open your Waveform.

2) Open the Calculator and click on button "wave" and then
choose the waveform. It will bring the waveform expression
into the Calulator buffer.

3) With the waveform expression in the calculator, click
on the PRINTVS button. The calculator will ask you for the
start, stop, and number of steps to use. Enter the start, stop, and
step and OK the Form. It will display the tables for the waveform in the
"Results Display Window". Now click on Expressions->Display Options.
In the Display Options form, set the Format to Scientific and click Apply.
Now you see the values in Scientific notation. Print these values to
a file by clicking on Window->Print. In the Print form set PrintTo to File
and give the fileName. You can use this filename in your vpwlf source.


4) Add a vpwlf device from AnalogLib to your schematic.
For each of these devices, you will need to specify a filename
to be used for the device. If you do not specify an explicit path
to the file, the file is assumed to reside in the netlist
directory. You cannot use the "~" shortcut for your home directory.
It is usually a good idea to use full pathnames. Enter the file name
in the PWL file Name field of the "vpwlf" component and continue
with your simulations.


If you are using an OCEAN script, you can use "ocnPrint" to print
the values of the waveform into a file.

Hope this will help.