CDSSPICE OUT OF MEMORY

Hi All

I use to run the spectreS simulation (because the models I have can not be
easily translated into spectre model). I have some time to time a CDSSPICE
out of memory error message. This error could run for 5-10 minute before the
simulation can start.
Is there any command that will allow more memory for the CDSSPICE process
when we launch the analogArtist SpectreS ??

Thank you.

Tritue Truong

 

Add a Design Framework variable for spectreS initialization
in your .cdsenv or in your .cdinit file or type it direct
in the Command Interpreter input line before you start the
simulation.

-For the .cdsenv file use:

spectreS.init languageSize int 500

-For .cdsinit or direct in the CIW use:

envSetVal("spectreS.init" "languageSize" 'int 500)

Bernd

 

Thank you

I look for that fix for a long time. Cadence does not has any mention about
this bug in source link.

 

It's on sourcelink. I just searched in the solutions (with search set
to Boolean expression) for:

spectreS AND OUT AND MEMORY

and one of the hits was titled "Spice Socket Running Out Of Memory"
solution number 1812024

So I guess you didn't search successfully!

Regards,

Andrew.

 

If, somehow, your models can not be translated into spectre syntax,
does not mean that you have to netlist with cdsSpice. You can still use
spectre direct netlisting rather than spectre-sockets, and leave your
models in spice syntax. For example, I know of a designkit that contains
hspice models for device modelling and these are used in AHDL modules
(subcircuits) in the model library; thus no spectre syntax and it works
like a charm with spectre-direct.

Direct netlisting is an improvement for both designers and
eda-support. You could give it another go, and look at the migration
toolbox and its' manuals.

 

However, if the models are in cdsSpice syntax (which is the common state of play
for spectreS), then you will still need to translate them. cdsSpice != spice.

Also, you still need spectre simInfo in the CDF for the devices in your design
kit for them to netlist properly in the direct interface.

In many cases doing this translation is not hard (the conversion toolbox does
much of it), but some are loathed to use something other than was supplied
by the kit provider. Some companies design kits are so incredibly (I was going
to say ridiculously!) complicated and so this can be off putting if you're
worried about breaking things.

So, good idea, and it will work in some cases, but not all...

Andrew.

 

There is a tool called spp from Cadence to convert spice/hspice to
spectre format. See spp -help.

 

hi, I have met a similar problem. When I used hspiceS to extract spice netlist
for my circuit, lots of error message "Run out of memory, please run cdsSpice by
using -s option". And I had to kill the process of icfb.
What can I do? use "hspiceS.init" ???
Thanks for your help.

 

Yes, set the same variable, but use hspiceS.init instead of spectreS.init.

Regards,

Andrew.