hspice dump file limit problem

spectre waveform fsdb

Hi
sometime we need long times simulation for oscillatior circuit
.. but hspice have limit 2G for dump file
even though , I already use .option post=binary probe
but dump file sitll too large over 2G byte ...

someone said 64bit hspice can support large dump file ..

if I only want to dump top.x1.* ..
aditspice can use v(top.x1.*) .. but hspice can not support this command..


ps. I know some method use .tran 100u 500u 1u 600u ..
but I need simulation accuracy time for a long time , can not use this method

hspice format fsdb

andy2000a said:

Hi
sometime we need long times simulation for oscillatior circuit
.. but hspice have limit 2G for dump file
even though , I already use .option post=binary probe
but dump file sitll too large over 2G byte ...

someone said 64bit hspice can support large dump file ..

if I only want to dump top.x1.* ..
aditspice can use v(top.x1.*) .. but hspice can not support this command..


ps. I know some method use .tran 100u 500u 1u 600u ..
but I need simulation accuracy time for a long time , can not use this method

Click to expand...

Are you output only the required waveform using the probe command. If you use hsim you can output diferent waveforms to diferent fsdb files during the simulation bypassing the 2Gb problem, but its not so precise as hspice.

Hspice 64 bit can output larger dumpfile, but to read the result you need a 64 bit reader in a 64 bit operating system, since 32 bit architecture are limited by the 2Gb.

Hope this helps. Bastos

split fsdb files

Spectre split the result file into 2G pieces. But to view them could take hours on the old waveform tool. I did not test Wavescan delivered with IC5141. But look for a method to reduce the amount of observed signals. Normally for big toplevel circuits only some % of the signals has to be observed.

fsdb 2gb dump limit

andy2000a said:

Hi

if I only want to dump top.x1.* ..
aditspice can use v(top.x1.*) .. but hspice can not support this command..

Click to expand...

As I knew,
Hspice2001.* did not support the wildcard expression like you mentioned above;
however, Hspice2003.* did support it...

ex:
.option probe
.probe v(top.x1.*)

Regards,
Ryan

wdf fsdb

bastos4321 wrote:
Are you output only the required waveform using the probe command. If you use hsim you can output diferent waveforms to diferent fsdb files during the simulation bypassing the 2Gb problem, but its not so precise as hspice.

How to use hsim to dump different waveforms to differenct fsdb file bypassing the 2Gb problem?

+hspice +fsdb

grace said:

bastos4321 wrote:
Are you output only the required waveform using the probe command. If you use hsim you can output diferent waveforms to diferent fsdb files during the simulation bypassing the 2Gb problem, but its not so precise as hspice.

How to use hsim to dump different waveforms to differenct fsdb file bypassing the 2Gb problem?

Click to expand...

Acording to the hsim manual:

.print <tran> <name1=>ov1 <<name2=>ov2 ... >
<subckt=sub_name> <level=val2> <matchport=val3>
<outputres=val4> <adonly=1> <branch=name> <file=name>
<format=name>

Example:
.param HSIMOUTPUT=fsdb
.print v(n1) file=foo format=out
.print v(n2) file=bar format=wdf
.print v(n3)

In this example, v(n1) will be written to foo.out,
v(n2) to bar.wdf, and v(n3) to hsim.fsdb
(since that is the default output file according to the
HSIMOUTPUT parameter). Note that now for this feature
to be activated, the user must specify BOTH file=and
format=. If either one is missing, the results will be
printed to the default file.

Hope that helps. Bastos

hspice probe wildcard

Use a Sun machine,that will solve problem