Couldn't access full transient simulation data

[bageduke]

I am doing long transient simulation for 100us. The simulation is
still running, but everytime when I tried to plot signal, it only
plotted up to 36us, but actually output log shows the simulation
already run more than 50us without any error, and the transient result
file size still keep increasing.

Have you ever seen this problem before? Does this mean the result is
corrupted? Or is there anyway I can fix the problem?

Thanks a lot.

 

[Andrew Beckett]

bageduke wrote, on 07/05/08 02:44:

I am doing long transient simulation for 100us. The simulation is
still running, but everytime when I tried to plot signal, it only
plotted up to 36us, but actually output log shows the simulation
already run more than 50us without any error, and the transient result
file size still keep increasing.

Have you ever seen this problem before? Does this mean the result is
corrupted? Or is there anyway I can fix the problem?

Thanks a lot.

Are you using IC5141 with spectre from an MMSIM release? If so, you probably
need to re-enable the "chunk" mode for writing PSF. In older spectre versions,
big files used to get split into 2Gbyte chunks, because large file support was
not particularly common in many OS versions. However, that's no longer true - so
spectre from MMSIM61 changed to write large transient PSF into a single big
file. However, support for reading such big files wasn't added into IC61 (I
think), and so if running a new spectre with IC5141, you need to do:

For Spectre writing PSF data:

setenv PSF_WRITE_CHUNK_MODE_ON true

For UltraSim writing PSF data:

setenv PSF_LARGE_FILE_ON false

Regards,

Andrew.

 

On Jul 7, 9:35 pm, Andrew Beckett <andr...@DcEaLdEeTnEcTe.HcIoSm>
wrote:

bageduke wrote, on 07/05/08 02:44:

I am doinglongtransientsimulation for 100us. The simulation is
still running, but everytime when I tried to plot signal, it only
plotted up to 36us, but actually output log shows the simulation
already run more than 50us without any error, and thetransientresult
file size still keep increasing.

Have you ever seen this problem before? Does this mean the result is
corrupted? Or is there anyway I can fix the problem?

Thanks a lot.

Are you using IC5141 with spectre from an MMSIM release? If so, you probably
need to re-enable the "chunk" mode for writing PSF. In older spectre versions,
big files used to get split into 2Gbyte chunks, because large file support was
not particularly common in many OS versions. However, that's no longer true - so
spectre from MMSIM61 changed to write largetransientPSF into a single big
file. However, support for reading such big files wasn't added into IC61 (I
think), and so if running a new spectre with IC5141, you need to do:

For Spectre writing PSF data:

  setenv PSF_WRITE_CHUNK_MODE_ON true

For UltraSim writing PSF data:

  setenv PSF_LARGE_FILE_ON false

Regards,

Andrew.

Hi Andrew,

I have a similar problem. I am simulating a sigma-delta converter and
only the first 19 clock cycles would be displayed, despite simulating
for 1024 or more, and the simulation clearly running through to
completion.

I enabled the above environment variables and found that I could see
the first 177 cycles in AWD - a vast improvement - and the entire
waveforms in Wavescan. But any calculator functions I do on those
waveforms are only using the first 177 cycles.

This does not appear to be related to the tran.tran file size - I have
tried using various errprst settings and only saving every 10 points,
etc.

Any ideas?

David.

 

[Andrew Beckett]

david.garner@dnae.co.uk wrote, on 09/03/08 17:18:

On Jul 7, 9:35 pm, Andrew Beckett <andr...@DcEaLdEeTnEcTe.HcIoSm
wrote:
bageduke wrote, on 07/05/08 02:44:

I am doinglongtransientsimulation for 100us. The simulation is
still running, but everytime when I tried to plot signal, it only
plotted up to 36us, but actually output log shows the simulation
already run more than 50us without any error, and thetransientresult
file size still keep increasing.
Have you ever seen this problem before? Does this mean the result is
corrupted? Or is there anyway I can fix the problem?
Thanks a lot.
Are you using IC5141 with spectre from an MMSIM release? If so, you probably
need to re-enable the "chunk" mode for writing PSF. In older spectre versions,
big files used to get split into 2Gbyte chunks, because large file support was
not particularly common in many OS versions. However, that's no longer true - so
spectre from MMSIM61 changed to write largetransientPSF into a single big
file. However, support for reading such big files wasn't added into IC61 (I
think), and so if running a new spectre with IC5141, you need to do:

For Spectre writing PSF data:

setenv PSF_WRITE_CHUNK_MODE_ON true

For UltraSim writing PSF data:

setenv PSF_LARGE_FILE_ON false

Regards,

Andrew.

Hi Andrew,

I have a similar problem. I am simulating a sigma-delta converter and
only the first 19 clock cycles would be displayed, despite simulating
for 1024 or more, and the simulation clearly running through to
completion.

I enabled the above environment variables and found that I could see
the first 177 cycles in AWD - a vast improvement - and the entire
waveforms in Wavescan. But any calculator functions I do on those
waveforms are only using the first 177 cycles.

This does not appear to be related to the tran.tran file size - I have
tried using various errprst settings and only saving every 10 points,
etc.

Any ideas?

David.

I've just found some issues related to changing the stop time when using SST2.
The problem seems to be that the wrong precision gets used if you lengthen the
stop time, and what can happen is that the x-values hit the 64 bit limit with
the original precision (summarizing it slightly). This is covered in CCRs 574546
and 517273 - for reference if you contact customer support.

This has just been fixed in IC 6.1.2.500.17 - but I don't believe it is due to
be fixed in IC5141 at the moment.

Probably the simplest thing would be to change the output format to PSF. Use
the following .cdsenv:

spectre.envOpts simOutputFormat string "psfbin"

or the following SKILL in your .cdsinit:

envSetVal("spectre.envOpts" "simOutputFormat" 'string "psfbin")

(note, you can't change this if you're already running ADE). You'll most likely
need to force a new netlist (Simulation->Netlist->Recreate) to ensure the
mappings are updated correctly.

Best Regards,

Andrew.