Stats

  • Locked Locked
  • Replies 4
  • Subscribers 126
  • Views 16128
  • Members are here 0
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

PSS not completing in post extraction design

praveenmv

I want to run PSS, Pnoise and Pstb analysis on my design. The problem is PSS doesn't complete when I used netlist created from QRC extracted design (i.e. after layout). All the above analysis run if I do it on schematic level netlist.  The netlist size is around 18.6 MB and I have a lot of switching in my design for e.g. chopping. 

I did the following to solve this problem:
1. Optimization during RC extraction. I used many options under the 'filtering' tab in Assura QRC extraction window. For e.g. set the minimum R to 0.1 Ohm, reducing parasitics option etc. The size reduced to 10 MB but still the PSS doesn't complete.
2. I am using ++aps with circuit preset as 'sampled' and enabling post-layout optimization with legacy RCR.
However, PSS still does not complete.
The machine I am using has 32 GB RAM. I have added the link to spectre.out and cds log file.
Is there anything I can do to make it run? I am running PSS with tstab as 300u (circuit will take that much time to settle) and not saving the transient result.
Spectre.out:
cds.log
  • Dimitra Papazoglou

    Hi,

     Can you set the 'Post-Layout Preset Mode' to 'Legacy-RF RCR' instead of 'Legacy RCR' ? This will print +postlayout=legacy_rf out in the spectre command in the spectre.out log file. The legacy_rf is recommended to be used for RF analyses like pss as it uses algorithm dedicated for RF usage. 

    If the sim is still hanging, try to move to a latest spectre version as you are using an old one. The latest release is Spectre 17.1.0.198.isr3 at the moment . Keep legacy_rf to run the simulations.

    If the problem still insists, then I'd recommend you to file a ticket on customer support and provide your testcase. If you cannot provide a testcase then give information about the design that is used, the pss settings and any other settings/log files you have but it's hard to debug this without a testcase. 

    Regards,

    Dimitra

  • praveenmv
    in reply to Dimitra Papazoglou

    It didn't work with the first solution of setting Legacy RF RCR as a post-layout preset mode. Switching to another version is not possible, as that is given by institute. I am trying to run it on a machine with greater RAM as of now. 

  • praveenmv
    in reply to Dimitra Papazoglou

    Hi!

    I realized that PSS uses RAM to store data. When I ran the analysis on a machine with 256 GB RAM the analysis completed. However, it used up 242 GB of memory and thus there is no memory left for pnoise analysis. Any way in which I can point pss or pnoise to use disk space instead of RAM?

    Thanks!

  • Dimitra Papazoglou
    in reply to praveenmv

    Hi,

    You can use the swapfile option in PSS (only supported with Shooting Engine). With this option, the data that needs to be saved for the next iteration gets saved to a conventional file than the virtual memory. The data that the simulator is actually saving to the disk file is the series of solution matrices from PSS analysis.

    To use swapfile in ADE, open the PSS Choosing Analyses form and click on the 'Options' button. Go to Reuse tab to find the swapfile option. Enter <path_to_file>/swap_file_name there. 

    Note that with the version you are using (15.1 ISR5) swapfile is not supported with APS (+aps & ++aps). Spectre throws a segmentation fault when it's time for the pnoise analysis. You can either run the simulation with basic Spectre (but this might affect the simulation time) or move to Spectre 16.1 ISR7 & onwards where swapfile is supported with APS.

    However, since you have a machine with lots of RAM memory, the 64 bit spectre (without swapfile) is recommended - so what you are actually doing. So the real issue is why your testcase needs so much memory. Thus information of the type of circuit and the simulator settings you are using are needed to figure out what forces the tool to take so much memory. The best way is to provide your testcase to the Cadence support. What is needed to be provided is the input.scs file - if you cannot provide the whole netlist inside the input.scs at least provide the top level of it. 

    As said, you should contact Cadence support. I guess you might need to contact with the person who is in charge of Cadence tools at your site and ask how you can get support. 

    Regards,

    Dimitra

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.