Designer’s Guide Community

cmos.analogvala

Community Member

Offline

Posts: 65
India

Long Cadence-Spectre Simulation Time
Apr 08^th, 2010, 9:30pm

We are trying to simulate 40,000 lines long netlist using spectre. This takes long time to simulate. We are using following configurations and tool setup.

Spectre sub-version 5.10.41.031208
Hierarchy: ICFB
Installationed ICFB: IC5141 ISR
OS: RHEL 4
We have tried using multi-threading option but enabling multi-thread option does not have any effect on simulation time. We tried to use this multi-thread option on RHEL5 machine. On this machine using 2 thread improve simulation time by only 25%. Is this the amount of improvement you generally with the increase in one thread ?
We found from some websites that this spectre version is old and we should install MMSIM7.2 and run spectre through that. How much performance improvement do you expect after installing MMSIM7.2?

Thanks
CA

Back to top

IP Logged

Andrew Beckett

Senior Fellow

Offline

Life, don't talk to
me about Life...

Posts: 1742
Bracknell, UK

Re: Long Cadence-Spectre Simulation Time
Reply #1 - Apr 11^th, 2010, 2:43am

Using MMSIM72 is an obvious first step - you may well get improvements from using that (spectre in IC5141 is very old - even though the date on the version you're using is only a couple of years old, spectre in IC5141 has had no development for 5-6 years).

Then in MMSIM72 you have Spectre Turbo and also APS (Accellerated Parallel Simulator) technology which allows significant speed improvements, and particularly in the case of APS, will take much more advantage of a multi-core machine (although it has significant speed improvments even without that). Note that these new technologies do not compromise accuracy to gain speed. High level info on this at http://www.cadence.com/products/cic/accelerated_parallel/pages/default.aspx.

You should also talk to your local Cadence office so that they can make you aware of the capabilities, and ensure that you're running the simulations appropriately (sometimes people tend to over-tighten tolerances, which may also be leading to slow simulation performance).

Regards,

Andrew

Back to top

IP Logged

ywguo

Community Fellow

Offline

Posts: 943
Shanghai, PRC

Re: Long Cadence-Spectre Simulation Time
Reply #2 - Apr 11^th, 2010, 7:54am

Hi cmos,

Sure the software version is important. As what Andrew said, the latest software makes a lot of progress.

We can explore the circuit and simulator options, simulation result/log files to find out the reason why it needs so long simulation time, too. I have a few points here.

Why do you think the simulation time is long? Do you have a reasonable comparison with that using other simulator, or other circuit?
It takes very long time to simulate some special circuit, like a PLL with very low bandwidth and very high oscillator frequency, a crystal oscillator with very, very high quality factor.
Overtight tolerance in simulator options
A few nodes that is not easy to approach convergence in the circuit. In the simulation log file, the iteration number is about 3 times of the convergent iteration number for a normal transient simulation.

Best Regards,
Yawei

Back to top

IP Logged

cmos.analogvala

Community Member

Offline

Posts: 65
India

Re: Long Cadence-Spectre Simulation Time
Reply #3 - Apr 11^th, 2010, 11:06pm

I find simulation time long because I am presently simulating only one third of my complete circuit and it's taking 48 hrs to complete transient simulation with stop time of 400ns.

No comparison with other simulators is done.
There are no PLLs in the circuit.
Accuracy parameters have default values

The problem I have to debug some functional errors and performance limiting factors in the circuit. For this I have to change some signals in stimuli and check the performance. Also have to change PVT corners and check the performance of the circuit. This is an iterative task. I can not do ultra-sim or some other simulations because that reduces the accuracy and I need to be able to measure delay difference of 100ps.

As rightly pointed out by Ywguo most of the time goes in finding appropriate initial conditions. This is because it's rc extracted netlist. There are large number of RCs in the netlist.

Are there some tricks to make spectre compute accurate initial conditions faster ?

Tricks to reduce number of RCs in the extracted netlist itself by using dangling R and float nets options in Assura rcx have already been used.

-CA

Back to top

IP Logged

Andrew Beckett

Senior Fellow

Offline

Life, don't talk to
me about Life...

Posts: 1742
Bracknell, UK

Re: Long Cadence-Spectre Simulation Time
Reply #4 - Apr 12^th, 2010, 9:41am

Yes, the "trick" is to try using "spectre +aps" from MMSIM72. DC convergence is noticeably improved with this, as well as being much better able to handle large parasitic networks (and large circuits in general). This will give you spectre accuracy, but with various techniques to improve simulation performance - things have moved on significantly over the last few years.

You also have the ability to use parasitic reduction within the simulator, but that's less likely to help you since you're already using that from the extractor.

You should ideally use the latest hotfix of IC5141 as well, so that you get the interface (in ADE for spectre) to allow APS to be used.

Regards,

Andrew.

Back to top

IP Logged

cmos.analogvala Community Member Offline Posts: 65 India	Re: Long Cadence-Spectre Simulation Time Reply #5 - Apr 18^th, 2010, 5:40am I think I am using latest hotfix of IC5141 icfb -W gives me following number 5.10.41.500.5.111 Is this latest hotfix? How to use spectre+aps through ADE? i.e. which option in ADE should be enabled or checked? -CA
Back to top	IP Logged

Andrew Beckett

Senior Fellow

Offline

Life, don't talk to
me about Life...

Posts: 1742
Bracknell, UK

Re: Long Cadence-Spectre Simulation Time
Reply #6 - Apr 19^th, 2010, 8:05am

That's not the latest version (by quite a way). IC5141 USR6 came out in October 2008, and you're using a hotfix build from before that (the "5" in the version number gives that away). The latest IC5141 hotfix is 5.10.41.500.6.141 .

You didn't say which version of spectre you're using. In order to take advantage of APS, you should use MMSIM72 - since something like December 2004, Cadence has shipped spectre separately from the IC stream (it's still in IC5141 because IC5141 was released earlier in 2004, before the decision was made to split out spectre from the IC stream; however, it doesn't have the many enhancements made in the 5-6 years between).

If you really are using such an old IC subversion and can't change (but can still use MMSIM72) you should be able to go to Setup->Environment and add "+aps" to the UserCmdLine option field in the UI.

It's cleaner though in the latest IC5141 hotfix though - you have a dedicated form under the Setup menu to control APS (and turbo) options, which make it very simple to use.

Regards,

Andrew.

Back to top

IP Logged

Andrew Beckett Senior Fellow Offline Life, don't talk to me about Life... Posts: 1742 Bracknell, UK	Re: Long Cadence-Spectre Simulation Time Reply #7 - Apr 19^th, 2010, 8:06am And you can check the version versions available on http://downloads.cadence.com Regards, Andrew.
Back to top	IP Logged

cmos.analogvala

Community Member

Offline

Posts: 65
India

Re: Long Cadence-Spectre Simulation Time
Reply #8 - Apr 29^th, 2010, 10:35am

Andrew ,

We were using following version of Spectre.
Result of Spectre -W 5.10.41.031208

We got license for MMSIM7.2 and simulated same netlist using spectre pointed by MMSIM. We found that the spectre with MMSIM takes more simulation time than Spectre using IC5141.

Here are the summery of results.

which spectre
/cad/cadence/test/package/tools.lnx86/spectre/bin/spectre

32_bit_old==Time used: CPU = 769 s (12m 49.3s), elapsed = 777 s (12m 57.0s),

64_bit_old==Time used: CPU = 769 s (12m 49.4s), elapsed = 791 s (13m 11.0s),
--------------------------------------------------------------------------------
----------------------------------------------------------------------
2. Newer version
which spectre
/home/MMSIM/tools/bin/spectre

32_bit_new==Time used: CPU = 990 s (16m 30.1s), elapsed = 999 s (16m 38.7s),

64_bit_new==Time used: CPU = 1.31 ks (21m 49.0s), elapsed = 1.32 ks (22m 1.5s),

Why so?

Thanks
-CA

Back to top

IP Logged

ywguo Community Fellow Offline Posts: 943 Shanghai, PRC	Re: Long Cadence-Spectre Simulation Time Reply #9 - May 27^th, 2010, 8:57am Good news that you have tried mmsim 7.2. In this thread, you said that it took over 48 hours for the simulation. Now it takes 12 or 13 minutes in your comparison. Do you simulate the same netlist? Would you please try again using your former circuit/netlist? Yawei
Back to top	IP Logged