Plotting gm Vs. time from PSS simulation (6.1.5-64b.500.11)

So...I must be growing older since I do not remember replying to myself in the past ;-)

Anyhow, I found out yesterday what the issue is. I was simulating using the 'High Performance Simulator -- APS'.

For some reason - I am in contact with the Support for this - it looks like the stored gm is just a DC value.

I had a glimpse yesterday and tried the same simulation with good ole Spectre and bam! My gm Vs. time was there!

Happiness!

Maybe this helps someone,

Michele 

Michele,

That sounds like a bug to me. This ought to work, so support should ensure that a CCR is filed to get this fixed.

That said, I tried to reproduce it with MMSIM12.1 ISR14, and for me I get the gm value saved during shooting in the pss_td database (as a waveform) even when using APS. This isn't true with harmonic balance, but then again that doesn't surprise me - with harmonic balance it would need to solve the gm as a harmonic series and then convert it back into the time domain - and it only computes the voltages and currents as a harmonic series.

Here's the netlist I used:

// test of saving gm during a pss analysis

model nch bsim4 type=n
model pch bsim4 type=p

MP1 (z a vdd vdd) pch w=2u l=0.5u
MN1 (z a 0 0) nch w=1u l=0.5u

Vz (a 0) vsource type=pulse period=40n width=20n rise=1n fall=1n val0=0 val1=1.5
Vvdd (vdd 0) vsource type=dc dc=1.5

save *:gm sigtype=dev devtype=bsim4
tran tran stop=200n
pss pss period=40n outputtype=all // harmonicbalance=yes

Regards,

Andrew.

Andrew,

yes I just sent my netlist to the Support via our internal channel. Will keep you posted here anyways.

I do not know which MMSIM version I am under (what's the command to see this?), just the Cadence version.

I could source from 500.4 to 500.15 but all gave me this (with APS).

By the way, I was under the impression that HB would not work for time rep of gm. Then why do you say 'harmonicbalance=yes' in your netlist?

Regards,

Michele 

Michele,

Type "spectre -W" or look at the top of your spectre output log - it will tell you the subversion you're using.

The harmonicbalance=yes in my netlist is commented out (it's preceded by // which is a comment).

Regards,

Andrew.

Surprised you're using the base MMSIM12.1 version - been quite a few hotfixes since then. However, with my netlist, that version works too - I get a waveform in the pss_td database for the gm.

Perhaps you can check? Run "spectre invpss.scs" and open the results in ViVA. Maybe there's some subtle difference in your testcase.

Regards,

Andrew.

Of course I meant "spectre +aps invpss.scs".

Andrew.

I like to encourage people to live on the edge now and again ;-)

In general I'd expect you to be running from ADE; obviously the benefit of a small command line example is that it's a bit easier to share in a forum like this (and I can throw it together in a few seconds). 

I look forward to hearing your findings!

Regards,

Andrew.

Thank you for fostering my growth Andrew ;-)

...And indeed, your netlist works like a charm! But what a crappy gm :-D

I then tried to use ADE instead of ADEXL for my circuit, however the result is the same: I get a curve with Spectre only. APS gives a sort of DC value out.

Same thing if I sim my circuit from the command line (now I'm a master :-)) 

I also noted that the whole sim setup is waaay faster when using cmd line. Ok, the circuit is two transitors but I got the impression that the processes *before* actual simulation took a fraction of the time.

Can you please point me to the help entries containing - possibly an overview - of topics like 'running Spectre from the command line' and directory structure...things like that.  Maybe the time has come for me to understand all this a little better.

Thanks,

Michele