Designer’s Guide Community

sugar

Community Member

Offline

Posts: 54

which is correct? spectre or hspice?
Sep 26^th, 2006, 7:26pm

I simulated a s-parameter package model in three ways and got three results.
- spectre rational interpolation method
- spectre spline interpolation method
- hspice
The stimulus is a 1v step vpwl with 50ohm source resistance.
The output of the package is connected to a 50ohm termination resistor.
Attached is the simulated waveform. Which tool should I believe?

Back to top

step_response.pdf

IP Logged

jbdavid Community Fellow Offline Posts: 378 Silicon Valley	Re: which is correct? spectre or hspice? Reply #1 - Oct 11^th, 2006, 10:51pm Why did you use an interpolation method for spectre? that is only needed for PSS and other shooting-newton Spectre_RF simulations.. Transient you can use sp data directly..
Back to top	jbdavid Mixed Signal Design Verification IP Logged

jbdavid Community Fellow Offline Posts: 378 Silicon Valley	Re: which is correct? spectre or hspice? Reply #2 - Oct 11^th, 2006, 10:54pm OTOH - they all look about the same to me.. (but hspice one looks less "smooth" - which makes sense since there is no interpolation going on.. )
Back to top	jbdavid Mixed Signal Design Verification IP Logged

sugar

Community Member

Offline

Posts: 54

Re: which is correct? spectre or hspice?
Reply #3 - Nov 12^th, 2006, 10:50pm

hi, jbdavid

thank you for your interest in this problem.

Let me explain in more detail.
To use a s-parameter model in spectre, we have to use 'nport' element of analogLib,
and also we should specify interpolation method which will be used by the simulator to
simulate the 'nport' element.

You said, "Transient you can use sp data directly.. ", seemingly, you are right,
but in fact, for transient simulation, the simulator has to first translate the s-parameter date
into time-domain data(by using some kind of interpolation method), and then carry out
the transient simulation. Am I right? Ken.

The simulation results are different.
The input is a step excitation, so after transient response, the output should be equal to the input,
but with spline interpolation method, the output is not equal to input, (that is not simulation accuracy
problem), so I think spline interpolation method might has some problems.

Rational method shows reasonable result, but it's transient response is different with Hspice
simulation result. The transient process is very important to me, so I have to make sure
which simulator is correct.

Back to top

IP Logged

Ken Kundert

Global Moderator

Offline

Posts: 2384
Silicon Valley

Re: which is correct? spectre or hspice?
Reply #4 - Nov 12^th, 2006, 11:39pm

Try Spectre's TDR analysis. It gives results in the time domain, but they are all based on AC small-signal analysis. The TDR should bypass any transient based algorithms and just use the raw S-parameters. It produces the step-response. Choose the transient results that are closest to the TDR results.

The TDR analysis is not a supported analysis in Artist, so you will have to access it by running Spectre stand alone (using a netlist). Use "spectre -h tdr" for details.

-Ken

Back to top

IP Logged

Andrew Beckett

Senior Fellow

Offline

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

Posts: 1742
Bracknell, UK

Re: which is correct? spectre or hspice?
Reply #5 - Dec 12^th, 2006, 2:52pm

There's also an application note on sourcelink which covers the various parameters for nport. Search for "nport application note" (the filename
is nportAN.pdf).

It's important that you have sufficient points in your s-parameter file, and that it has high enough bandwidth to cover the frequency of your input
signal and its harmonics. You probably should also use "usewindow=yes" on the nport (this is nearly always a good idea). Usually spline or linear are the right choices for interpolation method - even shooting PSS doesn't need rational these days, which is what rational was created for in the first place. spline and linear are similar, and use a convolution based approach - they just differ in the interpolation and extrapolation that is done.

Regards,

Andrew.

Back to top

IP Logged

OldHouseBlues

New Member

Offline

Posts: 4
Massachusetts, USA, Earth

Re: which is correct? spectre or hspice?
Reply #6 - Jan 17^th, 2007, 1:34pm

Hi, I'm new here ;)

I'll assume "Sugar" is still interested in some feedback. Modern versions of HSPICE (like 2006.09-SP1)
has several S-element options that can be used in transient analysis. I would recommend
interpolation=hybrid . This is explained in the Signal Integrity User Guide (release 2006.09).

BTW, HSPICE does interpolate for transient analysis (required for IFFT) and if required for AC analysis
(for frequency points that do not match that in the S-model).

Cheers.

Back to top

IP Logged

mg777 Senior Member Offline Posts: 131	Re: which is correct? spectre or hspice? Reply #7 - Feb 1^st, 2007, 7:11am The 200 ps delay seems to be due to a TEM line, so what are the wigglies just after t=0? Only the third plot (the one at the bottom) seems to be causal. When rational approximations are made by a simulator, is there any guarantee of physical realizability aka causality? M.G.Rajan www.eecalc.com
Back to top	IP Logged