Re: [SI-LIST] : About the AC analysis with HSPICE

Ray Anderson (raymonda@radium.eng.sun.com)
Wed, 1 Sep 1999 20:41:38 -0700 (PDT)

Rachild-

A couple comments on some of your questions:

We've seen the same phenomena where the measured loss of a line using
a network analyzer is more than the simulated loss. At this time
we don't have a real good answer, but it is looking like (at least in
our case) that some of the discrepancy is related to the fact that
the W element scales the skin loss as sqrt(freq) while we are seeing
losses in our measured data increasing directly with freq. We are still
investigating the root cause.

Also, if you have vias associated with your measured trace be sure to
account for parasitic effects (capacitive and inductive). These parasitics
are more significant as frequency increases and can cause a divergence
between measured and simulated data.

I'll defer to someone else on the details of the .NET statement as I'm at
home now and my Hspice books are at work except to say that I think the RIN
and ROUT parameters probably should be both set to 50 ohms if you are trying
to show software/hardware correlation with a 50 ohm network analyzer. Having
the wrong numbers will have two effects: it will cause a mismatch and hence
effect the ripple due to reflections, and the dB loss will not be correct.

The RLGC matrix values Ro,Lo,Co,Go,Rs,Gd will not change depending on the
frequency of analysis because:

Ro is a DC resistance so freq doesn't affect it.
Lo is a fixed number since the W element doesn't account for
frequency dependent inductance.
Co is a fixed number since W element doesn't account for
frequency dependent capacitance.
Go is fixed at the DC conductance
Rd is a normalized value that gets scaled by sqrt(freq) internal to the
W element. Rs = Ro + Rd
Gd is a normalized value that gets scaled directly with frequency
internal to the W element.

-Ray

> All Sirs,
>
> Thanks for your advice.But I still have some questions.
>
> I use the .AC analysis to simulate the high frequency loss of
> transmission line.I use the .NET option of the .AC analysis.I mainly
> simulate the S21 parameter. But I found that the loss DB between simulation
> and test (I test with HP network analyer) is more and more different with
> frequency increasing.The loss DB of simulation is less than that of test.I
> want to know the reason.The .sp file is following:
> ******************************************************************* .options
> probe post csdf .OPTION POST=1 ACOUT=1
> .OPTION BRIEF=0
> .OPTION SCALE=1u
> Vac nd_pin1 gnd ac 1v
> Rrerm cpin1 gnd 100k
> .NET V(cpin1) vac ROUT=50 RIN=50
> .AC DEC 100.00 30k 2000MEG
>
> Ws1 gnd nd_pin1 nd_pin2 gnd gnd gnd cpin1 cpin2 gnd gnd
> rlgcfile=hmbstrip42.rlgc n=4 l=14600mil
>
> .PRINT AC S11(DB) S21(DB)
>
> .END
> *************************************************************************
> The transmission line is from rlgcfile=hmbstrip42.rlgc which is extracted
> through :
>
>
> Vin1 nd_pin1 gnd pulse( 0v 3v 0.0n 0.3n 0.3n 2.15n 4.9n)
> Vin2 nd_pin2 gnd pulse(3v 0v 0.0n 0.3n 0.3n 2.15n 4.9n)
> *Vin1 nd_pin1 gnd pulse(0v 3.3v 0.0n 0.3n 0.3n 0.1n 4.8n)
> *Vin2 nd_pin1 gnd pulse(3.3v 0v 0.0n 0.3n 0.3n 0.1n 4.8n)
> *Vin3 nd_pin2 gnd pulse(0v 3.3v 0.0n 0.3n 0.3n 2.15n 4.9n)
> *Vin0 nd_pin4 gnd pulse(3v 0v 0.0n 0.3n 0.3n 2.15n 4.9n)
> .OPTION POST=2 ACOUT=1
> *.options brief = 0
> *.options probe post csd
> .options scale=1u
>
> Ws1 gnd nd_pin1 nd_pin2 gnd gnd gnd cpin1 cpin2 gnd gnd
> + Fsmodel=mother1 n=4 l=14600mil
> .material copper1 metal conductivity=5.96e+7 $inner
> .material copper2 metal conductivity=3.43e+7 $surface
> .material die_1 dielectric er=4.5 losstangent=1.7e-2
> conductivity=1.55e-7 .shape rect_1 rectangle
> width=10mil,height=1.38mil .layerstack stack_1 layer=(copper1,
> 1.38mil) layer=(die_1, 20mil ) layer=(die_1, 20.87mil ) layer=(copper1,
> 1.38mil) .Fsoptions wopt1 accuracy=high computegd=yes computers=yes
> computego=yes computero=yes printdata=yes gridfactor=3
>
> .model mother1 w modeltype=FieldSolver,layerstack=stack_1,fsoptions=wopt1,
> + rlgcfile='hmbstrip42.rlgc'
> + conductor= (material =copper1, shape=rect_1,origin=(0mil, 21.38mil))
> + conductor= (material =copper1, shape=rect_1,origin=(22mil,21.38mil))
> + conductor= (material =copper1, shape=rect_1,origin=(39mil, 21.38mil))
> + conductor= (material =copper1, shape=rect_1,origin=(61mil,21.38mil))
>
> .TRAN 100p 20n
> .end
>
********************************************************************************
> I want to know how should i assign values to 'ROUT' and 'RIN' in the .NET
> option of the .AC analysis of the HSPICE.I have seen that very different
> results can be got with different values of 'ROUT' and 'RIN'.What's the
> theory of .NET analysis to 'S21' in HSPICE?
> I also noticed that even i use different stimulus signals(100M,500M,1G or
> 2G) applying to transmission lines.There is no anything changed in the
> parameter matrix Ro,Lo,Co,Go,Rs,Gd.Why?How can i deal with these matrixes in
> exact frequency ?Perhaps it concerns somehow to the results of the loss of
> transmission line.
>
> Regards
>
> Rachild

**** To unsubscribe from si-list: send e-mail to majordomo@silab.eng.sun.com. In the BODY of message put: UNSUBSCRIBE si-list, for more help, put HELP. si-list archives are accessible at http://www.qsl.net/wb6tpu/si-list ****