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

Rachild Chen (rachel.chen@huawei.com.cn)
Fri, 03 Sep 1999 08:40:14 +0800

This is a multi-part message in MIME format.
--------------EC97E5719500E3745D9DC533
Content-Type: text/plain; charset=us-ascii
Content-Transfer-Encoding: 7bit

All sirs,

Thanks for your help.Now I understand why AMP simulate the GigaBits by RLGC(a EDA tools not a parameters) transmission line model in Hspice.I will try it by Ansoft.

Waiting for my results.

Best Regards,

Rachild

Dmitri Kuznetsov wrote:

> Rachild,
>
> The main cause of underestimated loss in your testcase is the Hspice's
> fieldsolver that extracts RLGC parameters from the input geometry. For
> ac analysis, the transmission-line model just uses the exact analytical
> solution for the given RLGC.
>
> The recent Rs correlation in SI reflector has shown that the Hspice's
> field solver produces Rs that is almost a factor of 2 smaller than Rs'
> from other fieldsolvers. This is because it assumes constant current
> distribution for Rs calculation whereas other quasi-static field solvers
> employ the perturbation approach which is more accurate at higher
> frequencies.
>
> The field solver I put into Hspice was written by TMA and uses my
> exponential approximation technique to accelerate solution for
> multilayered dielectric. As a result, it runs orders of magnitude
> faster than other fieldsolvers if you have many different dielectric
> layers. The same technique is used by Cadence's DFSigNoise. It is very
> good for quickly extracting large boards. If you want accurate
> wide-range correlation with measurements, you should use a full-wave
> fieldsolver, such as that from Ansoft, and you may still need to
> calibrate RLGC's with measurements.
>
> All quasi-static fieldsolvers solve only for L and C, and neglect
> resistive loss. R and Rs are computed using simple formulas by
> perturbation assuming lossless current distribution. But full-wave
> fieldsolvers are prohibitively slow for extracting large designs.
>
> Mike is absolutely right about the frequency-dependent RLGC. Hspice's W
> element uses parameterized frequency dependence: R(f) = Ro + Rs*Sqrt(f),
> G(f) = G0 + f*Gd. So Ro, Lo, Co, Go, Rs, and Gd parameters are
> constant, but R(f) and G(f) are frequency dependent.
>
> As Ray mentioned, there are also higher-order linear and even quadratic
> loss terms in microstrip due to radiation and surface wave
> propagation along the dielectric interfaces. However, all the
> microstrip measurements I have seen, fit the Sqrt() resistive loss very
> well up to at least 10 GHz.
>
> The .net in Hspice simply inserts reference resistors. S parameters are
> then readily calculated from the voltages at the insertion ports. You
> can easily use this technique manually in a simulator that does not have
> .net or if you need to extract S matrix for more than 2 ports.
>
> I would like to respond to Ron's comments. Spice is, among many other
> capabilities, a frequency-domain simulator. In particular, Hspice has
> an FFT/convolution model where one can specify an arbitrary frequency
> table. But the main advantage of this type of frequency-domain
> techniques is generality and straightforward algorithms, not accuracy.
>
> Best regards,
> Dmitri
>
> =======================================================
> Dmitri Kuznetsov, Ph.D.
> Principal Engineer
>
> ViewLogic Systems, Inc. e-mail: vdm@viewlogic.com
> 1369 Del Norte Rd. Tel: (805)278-6824
> Camarillo, CA 93010 Fax: (805)988-8259
> =======================================================
>
> Rachild Chen wrote:
> >
> > 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

--------------EC97E5719500E3745D9DC533
Content-Type: text/x-vcard; charset=us-ascii; name="vcard.vcf"
Content-Transfer-Encoding: 7bit
Content-Description: Card for Rachild Chen
Content-Disposition: attachment; filename="vcard.vcf"

begin: vcard
fn: Rachild Chen
n: Chen;Rachild
org: Huawei Technologies Co.,Ltd
email;internet: rachel.chen@huawei.com.cn
x-mozilla-cpt: ;0
x-mozilla-html: FALSE
version: 2.1
end: vcard

--------------EC97E5719500E3745D9DC533--

**** 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 ****