Ray has a good point about adding the 50 ohm source series impedance
and terminating the far end with ohms to ground. These are crucial to
mimick your network analyzer. To account for the
6dB loss, I normally put in a 2V source instead of 1V.
You show a 100 ohm resistor in your ckt shunting one of the nodes
to ground. I don't know why it is there but it could be one of your
problems.
And finally, since I see you are using hspice, you can use
the .net capability to simulate s-parameters. To do this you
apply a source to port 1 WITHOUT a 50 ohm series resistance.
The 2nd port is left high impedance which I do by terminating
with a 100kohm resistor. Just follow the example below if you'd
like.
vac port1 0 ac 1
wdutp n=1 port1 0 port2 0 RLGCfile=rlcg_test_w_file l=2.0
rterm port2 0 100k
.net v(port2) vac rout=50 rin=50
.ac lin 256 .1e9 25.6e9
.print s11(re) s11(im) s12(re) s12(im) s21(re) s21(im) s22(re) s22(im)
.options probe post csdf
.END
Mike
On Aug 20, 12:41pm, Ray Anderson wrote:
> Subject: Re: [SI-LIST] : About the AC analysis with HSPICE
>
> Could it have something to do with the fact that your simulation
> is driving the line from a zero impedance source while a real measurement
> is driven from a finite impedance (50 ohms) ?
>
> Try putting a 50 ohm series resistance between your voltage source and the
> transmission line. Make your load resistor 50 ohms. Be sure to account for
the
> extra 6dB of voltage loss that the voltage division across the source
resistor
> causes.
>
>
> -Ray Anderson
> Sun Microsystems
>
> > Hello,dear sir:
> >
> > These days I am busy doing the simulation to get the evaluation for loss of
> > the transmission line.Generally,the loss increases with frequency
> > increation.I find it difficult to get a satisfying result by doing the AC
> > analysis with HSPICE.The reflections due to the high frequency are very
> > terrific.What i did is:
> >
> ********************************************************************************
> *******************
> > .OPTION POST=2 ACOUT=0
> > .options brief = 0
> > .options scale = 1u
> > V5 nd_pin1 gnd AC 1v
> > .AC DEC 100.00 1K 1000MEG
> > R1 cpin1 gnd 100
> > Ws1 nd_pin1 gnd gnd cpin1 gnd gnd
> > + Fsmodel=mother1 n=2 l=19000mil
> > .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 *tline
> > model(W_ELEMENT)
> >
> > .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=(18mil,21.38mil))
> > *+ conductor= (material =copper1, shape=rect_1,origin=(28mil,
21.38mil))
> > *+ conductor= (material =copper1,
shape=rect_1,origin=(39mil,21.38mil))
> >
> > .PROBE AC VDB(cpin1,nd_pin1)
> > .end
> >
> ********************************************************************************
> *********************
> > From above ,you can know that I really use the 'AC sweep' analysis to get a
> > curve which has the Y--20log[V(cpin1)/V(nd_pin1)],X--frequency.But the
> > result is bad.I compared this result with the result i got by testing with
> > network analysiser,the difference is terrifying! I don't think it a good
way
> > to evaluate transmission loss with AC analysis in HSPICE.Would you kind to
> > recommend me a good way to evaluate transmission loss by SPICE simulation?
> >
> >
> > 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 ****
>
>-- End of excerpt from Ray Anderson
-- _______________________________________________________________ Mike Degerstrom Email: degerstrom.michael@mayo.edu Mayo Clinic 200 1st Street SW Gugg. Bldg. RM 1042A Phone: (507) 284-3292 Rochester, MN 55905 FAX: (507) 284-9171 WWW: http://www.mayo.edu/sppdg/sppdg_home_page.html _______________________________________________________________**** 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 ****