Designer’s Guide Community

wakizashi

New Member

Offline

Posts: 6

sp analysis with one port
Nov 30^th, 2007, 1:58pm

Hello,

I have a question concerning 1 port sp analysis with spectrerf. I would like to use sp analysis to calculate a node capacitance. Therefore I have created a simple circuit first. It is a port component and say 1pF capacitor (ideal). I would like to run sp analysis and calculate c as following:
C=imag(y11)/(2*pi*freq)
At least this is how I could do it in ADS. In spectre however it doesnt work. I get 0 for all the frequency sweep range.
Does anyone know how to prepare test bench and calculate it in spectre?

Thank you for your help.
Regards.

Back to top

IP Logged

pancho_hideboo

Senior Fellow

Offline

Posts: 1424
Real Homeless

Re: sp analysis with one port
Reply #1 - Nov 30^th, 2007, 8:25pm

Your question is not design issue but usage of EDA tool.
Please post to "The Designer's Guide Community Forum ≫ Simulators ≫ RF Simulators".

Quote:

C=imag(y11)/(2*pi*freq)
At least this is how I could do it in ADS.

This is because ADS saves frequency as "freq" in dataset.

Quote:

In spectre however it doesnt work. I get 0 for all the frequency sweep range.

Spectre doesn't save frequency as "freq" in PSF data.
So "freq" is not available in PSF. Instead of "freq" you have to use "xval(y11)".
This is true for RFDE(ADSsim) if you convert ADS dataset to PSF.

The following is example.
http://www.designers-guide.org/Forum/YaBB.pl?num=1133858081/1#1

Back to top

« Last Edit: Nov 30^th, 2007, 11:35pm by Forum Administrator »

Kita━━━━━━(ﾟ∀ﾟ)━━━━━━ !!!!!
http://www7.plala.or.jp/ungeromeppa/flash/kita.html
http://www.youtube.com/watch?v=mjIxGh55bMM&feature=related

IP Logged

wakizashi

New Member

Offline

Posts: 6

Re: sp analysis with one port
Reply #2 - Dec 1^st, 2007, 2:37am

Hi,

Thanks for the answer. I'm not so familiar with ocean but got your script to work somehow. However, I still get strange results from it even for inductor case like in your example. For example:
Q1@1kHz=-1.2833e+09
L1@1kHz=-2.53303e+14[nH]
I use an Rs Ls series connection and Cp (in parallel). Ideal elements. L=1nH.

Could you show your setup for the mentioned ocean script?
Do you configure anything special in sp analysis except for AC magnitude in port = 1V?
Thank you.

Back to top

IP Logged

pancho_hideboo

Senior Fellow

Offline

Posts: 1424
Real Homeless

Re: sp analysis with one port
Reply #3 - Dec 1^st, 2007, 2:43am

Sorry my example is for floating inductor.

port1 >---Inductor ----< port2

L1 is inductance evaluated with port2=gnd.
L2 is inductance evaluated with port1=gnd.

L1 = imag(1/y11)/(2*pi*xval(y11))
L2 = imag(1/y22)/(2*pi*xval(y22))

Q1 = imag(1/y11)/real(1/y11)
Q2 = imag(1/y22)/real(1/y22)

Quote:

I use an Rs Ls series connection and Cp (in parallel). Ideal elements. L=1nH.

Your DUT is grounded. So it is natural that L1 = imag(1/y11)/(2*pi*xval(y11)) doesn't match to your Ls=1nH.

Quote:

Do you configure anything special in sp analysis except for AC magnitude in port = 1V?

In sp analysis, AC magnitude in port is meaningless.

The following script for capacitance from grounded Y11.
Code:

awvSetOptionValue('dateStamp t)
awvSetOptionValue('displayGrids t)
awvSetOptionValue("cursorPrecision" 9)
awvSetOptionValue("displayAxesBy125" t)
pi = acos(-1.0)

base_dir = "~"
circuit_dir = "sim_cap"
sim_data = "schematic"
result_dir = strcat(base_dir, "/simulation/", circuit_dir, "/spectre/", sim_data)
openResults( strcat(result_dir, "/psf") )
selectResult("sp-sp")

y11 = yp(1 1) �
Cx = imag(y11)/(2*pi*xval(y11))

wid = newWindow()
bid = currentSubwindow(1)
plot( Cx ?expr '("C") )
awvSetXAxisLabel(wid "frequency [Hz]" �?subwindow bid)
awvSetYAxisLabel(wid 1 "Capacitance [F]" ?subwindow bid)

Back to top

« Last Edit: Dec 1^st, 2007, 4:27am by pancho_hideboo »

Kita━━━━━━(ﾟ∀ﾟ)━━━━━━ !!!!!
http://www7.plala.or.jp/ungeromeppa/flash/kita.html
http://www.youtube.com/watch?v=mjIxGh55bMM&feature=related

IP Logged

wakizashi

New Member

Offline

Posts: 6

Re: sp analysis with one port
Reply #4 - Dec 2^nd, 2007, 11:00am

Hello,

Thank you for the answer. Ok, now I have used the same setup as yours and I get new problems. In CIW I get:
*Error* ("error" 10 t nil ("*Error* gausex: Equations may be dependent (row 0)\n"))
when trying to plot YP(1 1). Im lost here.

My netlist is like this for reference:

L0 (net5 0) inductor
PORT0 (net5 0) port num=1 dc=0 type=sine
simulatorOptions options reltol=1e-3 vabstol=1e-6 iabstol=1e-12 temp=27 \
tnom=27 scalem=1.0 scale=1.0 gmin=1e-12 rforce=1 maxnotes=5 maxwarns=5 \
digits=5 cols=80 pivrel=1e-3 ckptclock=1800 \
sensfile="../psf/sens.output"
sp sp ports=[PORT0] start=1k stop=10G annotate=status

Its just a port and inductor connected together. Do you see any problem here?
Thank you for the reply.

Regards.

Back to top

IP Logged

Ken Kundert Global Moderator Offline Posts: 2384 Silicon Valley	Re: sp analysis with one port Reply #5 - Dec 2^nd, 2007, 12:53pm I tried your netlist in my version of Spectre and it ran fine. It computes s11 to be -1 over all frequencies, which is as I expect because you gave no value for the inductance of L0, and the default is 0. So the inductor is simply acting like a short circuit. -Ken
Back to top	IP Logged

wakizashi New Member Offline Posts: 6	Re: sp analysis with one port Reply #6 - Dec 2^nd, 2007, 1:15pm Hello, Thank you for spotting this. I have manually updated the netlist with an inductance value and now sp computes correctly the same value. Regards.
Back to top	IP Logged