Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

[SOLVED] Difference of S-parameters between Cadence Spectre and Keysight ADSsim

Status
Not open for further replies.

pancho_hideboo

Advanced Member level 5
Joined
Oct 21, 2006
Messages
2,847
Helped
767
Reputation
1,536
Reaction score
732
Trophy points
1,393
Location
Real Homeless
Activity points
17,490
Calculation method of S-parameters is different between Cadence Spectre and Keysight ADSsim.

Cadence Spectre evaluates Y-parameters first internally.
Then it converts Y-parameters to S-parameters using reference impedance values.

Some simulator has option to choose Y or Z parameters.

On the other hand, Keysigh ADSsim does not use Y or Z parameters to calculate S-parameters.
Keysigh ADSsim calculate S-parameters directly by power wave formulation.
Power wave is defined by voltage, current an reference impedance.

Assume 2-port DUT where Y-parameters don't exist.
For example, shunt element.

Cadence Spectre can not give S-parameters.
Keysigh ADSsim can give S-parameters.
 
Last edited:
I don't think so, otherwise it would be great shame for Cadence.
Which version of spectre do you use but it computes s-parameters of an shunt inductor.
shunt_inductor.pngsmith_shunt.png
 

I don't think so,
otherwise it would be great shame for Cadence.
This issue was filed as PCR(Product Change Request)-464911
"Systems which does not have a valid Y matrix give arithmetic exception"

Which version of spectre do you use
but it computes s-parameters of an shunt inductor.
Thanks for confirming.

I also confirmed.
Now this issue has been fixed in Cadence Spectre.

"sp_shunt.scs"
Code:
simulator lang=spectre
global 0

PORT1 (Vin 0) port r=50 num=1 type=dc mag=1
PORT2 (Vin 0) port r=50 num=2 type=dc

Rx (Vin 0) resistor r=50
//Rx (Vin 0) resistor r=50/2/(sqrt(2)-1)

heppoko options reltol=1e-5 vabstol=3e-8 iabstol=1e-13 temp=16.85 \
    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" rawfmt=psfascii 

aho noise values=[100M] annotate=status oprobe=PORT2 iprobe=PORT1

boke sp values=[100M] annotate=status donoise=yes oprobe=PORT2 iprobe=PORT1  

kasu ac values=[100M] annotate=status

hyottoko options save=allpub

"boke.sp"
Code:
HEADER
"PSFversion" "1.00"
"BINPSF creation time" "1564453319"
"simulator" "spectre"
"version" "17.1.0.307.isr6"
"date" "11:21:59 AM, Tue Jul 30, 2019"
"design" "(no title)"
"analysis type" "sp"
"analysis name" "boke"
"analysis description" "S-Parameter Analysis `boke': freq = 100 MHz"
"xVecSorted" "unknown"
"tolerance.relative" 1.00000e-05
"mode" "ss"
"number of ports" 2
"PORT2:r" 50.0000
"PORT2:num" 2
"PORT2:units" "Ohm"
"PORT1:r" 50.0000
"PORT1:num" 1
"PORT1:units" "Ohm"
TYPE
"sweep" FLOAT DOUBLE PROP(
"key" "sweep"
)
"S-Param" COMPLEX DOUBLE PROP(
"key" "SP"
)
SWEEP
"freq" "sweep" PROP(
"sweep_direction" 0
"units" "Hz"
)
TRACE
"s22" "S-Param"
"s12" "S-Param"
"s21" "S-Param"
"s11" "S-Param"
"cy22" "S-Param"
"cy12" "S-Param"
"cy21" "S-Param"
"cy11" "S-Param"
VALUE
"freq" 1.00000e+08
"s22" (-0.333333 0.00000)
"s12" (0.666667 0.00000)
"s21" (0.666667 0.00000)
"s11" (-0.333333 0.00000)
"cy22" (0.0200000 0.00000)
"cy12" (0.00000 0.00000)
"cy21" (0.00000 0.00000)
"cy11" (0.00000 0.00000)
END
 
Last edited:

That is why it is important to specify software version when discussing such issues. "Now" is not a useful specification.
 

I'm using Spectre 17.10.627 and it seems working..
But I personally don't like Spectre in RF simulation.You can even not attribute the frequency on Smith Chart to see impedance/admittance at particular frequency..Since 20 years..
My favorite one is Keysight GoldenGate. It's marvelous..
 

You can even not attribute the frequency on Smith Chart to see impedance/admittance at particular frequency..Since 20 years..
Right.
However this is not issue of Cadence Spectre.
This issue is for Cadence ViVA.

Simulation performance of current Cadence Spectre is fairly good even for multi-tone HB Analysis.

https://www.designers-guide.org/Forum/YaBB.pl?num=1170364605/2#2
https://designers-guide.org/forum/YaBB.pl?num=1205223090
https://designers-guide.org/forum/YaBB.pl?num=1162921214


My favorite one is Keysight GoldenGate.
It's marvelous..
It is very amazing.
I think no one use Keysight GoldenGate and even Keysight almost abandon promotion of GoldenGate anymore.
Keysight GoldenGate is almost EOL.

https://designers-guide.org/forum/YaBB.pl?num=1268404959#7
 


There is no thread about Goldengate in this forum.

I often think this forum is most popular among the lazy students, people trying to find someome to solve their homework. There's few power users here .. not exactly the community to discuss advanced EDA stuff.
 

Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top