+ Post New Thread
Results 1 to 3 of 3

1st November 2018, 12:03 #1
 Join Date
 Jul 2012
 Posts
 26
 Helped
 0 / 0
 Points
 1,329
 Level
 8
How to define port in cadence which has a impedance value that is frequency dependent
Hi Everyone,
I am trying to use a port with complex value as a output termination in SP simulation of cadence. For example output port impedance value is 1/(2*pi*freq*C) which is also frequency dependent. Is there any idea how to do this in cadence? Thanks in advance.

Advertisment

1st November 2018, 21:16 #2
 Join Date
 Nov 2001
 Location
 Turkey
 Posts
 4,117
 Helped
 1244 / 1244
 Points
 28,487
 Level
 41
Re: How to define port in cadence which has a impedance value that is frequency depen
Unfortunately "freq" variable cannot be used in Spectre sparameters simulations.However it's possible to use in ADS.

Advertisment

2nd November 2018, 11:45 #3
 Join Date
 Oct 2006
 Location
 Real Homeless
 Posts
 2,236
 Helped
 609 / 609
 Points
 14,791
 Level
 29
Re: How to define port in cadence which has a impedance value that is frequency depen
What simulator do you use ?
Use correct terminology.
We can use many simulators, e.g. Synopsys HSPICE, Mentor Eldo, Keysight ADSsim, Keysight Goldengate, etc. in Cadence Virtuoso.
What do you mean by "in cadence" ?
Wrong.
Frequency expressions are possible by using "$freq" even in Cadence Spectre.
This is available for "analogLib/res", "analogLib/ind" and "analogLib/cap".
However Spectre primitive, "resistor", "inductor" and "capacitor" don't have ability of treating frequency expressions actually.
Spectre treats frequency expressions by Spectre primitive, "bsource" internally.
See "spectre h bsource".
Currently, we can not use $freq for Spectre primitive, "port".
So use "analogLib/res" and "analogLib/ind" instead of "analogLib/port".
Here negative resistance is not available if you use $freq for r=func($freq) in "analogLib/res".
It seems Spectre primitive, "bsource" can not reflect negative resistance.
On the other hand, Spectre primitive, "resistance" can reflect negative resistance.
"test_freq_expression.scs"
Code:// Generated for: spectre // Generated on: Nov 2 13:55:42 2018 // Design library name: My_RFDE_Test // Design cell name: test_freq_expression // Design view name: schematic simulator lang=spectre global 0 // Library name: My_RFDE_Test // Cell name: test_freq_expression // View name: schematic PORT0 (x1 0) port r=50 x=0 num=1 type=dc R0 (x1 net1) resistor r=cos(2*acos(1)/100M*$freq) L0 (net1 0) inductor l=sin(2*acos(1)/100M*$freq)/(2*acos(1)*$freq) simulatorOptions options psfversion="1.1.0" reltol=1e3 vabstol=1e6 \ iabstol=1e12 temp=25.0 tnom=25.0 scalem=1.0 scale=1.0 gmin=1e12 \ rforce=1 maxnotes=5 maxwarns=5 digits=5 cols=80 pivrel=1e3 \ sensfile="../psf/sens.output" sp sp center=1G span=100M annotate=status saveOptions options save=selected
Last edited by pancho_hideboo; 2nd November 2018 at 11:59.
1 members found this post helpful.
+ Post New Thread
Please login