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.

deviding Y value by X values in Cadence Virtuoso calculator

Status
Not open for further replies.

Junus2012

Advanced Member level 5
Joined
Jan 9, 2012
Messages
1,552
Helped
47
Reputation
98
Reaction score
53
Trophy points
1,328
Location
Italy
Activity points
15,235
Hello,

I need to calcultae the input capacitance of the amplifier from

Cin_diff=imag(Yin_diff)/(2*pi*freq)

the frequency is the sweeping parameter comes by running the AC simulation in the x-axsis. How can I put in the formula of Cin ?

Thank you
 


Dear Pancho,

Thank you for your help,

I used the xval function as shown below

cin2.PNG

where i7 represent imag_Y which is measured at d from balun for CMOS fully differential amplifier.

the differential input capacitance is given below

cin1.PNG

I wondering why input capacitance is decreasing at a higher frequency, I was expecting it to increase as the parasitics starts to appear at high frequency

Thank you
 

Simply your equation is wrong.
You have to apply imag() for numerator.

Generally Capacitance is nearly constant over frequency.
 
Last edited:
Simply your equation is wrong.
You have to apply imag() for numerator.

Generally Capacitance is nearly constant over frequency.

Dear Pancho,

Thank you for your response

indeed that was the imaginary part, but it is not showing in the calculator. When I draw the i7 from result browser in ADE, I selected signal type as "Imaginary"
 

No.
It is absolute value.

Don’t believe Cadence ADE.

Dear Pancho,

it will be nice and very kind of you if you could then tell me the right procedure,

do you mean I first plot the current (which represent the admittance) in Magnitude, then I send this value to calculator and use the function "imag" ?

Thank you very much
 

Surely see legend of ViVA.
imag() is not applied.

Simply apply imag() in numerator.

If you plot complex value without applying any function, Cadence ViVA plots absolute value.
 
Last edited:
Dear Pancho,

Thank you again for your kind answer

I am applying the "imag" function to the magnitude signal and the result are the same, it shows both have the exact value as you see from the third image (result signal is the one with image fucntion applied)

below is the admitance in magnitude

cin1.PNG

here I sent the signal to calculator

cin2.PNG

here is the result after calculator

cin3.PNG

Thank you very much
 

If you plot complex value without applying any function,
Cadence ViVA plots absolute value.
See attached figure.

Rather I suspect your test bench, since you still can not understand linear circut basics such as differentail mode, common mode, ideal transfomer and etc. at all.
https://www.edaboard.com/showthread.php?386628

Show me netlist regarding signal sources, loads, balun and analysis statements.

"test_Junus2012.scs"
Code:
// Generated for: spectre
// Generated on: Sep 19 09:28:54 2019
// Design library name: My_RFDE_Test
// Design cell name: test_Junus2012
// Design view name: schematic
simulator lang=spectre
global 0

// Library name: My_RFDE_Test
// Cell name: test_Junus2012
// View name: schematic
V0 (net2 0) vsource dc=1 mag=1 type=dc
IPRB0 (net2 net1) iprobe
R0 (net1 0) resistor r=10
C0 (net1 0) capacitor c=100p
simulatorOptions options psfversion="1.1.0" reltol=1e-3 vabstol=1e-6 \
    iabstol=1e-12 temp=25.0 tnom=25.0 scalem=1.0 scale=1.0 gmin=1e-12 \
    rforce=1 maxnotes=5 maxwarns=5 digits=5 cols=80 pivrel=1e-3 \
    sensfile="../psf/sens.output" checklimitdest=psf 
ac ac start=10M stop=1G dec=50 annotate=status 
save IPRB0:in 
saveOptions options save=selected
 

Attachments

  • 2019-0919-0928-31.png
    2019-0919-0928-31.png
    68.6 KB · Views: 198
Last edited:
See attached figure.

Rather I suspect your test bench, since you still can not understand linear circut basics such as differentail mode, common mode, ideal transfomer and etc. at all.
https://www.edaboard.com/showthread.php?386628

Show me netlist regarding signal sources, loads, balun and analysis statements.

"test_Junus2012.scs"
Code:
// Generated for: spectre
// Generated on: Sep 19 09:28:54 2019
// Design library name: My_RFDE_Test
// Design cell name: test_Junus2012
// Design view name: schematic
simulator lang=spectre
global 0

// Library name: My_RFDE_Test
// Cell name: test_Junus2012
// View name: schematic
V0 (net2 0) vsource dc=1 mag=1 type=dc
IPRB0 (net2 net1) iprobe
R0 (net1 0) resistor r=10
C0 (net1 0) capacitor c=100p
simulatorOptions options psfversion="1.1.0" reltol=1e-3 vabstol=1e-6 \
    iabstol=1e-12 temp=25.0 tnom=25.0 scalem=1.0 scale=1.0 gmin=1e-12 \
    rforce=1 maxnotes=5 maxwarns=5 digits=5 cols=80 pivrel=1e-3 \
    sensfile="../psf/sens.output" checklimitdest=psf 
ac ac start=10M stop=1G dec=50 annotate=status 
save IPRB0:in 
saveOptions options save=selected

Dear Pancho thank you for your reply and sorry to make you upset,

here is the netlist
Code:
// Library name: analogLib
// Cell name: ideal_balun
// View name: schematic
subckt ideal_balun d c p n
    K0 (d 0 p c) transformer n1=2
    K1 (d 0 c n) transformer n1=2
ends ideal_balun
// End of subcircuit definition.

// Library name: sen_In_Amp_fully_11_layout2
// Cell name: In_Amp_fully_11_layout_AC3_test
// View name: schematic
V3 (net4 0) vsource dc=1.65 type=dc
V4 (net17 0) vsource dc=VCM type=dc
V1 (net018 0) vsource dc=1.65 type=dc
V0 (vdd! 0) vsource dc=3.3 type=dc
PD_S (PD 0) vsource dc=PD type=dc
XPD_S (XPD 0) vsource dc=XPD type=dc
R5 (Vout_diff 0) resistor r=200k
R1 (Vout\+ net33) resistor r=100
R2 (net33 net32) resistor r=100k
R3 (net32 Vout\-) resistor r=100
C1 (Vout_diff 0) capacitor c=2.5p
V11 (VID 0) vsource mag=1 type=sine ampl=1.6 freq=1K
I6 (0 PD net17 vdd! XPD net28 Vin\+ net4 Vout\+ Vout\- net4 vin\-) \
        In_Amp_fully2
I10 (vdd! net28) isource dc=Ibias type=dc
I7 (VID net018 Vin\+ vin\-) ideal_balun
I19 (Vout_diff VOC Vout\+ Vout\-) ideal_balun
simulatorOptions options reltol=100e-6 vabstol=1e-6 iabstol=1e-12 temp=27 \
    tnom=27 homotopy=all limit=delta scalem=1.0 scale=1.0 \
    compatible=spice2 gmin=1e-12 rforce=1 maxnotes=5 maxwarns=5 digits=5 \
    cols=80 pivrel=1e-3 sensfile="../psf/sens.output" checklimitdest=psf 
dcOp dc write="spectre.dc" maxiters=150 maxsteps=10000 annotate=status
dcOpInfo info what=oppoint where=rawfile
ac ac start=1 stop=100M dec=100 annotate=status 
designParamVals info what=parameters where=rawfile
primitives info what=primitives where=rawfile
subckts info what=subckts  where=rawfile
save I7:1 
saveOptions options save=allpub

and the circuit is

cin4.PNG

The circuit about is fully differential instrumentatin amplifier, it employes the same concept of fully differential amplifire where I want to test Cin
 

Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top