deviding Y value by X values in Cadence Virtuoso calculator

1. deviding Y value by X values in Cadence Virtuoso calculator

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  Reply With Quote

•

2. Re: deviding Y value by X values in Cadence Virtuoso calculator

1 members found this post helpful.  Reply With Quote

3. Re: deviding Y value by X values in Cadence Virtuoso calculator Originally Posted by pancho_hideboo Dear Pancho,

Thank you for your help,

I used the xval function as shown below where i7 represent imag_Y which is measured at d from balun for CMOS fully differential amplifier.

the differential input capacitance is given below 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  Reply With Quote

4. Re: deviding Y value by X values in Cadence Virtuoso calculator

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

Generally Capacitance is nearly constant over frequency.

1 members found this post helpful.  Reply With Quote

5. Re: deviding Y value by X values in Cadence Virtuoso calculator Originally Posted by pancho_hideboo 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"  Reply With Quote

•

6. Re: deviding Y value by X values in Cadence Virtuoso calculator Originally Posted by Junus2012 indeed that was the imaginary part
No.
It is absolute value.

1 members found this post helpful.  Reply With Quote

7. Re: deviding Y value by X values in Cadence Virtuoso calculator Originally Posted by pancho_hideboo No.
It is absolute value.

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  Reply With Quote

8. Re: deviding Y value by X values in Cadence Virtuoso calculator

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.

1 members found this post helpful.  Reply With Quote

9. Re: deviding Y value by X values in Cadence Virtuoso calculator

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 here I sent the signal to calculator here is the result after calculator Thank you very much  Reply With Quote

•

10. Re: deviding Y value by X values in Cadence Virtuoso calculator Originally Posted by pancho_hideboo 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.

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

1 members found this post helpful.  Reply With Quote

11. Re: deviding Y value by X values in Cadence Virtuoso calculator Originally Posted by pancho_hideboo 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.

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

--[[ ]]--