how to find slew rate of op amp

[ee01akk]

vcvs cadence negative gain

Hi,
Does anyone know how to work out the CMRR (Common Mode Rejection Ratio), PSRR (Power Supply Rejection Ratio) and slew rate using Cadence simulator for a 741 Op-Amp?
Could anyone explain to me how to work out the differential gain of my op-amp using the Cadence calculator?
Thankyou.

 

[mit80]

cadence ac magnitude

Hi
For measuring the differential gain, what i do is to add VCVS to subtract the two signals ( in the schematic), and then use calculator to display the gain of that node (output of VCVS). hope it helps.

 

[hqqh]

cadence gain

Hi,
if you have simulated your circuit (e.g using spectre) and have the necessary signals in the waveform display window --> start calculator --> click at the wave button --> select a wave in the waveform window --> the waveformId will be displayed in the calculator --> than you can execute nearly every operation with this waveform (e.g subtract an other waveform).
greetings,
hqqh

 

[uladz55]

cadence cmrr

Hi,

You can use the AC (small signal) analysis for CMRR, PSRR.
Put vdc source with DC amplitude=0, AC magnitude=1m (any value) in common mode input and power supplier for CMRR and PSRR respectively.
Run AC snslysis for desired operational point and frequency range.
Use calculator to plot ratio of an appropriate vf signals.

Regards,

Uladz55

 

[chinito]

psrr+

PSRR+:

Vout = Vn (connect output of the opamp to negative terminal)
Vp = GND
VDD 4 0 DC 0 AC 1 (for example, VDD between node 4 and 0)
VSS 5 0 DC 0

Run AC analysis, plot Vout

PSRR-:
Vout = Vn (connect output of the opamp to negative terminal)
Vp = GND
VDD 4 0 DC 0 (for example, VDD between node 4 and 0)
VSS 5 0 DC 0 AC 1

Run AC analysis, plot Vout

I don't know how to plot CMRR though. I just posted my question about CMRR plot, let's hope someone helps us out! Thanks.

Added after 55 minutes:

CMRR plot:

Let 1 = Vp, 2 = Vn, 3 = Vout of your opamp.

VCM 2 3 DC 0 AC 1 (common mode voltage between node 2 and 3)
E+ 1 0 2 3 1.0 (voltage control voltage source between 1 and 0 and copies what's between node 2 and 3 by a factor of 1)

.AC DEC 10 1 100Meg

plot DB(V(2)/V(3)) i.e. CMRR = Vcm/Vout

But remember this is not exact because this requires PSRR+ = PSRR- which usually isn't the case. But this is how it is done these days and it is an appx. (what isn't in analog)

 

[xiongshoufen]

common gain in cadence

i want to know why the DC of VDD is zero when do PSRR+ simulation, thus the input N transistor pairs(if is n input transistor) of opam is cut-off region.

PSRR+:

Vout = Vn (connect output of the opamp to negative terminal)
Vp = GND
VDD 4 0 DC 0 AC 1 (for example, VDD between node 4 and 0)
VSS 5 0 DC 0

Run AC analysis, plot Vout

PSRR-:
Vout = Vn (connect output of the opamp to negative terminal)
Vp = GND
VDD 4 0 DC 0 (for example, VDD between node 4 and 0)
VSS 5 0 DC 0 AC 1

Run AC analysis, plot Vout

I don't know how to plot CMRR though. I just posted my question about CMRR plot, let's hope someone helps us out! Thanks.

Added after 55 minutes:

CMRR plot:

Let 1 = Vp, 2 = Vn, 3 = Vout of your opamp.

VCM 2 3 DC 0 AC 1 (common mode voltage between node 2 and 3)
E+ 1 0 2 3 1.0 (voltage control voltage source between 1 and 0 and copies what's between node 2 and 3 by a factor of 1)

.AC DEC 10 1 100Meg

plot DB(V(2)/V(3)) i.e. CMRR = Vcm/Vout

But remember this is not exact because this requires PSRR+ = PSRR- which usually isn't the case. But this is how it is done these days and it is an appx. (what isn't in analog)

 

[alanbrooke]

common mode gain in cadence

for the PSRR (Power Supply Rejection Ratio)
you coud input the VIn VDD 0 DC=3.3 AC=1
and do the AC sweep,
and check the Gain and phase of the point you want to know the PSRR.

 

[qutang]

slew rate simulation with cadence

I use AC sweep ,then in the transient wave choose 20dB.

 

[jiangwp]

cadence post simulation vdd

Hi, the diffential gain can be present in the Cadence waveform.

u can see it by the menu (Wave -> Direct -> ac magnitude and phase) .

 

[heiwolf]

using ac sweep in cadence

I have the same question

 

[g.s.javed]

cadence gain waveform measurement

Can we do it using XF analysis anyway???

 

[dhaval4987]

Re: cadence cmrr

Hi,

You can use the AC (small signal) analysis for CMRR, PSRR.
Put vdc source with DC amplitude=0, AC magnitude=1m (any value) in common mode input and power supplier for CMRR and PSRR respectively.
Run AC snslysis for desired operational point and frequency range.
Use calculator to plot ratio of an appropriate vf signals.

Regards,

Uladz55

Hi,
I am using vdc source only and DC amplitude 0, AC amplitude 1, but when i run the analysis, i get this output... can u tell me the reason? I am attaching my schematic and plot...