2
\$\begingroup\$

I have imported a Spice model of an op-amp into OrCAD, but the part symbol is different from what I am used to, and I don't know what pins 4, 5, 8, and 11 represent here.

Link to spice model I used: https://www.eng.auburn.edu/~strouce/analogbc/opamp2.htm

Here is the symbol I am getting:

enter image description here

Edit: Found out what each pin represents. I made a voltage follower circuit, but no matter the input supply my output voltage is stuck at -13.53V

Voltage follower circuit I used: enter image description here enter image description here

\$\endgroup\$
1
  • \$\begingroup\$ Looks to me like the subcircuit intentionally uses SPICE2 syntax where "Nodes must be nonnegative integers..". This of course makes it confusing because you can't use names for the pins. Still poor form because the author can include comments (lines starting with asterisks) to give a legend to the user detailing the pinout. \$\endgroup\$
    – Ste Kulov
    Jul 27 at 4:38

2 Answers 2

1
\$\begingroup\$

The link you provide shows .subckt code which (mostly) matches the accompanying image of the opamp's internal schematic. I'll duplicate both for clarity and completeness below:

*operational ampplifier 2(Leap frog opamp)

.Subckt opamp 4 5 8 1 11
.MODEL mosn NMOS
+ vto=1 kp=17u gamma=1.3 lambda=0.01 phi=0.7
+pb=0.8 mj=0.5 mjsw=.3 cgso=350p cgdo=350p cgbo=200p
+cj=300u cjsw=500p ld=0.8u tox=80n
.MODEL mosp PMOS
+ vto=-1 kp=8u gamma=.6 lambda=0.02 phi=0.6
+pb=0.5 mj=0.5 mjsw=.25 cgso=350p cgdo=350p cgbo=200p
+cj=150u cjsw=400p ld=0.8u tox=80n
R1a 6 66 1
R1b 66 3 100meg
m1 66 4 3 3 mosp w=20u l=10u
R2a 7 77 1
R2b 77 3 100meg
m2 77 5 3 3 mosp w=20u l=10u
R3a 6 67 1
R3b 67 11 100meg
m3 67 6 11 11 mosn w=36u l=10u
R4a 7 78 1
R4b 78 11 100meg
m4 78 6 11 11 mosn w=36u l=10u
R5a 3 33 1
R5b 33 1 100meg
m5 33 2a 1 1 mosp w=30u l=10u
R6a 8 88 1
R6b 88 11 100meg
m6 88 7 11 11 mosn w=100u l=10u
R7a 8 89 1
R7b 89 1 100meg
m7 89 2 1 1 mosp w=42u l=10u
R8a 2 22 1
R8b 22 11 100meg
m8 22 6 11 11 mosn w=60u l=10u
R9a 2 23 1
R9b 23 1 100meg
m9 23 2 1 1 mosp w=30u l=10u
Rc 7 76 1
cc 76 8 6p
Rs 76 8 100meg
vbias 2a 0 .1
.ends 

enter image description here

Our goal is to try and map the node numbers listed on the .subckt line to the actual pins labeled on the schematic image.

.subckt opamp 4 5 8 1 11


The first clue I see is there is only one capacitor, and one of its sides is connected to Vout in the image. I can easily find the capacitor in the .subckt code because it's the only line that starts with the letter "C":

cc 76 8 6p

Therefore, pin 8 is Vout.


Next, the image shows M7 as a PMOS transistor with its source connected to Vdd. MOSFET transistors in SPICE follow the following syntax and pin ordering:

Mxxx <drain> <gate> <source> <body> <modelname> [W=<width>] [L=<length>]


So for M7 we have:

m7 89 2 1 1 mosp w=42u l=10u

and therefore, pin 1 is Vdd.


We can do the same with NMOS transistor M6 and Vss:

m6 88 7 11 11 mosn w=100u l=10u

which means pin 11 is Vss.


The noninverting (+) input is connected to the gate of M2:

m2 77 5 3 3 mosp w=20u l=10u

So following the syntax definition above, pin 5 is the noninverting input.


Lastly, we do the same with the inverting (-) input and M1:

m1 66 4 3 3 mosp w=20u l=10u

which means pin 4 is the inverting input.


Summarizing, we have the following:

4  = inverting (-) input
5  = noninverting (+) input
8  = Vout
1  = Vdd
11 = Vss

Shown below is a DC operating point example of a "gain of 2" noninverting amplifier. One thing to note about this opamp model is that it only functions well enough in DC with high valued resistors. Reduce the gain/feedback resistors by a factor of 10 or 100 to see what I'm talking about.

enter image description here

\$\endgroup\$
1
  • \$\begingroup\$ Could you also show me how to get the voltage db and phase voltage graph in the same link? I ran an AC sweep but my output isn't matching. \$\endgroup\$
    – Anshul
    Jul 29 at 5:38
0
\$\begingroup\$

The model you linked has this line: -

.Subckt opamp 4 5 8 1 11

And, if I look at similar op-amp models that I use, the pin order in my models are this: -

+Vin -Vin +Vsup -Vsup Output

So, it's a fair bet that if you connected up your model as an non-inverting voltage follower, you should get a response that looks like one. Do you know how to do this?

\$\endgroup\$
2
  • \$\begingroup\$ I did made a non-inverting voltage follower, connecting the output to -Vin, applying a DC source at +Vin and used +15/-15 as Vsup. My output is stuck at -14.11V no matter the input supply. \$\endgroup\$
    – Anshul
    Jul 25 at 10:18
  • \$\begingroup\$ Maybe you should add that schematic into your question within a clear edited section so that your original question is intact @AnshulMahawar \$\endgroup\$
    – Andy aka
    Jul 25 at 10:27

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.