supply current in opamps

[samcheetah]

the datasheet of the 741 operational amplifier says that the typical supply current of a 741 is 1.7mA. now this should be 1.7mA entering into the positive supply pin and 1.7mA leaving the negative supply pin. right???

but when i simulate a simple circuit in Multisim this is not true. the current entering the opamp is 0.7mA and the current leaving the opamp is 24mA and there is niether any load nor any input voltage connected to the amplifier. i believe that the spice model for the 741 in Multisim is quite accurate so there has to be something wrong that i am doing of which i dont know. could someone tell me whats wrong

 

[Nigel Goodwin]

could someone tell me whats wrong

You're playing with a simulator! - that's what's wrong!.

A simulator isn't the real world, and (from what I've seen of threads on this BBS!) it's common to have to modify a 'real world' design to make it work within a simulator.

For a start, try connecting it up properly, you wouldn't connect an opamp up unless you were doing something with it, connect the rest of the components and see what it says then?.

But do it for real as well! - then you KNOW it's right, with a simulator you can't be sure!.

 

[samcheetah]

You're playing with a simulator! - that's what's wrong!.

:lol: yeah i think you are right. actually i dont trust simulators myself but looking at the number of students using spice based simulators these days i cant deny its importance in the industry. all the analog IC design guys and the switcher design guys use a number of simulators to do their work. there are tens of variants of spice used by people in the industry. and i believe that the top universities have their own versions of spice which they teach to their students.

anyway i agree that i should have made a circuit and then checked the supply current. well i have now made a more practical circuit. its just a simple non-inverting amplifier having a gain of 11 and driven by a DC source of 1V. now both the supply currents are equal at a value of 24mA

 

[Oznog]

You're playing with a simulator! - that's what's wrong!.

A simulator isn't the real world, and (from what I've seen of threads on this BBS!) it's common to have to modify a 'real world' design to make it work within a simulator.

For a start, try connecting it up properly, you wouldn't connect an opamp up unless you were doing something with it, connect the rest of the components and see what it says then?

Still, you'd expect a simulator to at least follow Kirchoff's current law. I can't believe that it was dumb enough to make supply current unequal without another node for the current to flow out of.

 

[bmcculla]

Unless i'm missing something the simulation is still wrong. The + and - supplies shouldn't match any more because you now have 11mA flowing into the 1kohm load + some current for the feedback loop. The + supply should be supplying this extra current.

 

[audioguru]

Hi Sam,
Your simulator is totally messed up. It doesn't know anything about opamps and even less about the 741:
1) 11V output into a 1K load? With only a 12V dual supply? No way!
With a 15V dual supply, a 741 typically gives 13V into a 2K load. That's double the voltage drop of your sim at nearly half the load current.
2) If the 741 was low-spec, it would have 5 times the voltage drop of your sim at nearly half the load current.

 

[samcheetah]

you guyz are right, Multisim doesnt know Kirchoff current law. i have made another circuit with the same gain and same input voltage but with a different set of supply rails and a different opamp model. this time i used the national LM741CN that i usually use in the lab. although i dont think there is much difference between the generic 741 model and the LM741 model. the supply currents are same but still the current entering is not equal to the current leaving the opamp.

i have done all this in the lab but i just wanted to try it out on a simulator. now that i know that Multisim is seriously inaccurate, will you guys recommend me a good substitute. actually the reason i chose Multisim was because it didnt require any knowledge of Spice. so it made life much easier. but now it seems that its totally opposite to my expectations. anyway, ill be waiting for any suggestions from you guys.

 

[Nigel Goodwin]

i have done all this in the lab but i just wanted to try it out on a simulator. now that i know that Multisim is seriously inaccurate, will you guys recommend me a good substitute. actually the reason i chose Multisim was because it didnt require any knowledge of Spice. so it made life much easier. but now it seems that its totally opposite to my expectations. anyway, ill be waiting for any suggestions from you guys.

I think my views are already well known?, but just to repeat them:

I don't see any point in playing with simulators - from what I've seen of posts in these forums you often have to modify your design to make the simulator work.

If a simulator doesn't work EXACTLY as in real life, it seems pretty useless to me!.

 

[audioguru]

Hi Nigel,
I agree, the sim is useless. Look at its latest supply current for the LM741. Less than 2uA!

 

[Optikon]

you guyz are right, Multisim doesnt know Kirchoff current law. i have made another circuit with the same gain and same input voltage but with a different set of supply rails and a different opamp model. this time i used the national LM741CN that i usually use in the lab. although i dont think there is much difference between the generic 741 model and the LM741 model. the supply currents are same but still the current entering is not equal to the current leaving the opamp.

i have done all this in the lab but i just wanted to try it out on a simulator. now that i know that Multisim is seriously inaccurate, will you guys recommend me a good substitute. actually the reason i chose Multisim was because it didnt require any knowledge of Spice. so it made life much easier. but now it seems that its totally opposite to my expectations. anyway, ill be waiting for any suggestions from you guys.

I would like to add that it is ridiculous to think Multisim doesnt know the current laws. It does. I think what WE dont know is that there are likely currents that are inside the 741 model that are being returned to NODE 0 inside the part.

Sam, you need to look at the model of the 741. Maybe they could have done a better job with the model but the SPICE engine behind multisim solves the proper equations for bias points.

 

[samcheetah]

thanx for pointing that out Optikon. i was hoping that you would reply to this thread. i remember your thread some days back related to simulators.

now here is the SPICE model for the generic 741

VC 5 15 DC 1.68573V
VE 12 4 DC 1.68573V
IEE 10 4 DC 1.516e-005A
R1 10 0 10Gohm
R6 11 0 100Kohm
R7 5 4 1Kohm
Rc1 6 5 5305.16ohm
Rc2 5 7 5305.16ohm
Re1 9 10 1839.19ohm
Re2 8 10 1839.19ohm
Ro1 1 14 37.5ohm
Ro2 14 0 37.5ohm
Ree 10 0 1.31926e+007ohm
Rcc 0 13 2.20906e-005ohm
Cee 0 10 1e-012
Cc 14 11 3e-011
C1 6 7 1e-016
GA 11 0 6 7 0.000188496
GC 0 13 1 0 45268.1
GB 14 0 11 0 282.942
GCM 0 11 10 0 5.96075e-009
D1 14 13 Dopamp1
D2 13 14 Dopamp1
D3 1 15 Dopamp2
D4 12 1 Dopamp2
Qt1 6 2 9 Qopamp1
Qt2 7 3 8 Qopamp2
.MODEL Dopamp1 D (Is=7.53769e-014A Rs=0 Cjo=0F Vj=750mV Tt=0s M=0)
.MODEL Dopamp2 D (Is=8e-016A Rs=0 Cjo=0F Vj=750mV Tt=0s M=0)
.MODEL Qopamp1 NPN (Is=8e-016A BF=83.3333 BR=960m
+ Rb=0ohm Re=0ohm Rc=0ohm Cjs=0F Cje=0F Cjc=0F
+ Vje=750m Vjc=750m Tf=0 Tr=0 mje=0 mjc=0 VA=50)
.MODEL Qopamp2 NPN (Is=8.30948e-016A BF=107.143 BR=960m
+ Rb=0ohm Re=0ohm Rc=0ohm Cjs=0F Cje=0F Cjc=0F
+ Vje=750m Vjc=750m Tf=0 Tr=0 mje=0 mjc=0 VA=50)

 

[Optikon]

thanx for pointing that out Optikon. i was hoping that you would reply to this thread. i remember your thread some days back related to simulators.

now here is the SPICE model for the generic 741

VC 5 15 DC 1.68573V
VE 12 4 DC 1.68573V
IEE 10 4 DC 1.516e-005A
R1 10 0 10Gohm
R6 11 0 100Kohm
R7 5 4 1Kohm
Rc1 6 5 5305.16ohm
Rc2 5 7 5305.16ohm
Re1 9 10 1839.19ohm
Re2 8 10 1839.19ohm
Ro1 1 14 37.5ohm
Ro2 14 0 37.5ohm
Ree 10 0 1.31926e+007ohm
Rcc 0 13 2.20906e-005ohm
Cee 0 10 1e-012
Cc 14 11 3e-011
C1 6 7 1e-016
GA 11 0 6 7 0.000188496
GC 0 13 1 0 45268.1
GB 14 0 11 0 282.942
GCM 0 11 10 0 5.96075e-009
D1 14 13 Dopamp1
D2 13 14 Dopamp1
D3 1 15 Dopamp2
D4 12 1 Dopamp2
Qt1 6 2 9 Qopamp1
Qt2 7 3 8 Qopamp2
.MODEL Dopamp1 D (Is=7.53769e-014A Rs=0 Cjo=0F Vj=750mV Tt=0s M=0)
.MODEL Dopamp2 D (Is=8e-016A Rs=0 Cjo=0F Vj=750mV Tt=0s M=0)
.MODEL Qopamp1 NPN (Is=8e-016A BF=83.3333 BR=960m
+ Rb=0ohm Re=0ohm Rc=0ohm Cjs=0F Cje=0F Cjc=0F
+ Vje=750m Vjc=750m Tf=0 Tr=0 mje=0 mjc=0 VA=50)
.MODEL Qopamp2 NPN (Is=8.30948e-016A BF=107.143 BR=960m
+ Rb=0ohm Re=0ohm Rc=0ohm Cjs=0F Cje=0F Cjc=0F
+ Vje=750m Vjc=750m Tf=0 Tr=0 mje=0 mjc=0 VA=50)

Look at all those node 0's in there.. I'll bet my paycheck thats where your unaccounted-for currents are going. This is a typical issue with opamp models like this. You will also find MANY others from various vendors that have the same thing going on. You can have faith in multi-sims calculating abilities. Another side effect of these node 0's inside the model is it makes it impossible to accurately simulate a bootstrapped opamp.

With that said, analog devices has several models that do not contain an internal ground node. A real opamp doesnt have a ground pin some vendors model the gain stages and compensation areas with ground based circuits for frequency response shaping/higher order poles etc...