opamp input power amplifier - problems

[sparkle]

guys i have problems to make this amplifier work...what am i making wrong - it seems to me that i have problems with the input part of the amplifier....
can somebody help me....

 

[sparkle]

help needed....

 

[lumanauw]

Is it oscilating? Try 2x47pf from top and bottom of VBEmultiplier (Q12) to opamp's output (pin 6). The cap values may be experimented in the real cct.

 

[sparkle]

i made it in sim using Multisim 8....i have arround 13kV at pin 6 (and going up) of the opamp... because of the input problems (i assume) the complete amp is not is normal working point but i can't figure what is the problem....
when reading in simulator the bias current through output transistors is 19A....

right those values will never be reached in real life - my amp will be burned before they reach it to be measured....
but i can't figure what is the problem.....
is the input configuration o.k. (arround opamp)

i do not know - i am not sure....

please advise what to do
thanks
sunny

 

[sparkle]

here are some values on some points....

 

[andy_c]

i made it in sim using Multisim 8

One thing to check is your op-amp model. Many simulators including LTSpice use the ancient Boyle model for op-amps. The Boyle model will not simulate correctly with this type of design, because it has the very unrealistic property that the supply current does not change when the load current changes!

Try simulating the op-amp in a circuit by itself and see if the supply current changes with the load current. If it doesn't, you'll need another op-amp model.

 

[sparkle]

i am new in simulating things....

in oder words You want me to make new file where i will put an opamp in, lets say, inverting mode and to monitor if opamp supply current is changing with load current ?!

 

[sparkle]

i have made this circuit.....
for square signal at the input that is 1V i have 10V at the output....and the currents of the power supply seem to be steady and the current from the output seem to vary from 46.3mA upt to 50mA....

what to do ...
is my Multisim stupid or am i stupid... is everything working fine or we are not sure here.....
in other words this circuit might work without a problem but we will not know until i make it in real life and not in sim...

killing me softly with this sim


please advise thank you in advance

 

[andy_c]

i am new in simulating things....

in oder words You want me to make new file where i will put an opamp in, lets say, inverting mode and to monitor if opamp supply current is changing with load current ?!

Sure. Put a load of, say, 500 Ohms on the output and supply a DC input voltage so that the DC output is, say, positive 5 Volts. Then the load will be drawing 10 mA. This 10 mA should be coming from the positive supply, in addition to its normal supply current.

In the Boyle model, the supply draws a fixed current as the load current changes. This makes it so that power amp simulations like yours don't work, because it's the varying supply current that's driving the external devices.

 

[andy_c]

i have made this circuit.....
for square signal at the input that is 1V i have 10V at the output....and the currents of the power supply seem to be steady and the current from the output seem to vary from 46.3mA upt to 50mA....

what to do ...
is my Multisim stupid or am i stupid...

This is a bug in the Boyle op-amp model that your simulator is using. Try to find out how to use vendor-supplied op-amp models in your simulator. The models from Analog Devices are usually good (but not Linear Technology - they use the Boyle model also).

 

[sparkle]

i have tried it - my supplies are both the same - arround 12pA and the output is having 50mA of load current - this is not right (seems to be Boyle's model)....in other words this amplifier might work but because of the sim i can't see it there working correctly......man why am i using sim in the first place....crazy thing....

o.k.
QUESTION....can somebody please tell me if the schematic looks o.k. at least...so that i can be a little bit more relaxed to make it....
please
thank You ......

 

[andy_c]

....in other words this amplifier might work but because of the sim i can't see it there working correctly

Yes, exactly!

......man why am i using sim in the first place....crazy thing....

Don't get discouraged! . This is the "crummy models" SPICE trap that everybody who uses SPICE falls into at one time or another.

o.k.
QUESTION....can somebody please tell me if the schematic looks o.k. at least...so that i can be a little bit more relaxed to make it....
please

It looked okay to me, but it would be a good idea to get the sim running with a good op-amp model so you can tweak the frequency compensation for stability.

Edit: Have a look at this Analog Devices app note - at least the first couple of pages. It describes the pitfalls of the Boyle model. The one you experienced is described on the first page on the right, about two-thirds of the way down.

 

[sparkle]

Andy thank You,

now i am a little bit more calm......

whole another question is how to make a good opamp model that will simulate good......
since i am unexperienced with making models in Multisim or any other simulator (tried that with LT Spice with no luck) i think i will have to make it in real life to see if it is wokring

well, at least it seems it might work....at least this is o.k. lookin'

thank You again
regards

 

[andy_c]

Andy thank You,

You're welcome!

whole another question is how to make a good opamp model that will simulate good......

Well, you don't actually make the model. You download the model file from the op-amp vendor. I've had reasonable luck with Analog Devices models. The model file is a text file. That text file consists of a netlist (list of components and their interconnections, like a text representation of a schematic). The form this file takes is called a subcircuit. You decide on the op-amp you want to use and download its model file (subcircuit) from the op-amp vendor's web site. The trick is to look through your simulator documentation and find out how to assign this subcircuit text file to your op-amp symbol in the schematic. It might be as simple as right-clicking on the op-amp symbol and specifying the file name of the text file you downloaded from the op-amp vendor as an attribute of some kind. If you're using LTSpice, I could show you how to do it. But I don't know Multisim.

 

[sparkle]

thanks - i will try to do this these days ....

 

[sparkle]

i have been searching on analog devices home page for the model of AD797 but i can't find any...

does anyone have the model for this opamp...


Andy - i have found two things where i can edit ..."edit model" and "edit component in DB"....
the first one have only this for NE5534:

Vos 4 1 DC 0.0005V
Ib1 4 0 5.1e-007A
Ib2 2 0 4.9e-007A
G1 0 5 4 2 0.0464159
G2 0 6 5 0 154.72
G3 0 3 6 0 154.72
Ri 4 2 100000ohm
R1 5 0 1000ohm
R2 6 0 0.3ohm
R3 3 0 0.3ohm
C1 5 0 1.59155e-006
C2 6 0 5.30516e-033
Cc 5 0 3e-011

and the second one, in "model data part" has this

.SUBCKT NE5534A 1 2 3
* EWB Version 4 - 3 Terminal Opamp Model
* A= 100000 RI= 100000 RO= 0.3 VSW+= 13 VSW-= -13
* Vos= 0.0005 Ibs= 4e-007 Ios= 1e-008 SR+= 1.3e+007
* fu= 1e+007 fp2= 1e+032 CC= 3e-011
Vos 4 1 DC 0.0005V
Ib1 4 0 4.05e-007A
Ib2 2 0 3.95e-007A
G1 0 5 4 2 0.0464159
G2 0 6 5 0 154.72
G3 0 3 6 0 154.72
Ri 4 2 100000ohm
R1 5 0 1000ohm
R2 6 0 0.3ohm
R3 3 0 0.3ohm
C1 5 0 1.59155e-006
C2 6 0 5.30516e-033
Cc 5 0 3e-011
.ENDS


also i can ad model from file (but i am not sure if this will change completely how my model is made in library) and the files that i can use are *.vx, *.v, *.dll and *.cir........

 

[consort_ee_um]

You need to modify the 5534 model with this:
http://www.ecircuitcenter.com/OpModels/I_Supply/I_Supply.htm
That site is a great tutorial on spice

 

[jerluwoo]

This is a bug with multisim itself. This happens when using a generic current source model as a load on tubes and transistors also. Happens to me all the time.

 

[sparkle]

thank You guys....i have to read everything carefully and play a bit with Multisim and than i will have more to ask for sure....this is all new to me...
thanks again....and also for the link - i have to do read it first ......thanks....
sunny

 

[KSTR]

You might try TI's OPA551/552 for example. These have quite good models, including supply effects and more. Of course, their specs are not on par with an AD797...

- Klaus