Thread: AD8067 in Multisim - problem with supply!

Hi all!

I have pretty strange issue. I wanted to use AD8067 opamp in my design, but despite it's rated to to 5-24V supply voltages, when I supply it with anything above +-5.42V, then the output of amplifier in inverting topology is equal to almost -Vcc and there are ripples of similar shape to the input signal.

How to overcome that to be able to simulate circuit with +-12V supply as it can go ?


Best regards,
Micard

It doesn't make sense ..
If you can, post your *****.msxx file ..

IanP

Sure, here you are. When you change the voltage of DC power sources do 5V everything is as expected. But when i put +-6V . I have ~-Vcc and small ripple of signal's frequency.

Mike

Basic question: Dual or single supply? (Perhaps you have applied single supply without proper biasing?).
My question is because I cannot read your file - even after unzipping. Is it really necessary to zip?

It's dual.
Unfortunately yes - edaboard checks extensions. My file is opamp.ms10 The file in this post is just one with extension changed to *.r00

Another question: Which gain are you going to realize? (As I still cannot read your file). Do you know that the opamp is stable only for gain values larger than 8 (according to AD data sheet).?

I haven;t seen it.. thank you very much for pointing me this thing.

But still I use larger gain.

Se pictures below - only supply is changed

This is simulator, so you have to follow rules, and the rule says that a resistor should be connected to input(+) and its value should be equivalent to the impedance (or resistance) "seen" by input (-), what basically means R2 and R3 in parallel ..
Add R1 and all should go back to normal ..

IanP
:D

totally true !

Thank you very much.. I have already spent some time at this silly mistake :/

Originally Posted by micard

totally true !
Thank you very much.. I have already spent some time at this silly mistake :/

I can't understand. Was this really the cause of trouble?
Here is the reason for my doubts:
Quote IanP:
This is simulator, so you have to follow rules, and the rule says that a resistor should be connected to input(+) and its value should be equivalent to the impedance (or resistance) "seen" by input (-), what basically means R2 and R3 in parallel ..

There is absolutely no requirement (rule) that a resistor "should be connected to input(+)". Such a resistor is good for compensation of dc input currents in order to avoid a shift of the operating point. However, as far as I know, the opamp used has a FET input stage, does it not?. In this case, there is no need to compensate dc currents and I would be surprised that this was the cause of the problems mentioned. (Even for BJT input stages and a 1k gain resistor the dc input current should have liitle influence).
Please inform me about results.

This is simulator, so you have to follow rules, and the rule says that a resistor should be connected to input(+) and its value should be equivalent to the impedance (or resistance) "seen" by input (-), what basically means R2 and R3 in parallel ..
Add R1 and all should go back to normal ..

totally true !
Thank you very much.. I have already spent some time at this silly mistake :/

This thread goes into the wrong direction and the conclusion is false.

LvW is right. There is no such rule in a simulator to add a resistor in the non-inverting input. We might add a small resistor to help the simulator converge to a solution but this is not the case. The rule applies in real life for Op Amps with large input bias currents to help reduce the offset that otherwise would be generated by the voltage drop on the inverting input resistors. Not for AD8067 with its picoamp bias currents.

The AD8067 model is broken, or Multisim does not interpret it correctly. If you insert a current probe in the non-inverting input you will find a huge current. The suggested solution with a resistor in the non-inverting input compensates for this problem, but the offset is still large.

I suggest you create your own behavioral model for AD8067 from its data sheet.

Thanks, AdrianN !

So, the opamp model has errors as you have found out.
Now my conception of the analog world is again restored.

Thanks AdrianN for clearing the case. I indeed had a covergence problems sometimes (without use of a resistor) at non inverting input.

Do you know any tutorial explaining how to make own Spice models of opamps (or other devices)?

Kind regards,
Micard

Multisim has a Component Wizard under Tools. You start the wizard, then click on simulation only, then choose the number of pins (5 in this case), choose a symbol (an op amp, copy from database). At model, start Model Maker. Choose Operational Amplifier and then fill up a table with the component specs.

Multisim Help also has a section "Adding Components with the Create Component Wizard".

You could also buy a book, The SPICE Book by Andrei Vladimirescu. Search for it at www.Amazon.com or get a link from the list of books in my website at www.MasteringElectronicsDesign.com.

You can also create a "visual" model, by wiring one in Multisim. Start with a VCVS with a large gain (choose the AD8067 open loop gain), then add two input current sources for Ib, one voltage source for Vos in series with an input, one differential resistor between inputs, two common mode input resistors, a series output resistor for Ro. You can also add one pole with a VCCS and a combination of RC. You can also simulate the power supplies. Anyway, too long to explain here. The book should help you. I will soon have a short tutorial in my website. Keep an eye on it (RSS it).

I posted this tutorial. You can find it here:

Build an Op Amp SPICE Model from Its Datasheet – Part 1