Analog ground errors

[akis]

Hello

I think there are errors with version 12 invoving (a) the static probes (b) the analog ground and basic op-amp simulation.

(a) The static probes. Sometimes they give weird results, eg different current readings from two probes placed next to each other on the same wire. Deleting the "dodgy" probe and adding another one solves the issue.

(b) On the diagram below, we can see 25.7 mA going through R1 and into the op-amp. But where do these mA go to? Certainly not the power supply lines of the op-amp which has 9.53 mA in and 9.53 mA out. So it seems we have 25.7 mA magically entering the op-amp and then disappearing. Changing the op-amp results in similar "disappearing" currents of different values.

If we look at the top of the diagram Multisim is telling us those "missing" 25.7 mA seem to be coming from the Ground node. Why? Is there a secret connection inside the op-amp and the ground?

I now place the ground terminal at the bottom rail and I see more weird results. It seems the overall current draw has been increased - and the missing current that is entering the op-amp is again at the ground terminal.

Is there perhaps a fix/update that fixes these problems?

[johnsold]

I do not know what is in the multisim models, but it certainly looks like there are some ground connections in the model.

I looked at a SPICE model for the TL074 which I had on hand and it shows several connections to node 0 (ground), even if none of the pins are grounded.

Also, it appears that an error occurs in the second image you posted. The sum of the currents at the ground node is not zero.  The three probes sum to zero but the current in R2 must also be 5 mA.

Notice also that the results shown (output voltage) indicate that the op amp is outside its linear range. The output voltage is not equal to the voltage at pin 3 and the voltages at pins 2 and 3 are not close to equal.  It is possible that the model breaks down under that load.

However, the simulation should either throw an error or accurately follow Kirchhoff's Laws.

Lynn

[Miguel_V]

Hello,

Would you be able to attach your circuit (not just the picture) to reproduce the static probe errors? And in answer to (b), Yes! if you look into the SPICE model of the component you selected (the TI opamp), there is an entire subcircuit to reproduce real life conditions as best as possible from what the model says. From a quick view of the netlist, there are grounds, sources, jfets, resistors etc. Hopefully that answers your question. you can check it yourself by double clicking the component and hitting on Edit Model.

Cheers,

[akis]

Hello

I have tried the TL072, MC33072, LM833 and LM741.  I have also just tried the LM4562 - it is a bit better but not much : 17.34mA in and 16.7 mA out, with the difference appearing at the ground node. The TL072  is showing 19 mA in and 9 mA out, with 10 mA appearing at the ground node. 

The LM741 simulates properly, ie "current in == current out". 

The circuit is very simple but I do not understand the op-amp models to see what hidden connections to ground there are there (and why, and why at DC).

Maybe if there was an op-amp designer to allow us to enter very basic op-amp specifications without the "exotics" which tend to ruin the simulation ?

The probe errors are random. Even if I attach the circuit it is not going to fail reliably. For example I have a circuit that simulates nicely, then I add a probe and suddenly it fails with "simulation error". Are the probes may be real components that it inserts into the circuit and that is why they affect the simulation?

[johnsold]

You can certainly create your own simplified models.  If all you want is an ideal op amp, just use a controlled source.

Lynn

[akis]

I have stumbled upon "AN-138 : Spice compatible op amp macro models".

It says that most op-amp SPICE models use the Boyle model, which has everything referenced to ground rather than the supply rails, especially the ouput of the op-amp. I think this is the reason why all those op-amp simulations are failing. 

I will now try to use the new macro models and see if it works better.

[akis]

I had to reply because to this message as "i ran out of time to edit" just as I had finished editing...

So I have tried the OP-42 models and they work perfectly and they are as described in AN-138. I can now place the ground anywhere on the circuit.

I think this is something Multisim should warn about, all those other op-amp models should be listed in another directory. Simulation with those other op-amp models is not going to work until and unless you have a supply perfectly balanced around the ground. But when trying to simulate virtual ground and/or battery operated circuits then it is bad news.

****************************************

A bit more on the static probes trying to recreate the issues or determine better steps to show the problem.

1) it seems that randomly a probe will "lose" its "auto-resize" setting, so that it chops off fields that you want displayed.

2) it seems that randomly a probe will stop displaying I (current) and is not fixable unless you delete it and re-insert it.

3) many of these problems are caused by copying and pasting probes around the circuit.

[johnsold]

Which vendor produced the AN-138?  That nomenclature is used by several vendors.

Anytime you are using a simulation, it is important to look at all the assumptions and approximations used, including the internal structure of models. The results of a simulation can be no better than the most limiting factor in the model.  Sometimes the simple question: "Does this result make any sense?" can be a good guideline for when to dig deeper.

I am glad you found a way to get a model suitable for your needs.

Lynn

[akis]

It is Analog Devices ; they have created SPICE models for their own op-amps, quite a few to choose from.

[johnsold]

Thank you.

Lynn