current to voltage converter using ua741 op amp PSPICE

[TheFrisku]

Hi to all,
i'm a new member and my english isn't very good, sorry...

I need to create a circuit to convert 0-50mA to 0-3.3V, using a 741 op amp for my university. We want to use an opamp as a transresistance amplifier.

When i try my circuit on the pspice simulator the ua741 saturates...probably my circuit isn't good or i have to add other elements in my circuit.
We use the Orcad 9.1 Student version for our simulations.

So:
In input we have a current DC in the order of mA.
In output we want a voltage max of 3.3V .

If anybody could show me a circuit using a 741 op amp to achieve the above I would be greatly appreciative!!

 

[schmitt trigger]

You have drawn the circuit correctly.

But...
In an opamp I-to-V converter, the opamp's output has to sink ALL the current.
The 741, by a long shot, cannot sink 50 mA linearly.

 

[MikeMl]

Here is a way of boosting the current sinking capability of the 741. Not sure if the output is supposed to be -3.3V when the input is +50mA, or +3.3V.

The horiz axis (independent variable of the simulation) in the plots is the current flowing into the I/V.

 

[ccurtis]

Alternatively, you can force (shunt) some of the current to ground. The smaller, remaining amount of current will flow through the feedback resistor to virtual ground from which the output voltage is developed. Like this:

 

[TheFrisku]

You have drawn the circuit correctly.

But...
In an opamp I-to-V converter, the opamp's output has to sink ALL the current.
The 741, by a long shot, cannot sink 50 mA linearly.

Yes, i also supposed this with the use of 741 ...what kind of op amp (that is in the Orcad's libraries ) i have to use?

 

[TheFrisku]

Here is a way of boosting the current sinking capability of the 741. Not sure if the output is supposed to be -3.3V when the input is +50mA, or +3.3V.

The horiz axis (independent variable of the simulation) in the plots is the current flowing into the I/V.

Sorry, the output IS supposed to be -3.3V when the input is +50mA ....the op amp has to work like an inverting amplifier, so Vout has to be negative...

However thanks for this circuit!

 

[TheFrisku]

Thanks to all, at this point can you show me the same circuit


with the use of another op amp (from Orcad's libraries please) that is better than 741?

 

[alec_t]

The same principle applies to all op-amps. Just pick one from the Orcad library.

 

[MikeMl]

Sorry, the output IS supposed to be -3.3V when the input is +50mA ....the op amp has to work like an inverting amplifier, so Vout has to be negative...

However thanks for this circuit!

Then just take the output at "out~", and leave off the second inverting stage.

Orcad doesn't provide the specs (like current sinking capability); the manufacturer's data sheets do. By the time you sit down in front of a simulator, you should have selected the components you need to use.

 

[KeepItSimpleStupid]

I've successfully used the LT1010 for buffering the drive of a I-V converter. I did end up using the high capacitance driver in their application notes. You put the circuit in the application note inside the feedback loop.

So watch out for capacitive loads. In almost all implementations it's advantages to put a capacitor in parallel with Rf to limit bandwidth. f=1/(2*∏*R*C)

Also be aware that outputting 3.3 V at full scale may cause you other issues is your supply is 3.3V. You typically can't read at the supply voltages.

I haven't played with single supply versions, but you can bias it upwards so that your transfer function is Vout-Vb-Irf.

At 50 mA, you may still have lead resistance to deal with in your measurements. A 4-terminal I-V converter is pretty tough to design although I have.

Vos is generally the most critical parameter for an I to V converter, followed by the input bias current. Be sure to add offset nulling and know when you need it. Ib is very temperature dependent.

 

[TheFrisku]

I simulate your circuit and it works! So thanks a lot!

Then just take the output at "out~", and leave off the second inverting stage.

I don't understand what i have to do...sorry (probably is for my bad english)... Can you show me the img of the changed circuit?
Thanks!

And we would to know where do you find this model? We'd like to know some informations about this circuit....like some references or constitutive equations of this circuit....
All you can tell me about it, will definitely help our job.
Thanks!

 

[TheFrisku]

Alternatively, you can force (shunt) some of the current to ground. The smaller, remaining amount of current will flow through the feedback resistor to virtual ground from which the output voltage is developed. Like this:

Thanks for the circuit....it also works in Orcad!
But the output IS supposed to be -3.3V when the input is +50mA.... so can you show me how to change the circuit to have Vout=-3.3V ?

 

[MikeMl]

Just remove the inverting stage. The opamp forces the non-inverting input to virtual ground, so all of the input current flows through R1. The voltage at V(out~) is E=IR = 0.05χ(3.3/50m) = -3.3V. Since the opamp can't sink 50mA, Q1 is used as a current booster. Now the opamp only has to sink 50mA/hfe = 500uA (see red trace).

 

[ccurtis]

Thanks for the circuit....it also works in Orcad!
But the output IS supposed to be -3.3V when the input is +50mA.... so can you show me how to change the circuit to have Vout=-3.3V ?

Sure. Just swap the connections to the inputs of the op amp.

 

[TheFrisku]

Just remove the inverting stage. The opamp forces the non-inverting input to virtual ground, so all of the input current flows through R1. The voltage at V(out~) is E=IR = 0.05χ(3.3/50m) = -3.3V. Since the opamp can't sink 50mA, Q1 is used as a current booster. Now the opamp only has to sink 50mA/hfe = 500uA (see red trace).

Thanks! We used many models(Q2N3906 and Q2N2907A) of your Q1 in the orcad student version 9.1....we failed. Do you have a spice model of your BJT or some others that can be useful in orcad for this circuit?

 

[TheFrisku]

Alternatively, you can force (shunt) some of the current to ground. The smaller, remaining amount of current will flow through the feedback resistor to virtual ground from which the output voltage is developed. Like this:

We are interested in the use of R1 and R2.
What kind of equation is behind the use of R1 and R2? Why just 10 and 90 ohm? And why not 20 and 70?
We understand that with this sistem of resistences only the 10% of I1 flow through R4....but why? there is any connection with the opamp?

 

[ccurtis]

We are interested in the use of R1 and R2.
What kind of equation is behind the use of R1 and R2? Why just 10 and 90 ohm? And why not 20 and 70?
We understand that with this sistem of resistences only the 10% of I1 flow through R4....but why? there is any connection with the opamp?

Hi. In ideal op amp theory, the right side of R2 must be at zero volts (virtual ground) because the other input of the op amp is grounded (at zero volts). The equation then for the current through R2 is the common current divider with R1: I[SUB]R2[/SUB]=I[SUB]in[/SUB](R1/(R1+R2)). Since in ideal op amp theory there is no current flow into the opamp inputs, the current I[SUB]R4[/SUB] must also be the same as the current I[SUB]R2[/SUB]. So the output voltage V[SUB]out[/SUB] is then I[SUB]R4[/SUB]*R4, or I[SUB]R2[/SUB]*R4. Combining the two equations:

V[SUB]out[/SUB]=(I[SUB]in[/SUB]*R1*R4)/(R1+R2)

Of course, you can use other values of resistors to get the same result, but the current through R2 (and thus R4) must be less than the maximum output current handling capability of the op amp, whatever values you choose.

 

[MikeMl]

The problem is not likely the BJT model. I tried the LTSpice sim again with a both a 2n3906 and 2N2907 and the circuit worked as before. The only difference was the base current was a little bit different because those transistors have a different Hfe than the generic PNP in the circuit I posted.

More likely, the model of 741 is bad, or you are missing a connection. Try a basic current to voltage converter with just a single resistor (leave out my BJT current booster), and see if it works for currents less than ~25mA. Are you sure you have -15V connected to the negative supply pin on the 741?

 

[TheFrisku]

Thanks! The problem was a connection!

 

[TheFrisku]

Hi to all! Thank you for all the answers!
I have one final question for the circuit with BJT model.
I use "PSpice AD" program for simulations and i have to simulate that circuit for the frequency response.
So the circuit now is:

And the frequency response is:

You can see that the start GAIN is too big. In theory it has to be G=3,3V/50mA=66.
The DC simulation was good:

My question is...where is the error?? Is it my fault? Or the BJT model changes the total GAIN?