Voltage offset differential amplifier

11 replies · 4K views · last reply
Frank-95
Messages
51
Reaction score
1
Hi all!

I am trying to simulate a differential amplifier in LTSpice but I'm having some troubles.
First, I would like to know if you could suggest me some "basic", scholastic, MOSFET and BJT model, like the 1N4148 for diodes.

Secondly I designed this:
LTspice schematic of a MOSFET differential amplifier: two IRF2805S input transistors M1 and M2 with inputs Vin1 and Vin2, RRQ030P03 current-mirror load transistors M5 and M6 fed from V1 15 V, tail transistors M3 and M4 with R1 100 ohm and V4 15 V source.


Practically when I get the drain output I have a big amplification but with a HUGE DC offset: 12 volts about!
Do you know why?Did I mistaken somehitng?

Moreover I don't remember a thing from my electronics studies: should R1 be linked to ground or to V1?

Thank you very much
 
Perhaps it's better this way
Hand-drawn schematic of a push-pull output stage between +20V and -20V rails, with two IRF2805S MOSFETs M1 and M2 labelled Vin1 and Vin2, bipolar transistors, diodes, resistors, and a labelled Output node.

― the drain of M1 ought to be kept at the same voltage as M2.

It's better to use a dual matched pair of MOSFET in one package as M1 and M2.
 
Last edited:
Your solution makes sense, I have some thoughts though:
First, I would like to use as less resistors as possible, like if it was an IC amplifier.
Secondly, I would like to know why my circuit offsets the voltage so much. This is basically the easiest form of differential amplifier, so there must be a problem I cannot recognize.

Two schematics of a MOS differential amplifier: (a) a pair of NMOS input transistors Q1 and Q2 with a PMOS current mirror load Q3 and Q4, tail current I to -VSS, and output vO; (b) the same circuit annotated with branch currents I/2 and the output relation vO = VDD - VSG3.


This is from the Sedra-Smith; as as you see I replaced the current source with the mirror, but the offset is still there.

What I think is that there is some problem either with transistors model, or ltspice itself. In fact I simulated an exercise from Sedra-Smith:

Textbook circuit diagram of an NMOS common-source stage with drain resistor Rd to VDD = +2.5 V and source resistor Rs to VSS = -2.5 V, with labelled currents ID and VD.


Which results are Rd=5k and Rs=3.25; and LTSpice gives different values for Id and Vd! The model I used is:

.model M1 NMOS(Vto=0.7 Kp=100u L=1u W=32u)

Is the model wrong?
 
It may well be the channel length modulation effect (neglected in the textbook but not in LTspice) to blame. In ICs, MOSFETs with very low channel modulation must be used, otherwise all the mirrors would work wrong. With your differential amplifier, I would first try to decrease the positive supply so as to make the drain potentials (left and right) equal when both the inputs are grounded.
 
Frank-95 said:
Practically when I get the drain output I have a big amplification but with a HUGE DC offset: 12 volts about!
Do you know why?Did I mistaken somehitng?
You are operating the amplifier in open loop. What are you measuring the huge DC offset voltage relative to.

Frank-95 said:
Moreover I don't remember a thing from my electronics studies: should R1 be linked to ground or to V1?
Ground will be quieter and heat the resistor half as much.
 
Your output voltage, (drains of M2 and M6 ?), is centred about +12 volt above ground because that is the voltage on the drain of M5, (and on the gates of the symmetrical p-channel mirror).
 
  • Like
Likes   Reactions: Frank-95
Baluncore said:
Your output voltage, (drains of M2 and M6 ?), is centred about +12 volt above ground because that is the voltage on the drain of M5, (and on the gates of the symmetrical p-channel mirror).

Oh right, my bad, that is the bias point; I've avoided that bypassing the output with a capacitor. But now an abvious questions arises: in real multistage opamp, where the output of one stage is the input of the next stage, is the dc component kept in each stage, it doesn't seem so to me, does it? Moreover, even if it does, is the output always bypassed with a capacitor in real cases?
 
As pointed out by Baluncore we never use this type of circuit without some sort of a negative feedback to "set" DC conditions.
Frank-95 said:
Which results are Rd=5k and Rs=3.25; and LTSpice gives different values for Id and Vd! The model I used is:

.model M1 NMOS(Vto=0.7 Kp=100u L=1u W=32u)

Is the model wrong?

No, your model is just fine. I for Rd = 5k and Rs = 3.25k get Id≈400μA in LTspice
You can also use this model
.model n VDMOS (Vto=0.7 Kp=3.2m)
 
Here is an output stage added to the differential front end.
Attached is an LTspice file diff-amp.asc. Remove the .txt extension to view or run it.
 
Attachments
Last edited:
Jony130 said:
No, your model is just fine. I for Rd = 5k and Rs = 3.25k get Id≈400μA in LTspice
You can also use this model
.model n VDMOS (Vto=0.7 Kp=3.2m)

LTspice schematic of a series circuit: V1 2.5 V source, R1 5k, NMOS transistor M1, R2 3.25k, and V2 2.5 V source, with the model line .model M1 NMOS(Vto=0.7 Kp=100u L=1u W=32u) and .tran 1 directive.


Oh I don't know, this circuit keeps on yielding 54 uA :/

Baluncore said:
Here is an output stage added to the differential front end.
Attached is an LTspice file diff-amp.asc. Remove the .txt extension to view or run it.

Thank you very much, I got your point :)
 
Frank-95 said:
Oh I don't know, this circuit keeps on yielding 54 uA :/
Change NMOS name into M1 . Upper M1 is a transistor designation number not the sim MODEL.
 
  • Like
Likes   Reactions: Frank-95