How to calculate and simulate offset of OpAmp?

[tyanata]

pelgrom formula offset

Can some one tell how to calculate and how to simulate offset of operational
amplifier?

 

[Hughes]

opamp monte carlo simulation

Please refer to TI's application notes, **broken link removed**

 

[etherios]

floating voltage source op amp

If i remember correctly you connect the 2 inputs together and run an .op analysis in SPICE you will see so the difference in the output from the value you expect. If you use some other tool you should do the same.

 

[flatulent]

Re: Op amp offset

The offset is caused mostly by the input transistors not being equal in size and doping profile. The load current mirror being not a gain of 1.00000 will also cause problems.

There are several ways to do the simulation. One is to put an ideal voltage source in series with one of the inputs. Another way is to use the size scale factor and make one transistor 1.005 times the size of the other.

 

[bastos4321]

Re: Op amp offset

Thats not correct flatulent (wy the 1.005 factor).

The offset is get by doing a Monte Carlo simulation of the ampop using matching parameters of the transistors for a given process. Use at least 100 runs.

Other way is to account the matching of the input transistors and main other contributions from the other ones divided by the gain of the input stage. The matching parameters is divided by the square root of the transistor area. This is an estimation of the offset. The monte carlo method is more accurate.

bastos

 

[flatulent]

Re: Op amp offset

My suggestions were on how to put in some offset for seeing what effect it has on circuit performance. The added floating voltage source is the best way to add offset to a macromodel. If you are trying to find the range of offsets for an op amp design, you will have to vary the beta of all transistors as well as their areas and early voltages. The input transistors are made intentionally large so that the areas do not change much when the linear dimensions change from the oxide etching tolerances. That is why I suggested a low value of 1.005 for making a small offset.

The doping gas flow over the wafer is perturbed by the surface height changes which will make the transistor doping profiles different for each transistor. Small changes in gas flow rate will make the perturbation different. For MOS transistors the gate oxide thickness will be variable. For JFET types the pinchoff and gm will vary with these processing variations plus the implant dose and energy variations. These implant variations will also affect MOS thesholds.

One sneaky trick in the old days for DAC and ADC designs was to add dummy resistors to each end of the layout of the used resistors to make the gas flow perturbation more uniform over the used resistors.

Another source of offset is heating of the die by the transistor and resistor power dissipation which makes thermal gradients. The heating is different for different current draws caused by part parameter changes.

And to top it all off, many amps are laser trimmed for offset which makes these simulations not predict the final product performance.

 

[Hughes]

Re: Op amp offset

Hi, bastos4321,
Do you know how to do Monte Carlo analysis for VTH mismatch?

 

[bastos4321]

Re: Op amp offset

I agree with flatulent.

To model just the effect of the offset is as flatulent indicated. To get the value of the offset is needed the matching parameters.

I'm not used to bipolar designs, only CMOS, but one thing I have never seen yet is matching parameters for bipolar transistors. Do they vary with the square root of area as MOS ?

Bastos

 

[bastos4321]

Re: Op amp offset

For VTH mismatch I use a gausian distribution.


Ex:
.PARAM WMm1cp6=AGAUSS(7e-06 , 7.93725e-08 ,3) VtoMm1cp6=AGAUSS(0 , 0.00822073 ,3)
Mm1c y2 bias1 avdd avdd pmoshv w=WMm1cp6 l=4e-06 m=2 ad=5.95e-12
+ as=1.085e-11 pd=3.1e-06 ps=1.15e-05 nrd=0.0642857 nrs=0.0642857
+ DELVTO=VtoMm1cp6

Bastos

 

[flatulent]

Re: Op amp offset

I'm not used to bipolar designs, only CMOS, but one thing I have never seen yet is matching parameters for bipolar transistors. Do they vary with the square root of area as MOS ?

Bastos

For a fixed Vbe, the emitter (and therefore for high beta the collector current) scales as the emitter area. The Vbe is adjusted to get the current back to equal. Ic = constant x exp(Vbe/26mV) is the controlling equation at room temperature. Where constant is a function of all sorts of geometric and scientific parameters. You can solve this backwards to get Vbe equal to the natural log of the collector current.

 

[bastos4321]

Re: Op amp offset

I'm not used to bipolar designs, only CMOS, but one thing I have never seen yet is matching parameters for bipolar transistors. Do they vary with the square root of area as MOS ?

Bastos

For a fixed Vbe, the emitter (and therefore for high beta the collector current) scales as the emitter area. The Vbe is adjusted to get the current back to equal. Ic = constant x exp(Vbe/26mV) is the controlling equation at room temperature. Where constant is a function of all sorts of geometric and scientific parameters. You can solve this backwards to get Vbe equal to the natural log of the collector current.

Thanks flatulent for the answer.

The constant is the IS corrent (saturation current). This IS current is inversely to the base width W and directly proportional to the emitter area. What I ask is if the emitter area factor matching scales with the square root of area as in MOS.

Do you have some numbers about this matching. I would use this data in the design of bandgap circuits.

Bastos

 

[flatulent]

Re: Op amp offset

I do not have any current numbers. The last IC I designed used 10 micron lines and spaces and the mask was cut by hand on rubylith.

On the mismatch factor, I suspect that it is more of a linear function. The differential amplifier transfer curve is hyperbolic tangent which is a linear function in the crossover region. The square root is very linear for values near 1. sqrt(1 + a) = 1 + a/2 is a good approximation for small values of a of either polarity.

 

[bastos4321]

Re: Op amp offset

In MOS we have the Avt and Abeta matching parameters. The first approximation to the offset is calculated as Avt/sqrt(WL). The distance between the MOS also have some impact in the formula.

For bipolar I suspect that it has the same type of dependence, not linear with the area, since in origin (for a diferential pair), both transfer functions are aproximate linear. One with a hiperbolic tang and the other with a "square".

Just given the reference paper for MOS matching.

M. Pelgrom, "Matching proprieties of MOS transistors" IEEE, JSSC, vol 24, pp. 1433-1439, october 1989.

 

[kkoko]

Re: Op amp offset

Offset in operational amplifier is very difficult process, because the mismatches between different transistors produce random offset that we can simulate with help of worst case analysis

 

[jake]

Re: Op amp offset

Offset in operational amplifier is very difficult process, because the mismatches between different transistors produce random offset that we can simulate with help of worst case analysis

kkoko, what's the worst case for an operarional amplifire?

 

[crazyamd]

Re: Op amp offset

Monte Carlo simulation will do

 

[paladinzlp]

Op amp offset

Please read the book: CMOS analog circuit design.

 

[dasong]

Re: Op amp offset

I design a bandgap reference ,who can tell me how to redurce the offset of the OPA ,it make the bandgap working bad!!!

 

[Vamsi Mocherla]

Re: Op amp offset

Dear Dasong,

What is the architecture of your amp? If it is two staged, then you have to take care of the aspect ratios of the current mirrors in the first stage and the stage stage Common source amplifier.

 

[lunren]

Re: Op amp offset

I design a bandgap reference ,who can tell me how to redurce the offset of the OPA ,it make the bandgap working bad!!!

The OPA offset includes two parts, one is internal offset as previous reply said; the other part is caused by the mismatching between the input pair and the mirror load. To reduce the second part of offset, bigger transistor is better and you should pay more attention to layout: dymmy device, unit matching, common-centroid layout, sometimes, same current direction of the two pairs will be better.