JFET amp noise

If you have a gain of 10 and you are measuring 1.9 nV/rtHz output noise, that means your input noise is 0.19 nV/rtHz. That's not right for a JFET. The 1/f knee will probably be around 1 kHz.

The Siliconix data sheet states that the input noise is < 2 nV/rtHz (you might expect it to be in the 1 to 2 nV range). Thus, you might expect your output noise to be around 20 nV/rtHz if you disregard your drain resistor. At 500 Hz, the equivalent input noise will be higher due to 1/f noise.

You sure are driving this poor little JFET hard.

Try this model. It's an old National Semiconductor model. At least it has Kf. .model 2N5434 NJF(Beta=18.37m Betatce=-.5 Rd=1 Rs=1

• Lambda=25m Vto=-1.906 Vtotc=-2.5m Is=533.7f

• Isr=5.174p N=1 Nr=2 Xti=3 Alpha=152.8u

• Vk=111.9 Cgd=35.6p M=.4283 Pb=1 Fc=.5 Cgs=35.6p

• Kf=251.7E-18 Af=1)

Thanks for the model and help! I most likely misinterpreted the J-FET noise equations on pages 10 & 11 ->

Perhaps the first problems was converting to noise voltage. My second problem was probably misunderstanding the following (top of pg. 11) ->

"The amplifier effect of JFETs is based on changes in the channel resistor. This leads to describing the noise of the channel current ID also by thermal noise [the equation]"

On page 10 they display a model of a jfet. I see three resistors-- Rd, Rs, and gd. LTspice shows Rd & Rs as 1 ohm, but I'm uncertain how to determine the noise for gd. For gd noise I figure ->

Inoise^2 = 8/3 * k * T * gm * dF

, which I think is V = (8/3 * k * T * 1/gm * dF)^0.5

After an hour of google searching I concluded that gm was what LTspice called BETA, which is about 18E-3 for 2N5434.

Yes, lol. I was trying to keep the resister as low as possible for low thermal resister noise. That's why I picked the largest FET gm on my LTspice. Higher gm's equated to lower resistor. Although if the noise after gain of 10 is more like 20 nV/RtHz than I guess a few KOhms won't make much difference. :-)

I appreciate any help! Paul

Your source impedance is low, in the ballpark of 400 ohms, so one way to get low-noise gain would be a step-up transformer, which could drive a low-noise jfet or opamp and get you down around 0.1 nv/rthz. There are some stock super-shielded audio transformers that should work.

Resonating your inductive source might be interesting, too.

John

Hello Paul,

there has been a longer thread about low noise JFET amplifiers with the IF3601. Serach on this link for IF3601.

At which frequency is the self resonance of your 100mH sensor coil? The sensitivity may steeply fall above this frequency.

Best regards, Helmut

schrieb im Newsbeitrag news: snipped-for-privacy@u72g2000cwu.googlegroups.com...

It's certainly not right. My Spice program lets you also do a noise analysis, and displays it on the frequency axis.

With a BJT you will get much less noise with low source impedances, FETs are of advantage only above 20k. You could reach with a 2SA1083E around

.-----------+-------------------o+9V | | .-. .-. | |2k7 | | | | | |1k ||'-' ___ '-' 100uF GND||-+-|___|+ | ___ +|| ||+| 10k | +-|10R|---||-GND 10uF | | | ___ || | 4148 +->|-+-|3k3|-----------. | | | | | ||+ | |< | IN o--)--||--+--| 22p|| | | || |\\ .---||-. | .-.10uF | | || | | | | | | |\\ | | | |1k8 +--+-|-\\ | ___ | || ||'-' | | >-+-|___|-+--||-oOUT GND||-+-----------)----|+/ 100R || ||+| | |/OP37 10uF 10uF.-. .-. | |2k2 | | Gain 330 times | | | |1k '-' '-' | | === === GND GND (created by AACircuit v1.28 beta 10/06/04

are

Hello Ban, you have overlooked his 100mH input source(sensor). This will result in a source impedance of hundreds of kOhms at a few 100kHz. The high input noise current of bipolar transistors will result in a high noise voltage. His circuit doesn't has a low source impedance in the main fequency range of interest.

Best regards, Helmut

Helmut, I couldn't import his netlist and see the circuit, but someone talked about 400 ohms and so I thought it was microhenry, which corresponds better with the 700kHz. Anyway it doesn't make sense at all to have a sensor with this inductivity, it must have a Q of 10000. Seems to be only playing around with something. As long as the OP doesn't reveal his actual application, we can only speculate. I guess the FET will have some gate capacity, so certainly it will attenuate the signal beyond the resonance as well. Maybe it is a guitar pickup, but WTF it has to do with 700k, or it is a filter for a digital amp, who knows. I doubt the Q will be higher than 50, so with 400R DC-resistance you hardly will get more than a few 10s of k, doubtful any FET will be of much use then.

I think the 2N5434 has an input C around 30 pF. That would make his input resonate around 100 kHz. Probably lower resonance with Miller capacitance added in. He must have a magic coil if it can be used up to 700 kHz.

Hello Ban,

You are right that the bandwidth of 700kHz with a 100mH coil looks like mission impossible. Has anybody achieved such a high bandwidth with a large coil? It would be helpful to hear from others what they have achieved

Best regards, Helmut

PS: Ban, I will send you my LTspice schematic. Let's hope your email address is valid, if not then just send me a valid address if you are interested in the schematic. Btw, the original circuit had 0Ohm source resistance.

Hi,

Thanks for the help.

I have an updated LTspice .asc file below, which seems to demonstrate the FET amp working well from 700 to 700,000 Hz just by adding a cap in parallel to the inductive input source. I noticed on LTspice that if the cap is removed then the output drops to nearly zero at higher frequencies.

Does it seem realistic that adding a cap in parallel to the inductive source would extend the bandwidth? On paper it makes sense, but it seems to good to be true--just add a cap and you get more bandwidth.

I'm still trying to understand the FET noise equations on pages 10 & 11 of the following pdf ->

Where does the FET's amplification come in the equations? A FET with a gain of 10 should have more output noise than a gain of 5, but I'm not seeing "gain" in the equations.

Many thanks, Paul

Here's the LTspice .asc file ->

Version 4 SHEET 1 880 680 WIRE -192 288 -240 288 WIRE -80 288 -112 288 WIRE 48 288 0 288 WIRE 48 384 48 288 WIRE 64 384 48 384 WIRE 160 288 128 288 WIRE 160 384 128 384 WIRE 160 384 160 288 WIRE 208 32 208 -32 WIRE 208 144 208 112 WIRE 208 352 208 320 WIRE 320 224 208 224 FLAG 208 352 0 FLAG -240 288 0 FLAG 208 -32 0 FLAG 320 224 out SYMBOL voltage -96 288 R90 WINDOW 3 24 104 Invisible 0 WINDOW 39 0 0 Left 0 SYMATTR InstName V1 SYMATTR Value SINE(0 1e-6 700e+3 0) SYMATTR Value2 AC 0 0 SYMBOL njf 160 224 R0 SYMATTR InstName J1 SYMATTR Value 2N5434 SYMBOL res 192 128 R0 SYMATTR InstName R1 SYMATTR Value 80 SYMBOL Misc\\\\battery 208 128 R180 WINDOW 0 24 104 Left 0 WINDOW 3 24 16 Left 0 SYMATTR InstName V2 SYMATTR Value 8 SYMATTR Value2 AC 0 0 SYMBOL ind 32 304 R270 WINDOW 0 32 56 VTop 0 WINDOW 3 5 56 VBottom 0 SYMATTR InstName L1 SYMATTR Value 100e-3 SYMATTR SpiceLine Rser=5 Rpar=10e+6 Cpar=500e-12 SYMBOL cap 128 368 R90 WINDOW 0 0 32 VBottom 0 WINDOW 3 32 32 VTop 0 SYMATTR InstName C1 SYMATTR Value 1000e-12 SYMATTR SpiceLine Rser=2 Lser=0 Rpar=3000e+6 SYMBOL voltage 16 288 R90 WINDOW 3 24 104 Invisible 0 WINDOW 39 0 0 Left 0 SYMATTR InstName V3 SYMATTR Value SINE(0 1e-6 700 0) SYMATTR Value2 AC 0 0 TEXT 238 402 Left 0 !.tran 0 4e-3 0 1e-9

In article , qrk wrote: [....]

The signal at 700KHz will be down a fair bit but not zero. He may still get enough signal at the 700KHz frequency to consider it "working".

Paul, when you put a capacitor in parallel to the coil, it will conduct the high frequencies, which are attenuated by the coil. But this happens only in a simulation, because your voltage source is not distributed across the inductivity as in real life, but artificially put at the input. A simulation is only a *model* for the circuit and you should be aware of that continuously to not make erraneous assumptions. Also you will have a DC resistance of that pick-up, which can be modelled with a resistor in series. It should be included in the model. There is the possibility to make a noise analysis in spice, so select "edit simulation command" and specify the parameters for noise analysis. You can then compare your calculations to the result and see if they coincide. Usually the noise voltage is referred to the input, so the gain is multiplying this number. Actually you will see that only the "real" part of a complex impedance contributes to the noise. But since the input impedance of the amplifier and the parasitic capacitance of the coil attenuate the signal and require higher gain, noise will rise with higher frequencies and thus it will be impossible to use this sensor above a few tenths of kHz, let alone 0.7MHz.

Hello Ban,

I have checked your attached schematic and found a mistake in your coil model. If the coil is the sensor for magetic fields, then the voltage source is part of the coil and not externally as shown in your schematic. This makes a very big difference.

I will sent you and Ban a corrected version. Please take a look to the falling gain at frequencies above 20kHz. This corner frequency is the frequency of self resonance of your sensor coil. It mainly depends on the winding and stray capacitance of your coil.

JFET: Gain=4.8 (13.6dB) @ low frequencies Gain=38.1 (16dB) @ 19.6kHz, resonance Gain=0.0038 (-48.1dB) @ 700kHz Gain falls with 40dB/decade above resonance

PSPICE documentation : PSPPCREF.pdf Saturation region: Vds > (Vgs-Vto) Id = beta*(1+lambda*Vds)*(Vgs-Vto)^2 From the equation: Gm = dId/dVgs = 2*beta*(1+lambda*Vds)*(Vgs-Vto) Gds = dId/dVds = beta*lambda*(Vgs-Vto)^2

-> Vnoise = sqrt(InD^2)*RLoad/Gds/(RLoad+1/Gds)

Best regards, Helmut

Hi Helmut and all,

Words can thank you enough! That was one heck of a .asc file! I uncommented the .noise directive, which taught me how to use the LTspice noise simulation. Great stuff, great program. I see that by removing either Kf or Af from the fet model that it greatly reduces the noise, as expected. :)

It's a whole new ball game now. The coil capacitance needs to come down considerably, which is doable, but will increase the series resistance. Last, but not least is the fet-- it has way too much cap.

Can't thank you all enough. I'd like to post the results when complete ...

Many thanks, Paul

Hi,

I built several "Linear Technology" op-amp noise test circuits in LTspice and can't get anything close to Linear's results. Below are four LTspice .asc files. For the first test, "LTOpAmpNoise.asc", I tried the basic 1K noise test circuit found in the Linear LT1028 pdf on page 10 ->

I used the LT1028 for my tests. It's a 1 KHz noise test, which yields just over 1.3 mV/Hz1/2. Yes, that's milli, not nano. :( The output graph is on V(onoise).

OK, so I tried another test, 0.1 to 10 Hz noise test found in the same pdf on page 11. I tried 3 flavors of this particular circuit. First, I did a noise test of just the first stage of the circuit-- leaving out everything after the 2K resister. This circuit is "LTOpAmpNoiseB.asc" below. This yields 2.5 uV/Hz1/2 at 0.1 Hz and just over 1.3 uV/Hz1/2 at 10 Hz. Then I added the entire two-stage circuit, "LTOpAmpNoiseC.asc". It shows huge caps, up to 22 F, but I tried it anyways yielding approximately 81.5 pV/Hz1/2 from 0.1 Hz to 10 Hz. Then I thought maybe all the caps are microfarads. So I made all the caps microfarads and this circuit is "LTOpAmpNoiseD.asc," which yields values above 40 mV/Hz1/2.

Any ideas what might be wrong?

Thanks, Paul

Below are links to the files. Once downloaded, just change .txt to .asc

Hello pm,

Your choosen opamp model doesn't include a noise model. Please use the LT1028N model for .NOISE analysis. Many opamp models don't include a noise model circuit. This is true for other IC manufctureres as well.

Btw, you have forgotten the power supply connection on the LT1001 in circuit C and D.

Best regards, Helmut

There is a user group for LTspice.

This is a correct test circuit with the LT1028N. Copy the following text into a file named test.asc .

Version 4 SHEET 1 880 680 WIRE -304 144 -304 96 WIRE -304 256 -336 256 WIRE -304 256 -304 224 WIRE -304 272 -304 256 WIRE -304 400 -304 352 WIRE -144 192 -144 112 WIRE -144 336 -144 272 WIRE -144 352 -144 336 WIRE -80 112 -144 112 WIRE -80 336 -144 336 WIRE 48 112 0 112 WIRE 48 240 48 112 WIRE 48 336 0 336 WIRE 48 336 48 272 WIRE 64 112 48 112 WIRE 80 240 48 240 WIRE 80 272 48 272 WIRE 96 224 96 208 WIRE 112 304 112 288 WIRE 176 112 144 112 WIRE 176 256 144 256 WIRE 176 256 176 112 WIRE 224 112 176 112 FLAG 224 112 out FLAG -336 256 0 FLAG -304 96 +V FLAG -304 400 -V FLAG 96 208 +V FLAG 112 304 -V FLAG -144 352 0 SYMBOL Misc\\\\battery -304 128 R0 WINDOW 123 0 0 Left 0 SYMATTR InstName V2 SYMATTR Value 5 SYMATTR SpiceLine Rser=0 Cpar=0 SYMBOL Misc\\\\battery -304 256 R0 WINDOW 123 0 0 Left 0 SYMATTR InstName V3 SYMATTR Value 5 SYMATTR SpiceLine Rser=0 Cpar=0 SYMBOL voltage -144 288 R180 WINDOW 3 24 104 Invisible 0 WINDOW 123 0 0 Left 0 SYMATTR Value SINE(0 10n 1000) SYMATTR InstName V1 SYMATTR SpiceLine Rser=1m Cpar=1p SYMBOL res 48 128 R270 WINDOW 0 32 56 VTop 0 WINDOW 3 0 56 VBottom 0 SYMATTR InstName R2 SYMATTR Value 100K SYMBOL res -96 128 R270 WINDOW 0 32 56 VTop 0 WINDOW 3 0 56 VBottom 0 SYMATTR InstName R3 SYMATTR Value 100 SYMBOL res -96 352 R270 WINDOW 0 32 56 VTop 0 WINDOW 3 0 56 VBottom 0 SYMATTR InstName R4 SYMATTR Value 100 SYMBOL Opamps\\\\LT1028N 112 192 R0 SYMATTR InstName U2 TEXT -320 -8 Left 0 !.noise V(out) V1 dec 100 1 10k

Thanks again Helmut. Looks like I got lucky by choosing 1028. :) Mostly I wanted to learn how different op-amp changes affect output noise. It seems the LT1028N wants extremely low R's. In fact, there seems to be no lower limit. For example, by placing a short on all resisters, say 1 uOhm gives 200 fV/Hz1/2!

A few weeks ago I did some real noise tests using a NTE937M. I left R3 and R4 open and R1 and R2 shorted together-- open loop gain. This was fed to a Sample & Hold sampling at 780 Hz, which was fed to another op-amp that had a large feedback cap. The cap size was selected so that output noise did not fluctuate too fast. It's not too scientific, but without hooking it up to my computer for spectrum I'd guesstimate an output bandwidth of roughly a few Hz. This gave an average voltage fluctuation of a few nV per second. Now if I replicate that open loop op-amp using the LT1028N it gives 2.5 uV/Hz1/2 noise ! That's microvolts, not nanovolts. I understand high R's generate a lot of noise ... but no connection? I find it hard to believe that an air gap will generate thermal noise, but I guess it's possible. ... What about Los Angeles air, lol? If we follow that logic then what about a vacuum gap? Therefore, I wonder if the 2.5 uV/Hz1/2 open loop LT1028N simulation circuit is correct. If so, then perhaps some op-amps prefer open loop gain and some do not? NTE937M is a fet input op-amp btw.

Thanks, Paul

Hello Paul,

I cannot follow your circuit with the LT1028, because there is no R1 in the LTspice schematic above. What circuit have you used?

Open loop means the opamp is running without feedback and so it will have gain of more than 10.0e6 with the LT1028. You can't do any useful measurement with this gain. What's open loop for you in your description above?

Best regards, Helmut