LT Spice diode C-V graph

This is rude and crude but looks OK. Horizontal is 1 ns per volt, vertical is 1 volt per pF. That 1N914 keeps depleting past 1 kilovolt!

Version 4 SHEET 1 896 680 WIRE 48 80 0 80 WIRE 176 80 48 80 WIRE 320 80 240 80 WIRE 416 80 320 80 WIRE 512 80 464 80 WIRE 560 80 512 80 WIRE 0 144 0 80 WIRE 320 144 320 80 WIRE 464 144 464 80 WIRE 416 160 416 80 WIRE 0 272 0 224 WIRE 320 272 320 224 WIRE 416 272 416 208 WIRE 464 272 464 224 FLAG 0 272 0 FLAG 320 272 0 FLAG 416 272 0 FLAG 464 272 0 FLAG 512 80 CAP FLAG 48 80 RAMP SYMBOL diode 240 64 R90 WINDOW 0 -57 29 VBottom 2 WINDOW 3 -52 29 VTop 2 SYMATTR InstName D1 SYMATTR Value 1N914 SYMBOL res 304 128 R0 WINDOW 0 -58 44 Left 2 WINDOW 3 -61 74 Left 2 SYMATTR InstName R1 SYMATTR Value 1m SYMBOL voltage 0 128 R0 WINDOW 0 28 111 Left 2 WINDOW 3 -11 192 Left 2 WINDOW 123 0 0 Left 2 WINDOW 39 0 0 Left 2 SYMATTR InstName V1 SYMATTR Value PULSE(0 2000 0 2000n) SYMBOL e 464 128 R0 WINDOW 0 64 53 Left 2 WINDOW 3 58 85 Left 2 SYMATTR InstName E1 SYMATTR Value 1e6 TEXT 16 104 Left 2 ;RAMP 1 V/nS TEXT 496 112 Left 2 ;1 V / pF TEXT 538 315 Left 2 !.tran 500n TEXT 360 -40 Left 2 ;Capacitor C:V Curve TEXT 352 0 Left 2 ;J Larkin June 27, 2014

Grekhov should have lived to see this day. Spherical cows rule. ;)

Cheers

Phil Hobbs

Easy, is to buy the source/meter Keithley solution. They'd love to explain it all to you...

This one, I think; the small-signal capacitance versus voltage is a very good indicator of the doping profile inside the junction (as the depletion region boundary moves through the various dopant concentrations). Classic work on this was done at Bell Labs, by Lawrence and Warner Diffused Junction Depletion Layer Capacitance Caculations, BSTJ vol. 34, 1955

I bought an expensive Keithley source-meter. Crap. Sent it back.

But I meant in LT Spice, which is why I titled the post "LT Spice..."

I can read the C-V curve off the data sheet. What I want to do is make sure (or force) my Spice sim to behave like the actual diode, so I want to do a simulation of the diode c-v curve, to make sure I have everything right.

I mistakenly also thought you were trying to devise an instrument.

There's a better way in a Spice simulator, using a gimmick I devised to measure input capacitance in amplifiers... extracts both real and imaginary parts.

If I have time today, I'll post it. ...Jim Thompson

I don't know how to post-process data in LTspice, but here's how I do it in PSpice...

An alternative is to do it like the Keithley does, superimpose a small sinusoidal signal on the DC, and measure the co-sinusoidal current. ...Jim Thompson

The voltage ramp thing that I did seems OK.

It does report the initial capacitance of a 1N914 as 4 pF, which is high, but that's the value in the LT Spice model.

The PSpice model has the same CJ0. ...Jim Thompson

Various data sheets have typs from 4 to 0.85. Not the thing you'd want to use as a varicap.

I do need a "power varicap" for a weird thing I'm considering. I figured I'd fudge up some standard LT library parts, series and parallel or whatever, to see if my circuit might work. If it does, then I can try to find real diodes with the required CV curves.

What's your maximum voltage? You might want to try some zeners. ...Jim Thompson

Jim, I sent you all that stuff!

simply EXPORT the variable you want to work with. If you can live with uneven steps it's fast. if you cannot...

easiest way for me...after a .tran run ltsputil.exe in a batch file to make the steps uniform use N+1, like

after running the uniform step conversion, open the new example_eq.raw file and EXPORT something from that!

like V(out), which comes out as a text file in columnar form t, V(out) You can scoop if you want and put in Excel

I use a text editor and strip off the text header, rename, and save as vo.txt and load into octave

then I pull out the t, separate from the v and you're up and running doing anything you want.

You get a lot more power that way and avoid all the artifacts that LTspice puts into the FFT. Plus you can also do things not possible in LTspice [I think]

I'm talking a direct graphical display, called "Performance Analysis" built into Probe, the PSpice post-processor.

I have the opposite problem... actually the math is solved and I await my programmer son to be in-need to get him to write an executable for me: take _evenly_ spaced data and "sparse" it into as few points as necessary to meet an RMS error criterion.

...Jim Thompson

just install something like octave or scilab, simple scripting of every fil e handling, plotting and curve fitting function you can imagine

-Lasse

Oh, 4KV or so.

PSpice supports the Berkeley (dot)PRINT statement, so I can generate columnized data simply by adding, in LTspice lingo, a "Spice directive" .PRINT V(N_27) I(VDC:+) etc.

It's really odd that LTspice doesn't support that :-( ...Jim Thompson

Oooooh! And probably need 10:1 capacitance also ?:-) ...Jim Thompson

Which is better? ...Jim Thompson

do

ike

file handling, plotting and curve fitting function you can imagine

on windows probably scilab

Octave is much more Matlab compatible but to get a gui you need to get vers ion 3.8+ but that's "experimental" for windows

Matlab is the Rolls-Royce, but it comes at a Rolls-Royce price

-Lasse

Y5V capacitor?