In the lab I measured the Vgs x Id and Vds x Id curves of a MOSFET transistor (actually, the CD4007 IC that has 3 PMOS and 3 NMOS transistors within).
How would I go into turning this data into a SPICE model? I don't need high accuracy.
I tried writing a VDMOS model for LTspice but it looks like it is more suitable for power MOSFETs.
You could start with a SPICE model of the transistor in a CD4007 and fiddle with the parameters to get it to match your curves.
**************************************************
* Level 1 SPICE Models for the 4007 CMOS chip
**************************************************
* These Level 1 models were extracted from measured results. The
* model attempts to account for the package parasitics. The simulated and
* typical measured device capacitances are as follows:
*
* NMOS: Cgs = 18pF Cds = 14pF
* PMOS: Cgs = 17pF Cds = 26pF
*
* Gate-to-drain capacitances were not extracted but were adjusted to
* to help fit measured results.
*$
.MODEL CMOSP PMOS ( LEVEL = 1 L=5u W=100u
+VTO = -1.40 KP = 3.2e-5 GAMMA = 3.30
+PHI = 0.65 LAMBDA = 9e-2 CBD = 65e-12
+CBS = 2e-14 IS = 1e-15 PB = 0.87
+CGSO = 0 CGDO = 0 CGBO = 1e-5
+CJ = 2e-10 MJ = 0.5 CJSW = 1e-9
+MJSW = 0.33 JS = 1e-8 TOX = 6.89e-10)
*$
.MODEL CMOSN NMOS ( LEVEL = 1 L=5u W=20u
+VTO = 1.77 Kp = 2.169e-4 GAMMA = 4.10
+PHI = 0.65 LAMBDA = 1.5e-2 CBD = 20e-12
+CBS = 0 IS = 1e-15 PB = 0.87
+CBS = 2e-14 CGDO = 88e-8 CGBO = 0
+CJ = 2e-10 MJ = 0.5 CJSW = 1e-9
+MJSW = 0.33 JS = 1e-8 TOX = 1.265e-10)
**************************************************
* Macro for 4007 IC:
**************************************************
*
* Pinout:
*
* S4/psub G1,4 D5 S5 G5,2 S2 D2 * 1,2,3 - PMOS
* _||___||___||___||___||___||___||_ * 4,5,6 - NMOS
* | 7 6 5 4 3 2 1 | * All PMOS susbstrates
* | | connected to pin 14
* | * | * All NMOS susbstrates
* | | connected to pin 7
* | 8 9 10 11 12 13 14|
* _ ___ ___ ___ ___ ___ ___ _
* || || || || || || ||
* D4 S6 G3,6 S3 D3,6 D1 S1/nsub
*
* General Form of subcircuit call:
* X1 n1 n2 ... n14 CMOS4007
*
*$
.SUBCKT CMOS4007 1 2 3 4 5 6 7 8 9 10 11 12 13 14
* MOSFET DR GT SRC SUBS MODEL L W
M1 13 6 14 14 CMOSP L=5u W=100u
M2 1 3 2 14 CMOSP L=5u W=100u
M3 12 10 11 14 CMOSP L=5u W=100u
M4 8 6 7 7 CMOSN L=5u W=20u
M5 5 3 4 7 CMOSN L=5u W=20u
M6 12 10 9 7 CMOSN L=5u W=20u
.ENDS CMOS4007
*
*$
You need to know the device model and parameter extraction flow:.
Example: $$I_d=\frac{1}{2}\mu_n C_{ox} \frac{W}{L}(V_{GS}-V_T)^2(1+\lambda V_{DS}) $$
Data your measurement. (Id vs Vds/ Id vs Vgs)
Example determine Kn = Um.Cox
4.1 Hand cal. (use equation in section 3)
4.2 Curve fitting algorithm: (Levenberg Mardquardt, Gene Algorithm,...) Ref: Matlab, of other ref...
If you want to more accuracy; You should know flow for parameter extraction. It maybe take your time.
Example: Kp-E0 in EKV model:
Hope it help you.
$$Equation + Measurement data + Algorithm$$
In addition to @Spehro's fine answer, Modpex is a firm which produces SPICE models. They offer commercial support and creation of models, however this is likely very costly so is outside the range of everybody except corporations.
Shown on their page is a screenshot of their software titled "Parameter Extraction" and shows curve-fitting data-points to SPICE parameters. The image doesn't look like any OS I've ever seen, and the math they have developed for this goes way beyond what @ohenri100 has shown.
Googling "SPICE parameter extraction" yields many technical papers on the subject. However to successfully generate these parameters, both a PhD in mathematics as well as programming would likely be necessary. If anyone wanted to go down this road, the free R package for Statistical Computing might be a good start. It's free, can do higher-level math, and (with some optional packages) can do regression or curve-fitting a formula to data-points.
