Hochschule Kempten      
Fakultät Elektrotechnik      
Interface Electronics       Fachgebiet Elektronik, Prof. Vollrath      

Interface Electronics

02 SPICE

Prof. Dr. Jörg Vollrath


01 Introduction and basic properties

Video 2. lecture


Länge: 01:06:27
0:0:0 Review Introduction

0:0:44 Video recording

0:1:34 LTSPICE start

0:2:49 LTSPICE configuration white background and thick lines

0:5:13 Thick lines

0:7:29 Start schematic with resistor

0:8:44 Finished low pass placing parts

0:12:12 Values for components

0:12:44 Labels node names

0:13:19 Simulate .op

0:14:59 Turning a resistor changes polarity of current

0:16:12 Simulate .dc voltage ramp

0:17:1 Add trace to graph

0:18:44 Sine voltage at source

0:19:44 Transient simulation .tran

0:20:30 Graph discussion

0:21:6 Higher frequency

0:22:36 AC simulation, voltage source and command

0:24:14 Graph discussion

0:25:6 Corner frequency

0:26:56 Context sensitive menues

0:27:36 Measure command .MEAS

0:28:54 Verification of result

0:30:13 Data converter schematic 4 Bit DAC

0:31:36 Copying SPICE code to local drive

0:32:36 Copying subcircuits .asc .asy

0:33:56 ADC circuit download

0:34:37 ADC DAC test circuit

0:35:33 Explanation test circuit

0:36:33 Hierarchie

0:37:18 Sample and hold

0:38:43 .Save command

0:40:13 16 steps

0:41:53 Voltage probe

0:42:23 High frequency sampling

0:44:25 12 Bit test circuit

0:45:58 Tools for data processing and analysis

0:47:28 Webreport

0:48:28 Directories and files

0:51:1 Presentation and handout mode

0:51:33 Editor

0:53:28 HTML tags

0:55:11 LTSPICE schematics from files

0:57:44 Equations with MathJax

0:58:19 Animations

0:59:53 Insert images

1:1:33 Copy, paste, modify

Overview

  • Introduction to SPICE (Circuit Simulation)
    • Program Link
    • Syntax
    • Examples
    • Hierarchy

  • SPICE and data converters
    • Modelling level:
    • Transistors
    • Behavioral (analytic expressions)
  • Hierarchy
  • Waveform Generation, Data Export and Measurements
  • DAC model
  • ADC model

CMOS: Circuit Design, Layout and Simulation, Baker, Chap1, p.8-29

SPICE

  • Circuit Simulator
    • Draw Circuits
    • Generate a netlist
      What is a netlist?
    • Calculates voltage and currrents
    • Nonlinear Elements (Transistor/Diode)
    • Transient simulation: voltage and current over time
    • Frequency dependent Amplitude and Phase
  • Numerical solution

LTSPICE netlist

View, SPICE netlist

* C:\Programme\LTC\LTspiceIV\Draft1.asc
V1 N001 0 1
R1 N002 N001 50
R2 N002 0 50
.dc V1 0 2 0.1
.backanno
.end

V is a voltage source
N001, N002 node names
.dc simulation instruction

SPICE Elements


SPICE simulation statements


LTSPICE: First Steps

  • File, New Schematic
  • Edit, Place Ground
  • Edit, Component, Voltage
  • < ESC >: Stop drawing
  • Edit, Resistor
  • Value: Right click on component
  • 50 Ohm, 1V value without unit
  • Edit, Draw Wire
  • Simulate, Edit Simulation Command (Tab DC Sweep)
  • 1st Source, Name V1, Start 0, Stop 2, Step 0.1
  • Simulate, Run
  • Maus: right click, Add Trace
  • Info: lower left corner

LTSPICE: Configuration

  • White background
    • Tools, Color Preferences, Background
  • Thick lines
    • Tools, Control Panel
    • Waveforms plot data with thick lines
    • Drafting options, thick lines
  • Currents and voltages of subcircuits
    • Tools, Control Panel, Save Defaults
    • Caution: Generates big files on hard disc: Tools, Control Panel, Operation, Automatically delete
  • Documentation
    • Help
    • Tools, Copy bitmap to clipboard

Example Voltage divider operation point: .op

Schematic
  • Voltage source: Vin
  • Resistor: R1, R2
    (Orientation -> current)
  • Nodes: Vin, Vout, 0
  • Analysis: .op operation point
  • Modifier: k
Netlist
  • * Spannungsteiler.asc
  • V1 Vin 0 2
  • R1 Vout Vin 1k
  • R2 Vout 0 4k
  • .op
  • .backanno
  • .end
Output:
  • --- Operating Point ---
  • V(vin): 2 voltage
  • V(vout): 1.6 voltage
  • I(R2): 0.0004 device_current
  • I(R1): -0.0004 device_current
  • I(V1): -0.0004 device_current

Voltage source variation: .dc Vin 0 1 1m

Schematic
Netlist
  • * Spannungsteiler.asc
  • V1 Vin 0 2
  • R1 Vout Vin 1k
  • R2 Vout 0 4k
  • ;op
  • .dc V1 0 5 0.2
  • .backanno
  • .end

SPICE: Sinusodial source

  • Right click on the source symbol
    and choose advanced
  • SINE

  • Simulate Edit
  • Simulate Cmd
  • .tran 0 2m 0m 0.01

Transient simulation: .tran 1n 3u

Schaltplan
  • * Spannungsteiler_02.asc
  • V1 Vin 0 SINE(0 2 1MEG)
  • R1 Vout Vin 1k
  • R2 Vout 0 4k
  • .tran 0 4u 0
  • .backanno
  • .end

MOSFET transistors in LTSPICE

Netlist:
M1 NDrain NGate NSource PBulk NMOSModel
M2 PSource PGate PDrain PBulk PMOSModel
.model NX NMOS(LEVEL=1 KP=300u
+ VT0=0.8 LAMBDA=0.000 CGDO=400n)
.lib C:\Program Files (x86)\LTC\LTspiceIV\lib\cmp\standard.mos
.include cmosedu_models.txt
Example:
M1 VD VG VS VB N_50nm

The transistor model N_50nm can be specified in a model statement (.model), can be supplied in a library file (.lib) or in an external file (.include)
Symbol:

Transistor model

cmosedu_models.txt
Simple model Detailed model
.MODEL N_1u NMOS LEVEL  = 3
+ TOX  = 200E-10 NSUB = 1E17    GAMMA = 0.5
+ PHI  = 0.7     VTO  = 0.8     DELTA = 3.0
+ UO   = 650     ETA  = 3.0E-6  THETA = 0.1
+ KP   = 120E-6  VMAX = 1E5     KAPPA = 0.3
+ RSH  = 0       NFS  = 1E12    TPG   = 1
+ XJ   = 500E-9  LD   = 100E-9
+ CGDO = 200E-12 CGSO = 200E-12 CGBO  = 1E-10
+ CJ   = 400E-6  PB   = 1       MJ    = 0.5
+ CJSW = 300E-12 MJSW = 0.5
.model  N_50nm  nmos  level = 54
+binunit = 1         paramchk= 1          mobmod  = 0          
+capmod  = 2         igcmod  = 1          igbmod  = 1         geomod  = 1          
+diomod  = 1         rdsmod  = 0          rbodymod= 1         rgatemod= 1          
+permod  = 1         acnqsmod= 0          trnqsmod= 0         
+tnom    = 27        toxe    = 1.4e-009   toxp    = 7e-010    toxm    = 1.4e-009   
+epsrox  = 3.9       wint    = 5e-009     lint    = 1.2e-008  
+ll      = 0         wl      = 0          lln     = 1         wln     = 1          
+lw      = 0         ww      = 0          lwn     = 1         wwn     = 1          
+lwl     = 0         wwl     = 0          xpart   = 0         toxref  = 1.4e-009   
+vth0    = 0.22      k1      = 0.35       k2      = 0.05      k3      = 0          
+k3b     = 0         w0      = 2.5e-006   dvt0    = 2.8       dvt1    = 0.52       
+dvt2    = -0.032    dvt0w   = 0          dvt1w   = 0         dvt2w   = 0          
+dsub    = 2         minv    = 0.05       voffl   = 0         dvtp0   = 1e-007     
+dvtp1   = 0.05      lpe0    = 5.75e-008  lpeb    = 2.3e-010  xj      = 2e-008     
+ngate   = 5e+020    ndep    = 2.8e+018   nsd     = 1e+020    phin    = 0          
+cdsc    = 0.0002    cdscb   = 0          cdscd   = 0         cit     = 0          
+voff    = -0.15     nfactor = 1.2        eta0    = 0.15      etab    = 0          
+vfb     = -0.55     u0      = 0.032      ua      = 1.6e-010  ub      = 1.1e-017   
+uc      = -3e-011   vsat    = 1.1e+005   a0      = 2         ags     = 1e-020     
+a1      = 0         a2      = 1          b0      = -1e-020   b1      = 0          
+keta    = 0.04      dwg     = 0          dwb     = 0         pclm    = 0.18       
+pdiblc1 = 0.028     pdiblc2 = 0.022      pdiblcb = -0.005    drout   = 0.45       
+pvag    = 1e-020    delta   = 0.01       pscbe1  = 8.14e+008 pscbe2  = 1e-007     
+fprout  = 0.2       pdits   = 0.2        pditsd  = 0.23      pditsl  = 2.3e+006   
+rsh     = 3         rdsw    = 150        rsw     = 150       rdw     = 150        
+rdswmin = 0         rdwmin  = 0          rswmin  = 0         prwg    = 0          
+prwb    = 6.8e-011  wr      = 1          alpha0  = 0.074     alpha1  = 0.005      
+beta0   = 30        agidl   = 0.0002     bgidl   = 2.1e+009  cgidl   = 0.0002     
+egidl   = 0.8       
+aigbacc = 0.012     bigbacc = 0.0028     cigbacc = 0.002
+nigbacc = 1         aigbinv = 0.014      bigbinv = 0.004     cigbinv = 0.004
+eigbinv = 1.1       nigbinv = 3          aigc    = 0.017     bigc    = 0.0028
+cigc    = 0.002     aigsd   = 0.017      bigsd   = 0.0028    cigsd   = 0.002
+nigc    = 1         poxedge = 1          pigcd   = 1         ntox    = 1
+xrcrg1  = 12        xrcrg2  = 5          
+cgso    = 6.238e-010cgdo    = 6.238e-010 cgbo    = 2.56e-011 cgdl    = 2.495e-10     
+cgsl    = 2.495e-10 ckappas = 0.02       ckappad = 0.02      acde    = 1          
+moin    = 15        noff    = 0.9        voffcv  = 0.02      
+kt1     = -0.21     kt1l    = 0.0         kt2     = -0.042     ute     = -1.5
+ua1     = 1e-009    ub1     = -3.5e-019   uc1     = 0          prt     = 0
+at      = 53000
+fnoimod = 1         tnoimod = 0          
+jss     = 0.0001    jsws    = 1e-011     jswgs   = 1e-010    njs     = 1          
+ijthsfwd= 0.01      ijthsrev= 0.001      bvs     = 10        xjbvs   = 1          
+jsd     = 0.0001    jswd    = 1e-011     jswgd   = 1e-010    njd     = 1          
+ijthdfwd= 0.01      ijthdrev= 0.001      bvd     = 10        xjbvd   = 1          
+pbs     = 1         cjs     = 0.0005     mjs     = 0.5       pbsws   = 1          
+cjsws   = 5e-010    mjsws   = 0.33       pbswgs  = 1         cjswgs  = 3e-010     
+mjswgs  = 0.33      pbd     = 1          cjd     = 0.0005    mjd     = 0.5        
+pbswd   = 1         cjswd   = 5e-010     mjswd   = 0.33      pbswgd  = 1          
+cjswgd  = 5e-010    mjswgd  = 0.33       tpb     = 0.005     tcj     = 0.001      
+tpbsw   = 0.005     tcjsw   = 0.001      tpbswg  = 0.005     tcjswg  = 0.001      
+xtis    = 3         xtid    = 3          
+dmcg    = 0e-006    dmci    = 0e-006     dmdg    = 0e-006    dmcgt   = 0e-007     
+dwj     = 0.0e-008  xgw     = 0e-007     xgl     = 0e-008    
+rshg    = 0.4       gbmin   = 1e-010     rbpb    = 5         rbpd    = 15         
+rbps    = 15        rbdb    = 15         rbsb    = 15        ngcon   = 1

Transistor measurement

LTSPICE: Hierarchy

  • Create a schematic with Pins:
    • Edit->Label Net
      • Port Type
  • Create a symbol: preamp.asy for preamp.asc
    • Edit->Add Pinport
    • Make visible (TOP RIGHT BOTTOM LEFT)
  • Place Instance
    • Edit->Component
    • Select correct directory

Hierarchy

SPICE directive in Netlist
.model CN NMOS(LEVEL=1 KP=11m VT0=1 LAMBDA=0.018 CGDO=400n)
Make a voltage node (VDD) available
.global VDD
Include device models or subcircuits
.include cmosedu_models.txt

A Circuit can be reused
Nodes to be connected externally need to be set as input and output: label net
A symbol needs to be created: Hierarchy, Open this Sheets symbol
Insert this circuit using Edit, Components and select a local directory to make locally defined cirucits visible.

Use of a subcircuit is shown starting with X in netlist. Definition starts with .subckt and ends with ends name.

       XX1 IN D7 IN1 pipestageinv

      * block symbol definitions
      .subckt pipestageinv In Dout Vout
      M1 N001 In 0 0 CN
      …
      ends pipestageinv

Input waveforms and measurement

Waveforms
VA A 0 PWL file=a.txt
VB B 0 PWL file=B.txt
VC Ci 0 PWL file=C.txt

a.txt
0n 0
9n 0
10n 1
19n 0
20n 1
29n 1
30n 0
Calculation of average and rms value

Select the legend of a curve in the Waveformwindow.
< strg > Mouse left click

Measurement of time:

.Measure TAX00 WHEN V(ax)=0.5 FALL=1
.Measure TY101 WHEN V(y1)=0.5 RISE=1
.Measure DY101 PARAM (TY101-TAX00)*1E12

Result name: TAX00
Time when voltage of node ax is 0.5V
and ax is the first falling edge.

Hilfe LTSPICE für Temperaturvariation: Suchbegriff R, TEMP

Simulation with varying components

  • create a parameter with curly brackets.
  • {R2}
  • Set a value
  • .param R2 100
  • change the value:
  • .step parameter <name> <start> <stop> <step>
  • .step parameter R2 100 300 100

Behavioral data converter simulation


Example: 20 Bit ADC, fs = fclk = 100 MHz, Range 0..1 V, Vref = 1V
Simulation time: tsim = 2 20 + 4 /100MHz = 16M/100M s = 0.16777216s
Signal sine frequency: fsig = prime / tsim

Behavioral data converter simulation

Bits LSB Simulation time:
tsim
signal frequency:
fsig
LTSPICE run time LTSPICE output file size FFT pointsComment
20 1 μ V 167.77216ms 65.56510925 Hz 167.7ms/1.2us/s = 100 000s = 30 h 2MB/us => 600 GB minimal; 4600s => 6ms => 7.8GB
16 → 98 dB 16 μ V 220 * 10 ns = 10.48576 ms \( \frac{11}{t_{sim}} = 1049.04174804687 Hz \) 8467s = 2.5 h 900 MB \( 2^{20} = 1048576 \) → 57dB LTSPICE can't draw curve,
but can load data and do FFT
12 256 μ V 216 * 10 ns = 655.36 µs \( \frac{11}{t_{sim}} = 16784.66796875 Hz \) 378s =7 min 65 MB \( 2^{16} = 65536 \)
8
4 → 26 dB 62.5 mV 28 * 10 ns = 2.560 µ s \( \frac{11}{t_{sim}} = 4296875 Hz \) 1.4 s 500 kB \( 2^{8} = 256 \) →

.save dialog
.save V(in) V(d*) V(Vout)
This saves only V(in), all data channels and Vout and reduces the file size significantly.

; option can limit saved data
.option numdgt=12
precision of saved data

To be able to use simulated data for FFT with high precision use the following option:
.options plotwinsize=0

Scalable behavioral 4 Bit DAC

Behavioral voltage source BV with equation

V=V(in1)/16+V(D3)/2+V(D2)/4+V(D1)/8+V(D0)/16

Scalable DAC takes input signal In1 as high resolution input and adds D3..D0 information.
For high resolution more modules can be combined.

Scalable behavioral 4 Bit ADC

Behavioral voltage source BV
Rounding function:
V(D3) = round(V(IN))
V(D2) = round(V(IN)*2-V(D3))
...
Residue: V(Out) = V(in)*16-V(D3)*8-V(D2)*4-V(D1)*2-V(D0)

Residue allows extending the ADC for high resolution.

Test for 4 Bit ADC and DAC

A 4 Bit ADC and DAC test can be simulated in LTSPICE.
The output file size can be limited by using the .save dialog option.

The output shows the step size of the digitalisation.

Test for 12 Bit ADC and DAC

A 12 Bit ADC and DAC test can still be simulated in LTSPICE. The output file size can be limited by using the .save dialog option.

FFT 65k points gives: signal: -9dB, noise level: -116dB
Calculation:
6.07 * B dB + 1.76 dB + 10 log(N/2) dB =
6.07 * 12 dB + 1.76 dB + 10 log(65k/2) dB =
72 dB + 1.76 dB + 45 dB = 119 dB

Test data analysis


LTSPICE raw data file size reduction


    LTSPICE data can be reduced with a .save statement.

Reading LTSPICE raw data via a web page


    Read LTSPICE raw file for data converter analysis.

Data converter analysis via a web page


    FFT and INL, DNL data converter analysis.

ADC Calibration


    There is an option to do calibration before.

LTSPICE raw data file size reduction


LTSPICE data can be reduced with a .save statement.
.save V(vout)
The simulation of the 12-bit ideal ADC and DAC gives for 11 periods sine simulation running 5 min in LTSPICE generating 4 million points and 48 MB file size.
This file can be loaded into Matlab with a LTspice2Matlab code (watch out for UTF8 versus UTF16 encoding).

Adapt lines in the code accordingly:
153 - fid = fopen(filename, 'rb', 'n', 'UTF16LE');
156 - fid = fopen(sprintf( '%s.raw', filename ), 'rb', 'n', 'UTF16LE');

Reading LTSPICE raw data


It can also be processed on a web page:
Read LTSPICE raw file for data converter analysis.
Before reading the data choose a time step of 10E-9 to get data for each conversion step.
Choose a range of at least 65536 to get at least 16 bit for further processing.
After browsing for the file it takes quite some time, a couple of minutes, in Firefox until data is loaded and converter.
More then 65k points are generated.

Data converter analysis


Another web page will do the analysis:
FFT and INL, DNL data converter analysis.
First data is copied to the text input field.
Then read integer data is done.
Finishing with Generate charts.
FFT, INL and DNL are displayed. Further down on the page signal to noise is displayed.

ADC Calibration


A calibration file based on a positive input ramp can be loaded before to compensate for errors.
Load integer data into the input data field, read integer data and do a code calibration eliminating missing codes, or a code and slope calibration also compensating for non linearities.
After calibration is set, proceed with sine data for FFT, INL and DNL.