SPICE tutorial Using NGSpice and Cppsim

Transcription

1 SPICE tutorial Using NGSpice and Cppsim Instructor: Prof. Jintae Kim Mixed-Signal Electronics Lab Konkuk University

2 SPICE What is SPICE? - Simulation Program With Integrated Circuit Emphasis - Real-world circuit designs are way too complicated to do hand-analysis - SPICE helps you analyze/verify your circuits by computer simulations What we will learn today - How to install the software - How to create circuit schematics - How to run circuit simulations and check the results 2

3 Circuit Simulations in a Glance Schematic Diagram Done by software (SUE2 in our case) ***** Spice Netlist for Cell 'spice_example3' ***** ************** Module spice_example3 ************** q0 n0 n1 n4 vdd mod_npn m=1 r1 gnd n1 10k.end. op. tran Netlist (text-file) the contains - Description of Circuit - Type of analysis(dc, AC, transient, etc) Waveform viewer (CppSimView in our case) SPICE engine (NGsipce in our case) Operating point Text file (simrun.log) ***** Operating Point Values (Generated from.op Statement) ***** n1 = 2.467e+000 n4 = 1.793e+000 vdd = 5.000e+000 out = 8.700e-001 ***************** End of Operating Point Values 3

4 Software Installation Download Cppsim from Double click on setup_cppsim5.exe file and install the entire package Depending on your windows version, you may need to install some Visual C++ package from Microsoft. This is available at aylang=en&id=29 4

5 Icons on your Desktop SUE2 CppSimView The installation will create several icons on your desktops. Make sure you have - Sue2: Schematic Editor and Circuit simulation - CppSimView: Waveform viewer Now let s double click on Sue2 5

6 Before we begin Download the BJT model file for the class at - mod_npn npn bf=100 is=5.0e-16 vaf=50 + tf=.505ns rb=0 cje=8pf cjc=6.197pf + vjc=.087 mjc=.255.model mod_pnp pnp bf=100 is=1.53e-15 vaf=33 + tf=.609ns rb=0 cje=10pf cjc=14.3pf + vjc=0.55 mjc=0.5 Overwrite this file to your local model file at - Model file is at C:\CppSim\SpiceModels\bipolar.mod 6

7 SUE2 This is a window where you create your own circuits or load saved circuits. Manual is available at the menu: doc Sue 2 manual Also read Doc NGSpice with Cppsim Primer (page 4-17) 7

8 Opening an example Library tab Schematic entry Click on the library tab Synthesizer_Example on the right, and change it into Spice Library is a collection of circuit schematics. We will use cells on Spice library only. In the list of entries, choose spice_example4 8

9 Running the simulations Tools Ngspice Simulation Ngspice Run Menu windows will pop up Click on Netlist/HSPC/Ngspice - If you see Done!, the simulation is completed with no error NGSpice Run menu Wuindows 9

10 Checking DC-operating point In the Ngspice windows, click on View Log File - There is a line called Operating Point Values - It will list node voltages and current at the bias condition for given DC V/I sources in the schematic 10

11 Checking time-domain simulation Click on CppSimView icon in the desktop CppSimView windows pops up - Click on the button on No output file will change into simrun.raw - Click on plotsig( ) and choose plostsig(x, nodes ) (the 1 st entry) - Click on No Nodes will change into nodes and display nodes in the design - Choose in and double click on it - It should display the waveform shown in this slide - In CppSimView, click on Save to Clipboard to copy/paste for future use 11

12 Example: Step 1 File New Schematic - A new schematic window will pop up. Put my_example1 as a file name Click on the middle tab on the right change it into Spice (Cell library) Choose NPN and place it in the schematic window 12

13 Example: Step 2 Place DC_voltage in the schematic Double click on the DC_voltage Change the dc_voltage from 0 to 0.8 Connect + terminal of DC voltage to base using Edit add wire (short-key is w) Connect - terminal of DC voltage to emitter using short-key w 13

14 Example: Step 3 Add another DC_voltage and change voltage to 2.5V and Connect it between collector and emitter Click on global in the devices sub-window and place/connect it to the emitter. Name it as gnd Every schematic needs gnd (treated as a special net). Do File Save 14

15 Example: Step 4 To add name of a net, go to a devices window on the right, and click on name_net Place the symbol near emitter and connect it to emitter using w key Double click on the symbol, put vbe on the name field Do the same thing on vce on the collector node Save the design (shortkey is ctrl+s) 15

16 Example: Step 5 Click on Tools NGspice Simulation Click on Edit Simfile will open test.hspc file. This file contains the type of analysis you want to run. There are three main analyses -.tran is for time-domain simulation (transient simulation) -.op is for bias simulation (operating point simulation) -.dc is for DC sweep simulation (You sweep DC voltage of source) Adding * at the beginning of the line will comment out any statement in test.hspc file. Comment out.tran 5p 40n statement now. Add.probe vbe in the last line of test.hspc file Close test.hspc file, and click on Nsetlist/HSPC/NGSpice to run the simulation. If everything is done correctly, you should see Done! on the NGSpice Run Menu window. Click on View Log File and find out vbe, vbe, and q0_ic Note that q0_ic is the collector current of Q0 16

17 Test.hspc file and simrun.log ***** Parameters for Calculation of Diffusion Regions for CMOS Process > set_mode_diff geo > set_hdout.66u > set_hdin.74u > use_four_sided_perimeter ***** Transistor Model File ***** Specify appropriate CMOS and Bipolar model files below.include '../../../SpiceModels/cmos_013_bsim4.mod'.include '../../../SpiceModels/bipolar.mod ***** Temperature.temp 25 ***** Parameters.param vsupply=1.3 ***** DC Voltage Sources ***** Simulation Options.options post=1 delmax=5p relv=1e-6 reli=1e-6 relmos=1e-6 method=gear ***** Simulation Parameters (.tran or.ac or.dc statements) *.tran 5p 400n **.dc Vsup 0 'vsupply' 0.1 **.ac lin k 10Meg Vsup Test.hspc ***** Have operating point information sent to output file.op You can specify Which analysis you Want to run here Note: can't find init file. Circuit: ***** spice netlist for cell 'my_example1' ***** binary raw file Doing analysis at TEMP = and TNOM = No. of Data Columns : 3 No. of Data Rows : 1 Total elapsed time: seconds. Total DRAM available = MB. DRAM currently available = MB. Total ngspice program size = MB. ***** Operating Point Values (Generated from.op Statement) ***** vbe = 8.000e-001 vce = 2.500e+000 q0_ic = 1.267e-002 Operating Point Analysis result (== bias calculation, large-signal analysis) ***************** End of Operating Point Values ***************** ****** Selectively Probe Signals (uncomment below if you want this).probe vbe Specify which voltage/current In the current you want to measure simrun.log 17

18 Example: Step 6 (DC Sweep) Run DC sweep analysis by adding.dc V in the test.hspc file. This will sweep DC voltage source V1 from 0V to 1.5V with 0.01V step. Click on Netlist/HSPC/NGSpice to run the SPICE simulation again 18

19 Example: Step 7 Open CppSimView click on simrun.raw click on postsig( ) choose plotsig(x, nodes ) click on nodes double click on q0_ic You should see the black screen as shown in this slide. This is collector current of Q0. 19

20 Example: Step 8 Click on zoom tab in CppSimView windows, and it will create several buttons on the plot figure. Click on (M)easure and clik on the waveform. It will create a red circle. Right click on the red circle, and it will make a small pop-up window that shows the measured value You can save the figure by clicking on Save to Cilpboard in CppSimView window 20

21 DC Sweep Simulation I C V BE =0.8V Acceptable Region Soft- Saturation 0.4>V BC >0 Saturation V BC <0 Forward-Active V CE 21

22 Take-Home example: Time-Domain Simulation Construct the schematic shown in this slide and save as my_example3 Use capacitor and sine_voltage cell in Spice library 22

23 Setups for time-domain simulation Time-domain simulation = transient analysis test.hspc file defines what kinds of analysis will be performed. Click on Edit Sim File in NGSpice Run Menu window Modify the transient analysis is.tran 1p 100n. This means that the simulation runs until 100ns with 1ps time step 23

24 Simulation Result: Gain In CppSimView, type plotsig(x, vin; vout ) Vin: 50MHz sinusoid with peak-to-peak 1mV amplitude Vout: same frequency, and amplitude is ~1mV and there is no sign inversion simulated gain = ~1. 24

25 Summary Create a schematic design with transistor (npn, pnp) and voltage/current sources in SPICE library. - Don t forget to use global cell in devices and name it gnd for actual ground node Use name_net cell in devices library for specific net name Edit test.hspc file as you need..dc analysis is used for DC sweep..tran analysis is used for time-domain simulation..op is needed for operation point analysis.probe statement in test.hspc needs to used to specify which voltage and current will be saved for plotting and other post processing. 25