Galaxy Custom Designer – Quick Startup

Galaxy Custom Designer – Quick Startup
 Galaxy Custom Designer – Quick Startup -­‐ Schematic Editor -­‐ Simulation and Analysis Environment -­‐ CosmoScope -­‐ HSPICE Toolbox for MATLAB Page 1 of 37 1. Setting Up the Workspace Create a working directory mkdir ~/ee406/s14/analog/ Enter the workng directory: cd ~/ee406/s14/analog/ Setup the libraries by creating a file lib.defs in the working directory The file should look as follows: INCLUDE $SYNOPSYS_CUSTOM_INSTALL/samples/lib.defs DEFINE SAED_PDK_90 /usr/synopsys/SAED_PDK90nm/SAED_PDK_90/ DEFINE reference /usr/synopsys/SAED_PDK90nm/reference 2. Running custom designer: From the working directory: cdesigner & 3. Creating a new Library From the custom designer console: File  New  Library Page 2 of 37 4. Creating a New Cell From the custom designer console File  New  Cell Page 3 of 37 The schematic editor (SE) opens. Enter the schematic of the design, by adding the various instances, wires, wire names, etc.: Page 4 of 37 Save the design (Design  Save) often and make sure to check it for possible errors (Design  Check and Save). Once the schematic is finished and passes all checks (see the custom explorer console) it can be printed, exported as an image, exported as a netlist, etc. Page 5 of 37 Design  Print Submit (print to file) Page 6 of 37 Page 7 of 37 Design  Export Image (format jpeg; do not include background) Page 8 of 37 Page 9 of 37 Design  Export Netlist cat ee406Lib_cs_ee114.sp *Custom Designer (TM) Version H-­‐2013.03-­‐SP2-­‐1 *Mon Nov 25 10:58:00 2013 .GLOBAL gnd! ******************************************************************************** * Library : ee406Lib * Cell : cs_ee114 * View : schematic * View Search List : hspice hspiceD cmos.sch cmos_sch schematic veriloga * View Stop List : hspice hspiceD veriloga ******************************************************************************** .subckt cs_ee114 ib vdd dn dc=250u rin gn in r=20k r vb dn r=10k mn dn gn gnd! gnd! nmos4 w=40u l=1.6u vb vb gnd! dc=2.5 vdd vdd gnd! dc=5 vin in gnd! dc=1.08817 ac=1 .ends cs_ee114 Page 10 of 37 5. Running the Simulation and Analysis Environment (SAE) From the schematic Editor invoke Tools  SAE. The SAE window opens. Set up the model files to be used by the simulator Setup  Model files Page 11 of 37 Setup where to save the simulation: Setup  Simulator Save the location of the result directory in simu.xml (Defaults  Save) Setup the analysis to run: Setup  Analysis Page 12 of 37 Page 13 of 37 Set up your favorite HSPICE options: Simulation  options .OPTION NOMOD = 1 This option suppresses the printout of model parameters. Run the simulation Simulation  Netlist and Run Analyzing the results of the simulation: Annotating the schematic with the DC voltages: Results  Annotate  DC node Voltages Page 14 of 37 Annotating the schematic with the DC Operating point values: Results  Annotate  DC Operating Point Plotting the frequency response of the amplifier Results  Plot Signal  AC Bode Click on the node of interest in the schematic Custom waveView opens Page 15 of 37 Page 16 of 37 To change the default color of the background: Config  Preferences To save the preferences for future use click on Apply-­‐Save: To change the thickness and color of waveforms: Config  Waveform Attributes Page 17 of 37 Make sure to click over the signal names to make the change happen. Page 18 of 37 Measuring the gain and the BW of the designed amplifier: Tools  Measurements Page 19 of 37 Computing the BW using the equation Builder of Custom Explorer WaveView Results  Plot Signal  AC Magnitude Click on the node of interest in the schematic Custom waveView opens Tools  Equation Builder Right Click on the signal name  Add to Equation Page 20 of 37 Finally set a cursor at 5.29545 to find out the value of the BW (about 26.2 MHx) Axes  Cursor  Jump Settings Page 21 of 37 Page 22 of 37 Page 23 of 37 Setting up the results to output through the SAE output section Outputs  Select in design (click on the schematics’ net(s) of interest) Defining names for the observed outputs; creating expressions through the calculator, plotting the results Saving the simulation and analysis setting Session  Save State. Page 24 of 37 Exporting the Waveforms data for MATLAB Go to the Custom Explorer WaveView window and click on the signals to export. File  Export Waveform Data Page 25 of 37 Page 26 of 37 Using CosmosScope to view the simulation results The spice netlist generated by SAE is saved in: ~/ee406/s14/analog/simulations/ee406Lib/cs_ee114/schematic/HSPICE/nominal/netlist/input.spi * Generated for: HSPICE .option search='/home/talarico/ee406/s14/analog/hspicemod' .option PARHIER = LOCAL .option NOMOD = 1 .option ARTIST=2 PSF=2 .temp 25 .include 'ee114_hspice.sp' .GLOBAL gnd! ib vdd dn dc=250u r vb dn r=10k rin gn net18 r=20k mn dn gn gnd! gnd! nmos114 w=40u l=1.6u vb vb gnd! dc=2.5 vdd vdd gnd! dc=5 vin net18 gnd! dc=1.08817 ac=1 .ac DEC 100 1 100Meg .op All 0 .option opfile=1 split_dp=1 .end It is important to understand what the various options mean: .option PARHIER = LOCAL Use this option to specify scoping rules .OPTION NOMOD = 1 This option suppresses the printout of model parameters. .option ARTIST=2 Enables the Virtuoso® Analog Design Environment if ARTIST=2. This option is generally used together with .OPTION PSF. .option PSF=2 If .option PSF=2, HSPICE produces ASCII output Page 27 of 37 .option opfile=1 Use this option to output the operating point information to a file. • If value is 1, operating point information is output to a file named <design>.dp#. • If value is 0, the operating point information outputs to stdout The results of the simulation are put in: ~/ee406/s14/analog/simulations/ee406Lib/cs_ee114/schematic/HSPICE/nominal/results The HSPICE results produced by SAE are not in the correct format to be viewed with Cosmoscope In order to use Cosmoscope as viewer we need to overwrite the .option ARTIST=2 PSF=2 with .option POST. … .option artist=2 psf=2 .option post … and re-­‐run HSPICE simulation manually. For convenience name the new “hacked” spice netlist input.sp: .option search='/home/talarico/ee406/s14/analog/hspicemod' .option PARHIER = LOCAL .option NOMOD = 1 .option ARTIST=2 PSF=2 .option POST * added by Claudio .temp 25 .include 'ee114_hspice.sp' *Custom Designer (TM) Version H-­‐2013.03-­‐SP2-­‐1 *Wed Nov 27 11:43:47 2013 .GLOBAL gnd! ib vdd dn dc=250u rin gn net18 r=20k r vb dn r=10k mn dn gn gnd! gnd! nmos114 w=40u l=1.6u vb vb gnd! dc=2.5 vdd vdd gnd! dc=5 vin net18 gnd! dc=1.08817 ac=1 Page 28 of 37 .ac DEC 100 1 100Meg .op All 0 .option opfile=1 split_dp=1 .end make a copy of the runSimulation script: cp runSimulation runSimulationH and modify it as follows: hspice -­‐i input.sp -­‐o ../results/Hhspice > ../results/run.log 2>&1 Run the “hacked” spice simulation: ./runSimulationH and move to the result directory: cd ../results/ Invoke cosmoScope: cscope & File  Open Plot Files Double click on Hhspice.ac0 Select the signal to plot and click on the plot button. Page 29 of 37 Change the color and thickness of the waveform (right click on the name of the signal and edit the attributes), edit the title of the graph (click on the title and edit it), add measurements to the plot (click on Tools  Measurement Tool and then select the type of measurement you are interested in), etc. ... Make sure to change the background !! Graph  Color Map  Map 2 Page 30 of 37 The plots can be printed or exported as images. Page 31 of 37 File  Export Image Page 32 of 37 File  Print Before Printing make sure the printer is setup correctly: File  Printer  Setup Page 33 of 37 The colors can be further customized: Edit  Preferences  Graph Page 34 of 37 Using Matlab to import HSPICE simulations. Setup a directory for the matlab files: mkdir ~/ee406/s14/matlab We will use the HSPICE toolbox for MATLAB developed by M. Perrott. The HSPICE toolbox for Matlab is a collection of Matlab functions that allow you to manipulate and view signals generated by HSPICE simulations directly. The toolbox files are located at: /usr/local/MATLAB/personal/HspiceToolbox Note: the toolbox requires the HSPICE outputs to be in the format generated through the POST option. There are many functions in the toolbox, but we will focus mainly on three of them. See hspice_toolbox.pdf for more details. 1. loadsig (…) This function loads the circuit signals into MATLAB. It takes the hspice output file, such as DC (*.sw0) or AC (*.ac0) files as the function input. For example, if you simulated a common source amplifier in HSPICE and have CS.ac0 as the output file, the function call is: x = loadsig(‘CS.ac0’); 2. lssig(...) -­‐ This function lists the signals contained in the file loaded by the loadsig(...) function. Continuing with the above example, this function is called as: lssig(x); 3. evalsig(... , ...) -­‐ This function actually loads the signals from the HSPICE output file into vectors in MATLAB. For example, if have a signal called v_dn, the function is called as follows: vout = evalsig(x, ‘v_dn’) Once you have loaded a signal into a MATLAB vector, you can then proceed to do any mathematical manipulations on the data. Page 35 of 37 MATLAB example: % % author: C. Talarico % file: cad.m clear all; close all; clc; addpath('/usr/local/MATLAB/personal/HspiceToolbox') x = loadsig('/home/talarico/ee406/s14/analog/simulations/ee406Lib/cs_ee114/schem
atic/HSPICE/nominal/results/Hhspice.ac0') lssig(x) vout = evalsig(x,'v_dn'); freq = evalsig(x,'HERTZ'); mag = abs(vout); phase = angle(vout); % phase in rad magdb = 20*log10(mag); degree = phase.*180/pi; subplot(2,1,1); set(gca, 'fontsize',14); semilogx(freq*1e-­‐6,magdb,'linewidth',2,'color', 'b', 'linestyle','-­‐'); ylabel('Magnitude [dB]', 'fontsize', 12); xlabel('freq [MHz]', 'fontsize', 12); maxdb = max(magdb) + 5; axis([min(freq*1e-­‐6) max(freq*1e-­‐6) 0 maxdb]); % compute DC gain and f3dB format shorte; gain = magdb(1); idx = find(magdb < gain -­‐ 3, 1, 'first'); f3db = 1e-­‐6*freq(idx); % annotate the plot with DC gain and f3dB str0 = sprintf('CS Frequency Response'); str1 = sprintf('DC gain = %.2f [dB]', gain); str2 = sprintf('f3db = %.2f [MHz]', f3db); str = {str0, str1, str2}; % distribute the string on three lines title(str, 'fontsize', 16); g3db = gain-­‐3; % annotate the f3db point with "template lines" % horizontal line line([min(1e-­‐6*freq) 1e-­‐6*freq(idx)], [g3db g3db], 'linestyle', ':', ... 'linewidth', 3, 'color', 'r'); Page 36 of 37 %vertical line line([f3db f3db], [-­‐20 g3db], 'linestyle', ':', ... 'linewidth', 3, 'color', 'r'); subplot(2,1,2); set(gca, 'fontsize',14); semilogx(1e-­‐6*freq,degree,'linewidth',2,'color', 'm', 'linestyle','-­‐'); ylabel('Angle [degree]', 'fontsize', 14); xlabel('freq [MHz]', 'fontsize', 14); Page 37 of 37 
Was this manual useful for you? yes no
Thank you for your participation!

* Your assessment is very important for improving the work of artificial intelligence, which forms the content of this project

Download PDF