+An open source EDA tool for circuit design,
+simulation, analysis and PCB design
+
+
+eSim User Manual
+version 1.0.0
+Prepared By:
+eSim Team
+FOSSEE at IIT,Bombay
+
+
+Indian Institute of Technology Bombay
+
+August 2015
Electronic systems are an integral part of human life. They have
+simplified our lives to a great extent. Starting from small systems made of a few
+discrete components to the present day integrated circuits (ICs) with millions of
+logic gates, electronic systems have undergone a sea change. As a result, design of
+electronic systems too have become extremely difficult and time consuming. Thanks to
+a host of computer aided design tools, we have been able to come up with quick
+and efficient designs. These are called Electronic Design Automation or EDA
+tools.
+
Let us see the steps involved in EDA. In the first stage, the specifications of the system are
+laid out. These specifications are then converted to a design. The design could be in
+the form of a circuit schematic, logical description using an HDL language, etc.
+The design is then simulated and re-designed, if needed, to achieve the desired
+results. Once simulation achieves the specifications, the design is either converted to
+a PCB, a chip layout, or ported to an FPGA. The final product is again tested
+for specifications. The whole cycle is repeated until desired results are obtained
+ [9].
+
A person who builds an electronic system has to first design the circuit, produce a virtual
+representation of it through a schematic for easy comprehension, simulate it and finally
+convert it into a Printed Circuit Board (PCB). There are various tools available that will help
+us do this. Some of the popular EDA tools are those of Cadence, Synopys, Mentor Graphics
+and Xilinx. Although these are fairly comprehensive and high end, their licenses are
+expensive, being proprietary.
+
There are some free and open source EDA tools like gEDA, KiCad and Ngspice. The main
+drawback of these open source tools is that they are not comprehensive. Some of them are
+capable of PCB design (e.g. KiCad) while some of them are capable of performing simulations
+(e.g. gEDA). To the best of our knowledge, there is no open source software that can perform
+circuit design, simulation and layout design together. eSim is capable of doing all of the
+above.
+
eSim is a free and open source EDA tool. It is an acronym for Electronics Simulation.
+eSim is created using open source software packages, such as KiCad, Ngspice and Python.
+Using eSim, one can create circuit schematics, perform simulations and design PCB
+layouts. It can create or edit new device models, and create or edit subcircuits for
+simulation.
+
Because of these reasons, eSim is expected to be useful for students, teachers and other
+professionals who would want to study and/or design electronic systems. eSim is also useful
+for entrepreneurs and small scale enterprises who do not have the capability to invest in
+heavily priced proprietary tools.
+
This book introduces eSim to the reader and illustrates all the features of eSim with
+examples. Chapter 2 gives step by step instructions to install eSim on a typical computer
+system and to validate the installation. The software architecture of eSim is presented in
+Chapter 3. Chapter 4 gets the user started with eSim. It takes them through a tour
+
+of eSim with the help of a simple RC circuit example. Chapter 5 illustrates how
+to simulate circuits. Chapter 6 explains PCB design using eSim, in detail. The
+advanced features of eSim such as Model Builder covered in Chapter 7 and Sub
+circuiting is covered in Chapter 8. Chapter 9 illustrates how to use eSim for solving
+problems.
+
The following convention has been adopted throughout this manual.All the
+menu names, options under each menu item, tool names, certain points to be noted,
+etc., are given in italics. Some keywords, names of certain windows/dialog boxes,
+names of some files/projects/folders, messages displayed during an activity, names
+of websites, component references, etc., are given in typewriter font. Some key
+presses, e.g. Enter key, F1 key, y for yes, etc., are also mentioned in typewriter
+font.
+
+
Chapter 2 Installing eSim
+
+ 1.
eSim installation in Ubuntu: After downloading the zip file from https://github.com/FOSSEE/eSim to a local
+ directory unpack it using: $ unzip eSim.zip Now change directories in to the top-level source directory (where this INSTALL
+ file can be found).
+
To install eSim and other dependecies run the following command. $ ../install-linux.sh –install Above script will install eSim along with dependencies.
+
eSim will be installed to /opt/eSim
+
To run eSim you can directly run it from terminal as $ esim or you can double click on eSim icon created on desktop after installation.
+
+
Chapter 3 Architecture of eSim
+
eSim is a CAD tool that helps electronic system designers to design, test and analyse their
+circuits. But the important feature of this tool is that it is open source and hence the user can
+modify the source as per his/her need. The software provides a generic, modular and
+extensible platform for experiment with electronic circuits. This software runs on all
+Ubuntu Linux distributions and some flavours of Windows. It uses Python, KiCad and
+Ngspice.
+
The objective behind the development of eSim is to provide an open source EDA solution
+for electronics and electrical engineers. The software should be capable of performing
+schematic creation, PCB design and circuit simulation (analog, digital and mixed signal). It
+should provide facilities to create new models and components. The architecture of eSim has
+been designed by keeping these objectives in mind.
+
3.1 Modules used in eSim
+
Various open-source tools have been used for the underlying build-up of eSim. In this section
+we will give a brief idea about all the modules used in eSim.
+
+
3.1.1 Eeschema
+
+
+
Eeschema is an integrated software where all functions of circuit drawing, control, layout,
+library management and access to the PCB design software are carried out. It is the
+schematic editor tool used in KiCad [11]. Eeschema is intended to work with PCB layout
+software such as Pcbnew. It provides netlist that describes the electrical connections of the
+PCB. Eeschema also integrates a component editor which allows the creation, editing and
+visualization of components. It also allows the user to effectively handle the symbol
+libraries i.e; import, export, addition and deletion of library components. Eeschema
+also integrates the following additional but essential functions needed for a modern
+schematic capture software: 1. Design rules check (DRC) for the automatic control of
+incorrect connections and inputs of components left unconnected. 2. Generation of
+layout files in POSTSCRIPTor HPGLformat. 3. Generation of layout files printable via
+printer. 4. Bill of material generation. 5. Netlist generation for PCB layout or for
+simulation.
+This module is indicated by the label 1 in Fig. 3.1.
+
As Eeschema is originally intended for PCB Design, there are no fictitious
+
+components1
+such as voltage or current sources. Thus, we have added a new library for different types of
+voltage and current sources such as sine, pulse and square wave. We have also built a library
+which gives printing and plotting solutions. This extension, developed by us for eSim, is
+indicated by the label 2 in Fig. 3.1.
+
3.1.2 CvPcb
+
+
CvPcb is a tool that allows the user to associate components in the schematic to component
+footprints when designing the printed circuit board. CvPcb is the footprint editor tool in
+KiCad [11]. Typically the netlist file generated by Eeschema does not specify which printed
+circuit board footprint is associated with each component in the schematic. However, this is
+not always the case as component footprints can be associated during schematic capture by
+setting the component’s footprint field. CvPcb provides a convenient method of associating
+footprints to components. It provides footprint list filtering, footprint viewing, and 3D
+component model viewing to help ensure that the correct footprint is associated with each
+component. Components can be assigned to their corresponding footprints manually or
+automatically by creating equivalence files. Equivalence files are look up tables
+associating each component with its footprint. This interactive approach is simpler
+and less error prone than directly associating footprints in the schematic editor.
+This is because CvPcb not only allows automatic association, but also allows to
+see the list of available footprints and displays them on the screen to ensure the
+correct footprint is being associated. This module is indicated by the label 3 in
+Fig. 3.1.
+
+
3.1.3 Pcbnew
+
+
Pcbnew is a powerful printed circuit board software tool. It is the layout editor tool
+used in KiCad [11]. It is used in association with the schematic capture software
+Eeschema, which provides the netlist. Netlist describes the electrical connections of
+the circuit. CvPcb is used to assign each component, in the netlist produced by
+Eeschema, to a module that is used by Pcbnew. The features of Pcbnew are given
+below:
+
+
+
It manages libraries of modules. Each module is a drawing of the physical
+ component including its footprint - the layout of pads providing connections to the
+ component. The required modules are automatically loaded during the reading of
+ the netlist produced by CvPcb.
+
+
Pcbnew integrates automatically and immediately any circuit modification by
+ removal of any erroneous tracks, addition of new components, or by modifying
+ any value (and under certain conditions any reference) of old or new modules,
+ according to the electrical connections appearing in the schematic.
+
+
This tool provides a rats nest display, a hairline connecting the pads of modules
+ connected on the schematic. These connections move dynamically as track and
+ module movements are made.
+
+
It has an active Design Rules Check (DRC) which automatically indicates any error
+ of track layout in real time.
+
+
It automatically generates a copper plane, with or without thermal breaks on the
+ pads.
+
+
It has a simple but effective auto router to assist in the production of the
+ circuit. An export/import in SPECCTRA dsn format allows to use more advanced
+ auto-routers.
+
+
It provides options specifically for the production of ultra high frequency circuits
+ (such as pads of trapezoidal and complex form, automatic layout of coils on the
+ printed circuit).
+
+
Pcbnew displays the elements (tracks, pads, texts, drawings and more) as actual size
+ and according to personal preferences such as:
+
+
display in full or outline.
+
+
display the track/pad clearance.
+
+
+
This module is indicated by the label 4 in Fig. 3.1.
+
3.1.4 KiCad to Ngspice converter
+
We can provide analysis parameters, and the source details through this module. It also
+allows us to add and edit the device models and subcircuits, included in the circuit
+schematic. Finally, this module facilitates the conversion of KiCad netlist to Ngspice
+compatible ones. It is developed by us for eSim and it is indicated by the label 7 in
+Fig. 3.1.
+
+
3.1.5 Model Builder
+
+
This tool provides the facility to define a new model for devices such as, 1. Diode 2. Bipolar
+Junction Transistor (BJT) 3. Metal Oxide Semiconductor Field Effect Transistor
+(MOSFET) 4. Junction Field Effect Transistor (JFET) 5. IGBT and 6. Magnetic
+core.
+This module also helps edit existing models. It is developed by us for eSim and it is indicated
+by the label 5 in Fig. 3.1.
+
+
3.1.6 Subcircuit Builder
+
+
This module allows the user to create a subcircuit for a component. Once the subcircuit for a
+component is created, the user can use it in other circuits. It has the facility to define new
+components such as, Op-amps and IC-555. This component also helps edit existing
+subcircuits. This module is developed by us for eSim and it is indicated by the label 6 in
+Fig. 3.1.
+
+
3.1.7 Ngspice
+
+
Ngspice is a general purpose circuit simulation program for nonlinear dc, nonlinear transient,
+and linear ac analysis [12]. Circuits may contain resistors, capacitors, inductors, mutual
+inductors, independent voltage and current sources, four types of dependent sources, lossless
+and lossy transmission lines (two separate implementations), switches, uniform
+
+distributed RC lines, and the five most common semiconductor devices: diodes,
+BJTs, JFETs, MESFETs, and MOSFET. This module is indicated by the label 9 in
+Fig. 3.1.
+
+
3.2 Work flow of eSim
+
Fig. 3.1 shows the work flow in eSim. The block diagram consists of mainly three
+parts:
+
+
Schematic Editor
+
+
PCB Layout Editor
+
+
Circuit Simulators
+
+
+
+
+
+
+
Figure 3.1: Work flow in eSim. (Boxes with dotted lines denote the modules developed
+in this work).
+
+
+
Here we explain the role of each block in designing electronic systems. Circuit design is the
+first step in the design of an electronic circuit. Generally a circuit diagram is drawn on a
+paper, and then entered into a computer using a schematic editor. Eeschema is the schematic
+editor for eSim. Thus all the functionalities of Eeschema are naturally available in eSim.
+
+
Libraries for components, explicitly or implicitly supported by Ngspice, have been created
+using the features of Eeschema. As Eeschema is originally intended for PCB design, there are
+no fictitious components such as voltage or current sources. Thus, a new library for different
+types of voltage and current sources such as sine, pulse and square wave, has been added in
+eSim. A library which gives the functionality of printing and plotting has also been
+created.
+
The schematic editor provides a netlist file, which describes the electrical connections of
+the design. In order to create a PCB layout, physical components are required to be mapped
+into their footprints. To perform component to footprint mapping, CvPcb is used. Footprints
+have been created for the components in the newly created libraries. Pcbnew is used to draw
+a PCB layout.
+
After designing a circuit, it is essential to check the integrity of the circuit design. In the
+case of large electronic circuits, breadboard testing is impractical. In such cases, electronic
+system designers rely heavily on simulation. The accuracy of the simulation results can be
+increased by accurate modeling of the circuit elements. Model Builder provides the facility to
+define a new model for devices and edit existing models. Complex circuit elements can be
+created by hierarchical modeling. Subcircuit Builder provides an easy way to create a
+subcircuit.
+
The netlist generated by Schematic Editor cannot be directly used for simulation due to
+compatibility issues. Netlist Converter converts it into Ngspice compatible format. The
+type of simulation to be performed and the corresponding options are provided
+through a graphical user interface (GUI). This is called KiCad to Ngspice Converter in
+eSim.
+
eSim uses Ngspice for analog, digital, mixed-level/mixed-signal circuit simulation. Ngspice
+is based on three open source software packages [14]:
+
+
Spice3f5 (analog circuit simulator)
+
+
Cider1b1 (couples Spice3f5 circuit simulator to DSIM device simulator)
+
+
Xspice (code modeling support and simulation of digital components through an
+ event driven algorithm)
+
It is a part of gEDA project. Ngspice is capable of simulating devices with BSIM, EKV, HICUM,
+
+HiSim, PSP, and PTM models. It is widely used due to its accuracy even for the latest
+technology devices.
+
+
Chapter 4 Getting Started
+
In this chapter we will get started with eSim. We will run through the various options
+available with an example circuit. Referring to this chapter will make one familiar with
+eSim and will help plan the project before actually designing a circuit. Lets get
+started.
+
4.1 eSim Main Window
+
+
4.1.1 How to launch eSim in Ubuntu?
+
After installation is completed, to launch eSim 1. Go to terminal. 2. Type esim and hit enter. The first window that appears is workspace dialog as shown in Fig. 4.1.
+
+
+
+
+
+
Figure 4.1: eSim-Workspace
+
+
+
The default workspace is eSim-Workspace under home directory. To create new workspace
+use browse option.
+
4.1.2 Main-GUI
+
The main GUI window of eSim is as shown in Fig. 4.2
+
+
+
+
+
+
Figure 4.2: eSim Main GUI
+
+
+
The eSim main window consists of the following symbols.
+
+ 1.
Toolbar
+
+ 2.
Menubar
+
+ 3.
Project explorer
+
+ 4.
Dockarea
+
+ 5.
Console area
+
Toolbar
+
+
+
+
+
+
+
Figure 4.3: Toolbar
+
+
+
+
Open Schematic: The first tool on the toolbar i.e. Schematic Editor. Clicking on
+ this button will open Eeschema, the KiCad schematic editor.
+
+
Convert KiCad to Ngspice: This converter converts KiCad spice netlist into
+ Ngspice compatible netlist. The KiCad to Ngspice window consists of total five
+ tabs as namely Analysis, Device Model, Source Details, Model Library, Subcircuits.
+ Once the values have been entered, press the Convert key. It will generate
+ .cir.out file in the same project directory. Note that KiCad to Ngspice Converter can only be used if current project has
+ created the KiCad spice netlist file .cir.
+
The details of tabs under KiCad to Ngspice converter are as follows:
+
Analysis
+
This feature helps the user to perform different types of analysis such as Operating
+ point analysis, DC analysis, AC analysis, transient analysis. It has the facility
+ to
+
+
Insert type of analysis such as AC or DC or Transient
+
+
Insert values for analysis
+
+
Source Details
+
eSim sources are added from eSim_Sources library. Source such as SINE, AC, DC,
+ PULSE are in this library. The parameter values to all the sources added in the
+ shcematic can be given through ’Source Details’.
+
+
+
Ngspice Model
+
Ngspice has in built model such as flipflop(D,SR,JK,T),gain,summer etc. which can be
+ utilised while building a circuit. eSim allows to add and modify Ngspice model
+ parameter through Ngspice Model tab.
+
+
Device Modeling
+
Devices like Diode, JFET, MOSFET, IGBT, MOS etc used in the circuit can be
+ modeled using device model libraries. eSim also provides editing and adding new model
+ libraries. While converting KiCad to Ngspice, these library files are added to the
+ corresponding devices used in the circuit.
+
+
Subcircuits
+
Subcircuits are circuits within circuit. Subcircuiting helps to reuse the parts of the
+ circuits. The subcircuits in the main circuits are added using this facility. Also, eSim
+ provides us with the facility to edit already existing subcircuits.
+
+
Simulation: The netlist generated using the KiCad to Ngspice converter is
+ simulated using simulation button. Clicking on the Simulation button will run
+ the Ngspice simulation for current project. Python plotting window will open, as
+ shown in Fig. 4.4. It shows the output waveform of current project. In the
+ Ngspice tab we can view the output plotted by Ngspice.
+
Figure 4.4: Simulation Output in Python Plotting Window
+
+
+
Foot Print Editor: Clicking on the Footprint Editor tool will open the CvPcb
+ window. This window will ideally open the .net file for the current project. So,
+ before using this tool, one should have the netlist for PCB design (a .net
+ file).
+
+
PCB Layout: Clicking on the Layout Editor tool will open Pcbnew, the layout editor
+
+ used in eSim. In this window, one will create the PCB. It involves laying
+ tracks and vias, performing optimum routing of tracks, creating one or more
+ copper layers for PCB, etc. It will be saved as a .brd file in the current project
+ directory.
+
+
Model Editor: eSim also gives an option to re-configure the model library of a device. It
+ facilitates the user to change model library of devices such as diode, transistor,
+ MOSFET, etc.
+
+
Subcircuit: eSim has an option to build subcircuits. The subcircuits can again have
+ components having subcircuits and so on. This enables users to build commonly used
+ circuits as subcircuits and then use it across circuits. For example, one can build a 12
+ Volt power supply as a subcircuit and then use it as just a single component across
+ circuits without having to recreate it. Clicking on Subcircuit Builder tool will allow one
+ to edit or create a subcircuit.
+
+
Menubar
+
+
New Project: New projects are created in the eSim-workspace. When this
+ menu is selected, a new window opens up with Enter Project name field.
+ Type the name of the new project and click on OK. A project directory will
+ be created in eSim-Workspace. The name of this folder will be the same as
+ that of the project created. Make sure project name does not have any spaces.
+
+
Open Project: This opens the file dialog of defalut workspace where the
+ projects are stored. The project can be selected which is then added in the
+ project explorer.
+
+
Exit: This button closes the project window and exits.
+
+
Help: It opens user manual in the dockarea.
+
+
+
Project Explorer
+
Project explorer has tree of all the project previously added in it. On right clicking the
+ project we can simply remove or refresh the project in the explorer. Also on
+ double/right clicking, the project file can be opened in the text editor which can then be
+ edited.
+
+
Dockarea
+
This area is used to open the following windows.
+
+ 1.
KiCad to Ngspice converter
+
+ 2.
Ngspice plotting
+
+ 3.
Python plotting
+
+ 4.
Model builder
+
+ 5.
Subcircuit builder
+
+
Console Area
+
Console area provides information about the activity done in current project.
+
+
+
Chapter 5 Schematic Creation
The first step in the design of an electronic system is the
+design of its circuit. This circuit is usually created using a Schematic Editor and is called a
+Schematic. eSim uses Eeschemaas its schematic editor. Eeschema is the schematic editor of
+KiCad. It is a powerful schematic editor software. It allows the creation and modification of
+components and symbol libraries and supports multiple hierarchical layers of printed circuit
+design.
+
5.1 Familiarizing the Schematic Editor interface
+
Fig. 5.1 shows the schematic editor and the various menu and toolbars. We will explain them
+briefly in this section.
+
+
+
+
+
+
+
+
Figure 5.1: Schematic editor with the menu bar and toolbars marked
+
+
+
+
5.1.1 Top menu bar
+
The top menu bar will be available at the top left corner. Some of the important menu
+options in the top menu bar are:
+
+ 1.
File - The file menu items are given below:
+
+ (a)
New - Clear current schematic and start a new one
+
+ (b)
Open - Open a schematic
+
+ (c)
Open Recent - A list of recently opened files for loading
+
+ (d)
Save Whole Schematic project - Save current sheet and all its hierarchy.
+
+ (e)
Save Current Sheet Only - Save current sheet, but not others in a hierarchy.
+
+ (f)
Save Current sheet as - Save current sheet with a new name.
+
Plot - Plot the schematic in Postscript, HPGL, SVF or DXF format
+
+ (i)
Quit - Quit the schematic editor.
+
+
+
+
+
+
Figure 5.2: Print options
+
+
+
+ 2.
Place - The place menu has shortcuts for placing various items like components, wire
+ and junction, on to the schematic editor window. See Sec. 5.1.5 to know more about
+ various shortcut keys (hotkeys).
+
+ 3.
Preferences - The preferences menu has the following options:
+
Language - Shows the current list of translations. Use default.
+
+ (e)
Hotkeys - Access to the hot keys menu. See Sec. 5.1.5 about hotkeys.
+
+ (f)
Read preferences - Read configuration file.
+
+ (g)
Save preferences - Save configuration file.
+
+
+
5.1.2 Top toolbar
+
+
+
Some of the important tools in the top toolbar are discussed below. They are marked in
+Fig. 5.3.
+
+
+
+
+
+
Figure 5.3: Toolbar on top with important tools marked
+
+
+
+ 1.
Save - Save the current schematic
+
+ 2.
Library Editor - Create or edit components.
+
+ 3.
Library Browser - Browse through the various component libraries available
+
+ 4.
Navigate schematic hierarchy - Navigate among the root and sub-sheets in the
+ hierarchy
+
+ 5.
Print - Print the schematic
+
+ 6.
Generate netlist - Generate a netlist for PCB design or for simulation.
+
+ 7.
Annotate - Annotate the schematic
+
+ 8.
Check ERC - Do Electric Rules Check for the schematic
+
+ 9.
Create BOM - Create a Bill of Materials of the schematic
+
5.1.3 Toolbar on the right
+
+
+
The toolbar on the right side of the schematic editor window has many important tools. Some
+of them are marked in Fig. 5.4.
+
+
+
+
+
+
Figure 5.4: Toolbar on right with important tools marked
+
+
+
Let us now look at each of these tools and their uses.
+
+ 1.
Place a component - Load a component to the schematic. See Sec. 5.2.1 for more
+ details.
+
+ 2.
Place a power port - Load a power port (Vcc, ground) to the schematic
+
+ 3.
Place wire - Draw wires to connect components in schematic
+
+ 4.
Place bus - Place a bus on the schematic
+
+ 5.
Place a no connect - Place a no connect flag, particularly useful in ICs
+
+ 6.
Place a local label - Place a label or node name which is local to the schematic
+
+ 7.
Place a global label - Place a global label (these are connected across all schematic
+ diagrams in the hierarchy)
+
+ 8.
Place a text or comment - Place a text or comment in the schematic
+
5.1.4 Toolbar on the left
+
+
+
Some of the important tools in the toolbar on the left are discussed below. They are marked
+in Fig. 5.5.
+
+
+
+
+
+
Figure 5.5: Toolbar on left with important tools marked
+
+
+
+ 1.
Show/Hide grid - Show or Hide the grid in the schematic editor. Pressing the tool
+ again hides (shows) the grid if it was shown (hidden) earlier.
+
+ 2.
Show hidden pins - Show hidden pins of certain components, for example, power
+ pins of certain ICs.
+
5.1.5 Hotkeys
+
A set of keyboard keys are associated with various operations in the schematic editor. These
+keys save time and make it easy to switch from one operation to another. The list of hotkeys
+can be viewed by going to Preferences in the top menu bar. Choose Hotkeys and
+select List current keys. The hotkeys can also be edited by selecting the option
+Edit Hotkeys. Some frequently used hotkeys, along with their functions, are given
+below:
+
+
F1 - Zoom in
+
+
F2 - Zoom out
+
+
Ctrl + Z - Undo
+
+
Delete - Delete item
+
+
M - Move item
+
+
C - Copy item
+
+
A - Add/place component
+
+
P - Place power component
+
+
R - Rotate item
+
+
X - Mirror component about X axis
+
+
Y - Mirror component about Y axis
+
+
E - Edit schematic component
+
+
+
W - Place wire
+
+
T - Add text
+
+
S - Add sheet
+
Note: Both lower and upper-case keys will work as hotkeys.
+
+
5.2 Schematic creation for simulation
+
+
There are certain differences between the schematic created for simulation and that created
+for PCB design. We need certain components like plots and current sources. For simulation
+whereas these are not needed for PCB design. For PCB design, we would require connectors
+(e.g. DB15 and 2 pin connector) for taking signals in and out of the PCB whereas
+these have no meaning in simulation. This section covers schematic creation for
+simulation.
+
The first step in the creation of circuit schematic is the selection and placement of
+required components. The components are grouped under eSim-libraries as shown in Fig. 5.6.
+
+
+
+
+
+
+
Figure 5.6: eSim-Components Libraries
+
+
+
5.2.1 Selection and placement of components
+
+
We would need a resistor, a capacitor, a voltage source, ground terminal. To place a resistor
+on the schematic editor window, select the Place a component tool from the toolbar
+on the right side and click anywhere on the schematic editor. This opens up the
+component selection window. Resistor component can be found under eSim_Devices
+library. Fig. 5.7 shows the selection of resistor component. Click on OK. A resistor
+will be tied to the cursor. Place the resistor on the schematic editor by a single
+click.
+
+
+
+
+
+
+
Figure 5.7: Placing a resistor using the Place a Component tool
+
+
+
To place the next component, i.e., capacitor, click again on the schematic editor.Similarly,
+Capacitor component is found under eSim_Devices library. Click on OK. Place the capacitor
+on the schematic editor by a single click. Let us now place a sinusoidal voltage source. This is
+required for performing transient analysis. To place it, click again on the schematic editor. On
+the component selection window, choose the library eSim_source by double clicking on it.
+Select the component SINE and click on OK. Place the sine source on the schematic editor by
+a single click.
+
Place the component by clicking on the schematic editor. Similarly place gnd, a ground
+terminal and power_flag under power library. Once all the components are placed, the
+schematic editor would look like the Fig. 5.8.
+
+
+
+
+
+
Figure 5.8: All RC circuit components placed
+
+
+
Let us rotate the resistor to complete the circuit. To rotate the resistor, place the cursor
+on the resistor and press the key R. Note that if the cursor is placed above the letter R (not
+R?) on the resistor, it asks to clarify selection. Choose the option Component R. This can be
+avoided by placing the cursor slightly away from the letter R as shown in Fig. 5.9. This
+applies to all components.
+
+
+
+
+
+
Figure 5.9: Placing the cursor (cross mark) slightly away from the letter R
+
+
+
If one wants to move a component, place the cursor on top of the component and press the
+key M. The component will be tied to the cursor and can be moved in any direction.
+
+
5.2.2 Wiring the circuit
+
+
The next step is to wire the connections. Let us connect the resistor to the capacitor.
+To do so, point the cursor to the terminal of resistor to be connected and press
+the key W. It has now changed to the wiring mode. Move the cursor towards the
+terminal of the capacitor and click on it. A wire is formed as shown in Fig. 5.10a.
+
+
+
+
+
+
+(a)
+Initial
+stages
+ (b)
+ Wiring
+ done
+ (c)
+ Final
+ schematic
+ with
+ PWR_FLAG
+
Figure 5.10: Various stages of wiring
+
+
+
Similarly connect the wires between all terminals and the final schematic would look like
+Fig. 5.10b.
+
5.2.3 Assigning values to components
+
+
We need to assign values to the components in our circuit i.e., resistor and capacitor. Note
+that the sine voltage source has been placed for simulation. The specifications of sine source
+will be given during simulation. To assign value to the resistor, place the cursor above the
+letter R (not R?) and press the key E. Choose Field value. Type 1k in the Edit value field box
+as shown in Fig. 5.11. 1k means 1kΩ. Similarly give the value 1u for the capacitor. 1u means
+1μF.
+
+
+
+
+
+
+
Figure 5.11: Editing value of resistor
+
+
+
5.2.4 Annotation and ERC
+
+
+
+
+
The next step is to annotate the schematic. Annotation gives unique references to the
+components. To annotate the schematic, click on Annotate schematic tool from the
+top toolbar. Click on annotation, then click on OK and finally click on close as
+shown in Fig. 5.13. The schematic is now annotated. The question marks next to
+component references have been replaced by unique numbers. If there are more than
+one instance of a component (say resistor), the annotation will be done as R1, R2,
+etc.
+
Let us now do ERC or Electric Rules Check. To do so, click on Perform electric rules
+check tool from the top toolbar. Click on Test Erc button. The error as shown in Fig. 5.12
+may be displayed. Click on close in the test erc window.
+
+
+
+
+
+
Figure 5.12: ERC error
+
+
+
+
+
+
+
+
+
Figure 5.13: Steps in annotating a schematic: 1. First click on Annotation then 2. Click
+on Ok then 3. Click on close
+
+
+
There will be a green arrow pointing to the source of error in the schematic. Here it points
+to the ground terminal. This is shown in Fig. 5.14.
+
+
+
+
+
+
Figure 5.14: Green arrow pointing to Ground terminal indicating an ERC error
+
+
+
To correct this error, place a PWR_FLAG from the Eeschema library power. Connect the
+power flag to the ground terminal as shown in Fig. 5.10c. One needs to place PWR_FLAG
+wherever the error shown in Fig. 5.12 is obtained. Repeat the ERC. Now there are no errors.
+With this we have created the schematic for simulation.
+
5.2.5 Netlist generation
+
+
To simulate the circuit that has been created in the previous section, we need to generate its
+netlist. Netlist is a list of components in the schematic along with their connection
+information. To do so, click on the Generate netlist tool from the top toolbar. Click on spice
+from the window that opens up. Check the option Default Format. Then click on Generate.
+This is shown in Fig. 5.15. Save the netlist. This will be a .cir file. Do not change the
+directory while saving.
+
+
+
+
+
+
Figure 5.15: Steps in generating a Netlist for simulation: 1. Click on Spice then 2.
+Check the option Default Format then 3. Click on Generate
+
+
+
Now the netlist is ready to be simulated. Refer to [15] or [16] to know more about
+Eeschema.
+
+
Chapter 6 PCB Design
Printed Circuit Board (PCB) design is an important step in
+electronic system design. Every component of the circuit needs to be placed and connections
+routed to minimise delay and area. Each component has an associated footprint. Footprint
+refers to the physical layout of a component that is required to mount it on the PCB.PCB
+design involves associating footprints to all components, placing them appropriately to
+minimise wire length and area, connecting the footprints using tracks/vias and finally
+extracting the required files needed for printing the PCB. Let us see the steps to design PCB
+using eSim.
+
6.1 Schematic creation for PCB design
+
In Chapter 9, we will see the differences between schematic for simulation and schematic for
+PCB design. Let us design the PCB for a RC circuit. A resistor, capacitor, ground, power flag
+and a connector are required. Connectors are used to take signals in and out of the
+PCB.
+
Create the circuit schematic as shown in Fig. 6.1. The two pin connector (CONN_2) can
+be placed from the Eeschema library conn. Do the annotation and test for ERC. Refer to
+Chapter 9 to know more about basic steps in schematic creation.
+
+
+
+
+
+
+
Figure 6.1: Final circuit schematic for RC low pass circuit
+
+
+
6.1.1 Netlist generation for PCB
+
+
+
The netlist for PCB is different from that for simulation. To generate netlist for PCB, click on
+the Generate netlist tool from the top toolbar in Schematic editor. In the Netlist window,
+under the tab Pcbnew, click on the button Netlist. This is shown in Fig. 6.2. Click on
+Save in the Save netlist file dialog box that opens up. Do not change the directory
+or the name of the netlist file. Save the schematic and close the schematic editor.
+
+
+
+
+
+
+
Figure 6.2: Netlist generation for PCB
+
+
+
Note that the netlist for PCB has an extension .net. The netlist created for simulation
+has an extension .cir.
+
6.1.2 Mapping of components using Footprint Editor
+
+
+
+
Once the netlist for PCB is created, one needs to map each component in the netlist to a
+footprint. The tool Footprint Editor is used for this. eSim uses CvPcb as its footprint editor.
+CvPcb is the footprint editor tool in KiCad.
+
+
6.1.3 Familiarising the Footprint Editor tool
+
+
If one opens the Footprint Editor after creating the .net netlist file, the Footprint editor as
+shown in Fig. 6.3 will be obtained. The menu bar and toolbars and the panes are marked in
+this figure. The menu bar will be available in the top left corner. The left pane has a list of
+components in the netlist file and the right pane has a list of available footprints for each
+component.
+
+
+
+
+
+
Figure 6.3: Footprint editor with the menu bar, toolbar, left pane and right pane
+marked
+
+
+
Note that if the Footprint Editor is opened before creating a ‘.net’ file, then the left and
+right panes will be empty.
+
Toolbar
+
Some of the important tools in the toolbar are shown in Fig. 6.4. They are explained below:
+
+
+
+
+
+
+
Figure 6.4: Some important tools in the toolbar
+
+
+
+ 1.
Save netlist and footprint files - Save the netlist and the footprints that are
+ associated with it.
+
+ 2.
View selected footprint - View the selected footprint in 2D. See Sec. 6.1.4 for more
+ details.
+
+ 3.
Automatic footprint association - Perform footprint association for each
+ component automatically. Footprints will be selected from the list of footprints
+ available.
+
+ 4.
Delete all associations - Delete all the footprint associations made
+
+ 5.
Display filtered footprint list - Display a filtered list of footprints suitable to the
+ selected component
+
+ 6.
Display full footprint list - Display the list of all footprints available (without
+ filtering)
+
6.1.4 Viewing footprints in 2D and 3D
+
+
+
To view a footprint in 2D, select it from the right pane and click on View selected footprint
+from the menu bar. Let us view the footprint for SM1210. Choose SM1210 from
+the right pane as shown in Fig. 6.5. On clicking the View selected footprint tool,
+the Footprint window with the view in 2D will be displayed. Click on the 3D
+tool in the Footprint window, as shown in Fig. 6.6. A top view of the selected
+footprint in 3D is obtained. Click on the footprint and rotate it using mouse to get 3D
+views from various angles. One such side view of the footprint in 3D is shown in
+Fig. 6.7.
+
+
+
+
+
+
+
Figure 6.5: Viewing footprint for SM1210: 1. Choose the footprint SM1210 from the
+right pane, 2. Click on View selected footprint
+
+
+
+
+
+
+
+
+
Figure 6.6: Footprint view in 2D. Click on 3D to get 3D view
+
+
+
+
+
+
+
+
+
Figure 6.7: Side view of the footprint in 3D
+
+
+
6.1.5 Mapping of components in the RC circuit
+
Click on C1 from the left pane. Choose the footprint C1 from the right pane by double
+clicking on it. Click on connector P1 from the left pane. Choose the footprint SIL-2 from the
+right pane by double clicking on it. Similarly choose the footprint R3 for the resistor R1. The
+footprint mapping is shown in Fig. 6.8. Save the footprint association by clicking on the Save
+netlist and footprint files tool from the CvPcb toolbar. The Save Net and component List
+window appears. Browse to the directory where the schematic file for this project is saved and
+click on Save. The netlist gets saved and the Footprint Editor window closes automatically.
+
+
+
+
+
+
+
Figure 6.8: Footprint mapping done
+
+
+
Note that one needs to browse to the directory where the schematic file is saved and save
+the ‘.net’ file in the same directory.
+
6.2 Creation of PCB layout
+
+
+
The next step is to place the footprints and lay tracks between them to get the layout. This is
+done using the Layout Editor tool. eSim uses Pcbnew, the layout creation tool in KiCad, as its
+layout editor.
+
+
6.2.1 Familiarizing the Layout Editor tool
+
+
The layout editor with the various menu bar and toolbars is shown in Fig. 6.9.
+
+
+
+
+
+
+
Figure 6.9: Layout editor with menu bar, toolbars and layer options marked
+
+
+
+
+
+
+
+
+
Figure 6.10: Top toolbar with important tools marked
+
+
+
Top toolbar
+
Some of the important menu options in the top menu bar are shown in Fig. 6.10. They are
+explained below:
+
+ 1.
Save board - Save the printed circuit board
+
+ 2.
Module editor - Open module editor to edit footprint modules or libraries
+
+ 3.
Read netlist - Import the netlist whose layout needs to be created.
+
+ 4.
Perform design rules check - Check for design rules, unconnected nets, etc., in the
+ layout.
+
+ 5.
Select working layer - Selection of working layer
+
+ 6.
Show active layer selections and select layer pair for route and place - Select layer
+ in top and bottom layers. It also shows the currently active layer selections.
+
+ 7.
Mode footprint: Manual/automatic move and place - Move and place modules
+
+
6.2.2 Hotkeys
+
+
A list of hotkeys are given below:
+
+ 1.
F1 - Zoom in
+
+ 2.
F2 - Zoom out
+
+ 3.
Delete - Delete Track or Footprint
+
+ 4.
X - Add new track
+
+ 5.
V - Add Via
+
+ 6.
M - Move Item
+
+
+ 7.
F - Flip Footprint
+
+ 8.
R - Rotate Item
+
+ 9.
G - Drag Footprint
+
+ 10.
Ctrl+Z - Undo
+
+ 11.
E - Edit Item
+
The list can be viewed by selecting Preferences from the top menu bar and choosing List Current
+Keys from the option Hotkeys.
+
+
6.2.3 PCB design example using RC circuit
+
+
Click on Layout Editor from the eSim toolbar. Click on Read Netlist tool from the top
+toolbar. Click on Browse Netlist files on the Netlist window that opens up. Select the .net file
+that was modified after assigning footprints. Click on Open. Now Click on Read Current
+Netlist on the Netlist window. The message area in the Netlist window says that
+the RC_pcb.net has been read. The sequence of operations is shown in Fig. 6.11.
+
The footprint modules will now be imported to the top left hand corner of the layout
+editor window. This is shown in Fig. 6.12.
+
+
+
+
+
+
Figure 6.12: Footprint modules imported to top left corner of layout editor window
+
+
+
Zoom in to the top left corner by pressing the key F1 or using the scroll button of the
+mouse. The zoomed in version of the imported netlist is shown in Fig. 6.13.
+
Let us now place this in the center of the layout editor window.
+
+
+
+
+
+
Figure 6.13: Zoomed in version of the imported netlist
+
+
+
Click on Mode footprint: Manual/automatic move and place tool from the top toolbar.
+Place the cursor near the center of the layout editor window. Right click and choose Glob
+move and place. Choose move all modules. The sequence of operations is shown in Fig. 6.14.
+Click on Yes on the confirmation window to move the modules. Zoom in using the F1 key.
+The current placement of components after zooming in is shown in Fig. 6.15a.
+
+
+
+
+
+
+
Figure 6.14: Moving and placing modules to the center of layout editor. 1. Click on
+Mode footprint: Manual/automatic move and place, 2. Place cursor at center of layout
+editor and right click on it 3. Choose Glob Move and Place and then choose Move All
+Modules.
+
+
+
+
+
+
+
+
+(a)
+Zoomed
+in
+version
+of the
+current
+placement
+after
+moving
+modules
+to the
+center
+of the
+layout
+editor
+ (b)
+ Final
+ placement
+ of
+ footprints
+ after
+ rotating
+ and
+ moving
+ P1
+
Figure 6.15: Different stages of placement of modules on PCB
+
+
+
We need to arrange the modules properly to lay tracks. Rotate the connector P1 by
+placing the cursor on top of P1 and pressing R. Move it by placing the cursor on top of it and
+pressing M. The final placement is shown in Fig. 6.15b.
+
Let us now lay the tracks. Let us first change the track width. Click on Design rules from
+the top menu bar. Click on Design rules. This is shown in Fig. 6.16. The Design Rules Editor
+window opens up. Here one can edit the various design rules. Double click on the track width
+field to edit it. Type 0.8 and press Enter. Click on OK. Fig. 6.17 shows the sequence of
+operations.
+
+
+
+
+
+
Figure 6.16: Choose Design Rules from the top menu bar and Design Rules again
+
+
+
+
+
+
+
+
+
Figure 6.17: Changing the track width: 1. Double click on Track Width field and type
+0.8, 2. Click on OK
+
+
+
Click on Back from the Layer options as shown in Fig. 6.18.
+
+
+
+
+
+
Figure 6.18: Choosing the copper layer Back
+
+
+
Let us now start laying the tracks. Place the cursor above the left terminal of R1
+in the layout editor window. Press the key x. Move the cursor down and double
+click on the left terminal of C1. A track is formed. This is shown in Fig. 6.19a.
+
+
+
+
+
+
+(a) A
+track
+formed
+between
+resistor
+and
+capacitor
+ (b) A
+ track
+ formed
+ between
+ capacitor
+ and
+ connector
+ (c) A
+ track
+ formed
+ between
+ connector
+ and
+ resistor
+
Figure 6.19: Different stages of laying tracks during PCB design
+
+
+
Similarly lay the track between capacitor C1 and connector P1 as shown in
+Fig. 6.19b. The last track needs to be laid at an angle. To do so, place the cursor
+above the second terminal of R1. Press the key x and move the cursor diagonally
+down. Double click on the other terminal of the connector. The track will be laid
+as shown in Fig. 6.19c. All tracks are now laid. The next step is to create PCB
+edges.
+
Choose PCB_edges from the Layer options to add edges. Click on Add graphic line or
+polygon from the toolbar on the left. Fig. 6.20 shows the sequence of operations. Let us now
+start drawing edges for PCB.
+
+
+
+
+
+
Figure 6.20: Creating PCB edges: 1. Choose PCB_Edges from Layer options 2. Choose
+Add graphic line or polygon from left toolbar
+
+
+
Click to the left of the layout. Move cursor horizontally to the right. Click once to change
+orientation. Move cursor vertically down. Draw the edges as shown in Fig. 6.21. Double click
+to finish drawing the edges.
+
+
+
+
+
+
Figure 6.21: PCB edges drawn
+
+
+
Click on Perform design rules check from the top toolbar to check for design rules. The
+DRC Control window opens up. Click on Start DRC. There are no errors under the Error
+messages tab. Click on OK to close DRC control window. Fig. 6.22 shows the sequence of
+operations.
+
+
+
+
+
+
Figure 6.22: Performing design rules check: 1. Click on Start DRC, 2. Click on Ok
+
+
+
Click on Save board on the top toolbar.
+
To generate Gerber files, click on File from the top menu bar. Click on Plot. This is shown
+in Fig. 6.23. The plot window opens up. One can choose which layers to plot by
+selecting/deselecting them from the Layers pane on the left side. One can also choose the
+format used to plot them. Choose Gerber. The output directory of the plots created
+can also be chosen. By default, it is the project directory. Some more options can
+be chosen in this window. Click on Plot. The message window shows the location
+in which the Gerber files are created. Click on Close. This is shown in Fig. 6.24.
+
+
+
+
+
+
+
Figure 6.23: Choosing Plot from the File menu
+
+
+
+
+
+
+
+
+
Figure 6.24: Creating Gerber files: 1. Choose Gerber as the plot format, 2. Click on
+Plot. Message window shows location in which Gerber files are created, 3. Click on Close
+
+
+
The PCB design of RC circuit is now complete. To know more about Pcbnew, refer to
+ [15] or [16].
+
+
Chapter 7 Model Editor
+
Spice based simulators include a feature which allows accurate modeling of semiconductor
+devices such as diodes, transistors etc. eSim Model Editor provides a facility to define a new
+model for devices such as diodes, MOSFET, BJT, JFET, IGBT, Magnetic core etc. Model
+Editor in eSim lets the user enter the values of parameters depending on the type of
+device for which a model is required. The parameter values can be obtained from the
+data-sheet of the device. A newly created model can be exported to the model library
+and one can import it for different projects, whenever required. Model Editor also
+provides a facility to edit existing models. The GUI of the model editor is as shown in
+Fig. 7.1
+
+
+
+
+
+
+
Figure 7.1: Model Editor
+
+
+
7.1 Creating New Model Library
+
eSim lets us create new model libraries based on the template model libraries. On selecting
+New button the window is popped as shown in Fig. 7.2. The name has to be unique otherwise
+the error message appears on the window.
+
+
+
+
+
+
+
Figure 7.2: Creating New Model Library
+
+
+
After the OK button is pressed the type of model library to be created is chosen by
+selecting one of the types on the left hand side i.e. Diode, BJT, MOS, JFET, IGBT,
+Magnetic Core. The template model library opens up in a tabular form as shown in Fig. 7.3
+
+
+
+
+
+
+
Figure 7.3: Choosing the Template Model Library
+
+
+
+
New parameters can be added or current parameters can be removed using ADD
+and REMOVE buttons. Also the values of parameters can be changed in the table.
+Adding and removing the parameters in library files is shown in the Fig. 7.4 and
+Fig. 7.5
+
+
+
+
+
+
+
Figure 7.4: Adding the Parameter in a Library
+
+
+
+
+
+
+
+
+
Figure 7.5: Removing a Parameter from a Library
+
+
+
After the editing of the model library is done, the file can be saved by selecting the SAVE
+button. These libraries are saved in the User Libraries folder under deviceModelLibrary
+repository.
+
7.2 Editing Current Model Library
+
The existing model library can be modified using EDIT option. On clicking the EDIT button
+the file dialog opens where all the library files are saved as shown in Fig. 7.6. You can select
+the library you want to edit. Once you are done with the editing, click on SAVE
+button.
+
+
+
+
+
+
+
Figure 7.6: Editing Existing Model Library
+
+
+
7.3 Uploading external .lib file to eSim repository
+
eSim directly cannot use the external .lib file. It has to be uploaded to eSim repository before
+using it in a circuit. eSim provides the facility to upload library files. They are then converted
+into xml format, which can be easily modified from the eSim interface. On clicking UPLOAD
+button the library can be uploaded from any location. The model library will be
+saved with the name you have provided, in the User Libraries folder of repository
+deviceModelLibrary.
+
+
Chapter 8 SubCircuit Builder
Subcircuit is a way to implement hierarchical modeling.
+Once a subcircuit for a compo- nent is created, it can be used in other circuits.
+eSim provides an easy way to create a subcircuit. The following Fig. 8.1 shows
+the window that is opened when the SubCircuit tool is chosen from the toolbar.
+
+
+
+
+
+
+
Figure 8.1: Subcircuit Window
+
+
+
+
8.1 Creating a SubCircuit
+
The steps to create subcircuit are as follows.
+
+
After opening the Subcircuit tool, click on New Subcircuit Schematic button.
+ It will ask the name of the subcircuit. Enter the name of subcircuit (without any
+ spaces) and click OK as shown in Fig. 8.2.
+
+
Figure 8.2: New Sub circuit Window
+
+
+
After clicking OK button it will open KiCad schematic. Draw your circuit
+ which will be later used as a subcircuit. e.g the Fig. 8.3 shows the half adder
+ circuit.
+
+
Figure 8.3: New Sub circuit Window
+
+
+
+
Once you complete the circuit, assign port to the node of your circuit which will be
+ used to connect with the main circuit. The circuit will look like Fig. 8.4 after
+ adding PORT to it. The PORT symbol can be found in Eeschema as shown in
+ Fig. 8.5.
+
+
Figure 8.4: Half-Adder Subcircuit
+
+
+
Figure 8.5: Selection of PORT component
+
+
+
+
Next step is to save the schematic and generate KiCad netlist as explained in Chapter
+ 5.
+
+
To use this as a subcircuit, create a block in KiCad Eeschema by following steps given
+ below:
+
+ 1.
Go to library browser of Eeschema.
+
+ 2.
Select the working library as eSim_Subckt as shown in Fig. 8.6
+
Figure 8.6: Selecting Working Library
+
+
+
+ 3.
Click on create a new component with reference X as shown in Fig. 8.7
+
+
Figure 8.7: Creating New Component
+
+
+ 4.
Start drawing the subcircuit block. Update and save it as shown in Fig. 8.8.
+
+
Figure 8.8: Half-Adder Subcircuit Block
+
+
+
+
+
Close the Eeschema window and click on Convert KiCad to Ngspice button in subcircuit
+ builder tool. This will convert the KiCad spice netlist to Ngspice netlist. And it will
+ save your subcircuit into eSim repository, which you can add in your main
+ circuit.
+
+
+
8.2 Edit a Subcircuit
+
The steps to edit a subcircuit are as follows.
+
+
After opening the Subcircuit tool, click on Edit Subcircuit Schematic button.
+ It will open a dialog box where you can select any subcircuit for editing.
+
+
After selecting the subcircuit it will open it in KiCad Eeschema, where you can
+ edit the subcircuit.
+
+
Next step is to save the schematic and generate KiCad netlist.
+
+
If you have edited the number of ports then you have to change the block in KiCad
+ Eeschema accordingly.
+
+
Close the Eeschema window and click on Convert KiCad to Ngspice button in
+ subcircuit builder tool to convert the edited subcircuit KiCad netlist into Ngspice
+ netlist.
+
+
+
Chapter 9 Solved Examples
+
9.1 Solved Examples
+
+
9.1.1 Basic RC Circuit
+
+
Problem Statement:
+
Plot the Input and Output Waveform of an RC circuit whose input voltage (Vs) is 50Hz,
+3V peak to peak. The values of Resistor (R) and Capacitor(C) are 1k and 1uf
+respectively.
+
Solution:
+
+
Creating a Project: The new project is created by clicking the New icon on the
+ menubar. The name of the project is given in the pop up window as shown in
+ Fig. 9.1.
+
Figure 9.1: Creating New Project
+
+
+
Creating the Schematic: To create the schematic, click the very first icon of the left
+ toolbar as shown in the Fig. 9.2. This will open KiCad Eeschema.
+
+
Figure 9.2: Open Schematic Editor
+
+
To create a schematic in KiCad, we need to place the required components. Fig. 9.3
+ shows the icon on the right toolbar which opens the component library.
+
+
Figure 9.3: Place Component Icon
+
+
+
After all the required components of the simple RC circuit are placed, wiring is done
+ using the Place Wire option as shown in the Fig. 9.4
+
+
Figure 9.4: Place Wire Icon
+
+
Next step is ERC (Electric Rules Check). Fig. 9.5 shows the icon for ERC.
+
+
Figure 9.5: Electric Rules Check Icon
+
+
Fig. 9.6 shows the RC circuit after connecting the components by wire.
+
+
Figure 9.6: RC circuit
+
+
+
After clicking the ERC icon a window opens up. Click the Run button to run rules check.
+ The errors are listed in as shown in Fig. 9.7a. This error is handled by adding Power
+ Flag as shown in Fig. 9.7b.
+
+ (a)
+ ERC
+ Run
+ (b)
+ Power
+ Flag
+
Figure 9.7: ERC check and POWER FLAG
+
+
After adding the Power Flag the completed RC circuit is shown in Fig. 9.8a and the
+ netlist is generated as shown in Fig. 9.8b.
+
Convert KiCad to Ngspice: To convert KiCad netlist of RC circuit to NgSpice
+ compatible netlist click on KiCad to Ngspice icon as shown in Fig. 9.9.
+
+
Figure 9.9: Convert KiCad to Ngspice Icon
+
+
Now you can enter the type of analysis and source details as shown in Fig. 9.10a and
+ Fig. 9.10b respectively.
+
The other tab will be empty as RC circuit do not use any Ngspice model, device library
+ and subcircuit.
+
After entering the value, press the convert button. It will convert the netlist into
+ Ngspice compatible netlist.
+
+
+
Simulation: To run Ngspice simulation click the simulation icon in the tool bar
+ as shown in the Fig. 9.11.
+
Figure 9.11: Simulation Icon
+
+
In eSim, there are two types of plot. First is normal Ngspice plot and second is
+ interactive python plot as shown in Fig. 9.12a and Fig. 9.12b respectively.
+
+ (a)
+ Ngspice
+ Plot
+ of RC
+ (b)
+ Python
+ Plot
+ of RC
+
Figure 9.12: Ngspice and Interactive Python Plotting
+
+
In the interactive python plot you can select any node or branch to plot voltage or
+ current across it. Also it has the facility to plot basic functions across the node like
+ addition, substraction, multiplication, division and v/s.
+
+
+
+
9.1.2 Half Wave Rectifier
+
+
Problem Statement:
+
Plot the Input and Output Waveform of Half Wave Rectifier circuit where the input voltage
+(Vs) is 50Hz, 2V peak to peak. The value for Resistor (R) is 1k.
+
+
Solution:
+
The new project is created by clicking the New icon on the menubar. The name of the project
+is given in the window shown in Fig. 9.1.
+
+
Creating Schematic: To create the schematic, click the very first icon of the left
+ toolbar as shown in the Fig. 9.2. This will open KiCad Eeschema.
+
After the KiCad window is opened, to create a schematic we need to place the
+ required components. Fig. 9.3 shows the icon on the right toolbar which opens
+ the component library.
+
After all the required components of the simple Half Wave rectifier circuits are
+ placed, wiring is done using the Place Wire option as shown in the Fig. 9.4
+
Next step is ERC (Electric Rules Check). Fig. 9.5 shows the icon for ERC. After
+ completing all the above steps the final Half Wave Rectifier schematic will look
+ like Fig. 9.13.
+
+
Figure 9.13: Schematic of Half Wave Rectifier circuit
+
+
+
KiCad netlist is generated as shown in the Fig. 9.14
+
Convert KiCad to Ngspice: After creating KiCad netlist, click on the KiCad-Ngspice
+ converter button. This will open converter window where you can enter details of
+ Analysis, Source values and Device library.
+
Plot the input and output waveform of the Precision Rectifier circuit where input voltage
+(Vs) is 50Hz , 3V peak to peak.
+
+
Solution:
+
The new project is created by clicking the New icon on the menubar. The name of the project
+is given as shown in the Fig. 9.1.
+
+
Creating Schematic: To create the schematic, click the very first icon of the left
+ toolbar as shown in the Fig. 9.2. This will open KiCad Eeschema. After the KiCad window is opened, to create a schematic we need to place the
+ required components. Fig. 9.3 shows the icon on the right toolbar which opens
+ the component library. After all the required components of the precision rectifier circuit are placed,
+ wiring is done using the Place Wire option as shown in the Fig. 9.4. Next step is ERC (Electric Rules Check). Fig. 9.5 shows the icon for ERC. The
+ Fig. 9.17 shows the complete Precision Rectifier schematic after removing the
+ errors.
+
+
Figure 9.17: Schematic of Precision Rectifier circuit
+
+
The KiCad netlist is generated as shown in Fig. 9.18.
+
Figure 9.19: Analysis, Source, Device library and Subcircuit tab
+
+
Under device library you can add the library for the diode used in the circuit. If you do
+ not add any library it will take default Ngspice model for diode.
+
Under subcircuit tab you have to add the subciruit used in your circuit. If you forget to
+ add subcircuit it will throw an error.
+
+
+
Simulation: Once the KiCad-Ngspice converter runs successfully, you can run the
+ simulation by clicking the simulation button in the toolbar.
Plot the Input and Output Waveform of Inverting Amplifier circuit where the input voltage
+(Vs) is 50Hz, 2V peak to peak and gain is 2.
+
Solution:
+
+
Creating Schematic: To create the schematic, click the very first icon of the left
+ toolbar as shown in the Fig. 9.2. This will open KiCad Eeschema. After the KiCad window is opened, to create a schematic we need to place the
+ required components. Fig. 9.3 shows the icon on the right toolbar which opens
+ the component library. After all the required components of the inverting amplifier circuit are placed,
+ wiring is done using the Place Wire option as shown in the Fig. 9.4. Next step is ERC (Electric Rules Check). Fig. 9.5 shows the icon for ERC.
+
The Fig. 9.21 shows the complete Precision Rectifier schematic after removing
+ the errors.
+
+
Figure 9.21: Schematic of Inverting Amplifier circuit
+
+
The KiCad netlist is generated as shown in Fig. 9.22.
Plot the Input and Output Waveform of Half Adder circuit.
+
+
Solution:
+
+
Creating Schematic: To create the schematic, click the very first icon of the left
+ toolbar as shown in the Fig. 9.2. This will open KiCad Eeschema. After the KiCad window is opened, to create a schematic we need to place the
+ required components. Fig. 9.3 shows the icon on the right toolbar which opens
+ the component library. After all the required components of the Half Adder circuit are placed, wiring is
+ done using the Place Wire option as shown in the Fig. 9.4. Next step is ERC (Electric Rules Check). Fig. 9.5 shows the icon for ERC.
+
The Fig. 9.25 shows the complete Half Adder schematic after removing the
+ errors.
+
Figure 9.25: Schematic of Half Adder circuit
+
+
The KiCad netlist is generated as shown in Fig. 9.26.
+ [1]A. S. Sedra and K. C. Smith, Microelectronic Circuits - Theory and
+ Applications. Oxford University Press, 2009.
+
+
+ [2]K. M. Moudgalya, “Spoken Tutorial: A Collaborative and Scalable Education
+ Technology,” CSI Communications, vol. 35, no. 6, pp. 10–12, September 2011,
+ available at http://spoken-tutorial.org/CSI.pdf.
+
+ [6]K. Kannan and K. Narayanan, “Ict-enabled scalable workshops for engineering
+ college teachers in india,” in Post-Secondary Education and Technology: A Global
+ Perspective on Opportunities and Obstacles to Development (International and
+ Development Education), R. Clohey, S. Austin-Li, and J. C. Weldman, Eds.
+ Palgrave Macmillan, 2012.
+
+