Using KiCad with AimSpice Doc 0.2 CETA - Univ. Hartford, Connecticut, USA

Transcription

1 Using KiCad with AimSpice Doc 0.2 CETA - Univ. Hartford, Connecticut, USA KiCad is a open source software package for schematic capture and PC board layout. KiCad also provides some capability in producing a SPICE circuit description, useful for analog simulation. This tutorial outlines how to use the KiCad schematic capture tool to produce a netlist suitable for use with the AimSPICE tool. The primary audience for this document is undergraduate electrical and computer engineering students. Such students might be using KiCad and AimSPICE for classwork, laboratory work, or projects. This tutorial considers KiCad version and AimSPICE version 5.5 (October 12, 2009). During the writing of this tutorial several versions of the Windows operating system were used including XP home, XP professional, Vista Home Premium, and Windows 7 Starter. However the work performed does not represent a complete test. Make a New Project and Schematic KiCad works with so-called projects. A project involves many files all contained in a single folder. Of these files, the project file (.pro) is used to organize the project. It is strongly suggested that the first part of the project file name be the same as the folder containing the project. In this tutorial the project folder will be named divider01 and the corresponding project file is named divider01.pro. To start KiCad and produce the new project do the following: In Windows, with the mouse, select: Start => Programs => KiCad => KiCad In the KiCad project manager, select: File => New In the Create New Project window, navigate to a convenient location for your new project folder and use the Create New Folder icon to make a new folder Make New Folder icon Change the name of the new folder to divider01 Double click to enter the folder and in the File name field type in divider01 and click Save. You now have a new KiCad project. Click on the EESchema icon to start the schematic capture tool. A pop-up information window will tell you that the project top level schematic does not yet exist. Click OK. Finally, save the new schematic EESchema icon With the mouse select: File => Save Whole Schematic Project

2 Project Specific Library for SPICE To be able to use KiCad to produce circuit descriptions that make sense to SPICE, this tutorial uses a project specific library. Unlike the installed KiCad libraries, a project specific library is a library file that is included in the project folder. This specific file is named spicenn.lib where NN is a two digit version number. As of this writing the file is named spice01.lib. With the new project created, save the file spice01.lib to the project folder. While the library is actually located in the project folder, to be able to use the library it is necessary to refer to the library in the library search path. To include the project specific library, do the following: In the schematic capture window select Preferences => Libraries In the from window, in the Current search path list click to select your project folder To the right of the Component library files click on Add In the pop-up window, select the spice library file and click Open In the from window click OK In the Save Project Settings click Save Until there is an official SPICE library included with KiCad, the advantage of including the SPICE library file as a project specific library is that it will stay with the project, which is helpful if you use KiCad with several computers. Voltage Divider Example Inserting Components Voltage dividers like that below serve as a classic example. In the following you will use the schematic capture tool to enter the following schematic: Example voltage divider circuit With the new project and schematic capture tool open, the next step is to insert the corresponding components into the schematic. Let's start by inserting the independent voltage source.

3 Using the mouse, click the 'Place a component' icon and move the cursor inside the schematic. The new mode is indicated as the cursor includes a symbol that looks like a pencil. To return to normal mode either click the escape key (ESC) or click the arrow icon. 'Place a component' icon With the mouse, inside the schematic click left and in the pop-up 'Component selection' window click on, 'Select by browser'. In the 'Library browser' window, in the left pane look for and click left to select the 'spice01' library. In the middle pane click to select 'V-IND' and the corresponding symbol will appear in the right pane. Click the 'Insert component into schematic' icon and in the schematic click left to affix the component to a location..'insert component into schematic' icon Repeat the steps above to insert a GND0 symbol from the spice01 library. For the second GND0 note that once inserted into the schematic, a given symbol is listed in the component selection history list. To insert the second GND0 symbol, do the following: Click left to open the 'Component selection window' as you did before and in the 'History list' click left on GND0. In the schematic click left to affix the component to a location. Use the same method to insert two R resistor symbols from the device library. You will rotate one of the resistors. Some KiCad commands use a point and hot-key combination so that it is enough to use the mouse to point the cursor at the resistor and press the 'R' key on your keyboard. Editing Component Values and Designators The components inserted are all fairly generic. A component is customized by assigning an reference identifier which uniquely identifies that component among all those in the schematic, as well as a component value. Here we will use the component editor. With the mouse: Point the cursor at the voltage source, right click, select Edit Component => Edit The 'Component Properties' window appears. o In the 'Fields' pane, left click on 'Value' and in the 'Value Field' enter 'DC 6V ' o In the 'Fields' pane, left click on 'Reverence' and likewise enter 'V1' Click 'OK' Using the above outline, assign the reference identifier and value to each of the resistors.

4 Wiring and Assigning Net Names Here is a method to insert wiring. The following is the voltage source, ground, and first wire. To insert the wire, do the following: Click on the 'Place a wire' icon to start the wiring tool mode 'Place a wire' Point the cursor at the top middle part of the ground symbol and left click Move the cursor to the bottom terminal of the voltage source and left click Insert additional wires like that in the earlier schematic. Note that starting or ending a wire introduces a wire junction which is shown with a dot between the wires. It is strongly suggested that names be assigned to each wire, except those wires that connect directly to ground. Assigning names will help you identify the signals in your SPICE circuit description and SPICE simulation. The signals connecting to ground are automatically named 0 (zero) Click the 'Place a net name' icon 'Place a net name' icon Point the cursor at the wire connecting to the voltage source '+' terminal and click left In the 'Label Properties' enter 'V1' into the text field Change the size value to Click OK Follow the same outline to assign 'V2' to the wire to the right. Save your work: Click File => Save Whole Schematic Project

5 Annotation, Rules Check, and Producing a Net List Regardless of how the component reference designators are assigned, you will have to run the annotation tool. Click the 'Annotate schematic' icon Annotate schematic In the 'Annotate Schematic' window click the 'Annotation' button. In the pop-up window click 'OK' then click 'Close' To check your schematic: Click the 'Schematic Electric Rules Check' (ERC) icon 'Schematic Electric Rules Check' icon In the EEScema Erc window click the 'Test Erc' button If no errors are reported then click 'Close' The next step is to produce the net list. Click on the 'Netlist generation icon 'Netlist generation' icon In the 'Netlist' window click on the 'Spice' tab In the 'Netlist Options' field click to chose 'Use Net Names' Click 'Netlist' and in the navigation window click 'Save' At this moment you have produced a SPICE netlist. To save your work: Click File => Save Whole Schematic Project AimSPICE and KiCad The primary issue with AimSPICE is that it treats.cir files from other tools such as KiCad as a more traditional SPICE file. While doing so makes AimSPICE more compatible with other versions of SPICE, it also prevents us from using the convenient controls that AimSPICE provides. Thankfully there is a simple workaround so that we do not have to manually enter commands into the file. When AimSPICE creates a.cir file it inserts special text before and after your circuit description. The special text is what differentiates the file produced by AimSPICE. In using AimSPICE this special text is hidden from you. The workaround here is simple, we will use AimSPICE to produce a.cir file and

6 then use that to include the KiCad.cir file. In addition we have to make a minor change to the KiCad SPICE file. Start AimSPICE and Open the KiCad SPICE File Use your mouse to enter the start menu and then open the KiCad SPICE file In Windows, Start => Programs => AIM-Spice => AIM-Spice In AimSPICE, File => Open In the navigation window find and click to select divider01, click 'Open' Change the comment block at the top of the file. For every circuit description that you perform as an assignment, include a comment block that contains at least the following information. This information is helpful to the teaching staff and may be useful to you as well. The name of the file Your name The date A description of what the file describes or what it is for It is important that the.end is statement is either commented out or deleted. While an '.end' statement is part of a traditional SPICE file, it causes AimSPICE to perform incorrectly. The primary symptom is that simulations execute with zero iterations in zero seconds. With an opening comment block and the end statement commented, your file will be similar to the following: * divider01.cir - Your Name - The Date * Demonstration netlist produced by KiCad R1 /V2 /V1 1K R2 /V2 0 2K V1 /V1 0 DC 6V *.end Be sure to save your work. The next step is to create an AimSPICE.cir file File => New File => Save As In the navigation window enter the file name 'divider01_aim.cir' and click 'Save' Enter into the file the following text. The first line in the following is used as the simulation title, so be sure to include your name and the date in this file. * divider01_aim.cir - Your Name - The Date.include divider01.cir Be sure to save your work.

7 We will perform what is called an operating point analysis. In AimSPICE click on the 'Operating Point Analysis' icon. 'Operating Point Analysis' icon After a few moments the simulation statistics appear, click OK and the simulation results appear. Operating point simulation results Note to the reader This document is incomplete. Here are some topics the author has left, to later get started on expanding this document. Opening and closing inserted text Handling models MOSFET pins How is the layout impacted by this? Producing a schematic for sources so that spice simulations are possible with a design that will also have a corresponding layout. Version and Copyright Notice: While this document is written for students at the University of Hartford, located in Connecticut, USA, anyone can make copies, but only of this document as-is, for educational use, with this copyright notice attached. Author: Jonathan Hill ( jmhill at hartford dot edu ) Date: Sat Dec 18 22:12:18 EST 2010 Modified: Sat Dec 18 22:12:18 EST 2010