IEG3810 Microprocessor System Design Laboratory
2008-8-1
Experiment 1 Schematic Drawing and PCB Design
Objective
To study the use of EDA tool for electronic circuit design. To study the use of EDA tool for PCB layout.
Equipment and Software Applications
Personal computer with OrCad Version 9.0 or higher installed.
References
OrCad Capture Users Guide; OrCad Layout Plus Users Guide; OrCad Layout Autorouter User's Guide; OrCad Layout SmartRoute User's Guide.
Page 1
IEG3810 Microprocessor System Design Laboratory
Introduction
Electronic Design Automation is one of the most important applications in the field of computer science. Traditionally, electronic circuit design begins with the drawing of the circuit diagram. According to the circuit diagram, a prototype is built. Subsequently, a lot of testing and modifications will be followed in order to optimize the design. This kind of works is time consuming and requires a lot of manpower. Nowadays, electronic engineers can go through the design stage with a computer and the help of the EDA tools. Graphical interface tools and hardware description languages are available for design entry. Simulation tools such as SPICE (for analog design) & VHDL or Verilog (for digital design), shorten the time for testing and modification of the prototype. That means EDA tools can help to shorten the time to market. In this experiment, the OrCAD Capture and Layout tools are used. It is recommended that you study the manuals and learning lessons for OrCad Capture and Layout before the beginning of your experiment. Both manuals and learning lessons are available online. A demonstration session is also available before the laboratory sessions.
Procedure
A. Schematic Entry
A1. Log-on a PC in the laboratory with OrCad version 9.0 or higher installed. After logging on and entering the Windows environment, select Start > Program > OrCAD Release 9 > Capture. A2. From the OrCAD Capture environment, select New-Project from the File menu then enter the name for your project and select Schematic for your project. You may assign a location to store the whole project. Click OK to open a new schematic sheet. Based on the circuit diagram shown in Fig.1-1, sketch a circuit diagram of a 8088 microcomputer system in minimum mode with the 8088 MPU, clock generator, demultiplexer, address decoder, EPROM and the necessary components. Most of the symbols of the chips and components can be found from the installed library files including Microprocessor.olb Misc.olb Busdrivertransceiver.olb Prom.olb Pld.olb Discrete.olb Connector.olb Use the Place>Part from the menu bar to check them out and place on the suitable location of the sheet. You may use the part search function in the part place window to find the component in the installed library A3. In case you cannot find the symbol of the component to be used, you can use the New>Library from the File menu to create one. Save the newly created symbol to the user.lib in your home directory for future use.
Page 2
IEG3810 Microprocessor System Design Laboratory
A4. After placing all components, use the wire, bus and bus entry to connect the components on the sheet. Symbols for power (DC source) and GND (power ground) can also be found in the Part tool bar. Use the net alias to assign name of the wires or buses. A5. When you finish editing the circuit diagram, select Tools > Design Rule Check... to check the connections of the components in the sheet and fix the errors according to the DRC report output. In order to generate a netlist for PCB layout, each component on the sheet must have its PCB footprint attribute. You may assign the footprint to each component by double click on the component to open the property editor window of the component. Fill the suitable footprint name into the space for the footprint attribute. The following footprints are recommended. Component 8088 8284 20V8 74LS245 74LS373 27256 20-pin connector 8x1 resistor pack Resistor Capacitor Recommended footprint DIP.100/40/W.600/L2.100 DIP.100/18/W.300/L.900 DIP.100/24/W.300/L1.200 DIP.100/20/W.300/L1.000 DIP.100/20/W.300/L1.000 DIP.100/28/W.600/L1.400 WALCON.100/VH/TM2OES/W.325/20 SIP/TM/L.900/9 RAD/.100X.050/LS.100/.031 RAD/.100X.050/LS.100/.031
You may find other footprints from the installed libraries in the Library Manager of the OrCAD Layout tool. Fill in the data you decided to the title box at the lower right corner of the sheet. Also assign a text box with your and your partners name as well as the group number above the title box. A6. If the schematic page is accepted, save your design to the decided location. From the Design window, select Tools>Create Netlist for Layout (select the Layout tab) to generate a netlist of your design for the PCB layout tool. Submit one copy of the schematic design as your experiment result. Since the schematic diagram will be used in the other experiments, you are recommended to make an extra copy and keep it safely.
B. PCB Layout
B1. From the Windows environment, select Start > Program > OrCAD Release 9 to invoke the Layout Plus tool. B2. Once the Layout (or Layout Plus) window has been opened, select New from the file menu to use the default technology file for a new PCB and you have to give the name for the netlist file created from part A and the name of the PCB output file. Then the netlist of your design will be read in and the footprint of the components will be shown in the Layout window. If no footprint name is found from the installed footprint libraries, you will be asked to assign one from the existing footprints to the component.
Page3
IEG3810 Microprocessor System Design Laboratory
B3. From the tool bar, select View Spreadsheet>Layers to open the layers spreadsheet. Use only the top and bottom layer type for routing and set the others for unused. At the layer field, select the Global Layer. From the tool bar, select the Obstacle tool to draw a rectangle outline of the PCB with size 5000 mil by 6000 mil for a double sided PCB. Select the Obstacle tool and double click the left mouse button on the Layout window to invoke the Obstacle property window, you may select Route Keep-out or Via Keep-out to define specific areas for routing track inside the rectangle of the board outline. B4. Select and place the footprint of the components to the decided location of the PCB. B5. Use the default setup of the net rules and routing rules. Select the AutorouteBroad from the Auto menu to start the autorouter. B6. After the autorouter finishes its routing process, print the traces and vias of the routed top and bottom layer and save the completed PCB layout. Submit the Schematic diagram and the PCB output for grading.
Page 4
IEG3810 Microprocessor System Design Laboratory
Page5
