Circuit Design on Your Linux Box Using gEDA
A good way to understand how gEDA is used is to examine its individual pieces in the context of the overall design flow. The first design step involves schematic capture—that is, using a specialized drawing program to draw a schematic representation of your circuit. The gEDA Suite's schematic capture program is called gschem.
gschem is usually invoked from the command line; once started, it opens up a GUI composed of a drawing window surrounded by all the menus and buttons necessary to draw a schematic. gschem, like any schematic capture program, has a number of built-in graphical primitives corresponding to wires, component pins, resistors, capacitors, transistors and other items you need to connect when creating a circuit design. A screenshot of a typical session with gschem is shown in Figure 1.
As for electronic devices, gschem maintains a library of component symbols, which are drawings of individual circuit elements such as resistors, ICs, connectors and anything else you might want to place on your schematic. Each symbol is stored as an ASCII file; when you place a component symbol into your schematic, the corresponding symbol file is opened up and the information contained in it is used to draw the symbol on your screen.
Currently, gschem's symbol library holds more than 2,000 component symbols, including symbols for most common electronic parts. However, engineers commonly need to create new symbols for their designs, because it is likely that not all the parts they want to use are present in the symbol library. Therefore, gschem—like all schematic capture programs—incorporates a symbol editor, which allows users to create and save their own symbols, which they can then use in any design.
gschem understands electrical connectivity, an important property for any schematic capture program. That is, wires (called nets in EDA parlance) know that they can connect only to component pins and other nets. When two nets are connected together, gschem knows to draw a large dot at the connection point, indicating to the user that a connection exists at that point.
gschem enables engineers to attach attributes to each component, which is an important part of creating a design. For example, if you have a 499-ohm resistor in your schematic, gschem lets you place a resistor symbol from the library, double-click on the resistor and then attach a value=499 to the resistor itself. Later, when the design is netlisted, the component's attributes are written into the netlist file and made available for other programs.
Finally, gschem saves your design in a well-documented ASCII format. There are many advantages to ASCII file formats; readers of Linux Journal will appreciate that ASCII files can be parsed and manipulated using scripting languages, including Perl and Python. Scripts facilitate labor-saving design tasks like automated symbol generation and schematic merging. Many proprietary EDA programs do not use ASCII file formats because they are interested in locking in customers. Open-source EDA advocates believe that open file formats are a key superiority of toolsets like gEDA.
After you have captured your schematic, the next step in the design flow is to create a netlist. gnetlist is the gEDA/gaf program used to generate netlists from your schematic files. gnetlist is a command-line utility; when you run it, it generates output netlist files and also displays diagnostic information in your terminal window.
So what's a netlist? A netlist is a file holding your design's connectivity information in a structured format suitable for machine processing. Many different types of netlist exist; each represents a file format optimized for a particular type of subsequent processing. For example, SPICE analog simulators read files written in the SPICE netlist format, which calls out connections between analog components, as well as specifies the values of each component's parameters, such as a resistor's resistance. As another example, netlists used as the input to lay out programs typically hold information about each component's PCB footprint, which is the metalization pattern on the circuit board to which the component is soldered, as well as connectivity information between all component pins.
gnetlist is designed in a unique way. It incorporates a front end written in C that reads and parses your schematic files. Once the read-in is complete, gnetlist invokes a back-end netlist generator written in Scheme. The back end is specific to the desired output netlist. The back end to use is specified via a command-line flag when you invoke gnetlist. gnetlist was designed this way to facilitate easy extensibility. Users who want to create new netlisters simply need to write a Scheme program implementing their desired netlister; they don't need to learn C or fool around with the internals of reading or parsing schematic files.
At the time of this writing, gnetlist can output more than 20 netlist formats. Among the important netlist types output by gnetlist is SPICE. The powerful gEDA SPICE netlister spice-sdb supports the inclusion of vendor SPICE models into your spice netlist. It has proven very popular with EE students worldwide, perhaps because it is well documented in a HOWTO available on the Web. Also, netlisters for several different layout tools exist. Finally, gnetlist is also used for BOM (bill of materials) generation and DRC (design rule checking) using any of several back ends crafted to achieve these goals.
Important to PCB design is the question of how to translate a gschem schematic into a format suitable for layout using the open-source layout program pcb. Although this can be done using gnetlist alone, the procedure is complicated. Therefore, Bill Wilson made a recent contribution to the gEDA Project by writing gsch2pcb, a C utility that wraps gnetlist and outputs the correct files to read into pcb for layout. gsch2pcb is a key addition to the gEDA Suite because it makes the transition from a gschem schematic to a pcb layout easy, and it also illustrates the vibrancy of the gEDA on-line community.
|Designing Electronics with Linux||May 22, 2013|
|Dynamic DNS—an Object Lesson in Problem Solving||May 21, 2013|
|Using Salt Stack and Vagrant for Drupal Development||May 20, 2013|
|Making Linux and Android Get Along (It's Not as Hard as It Sounds)||May 16, 2013|
|Drupal Is a Framework: Why Everyone Needs to Understand This||May 15, 2013|
|Home, My Backup Data Center||May 13, 2013|
- Designing Electronics with Linux
- Making Linux and Android Get Along (It's Not as Hard as It Sounds)
- Dynamic DNS—an Object Lesson in Problem Solving
- Using Salt Stack and Vagrant for Drupal Development
- New Products
- Build a Skype Server for Your Home Phone System
- Validate an E-Mail Address with PHP, the Right Way
- A Topic for Discussion - Open Source Feature-Richness?
- Why Python?
- Tech Tip: Really Simple HTTP Server with Python
1 hour 14 min ago
- Reply to comment | Linux Journal
1 hour 22 min ago
- Understanding the Linux Kernel
3 hours 37 min ago
6 hours 7 min ago
- Kernel Problem
16 hours 9 min ago
- BASH script to log IPs on public web server
20 hours 36 min ago
1 day 12 min ago
- Reply to comment | Linux Journal
1 day 44 min ago
- All the articles you talked
1 day 3 hours ago
- All the articles you talked
1 day 3 hours ago
Enter to Win an Adafruit Pi Cobbler Breakout Kit for Raspberry Pi
It's Raspberry Pi month at Linux Journal. Each week in May, Adafruit will be giving away a Pi-related prize to a lucky, randomly drawn LJ reader. Winners will be announced weekly.
Fill out the fields below to enter to win this week's prize-- a Pi Cobbler Breakout Kit for Raspberry Pi.
Congratulations to our winners so far:
- 5-8-13, Pi Starter Pack: Jack Davis
- 5-15-13, Pi Model B 512MB RAM: Patrick Dunn
- 5-21-13, Prototyping Pi Plate Kit: Philip Kirby
- Next winner announced on 5-27-13!
Free Webinar: Hadoop
How to Build an Optimal Hadoop Cluster to Store and Maintain Unlimited Amounts of Data Using Microservers
Realizing the promise of Apache® Hadoop® requires the effective deployment of compute, memory, storage and networking to achieve optimal results. With its flexibility and multitude of options, it is easy to over or under provision the server infrastructure, resulting in poor performance and high TCO. Join us for an in depth, technical discussion with industry experts from leading Hadoop and server companies who will provide insights into the key considerations for designing and deploying an optimal Hadoop cluster.
Some of key questions to be discussed are:
- What is the “typical” Hadoop cluster and what should be installed on the different machine types?
- Why should you consider the typical workload patterns when making your hardware decisions?
- Are all microservers created equal for Hadoop deployments?
- How do I plan for expansion if I require more compute, memory, storage or networking?