| blob | 95ef68be2134accf7b533b23f0cddac4062249d3 |
3 <html>
4 <head>
5 <title></title>
11 </head>
12 <body>
15 <h1 class="sectionedit1010"><a name="geda_gschem_user_guide" id="geda_gschem_user_guide">gEDA gschem User Guide</a></h1>
18 <p>
20 </p>
22 <p>
23 The latest version of this document may be found at: <a href="http://geda.seul.org/wiki/geda:gschem_ug" class="urlextern" title="http://geda.seul.org/wiki/geda:gschem_ug" rel="nofollow">http://geda.seul.org/wiki/geda:gschem_ug</a>
24 </p>
26 <p>
27 This document is released under the <a href="geda-gfdl.html" class="wikilink1" title="geda-gfdl.html">GNU Free Documentation License (GFDL)</a>.
28 </p>
30 <p>
32 Please report any errors/inconsistencies in this document by commenting in the Discussion area at the bottom of the associated page.
33 </p>
35 </div>
36 <!-- EDIT1010 SECTION "gEDA gschem User Guide" [1-397] -->
37 <h1 class="sectionedit1011"><a name="about_this_document" id="about_this_document">About this document ...</a></h1>
40 <p>
41 gEDA gschem Users Guide
42 </p>
44 <p>
46 </p>
48 <p>
49 Copyright © 1993, 1994, 1995, 1996, Nikos Drakos, Computer Based Learning Unit, University of Leeds.
51 </p>
53 <p>
54 The command line arguments were:
55 latex2html -local_icons gschem
56 </p>
58 <p>
60 </p>
62 </div>
63 <!-- EDIT1011 SECTION "About this document ..." [398-873] -->
67 <p>
68 This document describes the installation, configuration, and operation of the <strong>gschem</strong> application.<br/>
70 This document does not describe the process of generating schematics. For this, refer to the various tutorials on using the gEDA Tool Suite:
71 </p>
72 <ul>
73 <li class="level1"><div class="li"> <a href="geda-gschem_warmup.html" class="wikilink1" title="geda-gschem_warmup.html">Bill Wilson's gschem warmup</a></div>
74 </li>
75 <li class="level1"><div class="li"> <a href="geda-gsch2pcb_tutorial.html" class="wikilink1" title="geda-gsch2pcb_tutorial.html">Bill Wilson's gsch2pcb tutorial</a></div>
76 </li>
77 <li class="level1"><div class="li"> “Optical Proximity Sensor for Robots (Part 1), Simple PCB Design with the gEDA Suite”, by Stuart Brorson (March 2006 Circuit Cellar article)</div>
78 </li>
79 <li class="level1"><div class="li"> <a href="http://www-mdp.eng.cam.ac.uk/urop05/files/gedalib/starting_gEDA.pdf" class="urlextern" title="http://www-mdp.eng.cam.ac.uk/urop05/files/gedalib/starting_gEDA.pdf" rel="nofollow">Starting with gEDA at the Cambridge University Engineering Department</a></div>
80 </li>
81 <li class="level1"><div class="li"> <a href="http://www.brorson.com/gEDA/SPICE/t1.html" class="urlextern" title="http://www.brorson.com/gEDA/SPICE/t1.html" rel="nofollow">"Circuit simulation using gEDA and SPICE -- HOWTO" by Stuart Brorson</a></div>
82 </li>
83 <li class="level1"><div class="li"> <a href="http://www.circuitcellar.com/magazine/176toc.htm" class="urlextern" title="http://www.circuitcellar.com/magazine/176toc.htm" rel="nofollow">"gEDA Design Suite for Linux" by Stuart Brorson, Ales Hvezda, & Dan McMahill (03 Mar 2005 Circuit Cellar article)</a></div>
84 </li>
85 <li class="level1"><div class="li"> <a href="http://www.linuxjournal.com/article/8438" class="urlextern" title="http://www.linuxjournal.com/article/8438" rel="nofollow">"Circuit Design on Your Linux Box Using gEDA" by Stuart Brorson (29 November 2005 Linux Journal article)</a></div>
86 </li>
87 <li class="level1"><div class="li"> Optical Proximity Sensor for Robots (Part 1): Simple PCB Design with the gEDA Suite, by Stuart Brorson, Circuit Cellar magazine, March 2006 (Issue 188), p. 48</div>
88 </li>
89 <li class="level1"><div class="li"> And, of course, <a href="http://www.google.com/search?hl=en&lr=&q=gEDA+%22schematic+capture%22+tutorial&btnG=Search" class="urlextern" title="http://www.google.com/search?hl=en&lr=&q=gEDA+%22schematic+capture%22+tutorial&btnG=Search" rel="nofollow">Google is your friend</a>.</div>
90 </li>
91 </ul>
93 <p>
95 This document assumes you understand basic schematic capture concepts. For example: that a component represents something and that nets and buses interconnect these components to form a schematic, etc… For a basic understanding of the various work-flows available in the gEDA Tool Suite, please read the above tutorials. For more detailed understanding of specific tool issues, please refer to <a href="geda-gschem_ug.html#how_to_ask_questions" class="wikilink1" title="geda-gschem_ug.html">How To Ask Questions</a> and to the <a href="geda-gschem_ug.html#resources" class="wikilink1" title="geda-gschem_ug.html">Resources</a>.
96 </p>
98 </div>
99 <!-- EDIT1012 SECTION "Introduction" [874-2809] -->
103 <p>
104 <strong>gschem</strong> is the schematic capture program in the gEDA Tool Suite. Its purpose is to facilitate the graphical input of:
105 </p>
106 <ul>
108 </li>
110 </li>
112 </li>
113 </ul>
115 <p>
117 Once <strong>gschem</strong> has been used to enter the symbols/schematics for your design, several gEDA Tool Suite “utility” programs are used to extract information for other purposes:
118 </p>
119 <ul>
120 <li class="level1"><div class="li"> <strong>gattrib</strong> – <strong>gattrib</strong> is a gEDA Tool Suite productivity aid. <strong>gattrib</strong> reads a [hierarchical set of] gschem schematic files and creates a spreadsheet showing all components in rows, with the associated component attributes listed in the columns. It allows the user to add, modify, or delete component attributes outside of <strong>gschem</strong>, and then save the .sch files.</div>
121 </li>
122 <li class="level1"><div class="li"> <strong>gnetlist</strong> – A tool that converts a [hierarchical set of] schematic files into an equivalent netlist (a textual representation of a schematic) in various formats. Various gnetlist back-ends are used to create:</div>
123 <ul>
125 </li>
127 </li>
128 <li class="level2"><div class="li"> Netlist files for use as input to various printed circuit board layout programs (e.g., Allegro, PADS, <strong>pcb</strong> (part of the gEDA Tool Suite), Protell, Tango, RACAL-REDAC, etc.).</div>
129 </li>
131 </li>
133 </li>
135 </li>
137 </li>
138 </ul>
139 </li>
140 <li class="level1"><div class="li"> <strong>grenum</strong> – <strong>grenum</strong> is a gEDA Tool Suite productivity aid that will renumber the reference designators (i.e., refdes) in a [hierarchical set of] schematic files.</div>
141 </li>
142 <li class="level1"><div class="li"> <strong>gsch2pcb</strong> – The prefered method to create a netlist for the <strong>pcb</strong> printed circuit board layout tool (part of the gEDA Tool Suite).</div>
143 </li>
144 <li class="level1"><div class="li"> <strong>gspiceui</strong> – GNU Spice <acronym title="Graphical User Interface">GUI</acronym> (i.e., <strong>gspiceui</strong>) provides a <acronym title="Graphical User Interface">GUI</acronym> for freely available Spice electronic cicuit simulation engines (e.g., <strong>gnucap</strong> and <strong>ngspice</strong>). It uses <strong>gnetlist</strong> (to convert schematic files to net list files) and <strong>gwave</strong> (to display simulation results). gSchem is the preferred schematic capture tool.</div>
145 </li>
146 <li class="level1"><div class="li"> <strong>gsymcheck</strong> – A checker for symbols created with gEDA Tool Suite (e.g., <strong>gschem</strong>, <strong>tragesym</strong>, etc.).</div>
147 </li>
148 <li class="level1"><div class="li"> <strong>pcb</strong> – A tool for the layout of printed circuit boards.</div>
149 </li>
150 <li class="level1"><div class="li"> <strong>refdes_renum</strong> – Reads a [hierarchical set of] <strong>gschem</strong> schematic files and renumbers all reference designators. The reference designators are numbered starting with 1 and the old schematic file is replaced by the modified schematic file.</div>
151 </li>
152 <li class="level1"><div class="li"> <strong>tragesym</strong> – A python script that creates geda symbols from structured textfiles. The symbols usually need to be “cleaned up” in gschem.</div>
153 </li>
154 </ul>
157 <td class="col0"> <a href="media/geda/gschem_workflow_01.jpg" class="media" target="_blank" title="geda:gschem_workflow_01.jpg"><img src="media/geda/gschem_workflow_01.jpg" class="media" alt="" /></a> </td>
158 </tr>
159 </table></div>
160 <!-- EDIT1014 TABLE [5353-5389] -->
161 </div>
162 <!-- EDIT1013 SECTION "Overview" [2810-5392] -->
166 <p>
168 </p>
169 <ul>
170 <li class="level1"><div class="li"> <a href="geda-gschem_warmup.html" class="wikilink1" title="geda-gschem_warmup.html">Bill Wilson's gschem warmup tutorial</a> – If you are new to the gEDA tools, read this before you read Bill's “Bill Wilson's gsch2pcb tutorial”.</div>
171 </li>
172 <li class="level1"><div class="li"> <a href="geda-gsch2pcb_tutorial.html" class="wikilink1" title="geda-gsch2pcb_tutorial.html">Bill Wilson's gsch2pcb tutorial</a> – If you are new to the gEDA tools, this tutorial will bring you up to speed quickly.</div>
173 </li>
174 <li class="level1"><div class="li"> <a href="http://www.circuitcellar.com/" class="urlextern" title="http://www.circuitcellar.com/" rel="nofollow">Circuit Cellar Magazine</a> – Practical, hands-on applications and solutions for embedded designers:</div>
175 <ul>
176 <li class="level2"><div class="li"> gEDA Design Suite for Linux, by Stuart Brorson, Ales Hvezda, & Dan McMahill, Circuit Cellar magazine, March 2005 (Issue 176), p. 12</div>
177 </li>
178 <li class="level2"><div class="li"> Optical Proximity Sensor for Robots (Part 1): Simple PCB Design with the gEDA Suite, by Stuart Brorson, Circuit Cellar magazine, March 2006 (Issue 188), p. 48</div>
179 </li>
180 <li class="level2"><div class="li"> Optical Proximity Sensor for Robots (Part 2): Open-Source PCB Layout Editor, by Stuart Borson, Circuit Cellar magazine, April 2006 (Issue 189), p. 40</div>
181 </li>
182 </ul>
183 </li>
184 <li class="level1"><div class="li"> <a href="http://www.gpleda.org/index.html" class="urlextern" title="http://www.gpleda.org/index.html" rel="nofollow">gEDA Project home page</a> – The homepage for the gEDA Tools Suite. </div>
185 </li>
186 <li class="level1"><div class="li"> <a href="https://bugs.launchpad.net/geda" class="urlextern" title="https://bugs.launchpad.net/geda" rel="nofollow">gEDA Bug Tracker</a> – On Launchpad</div>
187 </li>
188 <li class="level1"><div class="li"> <a href="http://geda.seul.org/wiki" class="urlextern" title="http://geda.seul.org/wiki" rel="nofollow">gEDA Project's Wiki</a> – All things related to the gEDA Tools Suite.</div>
189 </li>
190 <li class="level1"><div class="li"> <a href="http://www.gedasymbols.org" class="urlextern" title="http://www.gedasymbols.org" rel="nofollow">gedasymbols.org</a> – On-line repository of user-developed symbols for <strong>gschem</strong>, SPICE models, and footprints for <strong>pcb</strong>.</div>
191 </li>
192 <li class="level1"><div class="li"> John C. Luciani's proposed <a href="http://www.luciani.org/geda/pcb/footprint-name-spec.pdf" class="urlextern" title="http://www.luciani.org/geda/pcb/footprint-name-spec.pdf" rel="nofollow">Land Pattern Naming Convention</a> – Footprint naming conventions document, used by him, and often used by those submitting to the <a href="http://www.gedasymbols.org" class="urlextern" title="http://www.gedasymbols.org" rel="nofollow">gedasymbols.org</a> symbols/footprint repository.</div>
193 </li>
194 <li class="level1"><div class="li"> John C. Luciani's <a href="file:///shared/HomePages/dhart/index.html" class="urlextern" title="file:///shared/HomePages/dhart/index.html" rel="nofollow">PCB Footprints Library</a> – A rather inclusive collection of non-<acronym title="GNU General Public License">GPL</acronym> licensed footprints and the scripts used to create them.</div>
195 </li>
196 <li class="level1"><div class="li"> <a href="http://www.opencollector.org/" class="urlextern" title="http://www.opencollector.org/" rel="nofollow">OpenCollector</a> carries listings and news for free EDA software and circuit designs. Open Collector supports gEDA.</div>
197 </li>
198 <li class="level1"><div class="li"> <a href="http://alternatezone.com/electronics/files/PCBDesignTutorialRevA.pdf" class="urlextern" title="http://alternatezone.com/electronics/files/PCBDesignTutorialRevA.pdf" rel="nofollow">PCB Design Tutorial; RevA</a> – Document describing the process of taking a schematic to a pcb. Excellent for the beginner.</div>
199 </li>
200 <li class="level1"><div class="li"> <a href="http://pcblibraries.com/" class="urlextern" title="http://pcblibraries.com/" rel="nofollow">PCB Libraries website</a> – Advocates of the IPC standard Land Pattern (a.k.a., footprint) Naming Conventions and Land Pattern Calculators. A useful site if you have the money to subscribe to the services.</div>
201 <ul>
202 <li class="level2"><div class="li"> The free (windows-based) <a href="http://landpatterns.ipc.org/default.asp" class="urlextern" title="http://landpatterns.ipc.org/default.asp" rel="nofollow">IPC-7351 Land Pattern Viewer</a> is a very useful tool for viewing the latest IPC footprints.</div>
203 </li>
204 <li class="level2"><div class="li"> <a href="http://www.pcblibraries.com/resources/LibDoc.asp" class="urlextern" title="http://www.pcblibraries.com/resources/LibDoc.asp" rel="nofollow">CAD Data Files to be used with PCB Libraries' IPC-7351A LP Programs</a> – please note the license restrictions.</div>
205 </li>
206 </ul>
207 </li>
208 <li class="level1"><div class="li"> <a href="http://www-mdp.eng.cam.ac.uk/urop05/files/gedalib/starting_gEDA.pdf" class="urlextern" title="http://www-mdp.eng.cam.ac.uk/urop05/files/gedalib/starting_gEDA.pdf" rel="nofollow">Starting with gEDA at the Cambridge University Engineering Department</a> – The Cambridge University Engineering Department's tutorial for using gEDA.</div>
209 </li>
210 <li class="level1"><div class="li"> <a href="http://www.brorson.com/gEDA/" class="urlextern" title="http://www.brorson.com/gEDA/" rel="nofollow">Stuart Brorson's gEDA tools and tips</a> – gEDA related tools and information.</div>
211 </li>
212 </ul>
214 </div>
215 <!-- EDIT1015 SECTION "Resources" [5393-8589] -->
216 <h1 class="sectionedit1016"><a name="how_to_ask_questions" id="how_to_ask_questions">How To Ask Questions</a></h1>
219 <p>
220 <strong>gschem</strong> is an OpenSource, community driven, development. As such, the emphasis has been on developing the gEDA Tools Suite, not on developing commercial-level documentation and support. Much of the burden on learning how to use the gEDA Tools Suite applications is placed on the user, who must understand the basics of electronics, Electronics Design Automation (EDA), and the terminology used in schematic capture, circuit simulation, and printed circuit board design.<br/>
222 As a typical OpenSource development, the gEDA Tools Suite development community provides timely and insightful response to user inquiries, but please perform the following steps before bothering the developers (they need to focus on making gEDA Tools Suite applications better, and you can actually learn to answer your own questions and become independent of the developers):
223 </p>
224 <ol>
225 <li class="level1"><div class="li"> Read Rick Moen's <a href="http://www.catb.org/~esr/faqs/smart-questions.html" class="urlextern" title="http://www.catb.org/~esr/faqs/smart-questions.html" rel="nofollow">How To Ask Questions The Smart Way</a>, about how to ask for help. This is a must read for everybody.</div>
226 </li>
227 <li class="level1"><div class="li"> Read this document. I know, it's a lot to expect engineers to actually read a user's guide. The latest version of this document is maintained on the gEDA web-site at <a href="http://geda.seul.org/wiki/geda:gschem_ug" class="urlextern" title="http://geda.seul.org/wiki/geda:gschem_ug" rel="nofollow">gschem User Guide</a>. The information should be here. If it isn't, comment to the fact in one of the on-line document's “Discussion” areas (at the bottom of each wiki-page). Helpful comments are clear, to the point, and may even contain the wording that should be inserted into the document.</div>
228 </li>
229 <li class="level1"><div class="li"> Read the <a href="geda-faq-gschem.html" class="wikilink1" title="geda-faq-gschem.html">gschem Frequently Asked Questions (FAQ)</a> wiki-page. This on-line document is updated often to reflect user and developer experiences with <strong>gschem</strong>.</div>
230 </li>
231 <li class="level1"><div class="li"> Read the <a href="geda-documentation.html" class="wikilink1" title="geda-documentation.html">gEDA/gaf Documentation</a>. This information was installed on your computer if the gEDA Tools Suite was installed from the gEDA Binary Suite installer.</div>
232 </li>
233 <li class="level1"><div class="li"> <a href="http://www.google.com" class="urlextern" title="http://www.google.com" rel="nofollow">Google</a> is your friend. People that have asked questions that obviously didn’t do any simple Google search will not be treated well when asking for help. This is particularly true if your problem is not unique to the gEDA Tools Suite applications.</div>
234 </li>
235 <li class="level1"><div class="li"> Ask for a pointer to the right direction. It is considered good “net etiquette” to ask for a pointer to information, so that you can learn where such information can be found, rather than have someone search the information for you.</div>
236 </li>
237 <li class="level1"><div class="li"> If you are software literate, look at the source code to see what it is doing.</div>
238 </li>
239 <li class="level1"><div class="li"> Subscribe to the gEDA e-mail lists (i.e., you can only post to the e-mail lists if you are a subscriber). Then:</div>
240 <ol>
241 <li class="level2"><div class="li"> Start reading recent messages in the <a href="http://archives.seul.org/geda/user/" class="urlextern" title="http://archives.seul.org/geda/user/" rel="nofollow">geda-user e-mail list archives</a>. Get a feel for the list's ettiquite so that you learn how to properly ask questions.</div>
242 </li>
243 <li class="level2"><div class="li"> Search the archives for issues similar to yours. You may find the question has been asked of the developers and users before, and answered.</div>
244 </li>
245 <li class="level2"><div class="li"> In the event that you can find no information concerning your problem, submit a concise description of the problem and a request for the type of help you are requesting.</div>
246 </li>
247 </ol>
248 </li>
249 </ol>
251 </div>
252 <!-- EDIT1016 SECTION "How To Ask Questions" [8590-11759] -->
253 <h1 class="sectionedit1017"><a name="installing_gschem" id="installing_gschem">Installing gschem</a></h1>
256 <p>
257 As a mature OpenSource project, the gEDA Tools Suite and its components have been installed on many Linux distributions. The following are by no means the only methods of installing the gEDA Tools Suite and/or its components.
258 </p>
260 </div>
261 <!-- EDIT1017 SECTION "Installing gschem" [11760-12018] -->
265 <p>
266 <strong>gschem</strong> is a component of the gEDA/gaf set of tools which tend to integrate together in the development and maintenance of schematics and symbols. The term “gaf” stands for “<em class="u">g</em>EDA <em class="u">a</em>nd <em class="u">f</em>riends”).
267 The gEDA/gaf applications are actually rather stable, and receive significant testing prior to release.<br/>
269 There are multiple methods of installing <strong>gschem</strong>. The appropriate method depends on your distribution. See the following for some examples.
270 </p>
272 </div>
273 <!-- EDIT1018 SECTION "Latest Stable" [12019-12505] -->
274 <h3 class="sectionedit1019"><a name="geda_binary_suite" id="geda_binary_suite">gEDA Binary Suite</a></h3>
277 <p>
278 If you do not have gEDA packages available for your GNU/Linux distribution, you can install most of the tools using the gEDA Binary Suite Installer.
279 </p>
281 <p>
282 The latest version of this binary suite is available as a tarball from the <a href="http://www.gpleda.org/download.html" class="urlextern" title="http://www.gpleda.org/download.html" rel="nofollow">gEDA Downloads</a> web-page.
283 </p>
285 <p>
286 Please read the <a href="http://geda.seul.org/dist/suite/v0.0.2/README" class="urlextern" title="http://geda.seul.org/dist/suite/v0.0.2/README" rel="nofollow">README</a> for more information on how to install the gEDA Binary Suite.
287 </p>
289 </div>
290 <!-- EDIT1019 SECTION "gEDA Binary Suite" [12506-12961] -->
291 <h3 class="sectionedit1020"><a name="debian_based_distributions" id="debian_based_distributions">Debian based distributions</a></h3>
294 <p>
295 For Debian distributions, you may wish to download the <a href="http://www.geda.seul.org/download.html" class="urlextern" title="http://www.geda.seul.org/download.html" rel="nofollow">latest DEB binaries</a> prepared by Hamish Moffatt. These binary packages provide a hassle free way to install the core of geda.
296 </p>
298 </div>
299 <!-- EDIT1020 SECTION "Debian based distributions" [12962-13222] -->
300 <h3 class="sectionedit1021"><a name="fedora_and_redhat_distributions" id="fedora_and_redhat_distributions">Fedora and RedHat distributions</a></h3>
303 <p>
304 For RedHat distributions you may wish to download the <a href="http://www.sp5pbe.waw.pl/~sp5smk/software.html" class="urlextern" title="http://www.sp5pbe.waw.pl/~sp5smk/software.html" rel="nofollow"> RPM binaries</a> prepared by Wojciech Kazubski.
305 </p>
307 <p>
308 Since Fedora Core 5, major parts of gEDA are available from <a href="http://fedoraproject.org/" class="urlextern" title="http://fedoraproject.org/" rel="nofollow"> the Fedora Project</a>.
309 </p>
311 <p>
312 For more information, read the <a href="geda-fedora_rpm_installation.html" class="wikilink1" title="geda-fedora_rpm_installation.html"> Fedora RPM installation notes</a>.
313 </p>
315 </div>
316 <!-- EDIT1021 SECTION "Fedora and RedHat distributions" [13223-13628] -->
317 <h3 class="sectionedit1022"><a name="suse_and_opensuse_distributions" id="suse_and_opensuse_distributions">SuSE and OpenSuSE distributions</a></h3>
320 <p>
321 For SuSE and OpenSuSE distributions there are rpm packages for several gEDA related programms.
322 They've been prepared by Werner Hoch using the OpenSuSE Build Service.
323 </p>
325 <p>
326 You can install the rpm packages with YaST, yum or any other installation tool. The packages are located at <a href="ftp://ftp-1.gwdg.de/pub/opensuse/repositories/science/" class="urlextern" title="ftp://ftp-1.gwdg.de/pub/opensuse/repositories/science/" rel="nofollow">ftp://ftp-1.gwdg.de/pub/opensuse/repositories/science/</a>.
327 </p>
329 <p>
330 For more informations read the <a href="geda-suse_rpm_installation.html" class="wikilink1" title="geda-suse_rpm_installation.html"> SuSE rpm installation notes</a>.
331 </p>
333 </div>
334 <!-- EDIT1022 SECTION "SuSE and OpenSuSE distributions" [13629-14100] -->
335 <h3 class="sectionedit1023"><a name="mac_osx_distributions" id="mac_osx_distributions">Mac OSX distributions</a></h3>
338 <p>
339 For Mac OSX distributions you may wish to download the <a href="http://www.geda.seul.org/download.html" class="urlextern" title="http://www.geda.seul.org/download.html" rel="nofollow">latest Fink binaries</a> prepared by Charles Lepple.
340 </p>
342 </div>
343 <!-- EDIT1023 SECTION "Mac OSX distributions" [14101-14281] -->
344 <h2 class="sectionedit1024"><a name="developer_unstable_testing" id="developer_unstable_testing">Developer Unstable/Testing</a></h2>
347 <p>
348 For those already familiar with the gEDA/gaf applications, access to the development repository is available. This is the latest developer source-code version of the application.<br/>
350 Installation from development repository (git based) is appropriate for those:
351 </p>
352 <ul>
353 <li class="level1"><div class="li"> Seeking a solution to a specific problem that was submitted to the development team, to test the “fix” so that the developers can be informed that the “fix” works.</div>
354 </li>
355 <li class="level1"><div class="li"> With significant working knowledge of the “gEDA Suite” and industry expertise, wishing to test the latest version of the application(s) prior to the next release. This usually requires access to several existing designs known to work in the current stable release of the “gEDA Suite”, so that comparisons can be made and issues brought to the attention of the developer/user community (via the e-mail lists).</div>
356 </li>
357 </ul>
359 </div>
360 <!-- EDIT1024 SECTION "Developer Unstable/Testing" [14282-15167] -->
361 <h1 class="sectionedit1025"><a name="configuring_gschem" id="configuring_gschem">Configuring gschem</a></h1>
364 <p>
365 Assume that you have installed the gEDA Binary Suite (the most common installation method), and that you are ready to configure <strong>gschem</strong> to your personal likes. When installing, you were prompted for the path where the gEDA executables would be placed. The default was the <strong>/home/{login id}/geda-install</strong> directory, where {login id} is the username you logged into your account with, but you may have changed this to another directory on the computer. This directory is referred to below as the <strong>{binary-install-path}</strong> because this is where the gEDA binary executables are placed. If you forgot where the binaries were installed, simply issue the following command to find where <strong>gschem</strong> is installed (in this case the {binary-install-path} is <strong>/usr/local/gEDA-20060124</strong>):
368 /usr/local/gEDA-20060124/bin/gschem
369 %</font></pre>
370 </p>
372 <p>
373 The gEDA Tools Suite applications follow normal Unix/Linux conventions for placement of configuration files; there are usually system-wide, user-wide, and project-specific configuration settings. The system-wide settings are placed in a sub-directory of the {binary-install-path}. The user-wide settings are placed in the user's home directory, also known as the login directory (referred to in Unix/Linux parlance as the <strong>$HOME</strong> directory). The project-specific settings are placed in a project-specific directory.<br/>
375 </p>
377 <p>
380 <strong>gschem</strong> is highly configurable. All configuration is handled through the following resource files (written using the GNU Guile programming language, an interpreter for Scheme, a version of Lisp):
381 </p>
382 <ul>
383 <li class="level1"><div class="li"> <strong>system-gschemrc</strong>: The system-wide initialization file for <strong>gschem</strong>. Installed in the {binary-install-path}/share/gEDA/system-gschemrc file, it is required for <strong>gschem</strong> to run. Users should not modify this file, but should override the settings in this file by creating their own $HOME/.gEDA/gschemrc file and/or 'pwd'/gschemrc file and putting the new settings in those files. The {binary-install-path} directory is where your gEDA/gaf executables were installed, including <strong>gschem</strong>. Depends on your install method. Refer to <a href="docs-20060124-gschem_ug-installing_gschem.html" class="wikilink2" title="docs-20060124-gschem_ug-installing_gschem.html">Installing gschem</a> for more details.</div>
384 </li>
385 <li class="level1"><div class="li"> <strong>$HOME/.gEDA/gschemrc</strong>: The per-user initialization file for <strong>gschem</strong>. Created by the user under the user's home directory. Settings placed in this file will override settings in the system-gschemrc file. Users should put settings in this file they want to apply to all of their sessions, such as (to change the default black background color scheme to a light background color scheme):</div>
386 </li>
387 </ul>
389 <p>
392 (load (build-path geda-rc-path "gschem-colormap-lightbg")) ; light background</font></pre>
393 </p>
394 <ul>
395 <li class="level1"><div class="li"> <strong>'pwd'/gschemrc</strong>: The per-project initialization file for <strong>gschem</strong>. Created by the user in the user's project directory. Settings placed in this file will override settings in both the system-gschemrc file and the $HOME/.gEDA/gschemrc file. Users should put settings in this file they want to apply to this particular project, such as (to autonumber reference designators when components are placed on the schematic):</div>
396 </li>
397 </ul>
399 <p>
401 margin-left : 2em"><font size="+0">; Comment in this scheme code if you want automatic numbering when
402 ; placing new component and copying components
403 ;
405 (add-hook! add-component-hook auto-uref)</font></pre>
406 </p>
407 <ul>
408 <li class="level1"><div class="li"> <strong>system-gafrc</strong>: The system-wide initialization file for gEDA/gaf applications (includes <strong>gschem</strong>, <strong>gnetlist</strong>). Installed in the {binary-install-path}/share/gEDA/system-gafrc file, it is required for <strong>gschem</strong> to run. Users should not modify this file, but should override the settings in this file by creating their own $HOME/.gEDA/gafrc file and/or 'pwd'/gafrc file and putting the new settings in those files. The {binary-install-path} directory is where your gEDA/gaf executables were installed, including <strong>gschem</strong>. Depends on your install method. Refer to <a href="docs-20060124-gschem_ug-installing_gschem.html" class="wikilink2" title="docs-20060124-gschem_ug-installing_gschem.html">Installing gschem</a> for more details.</div>
409 </li>
410 <li class="level1"><div class="li"> <strong>$HOME/.gEDA/gafrc</strong>: The per-user initialization file for gEDA/gaf applications. Created by the user under the user's home directory. Settings placed in this file will override settings in the system-gafrc file. Users should put settings in this file they want to apply to all of their sessions. </div>
411 </li>
412 <li class="level1"><div class="li"> <strong>'pwd'/gafrc</strong>: The per-project initialization file for the gEDA/gaf applications. Created by the user in the user's project directory. Settings placed in this file will override settings in both the system-gafrc file and the $HOME/.gEDA/gafrc file. Users should put settings in this file they want to apply to this particular project. Settings such as the <strong>component-library</strong> or <strong>source-library</strong> keywords go into this file.</div>
413 </li>
414 <li class="level1"><div class="li"> <strong>gschem-gtkrc</strong>: Installed in the {binary-install-path}/share/gEDA/gschem-gtkrc file. Used to define the font for all gtk+ widgets in <strong>gschem</strong>.</div>
415 </li>
416 </ul>
418 <p>
420 A few comments about changing the files:
421 </p>
422 <ul>
423 <li class="level1"><div class="li"> Don't break any guile syntax rules. Doing so will cause the scheme interpreter (guile) to stop interpreting.</div>
424 </li>
425 <li class="level1"><div class="li"> To add a setting to the $HOME/.gEDA/gschemrc file (or to the 'pwd'/gschemrc file), copy the setting's text from the {binary-install-directory}/share/gEDA/system-gschemrc file to the $HOME/.gEDA/gschemrc file (or the 'pwd'/gschemrc file) and make the setting change there.</div>
426 </li>
427 <li class="level1"><div class="li"> To add a setting to the $HOME/.gEDA/gafrc file (or the 'pwd'/gafrc file), copy the relevant setting's text from the {binary-install-directory}/share/gEDA/system-gafrc file to the $HOME/.gEDA/gafrc file (or the 'pwd'/gafrc file) and make the setting change there.</div>
428 </li>
429 <li class="level1"><div class="li"> Keywords/defaults always override what came before, with the exception of cumulative keywords (like component-library).</div>
430 </li>
431 </ul>
433 </div>
434 <!-- EDIT1025 SECTION "Configuring gschem" [15168-20950] -->
438 <p>
439 The {binary-install-path}/share/gEDA/system-gschemrc file is well commented. Read this file for more details on the settings available.<br/>
441 Some of the settings appropriate for override (by placing in either the user's $HOME/gschemrc file or the project's 'pwd'/gschemrc file) are:
442 </p>
444 </div>
445 <!-- EDIT1026 SECTION "gschemrc" [20951-21252] -->
449 <p>
450 The {binary-install-path}/share/gEDA/system-gafrc file is well commented. Read this file for more details on the settings available.<br/>
452 Some of the settings appropriate for override (by placing in either the user's $HOME/gafrc file or the project's 'pwd'/gafrc file) are:
453 </p>
455 </div>
456 <!-- EDIT1027 SECTION "gafrc" [21253-21542] -->
457 <h1 class="sectionedit1028"><a name="running_gschem" id="running_gschem">Running gschem</a></h1>
460 </div>
461 <!-- EDIT1028 SECTION "Running gschem" [21543-21574] -->
462 <h2 class="sectionedit1029"><a name="confirming_gschem_is_installed" id="confirming_gschem_is_installed">Confirming gschem is installed</a></h2>
465 <p>
466 You should determine if <strong>gschem</strong> has been correctly installed on your Linux computer.<br/>
468 Log into your Linux account, and launch your favorite interactive shell. The different Linux distributions will usually offer more than one interactive shell such as xterm, gnome-term, konsole, etc.<br/>
470 You will see a shell prompt, which will depend on your Linux distribution and on your selection of interactive shell. It is common practice in Linux documentation to refer to the user's interactive login shell prompt as “<strong>%</strong>”, and to refer to the superuser's (i.e., user “root”) interactive login shell prompt as “<strong>#</strong>”.<br/>
472 At the shell prompt, enter the following commands to determine if <strong>gschem</strong> is installed:
473 </p>
475 <p>
478 <strong>/usr/local/gEDA-20060124/bin</strong>:/usr/kerberos/bin:/usr/local/bin:/bin:/usr/bin:/usr/X11R6/bin:/home/<strong>gEDA</strong>/bin
480 /usr/local/gEDA-20060124/bin/gschem
519 </p>
521 <p>
522 The <strong>echo $PATH</strong> command displays the user's current setting for the <strong>PATH</strong> environment variable. In the above example for a Fedora Core 4 installation, user <strong>gEDA</strong> executed the command and determined that the <strong>PATH</strong> included the /usr/local/gEDA-20060124/bin directory (this will differ depending on where you put the gEDA Tools Suite executables).
524 </p>
525 <ol>
526 <li class="level1"><div class="li"> Set your $PATH environment variable to {the directory where you installed the gEDA executables}</div>
527 </li>
528 <li class="level1"><div class="li"> Set your $LD_LIBRARY_PATH environment variable to {the directory in where you installed the gEDA libraries}</div>
529 </li>
530 </ol>
532 <p>
534 The <strong>which</strong> command displays the full path of a command's executable, searching for the command on the user's list of directories, as defined in the <strong>PATH</strong> environment variable. In this case, it will return the full path to the <strong>gschem</strong> executable if it is on the user's <strong>PATH</strong>. If this command does not return the full path to the <strong>gschem</strong> executable, make sure your <strong>PATH</strong> environment variable has been properly set.
535 </p>
537 <p>
538 The <strong>ldd</strong> command displays shared libraries required by a program. All of the requested libraries must be found for <strong>gschem</strong> to run. Don't be intimidated by the long list of libraries, this is common for mature Linux applications. If we had not received this output (or something very similar), we would have to check on our setting for the <strong>LD_LIBRARY_PATH</strong> environment variable.
539 </p>
541 <p>
545 Usage: gschem [OPTIONS] schematic_filename1 ... schematic_filenameN
546 -q Quiet mode
547 -v Verbose mode on
548 -r filename Rc filename
549 -s filename Script (guile) filename
550 -o filename Output filename (for printing)
551 -p Automatically place the window
552 -t Print stroke information
553 -h Help; this message</font></pre>
554 </p>
556 <p>
558 </p>
560 <p>
561 If these commands do not return the expected results, then most likely the gEDA tools are not installed properly. Please see the appropriate INSTALL docs (which came with the gEDA distribution) for more info on installing the gEDA tools. <br/>
563 </p>
565 </div>
566 <!-- EDIT1029 SECTION "Confirming gschem is installed" [21575-26982] -->
567 <h2 class="sectionedit1030"><a name="the_shell_prompt" id="the_shell_prompt">The Shell Prompt</a></h2>
571 <td class="col0"> <a href="media/geda/terminal_screenshot_001.jpg" class="media" target="_blank" title="geda:terminal_screenshot_001.jpg"><img src="media/geda/terminal_screenshot_001.jpg" class="media" alt="" /></a> </td>
572 </tr>
575 </tr>
576 </table></div>
577 <!-- EDIT1031 TABLE [27012-27084] -->
578 <p>
580 You launch <strong>gschem</strong> from your favorite shell prompt (in this case, gnome-terminal on Fedora Core 4).<br/>
582 There are several command-line switches:
583 </p>
584 <ul>
586 Turns on “quiet mode”. Output (i.e., stdout and stderr) is not generated to the shell. Useful if calling <strong>gschem</strong> from a script (e.g., bash, sh, csh, etc.) to perform batch operations such as printing a large number of schematics or symbols.</div>
587 </li>
590 </li>
591 <li class="level1"><div class="li"> <strong>-r filename</strong> – Process additional configuration settings from <strong>filename</strong><br/>
592 <strong>filename</strong> is a file containing settings of the form found in either system-gschemrc or system-gafrc<br/>
593 In addition to the following files, <strong>gschem</strong> will process <strong>filename</strong> for additional configuration settings:<br/>
594 * {binary-install-path}/share/gEDA/system-gschemrc<br/>
595 * $HOME/gschemrc<br/>
597 * {binary-install-path}/share/gEDA/system-gafrc<br/>
598 * $HOME/gafrc<br/>
600 </li>
601 <li class="level1"><div class="li"> <strong>-s filename</strong> – Process <strong>filename</strong> as a guile script<br/>
603 Refer to <a href="docs-20060124-gschem_ug-app_b.html" class="wikilink2" title="docs-20060124-gschem_ug-app_b.html">Appendix B -- Printing Schematics and Symbols</a> and <a href="docs-20060124-gschem_ug-app_c.html" class="wikilink2" title="docs-20060124-gschem_ug-app_c.html">Appendix C -- Writing guile Scripts</a> for more details.<br/>
604 For example, in your $HOME/geda-sources/gedagaf/{gEDA Tools Suite version}/scripts/ directory is the <strong>print.scm</strong> file, a template script file directing <strong>gschem</strong> to generate a PostScript file of a schematic appropriate for printing. This <strong>print.scm</strong> file works as is, but you may want to customize it for your own needs. To print the schematic_1.sch schematic to the schematic_1.ps PostScript file from within a bash script, you would enter: <code>gschem -q -p -o schematic_1.ps -s print.scm schematic_1.sch</code><br/>
605 Then, simply use your favorite printing solution to print the file, such as: <code>lp schematic_1.ps</code><br/>
606 to a PostScript printer.</div>
607 </li>
608 <li class="level1"><div class="li"> <strong>-o filename</strong> – Output <strong>filename</strong> (e.g., for printing)<br/>
609 Specify the output filename. For example, as used to specify the Postscript filename in the example above.</div>
610 </li>
613 When a new window is opened, some window managers display the bounding box of the window and wait for the user to place the window manually. The ”-p” option avoids that, letting the window manager decide where to put the new window.</div>
614 </li>
616 </div>
617 </li>
619 Generate a short usage printout.</div>
620 </li>
621 </ul>
623 <p>
625 Running <strong>gschem</strong> is straightforward once you have installed it on your GNU/Linux system.<br/>
627 Although <strong>gschem</strong> is a <acronym title="Graphical User Interface">GUI</acronym> application, <strong>gschem</strong> is meant to be launched from the command-line, as it takes command-line arguements (see Figure 1 above).<br/>
631 </p>
633 <p>
634 To open a specific schematic, run: <code><strong>% gschem schematic_name.sch</strong></code><br/>
636 </p>
638 <p>
639 To open a list of schematics, run: <code><strong>% gschem schematic_1.sch schematic_2.sch, schematic_3.sch …</strong></code><br/>
640 or use wildcards to specify multiple filenames: <code><strong>% gschem schematic_*.sch</strong></code>
641 </p>
643 <p>
644 As operations are performed in the <strong>gschem</strong> <a href="docs-20060124-gschem_ug-the_main_window.html" class="wikilink2" title="docs-20060124-gschem_ug-the_main_window.html">Main Window</a> the <strong>gschem</strong> <a href="docs-20060124-gschem_ug-the_status_window.html" class="wikilink2" title="docs-20060124-gschem_ug-the_status_window.html">Status Window</a> continues to output information, and the shell prompt's window continues to output information, consisting of:
645 </p>
646 <ul>
648 </li>
649 </ul>
651 </div>
652 <!-- EDIT1030 SECTION "The Shell Prompt" [26983-30517] -->
656 <p>
657 There are two basic mechanisms in <strong>gschem</strong> for backing up schematics and symbols, classic Linux backups and incremental backups.
658 </p>
660 </div>
661 <!-- EDIT1032 SECTION "Backups" [30518-30669] -->
662 <h3 class="sectionedit1033"><a name="classic_linux_backups" id="classic_linux_backups">Classic Linux backups</a></h3>
665 <p>
666 While creating and/or editing schematic file(s) or symbol file(s), snapshots are triggered by the <strong>autosave</strong> interval setting in the {binary-install-path}/share/gEDA/system-gschemrc file (see <a href="#relevant_configuration_settings" title=":geda:gschem_ug.txt ↵" class="wikilink1">Relevant configuration settings</a> below). If the file has not been manually saved, and the interval expires (current default 2 minutes), the snapshot is saved the next time a change is made in the <strong>gschem</strong> main window (to either a schematic or to a symbol). The interval timer starts again as soon as the snapshot file(s) have been written, and once the timer expires the next change to the main window will trigger the snapshot to be written.<br/>
668 This snapshot includes all work up to, but not including, the last operation performed in the <strong>gschem</strong> main window. This is to allow for easier recovery from a crash that may have been caused by the last operation.<br/>
670 When <strong>gschem</strong> exits normally, the snapshot file(s) are deleted. So, if <strong>gschem</strong> were to crash, or not terminate normally for some reason (e.g., power failure, soda → keyboard, etc.), the shapshot file(s) would be found the next time <strong>gschem</strong> opened the file(s). <strong>gschem</strong> will display the following warning message when it finds a snapshot file associated with the schematic file(s) or symbol file(s) it opens:
673 {full path to autosave file}
675 The backup copy is newer than the schematic, so it seems you
676 should load it instead of the original fil.
677 Gschem usually makes backup copies automatically, and this
678 situation happens when it crashed or it was forced to exit
679 abruptely.
681 If you load the original file, the backup file will be overwritten in
682 the next autosave timeout and it will be lost.
684 Do you want to load the backup file?</font></pre>
685 </p>
687 <p>
688 The snapshots are saved to a file whose filename is constructed from the original filename (schematic or symbol) as follows:
689 </p>
690 <ul>
692 </li>
694 </li>
695 </ul>
697 <p>
699 so that:
700 </p>
701 <ul>
703 </li>
705 </li>
706 </ul>
708 <p>
710 And yes, the ”#” at the front and back of the filename are part of the filename.<br/>
712 </p>
714 <p>
715 When the user does finally manually save the file, the original file (i.e., the file that was opened) is renamed to ”{filename~}” and the latest snapshot file (i.e., ”#{filename}#”) gets copied as ”{filename}”. Note that this new ”{filename}” file may not contain the latest information as displayed on the <strong>gschem</strong> main window, as the <strong>autosave</strong> interval timer may not have expired since the last change to the schematic/symbol.<br/>
717 When the user finally decides to close <strong>gschem</strong>, the latest snapshot file (i.e., ”#{filename}#”) is saved to the original file (i.e., ”{filename}”.<br/>
719 When you exit <strong>gschem</strong> and are prompted to save any unsaved schematic file(s) or symbol file(s), this constitutes a manual save.
720 </p>
722 </div>
723 <!-- EDIT1033 SECTION "Classic Linux backups" [30670-33576] -->
724 <h3 class="sectionedit1034"><a name="incremental_backups" id="incremental_backups">Incremental backups</a></h3>
727 </div>
728 <!-- EDIT1034 SECTION "Incremental backups" [33577-33610] -->
729 <h3 class="sectionedit1035"><a name="relevant_configuration_settings" id="relevant_configuration_settings">Relevant configuration settings</a></h3>
732 <p>
733 There are the following configuration settings in the {binary-install-path}/share/gEDA/system-gschemrc file that effect backups:
734 </p>
735 <ul>
736 <li class="level1"><div class="li"> <strong>undo-control</strong> : Controls if the undo feature is enabled or not.</div>
737 </li>
738 <li class="level1"><div class="li"> <strong>undo-levels</strong> : Determines the number of levels of undo. Basically this number decides how many backup schematics are saved.</div>
739 </li>
740 <li class="level1"><div class="li"> <strong>undo-type</strong> : Controls which kind of undo is used, disk or memory. The default is to use the disk as the storage medium (i.e., after every action the undo information is stored to a new file on disk). The disk mechanism is nice because you get that many backups of the schematic, written to disk as backups, so you should never lose a schematic due to a crash.</div>
741 </li>
742 <li class="level1"><div class="li"> <strong>autosave</strong> : Controls if a backup copy is made every “interval” seconds. Note that a backup copy is only made when you make some change to the schematic, and there were more than “interval” seconds from the last autosave. Autosaving will not be allowed if the “interval” setting is set to zero.</div>
743 </li>
744 </ul>
746 </div>
747 <!-- EDIT1035 SECTION "Relevant configuration settings" [33611-34652] -->
748 <h2 class="sectionedit1036"><a name="on-line_documentation" id="on-line_documentation">On-line documentation</a></h2>
751 <p>
752 The <code>-h</code> option to gschem provides a list of the various command line flags that gschem supports.
755 Usage: gschem [OPTIONS] schematic_filename1 ... schematic_filenameN
756 -q Quiet mode
757 -v Verbose mode on
758 -r filename Rc filename
759 -s filename Script (guile) filename
760 -o filename Output filename (for printing)
761 -p Automatically place the window
762 -t Print stroke information
763 -V Show version information
764 -h Help; this message</font></pre>
765 </p>
767 <p>
768 For a detailed explanation of the command line flags look at the <strong>gschem</strong> man page:
771 </p>
773 <p>
774 Access to this documentation can also be obtained directly from gschem's <strong>Help</strong> menu.
776 </p>
778 </div>
779 <!-- EDIT1036 SECTION "On-line documentation" [34653-35431] -->
780 <h1 class="sectionedit1037"><a name="electrical_connectivity" id="electrical_connectivity">Electrical Connectivity</a></h1>
783 <p>
784 As you draw schematics you need be aware of what is considered to be electrically connected by the gEDA programs.
785 </p>
787 <p>
788 Nets which are visually connected to other nets are electrically connected. This connection may be endpoint to endpoint or endpoint to midpoint. When a single endpoint to endpoint (net or pin endpoint) connection is drawn, the visual dangling net cue disappears. When an endpoint ends in the middle of another net (or multiple endpoints coming together at a single point) then a circular filled connectivity cue is drawn. You cannot connect a net to the middle of a pin. Nets can only be connected to the endpoints of pins. You cannot connect to a net if that net is not orthogonal (horizontal or vertical). The visual cues are the primary way of telling if nets/pins are connected.
789 </p>
791 <p>
792 Bus are similar to nets with the exception that you cannot connect a net to the endpoint of a bus (only to the middle). If you do try to connect a net to the end of a bus you will see a big red X at the invalid endpoint connection. Buses are still very new so there are still many quirks.
793 </p>
795 <p>
796 You can label nets by using the <code>netname=</code> attribute. Do not attach more than one <code>netname=</code> to a net. You only need to attach the <code>netname=</code> attribute to one net segment. Different nets (i.e. multiple net segments which aren’t connected together) which have the same attribute <code>netname=</code> attached to them are also considered electrically connected. You will not get any indication of this connection by <strong>gschem</strong>, but the netlister (<strong>gnetlist</strong>) considers nets with the same <code>netname=</code> attribute electrically connected. The naming convention for buses has not been formalized yet.
797 </p>
799 </div>
800 <!-- EDIT1037 SECTION "Electrical Connectivity" [35432-37155] -->
801 <h1 class="sectionedit1038"><a name="components_symbols_objects_attributes" id="components_symbols_objects_attributes">Components & Symbols & Objects & Attributes</a></h1>
804 <p>
805 There is a hierarchical association between components, symbols, objects, and attributes.
806 </p>
808 </div>
809 <!-- EDIT1038 SECTION "Components & Symbols & Objects & Attributes" [37156-37304] -->
813 <p>
814 A component is the instantiation of a specific symbol, as placed on the schematic. When discussing a schematic you refer to <em class="u">components</em> on the schematic, not <em class="u">symbols</em> on the schematic. Think of symbols as being <em class="u">conceptual</em>, and components as being <em class="u">concrete</em>.<br/>
816 The component consists of a graphic representation and the attributes describing the component's features.<br/>
818 The component inherits all of the attributes defined in the symbol. Certain attributes in the symbol:
819 </p>
820 <ul>
821 <li class="level1"><div class="li"> those explicitly defined as visible unattached attributes (see <a href="#attributes" title=":geda:gschem_ug.txt ↵" class="wikilink1">Attributes</a>)</div>
822 </li>
823 <li class="level1"><div class="li"> specific attributes such as <code>symversion</code> and <code>refdes</code></div>
824 </li>
825 </ul>
827 <p>
829 are promoted to the component level for manipulation by the circuit designer. These attributes may optionally be exposed (made viewable) with the component's graphic, and their values may be changed.<br/>
831 Any attribute not defined in the symbol may be defined in the component. For example, if the symbol does not define the <code>comment</code> attribute, this attribute may be added to the component, perhaps to add a comment for the Bill of Material or Assembly Instructions.<br/>
833 Unfortunately, it is difficult to determine a component's attributes from <strong>gschem</strong> while entering the schematic. You have to place a symbol on the schematic, select the resulting component, and select <strong>Hierarchy | Down Symbol</strong> from the pull-down menus. Then, you have to unhide all attributes with <strong>Edit | Make Inv Text Vis</strong> from the pull-down menus. Then you have to expand your view of the symbol with <strong>View | Extents</strong>. Then, you have to go back to the schematic by selecting <strong>Hierarchy | Up</strong> from the pull-down menus. Then, you have to select <strong>Edit | Edit…</strong> to bring up the “Edit Attributes” dialog box to determine if any attributes have been added at the component level.
834 </p>
836 </div>
837 <!-- EDIT1039 SECTION "Components" [37305-39119] -->
841 <p>
842 Symbols are just a collection of objects and attributes.<br/>
844 The objects have positional significance in the symbol, and define the graphic that is viewed.<br/>
846 Attributes may be attached to objects, or they may be attached to the symbol itself (termed as “unattached” attributes, because they are not attached to an object).
847 </p>
849 </div>
850 <!-- EDIT1040 SECTION "Symbols" [39120-39461] -->
854 <p>
855 The following are objects:
856 </p>
857 <ul>
859 </li>
861 </li>
863 </li>
865 </li>
867 </li>
869 </li>
871 </li>
872 </ul>
874 </div>
875 <!-- EDIT1041 SECTION "Objects" [39462-39575] -->
879 <p>
880 An attribute is text which is in the form <code>name=value</code> (there are no spaces to the left or right of the name,value pair). An attribute can be either attached to an object or unattached. Attributes are used extensively in the gEDA project to convey information (e.g., device name, pin numbers, hidden nets, and unit reference numbers). Check <a href="geda-master_attributes_list.html" class="wikilink1" title="geda-master_attributes_list.html">gEDA/gaf Master Attribute Document</a> for a complete list of attributes.<br/>
882 There are three kinds of attributes:
883 </p>
884 <ul>
885 <li class="level1"><div class="li"> <strong>Attached attributes:</strong> These are attributes which take on the standard form and are attached to some object (pin, net, component, or box etc…) to associate a value with the attribute. For example: a pin number associated with a pin. <span class="hilited">These attributes are usually yellow in color.</span></div>
886 </li>
887 <li class="level1"><div class="li"> <strong>Unattached attributes:</strong> These are attributes which take on the standard form, but are not attached to any object and usually convey some information which is global in nature. For example: a <code>device=</code> attribute (which lives inside symbols) and specifies what device the entire symbol represents. These attributes are also known as floating or toplevel attributes.</div>
888 </li>
889 <li class="level1"><div class="li"> <strong>Promoted attributes:</strong> These are unattached attributes in the symbol's definition that get turned into attached attributes in the component's definition when the symbol is instantiated as a component when placed in the schematic. If you place an unattached visible attribute inside a symbol and then instantiate that symbol, then that unattached attribute gets “promoted”; that is, it becomes an attached attribute. This mechanism of attribute reattachement (from within a symbol) is known as attribute promotion.</div>
890 </li>
891 </ul>
893 <p>
895 There are some gotchas about attribute promotion:
896 </p>
897 <ul>
898 <li class="level1"><div class="li"> Promotion <strong>only</strong> happens when the symbol is first placed. That means that if you place a symbol (e.g., sym1) and then change it on disk (by adding or removing new unattached attributes), existing sym1's will not reflect these new unattached attributes (i.e., they won't get promoted) in any schematic.</div>
899 </li>
901 </li>
902 <li class="level1"><div class="li"> Invisible attributes are not promoted by default. If you add an unattached attribute (e.g., numslots=#) and make it invisible, it will not be promoted.</div>
903 </li>
904 </ul>
906 <p>
908 Now, in order to make everybody happy, this attribute promotion behavior is configurable.<br/>
910 The system-gschemrc file defines:
912 </p>
913 <pre class="code lisp"><pre class="code lisp"><span class="br0">(</span>attribute-promotion <span class="st0">"enabled"</span><span class="br0">)</span></pre></pre>
915 <p>
916 which enables attribute promotion.<br/>
918 If you override the system-gschemrc's default promote-invisible setting by adding:
920 </p>
921 <pre class="code lisp"><pre class="code lisp"><span class="br0">(</span>promote-invisible <span class="st0">"enabled"</span><span class="br0">)</span></pre></pre>
923 <p>
924 to either your user's ~/gschemrc or local 'pwd'/gschemrc file, invisible unattached attributes will also be promoted <span class="hilited">(and in memory removed)</span>.
925 </p>
927 <p>
928 However, if you do this, component slotting will break because <strong>gschem</strong> expects certain unattached attributes inside the symbol <span class="hilited">(in memory even though they are invisible)</span>.<br/>
930 So you can add:
932 </p>
933 <pre class="code lisp"><pre class="code lisp"><span class="br0">(</span>keep-invisible <span class="st0">"enabled"</span><span class="br0">)</span></pre></pre>
935 <p>
936 to either your user's ~/gschemrc or local 'pwd'/gschemrc file. This is enabled by default, but has no effect unless promote-invisible is enabled.
937 </p>
939 <p>
940 So, to summarize, attribute promotion takes unattached attributes inside symbols and attaches them to the outside of a placed symbol. Three *rc keywords control this behavior: attribute-promotion, promote-invisible, and keep-invisible.
941 </p>
943 </div>
944 <!-- EDIT1042 SECTION "Attributes" [39576-42948] -->
945 <h1 class="sectionedit1043"><a name="the_main_window" id="the_main_window">The Main Window</a></h1>
949 <td class="col0"> <a href="media/geda/gschem_screenshot_001.jpg" class="media" target="_blank" title="geda:gschem_screenshot_001.jpg"><img src="media/geda/gschem_screenshot_001.jpg" class="media" alt="" /></a> </td>
950 </tr>
951 </table></div>
952 <!-- EDIT1044 TABLE [42979-43018] -->
953 <p>
955 There are several ways to interact with <strong>gschem</strong>. <strong>gschem</strong> requires a keyboard and mouse. There are three ways to initiate an operation or command:
956 </p>
957 <ul>
959 </li>
961 </li>
962 <li class="level1"><div class="li"> Draw the appropriate stroke (if stroke support is enabled)</div>
963 </li>
964 </ul>
966 <p>
968 To make usage matters more confusing, selecting an operation off of the menus behaves slightly differently than typing the keyboard shortcut. Most of the operations operate on the currently selected object(s), hence you need to select the object first before manipulating them. The menu selected operations usually require some more input (usually a mouse click) after they are picked off of the menu. The keyboard shortcut operations take that required input as the current mouse position. This saves an extra click since you can position the mouse at the right place, type in the shortcut(s), and the command then executes. Note, you can change this so that both menu and shortcut behavior is exactly the same. See the section on the resource file for more info on how to configure this.<br/>
970 Most of the interaction with <strong>gschem</strong> is fairly mode oriented (similar to the great text editor vi). If you select operations off of the menu, then you are placed into the corresponding mode (like copy or move mode). You must then select an anchor point (or whatever the appropriate point is) to continue the operation. Most of the commands off of the menu expect the objects to be already selected. Some of the modes persist after being execute while other immediately return you into select mode (the default mode).<br/>
972 The shortcuts are also mode like in nature. Most of the default shortcuts are for the various commands are not single keystrokes. There are a few which are single keystrokes (like zoom in: `z' or pan: `x'), but most are typically two keystrokes long. As examples, to execute File/Save you would type `f' and `s' (without the quotes) or Add/Line is `a' and `l'. You can get a listing of the shortcuts by picking Help/Hotkeys. You can also see the hotkey assignments in the pulldown menus as well. The shortcuts are defined in the resource files (<strong>system-gschemrc</strong>, <strong>/.gEDA/gschemrc</strong>, or <strong>`pwd`/gschemrc</strong>). See the section on the resource file for more info.<br/>
974 The mouse button actions in <strong>gschem</strong> are mostly configurable. The first mouse button is always used to select objects or pick points. This button is not configurable. The second mouse button is either a copy/move action (when held down over an object), a repeat last command or used to draw a stroke to execute a command. The third mouse button is either a mouse pan (when held down as the mouse is moved) or a popup menu. The behavior of the second and third mouse buttons is controlled through the resource file (see the section below for more info).
975 </p>
977 </div>
978 <!-- EDIT1043 SECTION "The Main Window" [42949-45862] -->
979 <h1 class="sectionedit1045"><a name="the_status_window" id="the_status_window">The Status Window</a></h1>
983 <td class="col0"> <a href="media/geda/status_screenshot.jpg" class="media" target="_blank" title="geda:status_screenshot.jpg"><img src="media/geda/status_screenshot.jpg" class="media" title=":geda:status_screenshot.jpg" alt=":geda:status_screenshot.jpg" /></a> </td>
984 </tr>
985 </table></div>
986 <!-- EDIT1046 TABLE [45895-45958] -->
987 <p>
989 Add some details about what gets displayed in the status window.
990 </p>
992 </div>
993 <!-- EDIT1045 SECTION "The Status Window" [45863-46025] -->
994 <h1 class="sectionedit1047"><a name="the_schematic_file" id="the_schematic_file">The Schematic File</a></h1>
997 <p>
998 Schematic files. These files contain components, nets, text, and sometimes primitive objects (like lines, circles, box etc…) Schematics do not contain pins. Schematic filenames should follow this convention: name_#.sch where:
999 </p>
1000 <ul>
1001 <li class="level1"><div class="li"> name is a text string which describes what this schematic contains.</div>
1002 </li>
1003 <li class="level1"><div class="li"> _# is an underscore and a number (like _1, _2, _7, _13, etc…) This number is used to sequence schematic pages in a multiple page schematic.</div>
1004 </li>
1005 <li class="level1"><div class="li"> .sch is the schematic extension/suffix. It is important the schematic pages have this extension.</div>
1006 </li>
1007 </ul>
1009 <p>
1011 Schematic files are pure <acronym title="American Standard Code for Information Interchange">ASCII</acronym> and will always be pure <acronym title="American Standard Code for Information Interchange">ASCII</acronym>. gEDA does not support any binary file formats. The file format for schematics is described in the gEDA file formats document.
1012 </p>
1014 </div>
1015 <!-- EDIT1047 SECTION "The Schematic File" [46026-46795] -->
1016 <h1 class="sectionedit1048"><a name="the_symbol_file" id="the_symbol_file">The Symbol File</a></h1>
1019 <p>
1020 Symbol files. The schematic and symbol file formats are identical. <strong>gschem</strong> (or a text editor) is used to create symbol files as well as schematics. Symbol files contain lines, circles, boxes, arcs, pins, text, and attributes.<br/>
1022 The naming convention for symbol files is: name-#.sym where:
1023 </p>
1024 <ul>
1025 <li class="level1"><div class="li"> name is a text string which describes what the symbol represents.</div>
1026 </li>
1027 <li class="level1"><div class="li"> -# is a dash and a number (like -1, -2 etc…) The number is used to allow for a symbols to have the same name yet different contents. There might be multiple representations for resistors so these symbols should be called: resistor-1.sym, resistor-2.sym, and resistor-3.sym.</div>
1028 </li>
1029 <li class="level1"><div class="li"> .sym is the symbol extension/suffix. It is important the symbols have this extension.</div>
1030 </li>
1031 </ul>
1033 <p>
1035 The way of specifying hierarchy is by using the source= attribute. Please see the master attribute document for info on this mechanism.<br/>
1037 The hierarchy mechanism is still in heavy flux, so there might be some more changes.
1038 </p>
1040 </div>
1041 <!-- EDIT1048 SECTION "The Symbol File" [46796-47782] -->
1042 <h1 class="sectionedit1049"><a name="symbol_libraries" id="symbol_libraries">Symbol Libraries</a></h1>
1045 <p>
1046 Components are searched for by specifying (component-library ”…”) inside one of the *rc files. See below for more info.
1047 </p>
1049 </div>
1050 <!-- EDIT1049 SECTION "Symbol Libraries" [47783-47936] -->
1054 <p>
1055 Log file. This file contains informative, error, warnings etc… messages when <strong>gschem</strong> was run. This file is created in the working directory that <strong>gschem</strong> was started in. This allows the user to preserve log files between independent projects.
1056 </p>
1058 </div>
1059 <!-- EDIT1050 SECTION "The Log File" [47937-48214] -->
1063 <p>
1064 Grips are a mechanism used in <strong>gschem</strong> to provide an easy way of modifying objects inside schematics. When you select an object, little squares are placed in strategic locations (line end points or circle radius point or corners of a box) which allow you to change the object quickly. Grip support currently exists for lines, nets, pins, buses, circles, and boxes. Arcs do not yet have grips, but will eventually have them.
1065 </p>
1067 <p>
1068 Using grips is easy:
1069 </p>
1070 <ul>
1071 <li class="level1"><div class="li"> Select the object you want to change. The grips (the little boxes) will appear.</div>
1072 </li>
1073 <li class="level1"><div class="li"> Click and hold the first mouse button inside the box.</div>
1074 </li>
1075 <li class="level1"><div class="li"> Move the mouse around till you have the object where you want it</div>
1076 </li>
1078 </li>
1079 </ul>
1081 </div>
1082 <!-- EDIT1051 SECTION "Grips" [48215-48924] -->
1083 <h1 class="sectionedit1052"><a name="menu_operations" id="menu_operations">Menu Operations</a></h1>
1086 </div>
1087 <!-- EDIT1052 SECTION "Menu Operations" [48925-48954] -->
1091 <p>
1092 The <strong>gschem</strong> application is primarily used for the creation of schematic files (i.e., filename.sch) and symbol files (filename.sym).<br/>
1094 The following operations are related to the manipulation of these files.<br/>
1096 Note that <strong>gschem</strong> automatically maintains backups of open schematic/symbol files, in the /tmp directory, for the purpose of Undo/Redo. <strong>gschem</strong> cleans up these files when it exits gracefully. If <strong>gschem</strong> does not exit gracefully, the next time you launch <strong>gschem</strong> you will be prompted with a dialog similar to:
1099 {filename}
1101 The backup copy is newer than the schematic, so it seems you
1102 load it instead of the original file.
1103 gschem usually makes backup copies automatically, and this
1104 situation happens when it crashed or it was forced to exit
1105 abruptly.
1107 If you load the original file, the backup file will be overwritten in
1108 the next autosave timeout and it will be lost.
1110 Do you want to load the backup file?</font></pre>
1111 </p>
1113 <p>
1114 The following are available from the <strong>gschem</strong> main window's menu-bar when you expand <strong>File</strong>:
1115 </p>
1117 </div>
1118 <!-- EDIT1053 SECTION "File" [48955-50108] -->
1119 <h3 class="sectionedit1054"><a name="new_window_fw" id="new_window_fw">New Window (fw)</a></h3>
1122 <p>
1123 <strong>File | New Window</strong> opens a new window, in addition to any already open windows. Each window is totally separate from the other windows.
1124 </p>
1126 </div>
1127 <!-- EDIT1054 SECTION "New Window (fw)" [50109-50274] -->
1131 <p>
1132 <strong>File | New Page</strong> opens a new page, in addition to any existing open pages. Usually this page will be named “untitled_N.sch”, where N is an incrementing number.
1133 </p>
1135 </div>
1136 <!-- EDIT1055 SECTION "New Page (fn)" [50275-50462] -->
1137 <h3 class="sectionedit1056"><a name="open_page_fo" id="open_page_fo">Open Page... (fo)</a></h3>
1140 <p>
1143 The “Open…” dialog box pops up providing:
1144 </p>
1145 <ul>
1147 </li>
1149 <ul>
1151 </li>
1153 </li>
1155 </li>
1157 </li>
1158 </ul>
1159 </li>
1160 </ul>
1162 </div>
1163 <!-- EDIT1056 SECTION "Open Page... (fo)" [50463-50750] -->
1164 <h3 class="sectionedit1057"><a name="close_page_pc" id="close_page_pc">Close Page (pc)</a></h3>
1167 <p>
1168 <strong>File | Close Page</strong> closes the currently displayed page. This will prompt you to save if you have modified the page.
1169 </p>
1171 </div>
1172 <!-- EDIT1057 SECTION "Close Page (pc)" [50751-50896] -->
1173 <h3 class="sectionedit1058"><a name="revert_page_pr" id="revert_page_pr">Revert Page (pr)</a></h3>
1176 <p>
1177 <strong>File | Revert Page</strong> closes and reopens the currently displayed page. This will not prompt you to save the current page, but will quickly discard any changes you have made and reopen the saved schematic from disk. Use with caution.
1178 </p>
1180 </div>
1181 <!-- EDIT1058 SECTION "Revert Page (pr)" [50897-51158] -->
1185 <p>
1186 <strong>File | Save Page</strong> saves the current page. The current filename is displayed in the <strong>gschem</strong> status-bar.<br/>
1188 If the page's filename is “untitled_N.sch” (where N is a integer), then the Save As… dialog box will be displayed, prompting for a new filename.<br/>
1190 If the page's filename is NOT “untitled_N.sch” (where N is a integer), then the Save As… dialog box will NOT be displayed, and:
1191 </p>
1192 <ul>
1193 <li class="level1"><div class="li"> the backup file will be created for the previous version, named {filename}~ That is, the ”~” (tilde character) is appended to the filename. Any previous backup file is lost.</div>
1194 </li>
1196 </div>
1197 </li>
1198 </ul>
1200 </div>
1201 <!-- EDIT1059 SECTION "Save Page (fs)" [51159-51806] -->
1202 <h3 class="sectionedit1060"><a name="save_page_as_fa" id="save_page_as_fa">Save Page As... (fa)</a></h3>
1205 <p>
1208 If the current filename is “untitled_N.sch”, the Save As… dialog box prompts for a new filename.<br/>
1210 If the current filename is NOT “untitled_N.sch”, the Save As… dialog box prompts for a new filename, filling in the current filename as a default.<br/>
1212 In either case the filename may be changed, and a new file created when the Save As button is clicked.
1213 </p>
1215 </div>
1216 <!-- EDIT1060 SECTION "Save Page As... (fa)" [51807-52254] -->
1217 <h3 class="sectionedit1061"><a name="save_all_fl_fl" id="save_all_fl_fl">Save All (fl) (fl)</a></h3>
1220 <p>
1222 </p>
1224 </div>
1225 <!-- EDIT1061 SECTION "Save All (fl) (fl)" [52255-52359] -->
1229 <p>
1232 The following may be selected:
1233 </p>
1234 <ul>
1235 <li class="level1"><div class="li"> Filename (if <strong>gschem</strong> has multiple pages loaded, this filename defaults to the page currently displayed).</div>
1236 </li>
1238 </li>
1240 <ul>
1241 <li class="level2"><div class="li"> Extents with margins – the current page, with margins where the printer doesn't output.</div>
1242 </li>
1243 <li class="level2"><div class="li"> Extents no margins – the current page, but without margins where the printer doesn't output. The printer output may be scaled larger than when using “Entents with margins”, but at the loss along the borders of the schematic.</div>
1244 </li>
1245 <li class="level2"><div class="li"> Current window – Scaled to fit the page size, but not optimally.</div>
1246 </li>
1247 </ul>
1248 </li>
1250 <ul>
1252 </li>
1254 </li>
1255 </ul>
1256 </li>
1257 </ul>
1259 <p>
1261 Pressing Print will generate a PostScript file with the filname format of the form {filename}.ps (e.g., printing schematic file First_1.sch would generate First_1.ps).<br/>
1263 Printing the PostScript file to your printer is distribution dependent:</p>
1264 <dl>
1267 </dl>
1270 </div>
1271 <!-- EDIT1062 SECTION "Print... (fp)" [52360-53406] -->
1272 <h3 class="sectionedit1063"><a name="write_png_fi" id="write_png_fi">Write PNG... (fi)</a></h3>
1275 <p>
1276 <strong>File | Write <acronym title="Portable Network Graphics">PNG</acronym>…</strong> brings up the Write <acronym title="Portable Network Graphics">PNG</acronym>… dialog box. Note you must have libgdgeda installed (and any required dependencies) if you want to output images.<br/>
1278 The dialog box allows you to select:
1279 </p>
1280 <ul>
1282 <ul>
1284 </li>
1286 </li>
1288 </li>
1290 </li>
1292 </li>
1294 </li>
1296 </li>
1297 </ul>
1298 </li>
1299 <li class="level1"><div class="li"> Filename (if <strong>gschem</strong> has multiple pages loaded, the currently displayed page's filname is given)</div>
1300 </li>
1301 </ul>
1303 <p>
1305 When the OK button is clicked, a <acronym title="Portable Network Graphics">PNG</acronym> graphic file with a filename of the form {filename}.png is created (e.g., writing a <acronym title="Portable Network Graphics">PNG</acronym> for schematic file First_1.sch will generate a First_1.png file).<br/>
1307 This file may be used any way a <acronym title="Portable Network Graphics">PNG</acronym> file is used (e.g., web-page, document insertion, image manipulation with the GIMP, etc.).
1308 </p>
1310 </div>
1311 <!-- EDIT1063 SECTION "Write PNG... (fi)" [53407-54201] -->
1312 <h3 class="sectionedit1064"><a name="execute_script_ft" id="execute_script_ft">Execute Script... (ft)</a></h3>
1315 <p>
1317 </p>
1319 </div>
1320 <!-- EDIT1064 SECTION "Execute Script... (ft)" [54202-54273] -->
1321 <h3 class="sectionedit1065"><a name="close_window_fc" id="close_window_fc">Close Window (fc)</a></h3>
1324 <p>
1325 <strong>File | Close Window</strong> closes the current window. If there are any modified schematics, the “There are unsaved schematics” dialog box will appear. Clicking OK will cause all unsaved schematics to be lost.
1326 </p>
1328 </div>
1329 <!-- EDIT1065 SECTION "Close Window (fc)" [54274-54512] -->
1333 <p>
1334 <strong>File | Quit</strong> closes all opened windows and exits <strong>gschem</strong>. A “There are unsaved schematics” dialog box will appear for each window that has unsaved schematics.
1335 </p>
1337 </div>
1338 <!-- EDIT1066 SECTION "Quit (Alt-q)" [54513-54705] -->
1342 <p>
1343 The following are available from the <strong>gschem</strong> main window’s menu-bar when you expand <strong>Edit</strong>:
1344 </p>
1346 </div>
1347 <!-- EDIT1067 SECTION "Edit" [54706-54822] -->
1351 <p>
1352 <strong>Edit | Undo</strong> does exactly that, it undos the last action which changed the schematic.<br/>
1354 The depth of undo (how many undo steps can be performed) is set in the system-gschemrc file. The default is 10. Simply override this setting by placing the following lines in either your ~/.gEDA/gschemrc file or your local gschemrc file:
1357 ;
1358 ; Determines the number of levels of undo. Basically this number decides
1359 ; how many backup schematics are saved on disk.
1360 ;
1362 </p>
1364 <p>
1365 After every action (including zooming and panning) the schematic is saved to disk (in /tmp). The undo-levels setting determines how many of these temporary files are maintained in the /tmp directory. <strong>gschem</strong> does clean-up after itself when you exit.<br/>
1367 Should <strong>gschem</strong> crash, the saved files remain in /tmp for disaster recovery. You will be prompted the next time the schematic is opened to recover from the backup.<br/>
1369 </p>
1371 </div>
1372 <!-- EDIT1068 SECTION "Undo (shift-u)" [54823-55781] -->
1376 <p>
1377 <strong>Edit | Redo</strong> only applies after you have done an <strong>Edit | Undo</strong>. You can undo something and then immediately redo it. However if you do anything in between you will lose the undo info. You can undo and redo to your hearts desire up and down till you reach the max undo levels.<br/>
1379 </p>
1381 </div>
1382 <!-- EDIT1069 SECTION "Redo (shift-r)" [55782-56090] -->
1383 <h3 class="sectionedit1070"><a name="select_mode_s" id="select_mode_s">Select Mode (s)</a></h3>
1386 <p>
1387 <strong>Edit | Select Mode</strong> is the initial mode in which <strong>gschem</strong> starts.<br/>
1389 When in <strong>Select Mode</strong>, an unlocked object (i.e., component, line, box, circle, …) may be selected by placing the mouse pointer within the outline of the object and single-clicking, or by dragging a box (i.e., holding down the first mouse-button) around the object. Selecting an already selected object will leave the object selected (i.e., you can not unselect an object by single-clicking it). Multiple unlocked objects may be selected by dragging a box around the objects.<br/>
1391 A locked object may be selected by dragging a box around the object.<br/>
1393 To de-select all objects, single-click anywhere on the schematic where there is no object.<br/>
1395 A visible attribute for an unlocked component may be selected by placing the mouse pointer over the component's visible attribute and single-clicking. Placing the mouse pointer over the unlocked component's visible attribute and double-clicking will open the edit dialog box appropriate for the attribute.<br/>
1397 Objects will change color when selected.<br/>
1399 You stay in <strong>Select Mode</strong> until you select one of the other Modes (e.g., Line, Copy, Move, etc.).<br/>
1401 Your current Mode is displayed on the status-bar, in the lower-right corner of the <strong>gschem</strong> window.<br/>
1403 If multiple objects overlap, single-clicking where they overlap will cycle through the objects.<br/>
1405 If you hold down the SHIFT key and single-click, you can select and deselect multiple objects. Doing this with multiple overlapping objects will cause the selection to cycle among the possible object selections.<br/>
1407 If you hold down the CONTROL key and single-click, you will toggle the object in and out of the current selection list.<br/>
1409 If you hold down the SHIFT key while drawing a selection box you will add to the currently selected objects. Objects cannot be removed using the selection box and holding down the SHIFT key.<br/>
1411 If you hold down the CONTROL key while drawing a selection box then you will toggle any encompassed objects. If an object was selected then it will be unselected and vice versa.<br/>
1413 If you pick a component, its visible and invisible attributes are selected as well.
1414 If you just want to select the object, you must deselect the attributes.<br/>
1416 The selection mechanisms are not obvious and do require some practice. There are some quirks so please report them as you come across them.
1417 </p>
1419 </div>
1420 <!-- EDIT1070 SECTION "Select Mode (s)" [56091-58498] -->
1424 <p>
1427 If the object is a component, <strong>Edit | Edit…</strong> then pops up a dialog box that allows you to edit the component's attributes:
1428 </p>
1429 <ul>
1431 </li>
1432 <li class="level1"><div class="li"> A drop-down list of pre-defined attributes permits selection, and a edit-box provides association of a value to the attribute.</div>
1433 </li>
1434 <li class="level1"><div class="li"> The attribute' name and/or value may be made visible or invisible,</div>
1435 </li>
1436 </ul>
1438 <p>
1440 If the ojbect is a text string, <strong>Edit…</strong> then pops up a dialog box that allows you to modify the text string's attributes:
1441 </p>
1442 <ul>
1443 <li class="level1"><div class="li"> The text string may be modified. Multiple lines of text may be entered by inserting carriage-returns.</div>
1444 </li>
1446 </li>
1448 </li>
1450 <ul>
1452 </li>
1454 </li>
1456 </li>
1457 </ul>
1458 </li>
1459 </ul>
1461 <p>
1463 Apply the changes by pressing OK.
1464 </p>
1466 <p>
1469 If you need to change the attributes to more than just a few components, consider saving your schematics, closing <strong>gschem</strong>, and using the <strong>gattrib</strong> application, the <strong>grenum</strong> application, or the <strong>refdes_renum</strong> application to make the changes.
1470 </p>
1472 </div>
1473 <!-- EDIT1071 SECTION "Edit... (ee)" [58499-59693] -->
1474 <h3 class="sectionedit1072"><a name="edit_text_ex" id="edit_text_ex">Edit Text... (ex)</a></h3>
1477 <p>
1482 <strong>Edit | Edit Text…</strong> then pops up a dialog box that allows you to modify the text string's attributes:
1483 </p>
1484 <ul>
1485 <li class="level1"><div class="li"> The text string may be modified. Multiple lines of text may be entered by inserting carriage-returns.</div>
1486 </li>
1488 </li>
1490 </li>
1492 <ul>
1494 </li>
1496 </li>
1498 </li>
1499 </ul>
1500 </li>
1501 </ul>
1503 <p>
1505 Apply the changes by pressing OK.
1506 </p>
1508 <p>
1511 If you need to change the attributes to more than just a few text strings, consider saving your schematics, closing <strong>gschem</strong>, and using the <strong>gattrib</strong> application, the <strong>grenum</strong> application, or the <strong>refdes_renum</strong> application to make the changes.
1512 </p>
1514 </div>
1515 <!-- EDIT1072 SECTION "Edit Text... (ex)" [59694-60552] -->
1519 <p>
1520 <strong>Edit | Copy Mode</strong> allows you to copy (i.e., duplicate) the currently selected objects.<br/>
1522 To copy the object(s):
1523 </p>
1524 <ul>
1525 <li class="level1"><div class="li"> Select the objects to be copied (i.e., in <strong>Select Mode</strong>)</div>
1526 </li>
1528 </li>
1529 <li class="level1"><div class="li"> Observe the status-bar now indicates <strong>Copy Mode</strong></div>
1530 </li>
1531 <li class="level1"><div class="li"> Click on the selected component(s) to establish an origin of reference</div>
1532 </li>
1533 <li class="level1"><div class="li"> Observe a shadow/outline appears for the selected components that moves with the mouse</div>
1534 </li>
1536 </li>
1538 </li>
1539 </ul>
1541 <p>
1545 Holding down the CONTROL key as you move the outline around will constrain the movement to be either horizontal or vertical.<br/>
1547 To copy objects using the shortcut keys is almost the same as above except that the origin point is selected automatically for you once you hit the copy mode shortcut.<br/>
1549 </p>
1551 </div>
1552 <!-- EDIT1073 SECTION "Copy Mode (ec)" [60553-61477] -->
1556 <p>
1559 To move the object(s):
1560 </p>
1561 <ul>
1562 <li class="level1"><div class="li"> Select the objects to be moved (i.e., in <strong>Select Mode</strong>)</div>
1563 </li>
1565 </li>
1566 <li class="level1"><div class="li"> Observe the status-bar now indicates <strong>Move Mode</strong></div>
1567 </li>
1568 <li class="level1"><div class="li"> Click on the selected component(s) to establish an origin of reference</div>
1569 </li>
1570 <li class="level1"><div class="li"> Observe a shadow/outline appears for the selected components that moves with the mouse</div>
1571 </li>
1573 </li>
1575 </li>
1576 </ul>
1578 <p>
1582 Holding down the CONTROL key as you move the outline around will constrain the movement to be either horizontal or vertical.<br/>
1584 To move objects using the shortcut keys is almost the same as above except that the origin point is selected automatically for you once you hit the copy mode shortcut.<br/>
1586 </p>
1588 <p>
1591 </p>
1592 <ul>
1593 <li class="level1"><div class="li"> Select the objects to be moved (i.e., in <strong>Select Mode</strong>).<br/>
1594 </div>
1595 </li>
1596 <li class="level1"><div class="li"> Put the mouse pointer on one of the selected objects, then drag the objects and drop them where you want them.<br/>
1597 </div>
1598 </li>
1599 </ul>
1601 </div>
1602 <!-- EDIT1074 SECTION "Move Mode (em)" [61478-62631] -->
1603 <h3 class="sectionedit1075"><a name="delete_delete-key" id="delete_delete-key">Delete (Delete-key)</a></h3>
1606 <p>
1609 To delete objects:
1610 </p>
1611 <ul>
1612 <li class="level1"><div class="li"> Select the desired object(s) (i.e., in <strong>Select Mode</strong>)</div>
1613 </li>
1615 </li>
1616 </ul>
1618 <p>
1620 The object(s) will be deleted immediately. If you inadvertantly delete a component, you can use Undo to recover.
1621 </p>
1623 </div>
1624 <!-- EDIT1075 SECTION "Delete (Delete-key)" [62632-62950] -->
1625 <h3 class="sectionedit1076"><a name="rotate_90_mode_er" id="rotate_90_mode_er">Rotate 90 Mode (er)</a></h3>
1628 <p>
1629 <strong>Edit | Rotate 90 Mode</strong> allows you to rotate objects 90 degrees around a pivot/center point.<br/>
1631 To rotate objects:
1632 </p>
1633 <ul>
1634 <li class="level1"><div class="li"> Select the desired object(s) (i.e., in <strong>Select Mode</strong>)</div>
1635 </li>
1637 </li>
1639 </li>
1640 </ul>
1642 <p>
1644 The object(s) will be rotated 90º counter-clockwise immediately. If you inadvertantly rotate a component, you can use Undo to recover.<br/>
1646 Rotating objects using the shortcut keys is similar to above except that the center point is the last mouse position at which you typed the shortcut.<br/>
1648 </p>
1650 </div>
1651 <!-- EDIT1076 SECTION "Rotate 90 Mode (er)" [62951-63540] -->
1652 <h3 class="sectionedit1077"><a name="mirror_mode_ei" id="mirror_mode_ei">Mirror Mode (ei)</a></h3>
1655 <p>
1656 <strong>Edit | Mirror Mode</strong> allows you to mirror objects horizontally around a pivot point.<br/>
1658 To mirror objects:
1659 </p>
1660 <ul>
1661 <li class="level1"><div class="li"> Select the desired object(s) (i.e., in <strong>Select Mode</strong>)</div>
1662 </li>
1664 </li>
1666 </li>
1667 </ul>
1669 <p>
1671 Mirroring objects using the shortcut keys is similar to above except that the pivot point is the last mouse position at which you typed the shortcut.<br/>
1673 Objects are mirrored horizontally about the pivot point. If you want to get a vertical mirror then rotate and mirror the object(s) till you get the desired position.<br/>
1675 Mirroring of embedded components is not supported.
1676 </p>
1678 </div>
1679 <!-- EDIT1077 SECTION "Mirror Mode (ei)" [63541-64197] -->
1680 <h3 class="sectionedit1078"><a name="slot_e_shift-s" id="slot_e_shift-s">Slot... (e shift-s)</a></h3>
1683 <p>
1684 Some physical packages (e.g., the classic 7400 Quad NAND gate) contain more than one logical component (e.g., one of the NAND gates). In <strong>gchem</strong> terminology, each of these logical components is termed a “slot” (e.g., there would be 4 slots in the 7400 Quad NAND gate). Each slot is associated with specific pins on the physical package.<br/>
1686 <strong>Edit | Slot…</strong> allows you to change the slot number of a multiple-slot package. The package must support slotting. Refer to the <a href="http://www.geda.seul.org/docs/current/symbols/index.html" class="urlextern" title="http://www.geda.seul.org/docs/current/symbols/index.html" rel="nofollow">gEDA/gaf Symbol Creation Document</a> for more details.<br/>
1688 To change the slot number (i.e., select which package pins are associated with a logical component):
1689 </p>
1690 <ul>
1691 <li class="level1"><div class="li"> Select the desired logical component (i.e., in <strong>Select Mode</strong>)</div>
1692 </li>
1694 </li>
1695 <li class="level1"><div class="li"> Change the “slot=n” value in the “Edit slot number” dialog box</div>
1696 </li>
1698 </li>
1699 </ul>
1701 <p>
1703 Note that selecting the slot on a package often effects the layout of the printed circuit board, as the slot may be on the wrong side of the package for effecient routing of nets. Don't worry, you can always come back and change the slot selection once you start laying out your board and know which slots route best.
1704 </p>
1706 </div>
1707 <!-- EDIT1078 SECTION "Slot... (e shift-s)" [64198-65414] -->
1711 <p>
1712 <strong>Edit | Color…</strong> allows you to change the color of any selected object (with the exception of components).<br/>
1714 To change the color of the currently selected objects:
1715 </p>
1716 <ul>
1717 <li class="level1"><div class="li"> Select the desired object(s) (i.e., in <strong>Select Mode</strong>)</div>
1718 </li>
1720 </li>
1721 <li class="level1"><div class="li"> The “Edit | Color Edit” dialog box, with a drop down list for colors, will appear:</div>
1722 <ul>
1724 </li>
1726 </li>
1728 </li>
1730 </li>
1732 </li>
1734 </li>
1736 </li>
1738 </li>
1740 </li>
1742 </li>
1744 </li>
1746 </li>
1748 </li>
1750 </li>
1751 </ul>
1752 </li>
1754 </li>
1756 </li>
1757 </ul>
1759 <p>
1761 The color change will take effect once you press Apply.<br/>
1763 You can leave this dialog box up and select other objects and change their color by pressing Apply.
1764 </p>
1766 </div>
1767 <!-- EDIT1079 SECTION "Color... (eo)" [65415-66373] -->
1768 <h3 class="sectionedit1080"><a name="lock_el_unlock_e_shift-l" id="lock_el_unlock_e_shift-l">Lock (el) / Unlock (e shift-l)</a></h3>
1771 <p>
1772 <strong>Edit | Lock</strong> and <strong>Edit | Unlock</strong> allow you to lock/unlock components in a schematic. A locked component cannot be selected by a single click. To select locked component(s), drag a box around the component(s).<br/>
1774 Locking a component is useful for components such as title blocks, which should not be selectable because there are other objects inside its boundaries. If the titleblock was not locked, and you missed selecting a component by clicking it with the mouse, you would end up selecting the titleblock instead.<br/>
1776 Locking a component is also useful just to prevent it from being inadvertantly selected.<br/>
1778 To lock/unlock components:
1779 </p>
1780 <ul>
1781 <li class="level1"><div class="li"> Select the desired object(s) (i.e., in <strong>Select Mode</strong>)</div>
1782 </li>
1783 <li class="level1"><div class="li"> Select <strong>Edit | Lock</strong> or <strong>Edit | Unlock</strong></div>
1784 </li>
1785 </ul>
1787 <p>
1789 The locked/unlocked state of components is preserved when <strong>gschem</strong> exits, so components which were locked remain locked the next time the schematic is opened.<br/>
1791 You can lock and unlock regular objects (e.g., lines, pins, boxes…). This is nice when you are drawing something and an object is in the way. Just lock it, and you will not have to think about it when you click to select other objects. Locking an object is not preserved in the file format, so once you quit <strong>gschem</strong> any locked objects will be unlocked the next time the schematic is opened.<br/>
1793 Note that if a component is locked, you can not single-click to select a visible attribute, or double-click to select and edit a visible component. First unlock such locked components.
1794 </p>
1796 </div>
1797 <!-- EDIT1080 SECTION "Lock (el) / Unlock (e shift-l)" [66374-67912] -->
1798 <h3 class="sectionedit1081"><a name="line_width_type_ew" id="line_width_type_ew">Line Width & Type... (ew)</a></h3>
1801 <p>
1802 The <strong>Edit | Line Width & Type…</strong> dialog box lets you control the width and type of lines, boxes, circles, and arcs on the schematic/symbol.<br/>
1805 </p>
1806 <ul>
1807 <li class="level1"><div class="li"> Select the desired object(s) (i.e., in <strong>Select Mode</strong>)</div>
1808 </li>
1809 <li class="level1"><div class="li"> Select <strong>Edit | Line Width & Type…</strong></div>
1810 </li>
1812 </li>
1814 <ul>
1816 </li>
1818 </li>
1820 </li>
1822 </li>
1823 </ul>
1824 </li>
1826 </li>
1827 </ul>
1829 <p>
1831 Note that if the line width doesn't seem to change, just pick a larger value.
1832 </p>
1834 </div>
1835 <!-- EDIT1081 SECTION "Line Width & Type... (ew)" [67913-68528] -->
1836 <h3 class="sectionedit1082"><a name="fill_type_ef" id="fill_type_ef">Fill Type... (ef)</a></h3>
1839 <p>
1842 To fill a box or circle:
1843 </p>
1844 <ul>
1846 </li>
1847 <li class="level1"><div class="li"> Select <strong>Edit | Fill Type…</strong>. The “Edit FIll Type” dialog box is displayed.</div>
1848 </li>
1850 <ul>
1852 </li>
1854 </li>
1856 </li>
1858 </li>
1860 </li>
1862 </li>
1863 </ul>
1864 </li>
1866 </li>
1867 </ul>
1869 </div>
1870 <!-- EDIT1082 SECTION "Fill Type... (ef)" [68529-68869] -->
1871 <h3 class="sectionedit1083"><a name="symbol_translate_et" id="symbol_translate_et">Symbol Translate... (et)</a></h3>
1874 <p>
1875 <strong>Edit | Symbol Translate…</strong> is used when creating a symbol, to translate the symbol to an origin for subsequent placement. The symbol may take an optional offset (in mils), as appropriate to the symbol.<br/>
1877 To translate the symbol:
1878 </p>
1879 <ul>
1881 </li>
1882 <li class="level1"><div class="li"> Set the grid snap spacing to 100 mils (<strong>Options</strong> | <strong>Snap Grid Spacing…</strong>).</div>
1883 </li>
1884 <li class="level1"><div class="li"> Toggle the grid ON (<strong>Options</strong> | <strong>Toggle Grid On/Off</strong>)</div>
1885 </li>
1886 <li class="level1"><div class="li"> Toggle the grid snap ON (<strong>Options</strong> | <strong>Toggle Snap On/Off</strong>)</div>
1887 </li>
1889 </li>
1890 <li class="level1"><div class="li"> Draw the symbol, according to the recommendations in the <a href="http://www.geda.seul.org/docs/current/symbols/index.html" class="urlextern" title="http://www.geda.seul.org/docs/current/symbols/index.html" rel="nofollow">gEDA/gaf Symbol Creation Document</a></div>
1891 </li>
1893 </li>
1895 </li>
1896 <li class="level1"><div class="li"> Enter 0 to translate to the origin, or enter a value (in mils), positive or negative, to offset the symbol from the origin.</div>
1897 </li>
1899 </li>
1901 </li>
1902 </ul>
1904 <p>
1908 If you enter a non-zero offset, this will be applied equally in both the X and the Y directions.<br/>
1910 </p>
1912 </div>
1913 <!-- EDIT1083 SECTION "Symbol Translate... (et)" [68870-70034] -->
1914 <h3 class="sectionedit1084"><a name="embed_component_picture_eb" id="embed_component_picture_eb">Embed Component/Picture (eb)</a></h3>
1917 <p>
1918 <strong>gschem</strong> supports the concept of embedded components and graphics, where all the information necessary to display a component/graphic is placed in the schematic file. <strong>Edit | Embed Component/Picture</strong> causes schematic files to be significantly larger, but it makes it easy to share schematics with other people or archive schematics. You should only embed components when absolutely necessary.<br/>
1921 </p>
1922 <ul>
1923 <li class="level1"><div class="li"> Select the component/picture (in <strong>Select Mode</strong>)</div>
1924 </li>
1925 <li class="level1"><div class="li"> Select <strong>Edit | Embed Component/Picture</strong></div>
1926 </li>
1927 </ul>
1929 <p>
1931 Save the schematic. The schematic file will now contain the text strings for the embedded component or embedded graphic.<br/>
1933 The <strong>Add Component…</strong> dialog box allows you to optionally embed the component.<br/>
1935 The <strong>Add Picture…</strong> dialog box does NOT allow you to optionally embed the component.<br/>
1937 You can only embed and unembed components. Also, you cannot embed and then mirror a component (this is a limitation of <strong>gschem</strong> and will eventually be fixed).
1938 </p>
1940 </div>
1941 <!-- EDIT1084 SECTION "Embed Component/Picture (eb)" [70035-71064] -->
1942 <h3 class="sectionedit1085"><a name="unembed_component_picture_eu" id="unembed_component_picture_eu">Unembed Component/Picture (eu)</a></h3>
1945 <p>
1946 <strong>Edit | Unembed Component/Picture</strong> will move the component's or graphic's information from the schematic file's contents and output it to the original file's path/filename (i.e., the schematic file includes the path/filename information).
1948 </p>
1949 <ul>
1950 <li class="level1"><div class="li"> Select the component/picture (in <strong>Select Mode</strong>)</div>
1951 </li>
1952 <li class="level1"><div class="li"> Select <strong>Edit | Unembed Component/Picture</strong></div>
1953 </li>
1954 </ul>
1956 <p>
1958 Save the schematic. The schematic file will now NOT contain the text strings for the embedded component or embedded graphic.<br/>
1960 You can only embed and unembed components.
1961 </p>
1963 </div>
1964 <!-- EDIT1085 SECTION "Unembed Component/Picture (eu)" [71065-71654] -->
1965 <h3 class="sectionedit1086"><a name="update_component_ep" id="update_component_ep">Update Component (ep)</a></h3>
1968 <p>
1972 </p>
1973 <ul>
1974 <li class="level1"><div class="li"> Select the component for which the symbol should be changed.</div>
1975 </li>
1976 <li class="level1"><div class="li"> Select <strong>Hierarchy | Down Symbol</strong>. This takes you to the symbol editor</div>
1977 </li>
1978 <li class="level1"><div class="li"> Modify the symbol. This includes modifying the symbol's graphic objects, adding/changing/deleting attributes, and moving objects with respect to the origin</div>
1979 </li>
1980 <li class="level1"><div class="li"> Don't forget to <strong>Edit | Symbol Translate</strong></div>
1981 </li>
1982 <li class="level1"><div class="li"> Select <strong>File | Save Page</strong> to save the symbol to it's file</div>
1983 </li>
1984 <li class="level1"><div class="li"> Select <strong>Hierarchy | Up Symbol</strong>. This returns you to the schematic editor</div>
1985 </li>
1986 <li class="level1"><div class="li"> With the component still selected, select <strong>Edit | Update Component</strong> to update the componet's description from the modified symbol's definition</div>
1987 </li>
1988 <li class="level1"><div class="li"> Select each component on the schematic(s) made from this symbol, and select <strong>Edit | Update Component</strong></div>
1989 </li>
1990 </ul>
1992 <p>
1994 New components placed on the schematic from this updated symbol will use the new symbol definition.<br/>
1996 Components placed on the schematic from this symbol will be updated the next time this schematic is opened.<br/>
1998 The symbol's <code>symversion</code> attribute will automatically be incremented for non-trivial changes when the symbol is saved. When a schematic is opened by <strong>gschem</strong>, all symbols used by the schematic are read from their libraries. The <code>symversion</code> attribute of the symbol read from the library is compared to the <code>symversion</code> attribute of the components in the schematic. If the <code>symversion</code> attributes are different, the <code>symversion</code> attribute is exposed on the schematic for those symbols effected. Note that:
1999 </p>
2000 <ul>
2001 <li class="level1"><div class="li"> This is a “hint” to the designer to check the symbol.</div>
2002 </li>
2003 <li class="level1"><div class="li"> You need to actually open a schematic file with <strong>gschem</strong> for the components to be updated.</div>
2004 </li>
2005 </ul>
2007 </div>
2008 <!-- EDIT1086 SECTION "Update Component (ep)" [71655-73464] -->
2009 <h3 class="sectionedit1087"><a name="show_hide_inv_text_en" id="show_hide_inv_text_en">Show/Hide Inv Text (en)</a></h3>
2012 <p>
2013 <strong>Edit | Show/Hide Inv Text</strong> is most appropriate when creating or editing symbols, to view or hide the text for all of the symbol's invisible attributes.<br/>
2015 <a href="#make_inv_text_vis" title=":geda:gschem_ug.txt ↵" class="wikilink1">Make Inv Text Vis</a> is most appropriate when adding symbols to schematics, to view the text for the symbol's modifiable invisible attributes.<br/>
2017 <strong>Edit | Show/Hide Inv Text</strong> toggles between making all invisible text visible and hiding all invisible text. When selected, all objects in the symbol are effected.<br/>
2019 Visible text always remains visible.<br/>
2022 </p>
2023 <ul>
2025 </li>
2027 </li>
2029 </li>
2031 </li>
2033 </li>
2035 </li>
2037 </li>
2039 </li>
2041 </li>
2043 </li>
2045 </li>
2047 </li>
2049 </li>
2051 </li>
2053 </li>
2055 </li>
2057 </li>
2059 </li>
2061 </li>
2063 </li>
2065 </li>
2066 </ul>
2068 <p>
2070 Not all attributes need to be used to define a symbol (see the discussion of <a href="docs-20060124-gschem_ug-app_a.html" class="wikilink2" title="docs-20060124-gschem_ug-app_a.html">Appendix A -- Heavy vs Light Symbol Libraries</a>). The <strong>gschem</strong> default is to define symbols as “light”, indicating that the symbol includes as few attributes as necessary to describe the symbol. “light” symbols depend on the designer attaching additional descriptive attributes to the symbol when the symbol is placed on the schematic. For example: a “light” symbol for a resistor might include just the graphic for a resistor, its pin attributes, and the “refdes” attribute. This describes a resistor. It would be the designer's responsibility, after the resistor has been placed on the schematic, to add the “value” and “footprint” attributes appropriate for the specific resistor in the circuit. A “heavy” symbol includes more descriptive attributes. Using “light” vs. “heavy” symbols is up to the designer.<br/>
2072 A symbol's attributes may be flagged as either visible or invisible. Attributes are flagged as invisible to reduce the clutter around a symbol on the schematic.<br/>
2074 When creating or editing the symbol, and changing a visible attribute to an invisible attribute, the attribute can not be viewed during further editing of the symbol. It becomes difficult to place attribute text. To view both the visible and invisible text, select <strong>Edit | Show/Hide Inv Text</strong>.<br/>
2076 When a symbol is instantiated on a schematic as a component, only the symbol's visible attributes are promoted to the component. For example: if a resistor's symbol defines “refdes” as the only visible attribute defined in the symbol, the only attribute that the component contains is the “refdes” attribute). Those attributes not included in the symbol definition may be added at the schematic level, component-by-component.<br/>
2078 This operation is useful when drawing/debugging symbols.<br/>
2080 When hidden text is visible, “Show Hidden” will appear on the status-bar in the lower right.
2081 </p>
2083 </div>
2084 <!-- EDIT1087 SECTION "Show/Hide Inv Text (en)" [73465-76292] -->
2085 <h3 class="sectionedit1088"><a name="make_inv_text_vis_ev" id="make_inv_text_vis_ev">Make Inv Text Vis (ev)</a></h3>
2088 <p>
2089 <strong>Edit | Make Inv Text Vis</strong> is a quick method of making all of a component's invisible attributes visible. The same effect can be accomplished by double-clicking on the component and marking all of the entries in the Attributes listbox as “Vis?” (i.e., visible).<br/>
2092 </p>
2093 <ul>
2094 <li class="level1"><div class="li"> Select the component(s) in <strong>Select Mode</strong></div>
2095 </li>
2097 </li>
2098 </ul>
2100 <p>
2102 The attributes that had been hidden are displayed.<br/>
2104 To hide the attributes again, you need to double-click the component to bring up it's “Edit Attributes” dialog box, and explicitly place a check for each attribute you want hidden.
2105 </p>
2107 </div>
2108 <!-- EDIT1088 SECTION "Make Inv Text Vis (ev)" [76293-76956] -->
2112 <p>
2113 <strong>gschem</strong> supports 5 copy/cut/paste buffers which are visible across all opened pages and windows.
2114 </p>
2116 </div>
2117 <!-- EDIT1089 SECTION "Buffer" [76957-77076] -->
2118 <h3 class="sectionedit1090"><a name="copy_into_1_2_3_4_5_yc" id="copy_into_1_2_3_4_5_yc">Copy into 1/2/3/4/5 (yc)</a></h3>
2121 <p>
2122 To copy something into a buffer:
2123 </p>
2124 <ol>
2126 </li>
2128 </li>
2129 </ol>
2131 </div>
2132 <!-- EDIT1090 SECTION "Copy into 1/2/3/4/5 (yc)" [77077-77229] -->
2133 <h3 class="sectionedit1091"><a name="cut_into_1_2_3_4_5_yu" id="cut_into_1_2_3_4_5_yu">Cut into 1/2/3/4/5 (yu)</a></h3>
2136 <p>
2137 Cut is like copy in that it removes the objects from the schematic
2138 </p>
2140 </div>
2141 <!-- EDIT1091 SECTION "Cut into 1/2/3/4/5 (yu)" [77230-77331] -->
2142 <h3 class="sectionedit1092"><a name="paste_from_1_2_3_4_5_yp" id="paste_from_1_2_3_4_5_yp">Paste from 1/2/3/4/5 (yp)</a></h3>
2145 <p>
2146 To paste a buffer into the current schematic:
2147 </p>
2148 <ol>
2150 </li>
2152 </li>
2154 </li>
2155 <li class="level1"><div class="li"> Click the first mouse button to pick an anchor point.</div>
2156 </li>
2158 </li>
2160 </li>
2161 </ol>
2163 </div>
2164 <!-- EDIT1092 SECTION "Paste from 1/2/3/4/5 (yp)" [77332-77685] -->
2168 </div>
2169 <!-- EDIT1093 SECTION "View" [77686-77703] -->
2173 <p>
2176 This is useful when you have mouse/component/line/text etc… droppings left over from a previous action. It is also useful when you want to update all visual connectivity cues.
2177 </p>
2179 </div>
2180 <!-- EDIT1094 SECTION "Redraw (vr)" [77704-77954] -->
2184 <p>
2187 To pan the display:
2188 </p>
2189 <ul>
2191 </li>
2192 <li class="level1"><div class="li"> Click the first mouse button at the new center of the display.</div>
2193 </li>
2194 </ul>
2196 <p>
2198 To pan the display using the shortcut is much simpler, simply place the mouse pointer where you want the display centered and type “x”. The display will jump to the mouse's location.<br/>
2200 Pan behavior is configurable. The system-gschemrc file defines:
2203 </p>
2205 <p>
2206 If you override the system-gschemrc's default, of popping up a menu when the third mouse button is clicked, by adding:
2209 </p>
2211 <p>
2212 to either your user's ~/gschemrc file or local 'pwd'/gschemrc file, the third mouse button (i.e., the right mouse button on scroll-wheel mice) will allow you to pan the schematic by holding down the third mouse button and dragging.<br/>
2214 The system-gschemrc file also defines:
2217 </p>
2219 <p>
2220 If you override the system-gschemrc's default by adding:
2223 </p>
2225 <p>
2226 to either your user's ~/gschemrc file or local 'pwd'/gschemrc file, text will be displayed properly when the third mouse button is held down while dragging. The <code>(third-button “mousepan”)</code> setting must also be applied for this to work. Disabling <code>fast-mousepan</code> adversely effects rendering speed while panning on large “complicated” schematics.<br/>
2228 The system-gschemrc file also defines:
2231 </p>
2233 <p>
2234 If you override the system-gschemrc's default by adding:
2237 </p>
2239 <p>
2240 to either your user's ~/gschemrc file or local 'pwd'/gschemrc file, whenever you zoom in/out, the zoom will NOT center on the mouse pointer, effectively removing the pan feature of the zoom in/out operations.
2241 </p>
2243 </div>
2244 <!-- EDIT1095 SECTION "Pan (x)" [77955-79751] -->
2248 <p>
2249 <strong>View | Zoom Box</strong> allows you to draw a box around a part of the <strong>gschem</strong> window and zoom in.<br/>
2252 </p>
2253 <ul>
2255 </li>
2256 <li class="level1"><div class="li"> Position the mouse pointer at one corner of the box you want to draw</div>
2257 </li>
2259 </li>
2260 <li class="level1"><div class="li"> Drag the mouse, drawing the zoom box around the area to which you want to zoom</div>
2261 </li>
2263 </li>
2264 </ul>
2266 <p>
2268 To use <strong>View | Zoom Box</strong> by typing the equivalent shortcut (i.e., “<strong>w</strong>”) is more convenient. Simply position the mouse pointer at one corner of the zoom box, then type “<strong>w</strong>”. The zoom box will start immediately using the current mouse location as the first corner of the box.<br/>
2270 <strong>View | Zoom Box</strong> will attempt to zoom to the requested area, but some boxes are not legal and <strong>gschem</strong> will do it's best to zoom the requested area.
2271 </p>
2273 </div>
2274 <!-- EDIT1096 SECTION "Zoom Box (w)" [79752-80632] -->
2275 <h3 class="sectionedit1097"><a name="zoom_extents_ve" id="zoom_extents_ve">Zoom Extents (ve)</a></h3>
2278 <p>
2279 <strong>View | Extents</strong> will zoom the display to fit all of the placed objects into the current window.<br/>
2281 To view all of the current window's objects:
2282 </p>
2283 <ul>
2285 </li>
2286 </ul>
2288 <p>
2290 Typing the <strong>View | Extents</strong> shortcut (i.e., “<strong>ve</strong>”) is particularly convenient for those that have learned to navigate the schematics using the shortcuts.<br/>
2292 </p>
2294 </div>
2295 <!-- EDIT1097 SECTION "Zoom Extents (ve)" [80633-80999] -->
2299 <p>
2300 <strong>View | Zoom In</strong> zooms the display in. The current center of the window is the center of the new window. This command zooms in by a factor.<br/>
2302 To zoom in:
2303 </p>
2304 <ul>
2306 </li>
2307 </ul>
2309 <p>
2311 The (zoom-with-pan “enabled”) configuration setting in the gschemrc files effects the operation of the zoom in shortcut (i.e., “<strong>z</strong>”). The default system-gschemrc setting for:
2314 </p>
2316 <p>
2317 enables zooming in, using the mouse pointer's location as the new center of the window. If this changed to:
2320 </p>
2322 <p>
2323 in either your user's ~/gschemrc file or local 'pwd'/gschemrc file, whenever you zoom in, the zoom will NOT center on the mouse pointer but will center on the current center of the window, effectively removing the pan feature of the zoom in operation.<br/>
2325 To zoom in using the shortcut:
2326 </p>
2327 <ul>
2328 <li class="level1"><div class="li"> If the default (zoom-with-pan “enabled”) is configured in one of the gschemrc files, position the mouse pointer in the window where you want the new center</div>
2329 </li>
2331 </li>
2332 </ul>
2334 <p>
2336 Typing “<strong>z</strong>” is particularly convenient for those that have learned to navigate the schematics using the shortcuts.
2337 </p>
2339 </div>
2340 <!-- EDIT1098 SECTION "Zoom In (z)" [81000-82161] -->
2344 <p>
2345 <strong>View | Zoom Out</strong> zooms the display out. The current center of the window is the center of the new window. This command zooms out by a factor.<br/>
2347 To zoom out:
2348 </p>
2349 <ul>
2351 </li>
2352 </ul>
2354 <p>
2356 The (zoom-with-pan “enabled”) configuration setting in the gschemrc files effects the operation of the zoom out shortcut (i.e., “<strong>z</strong>”). The default system-gschemrc setting for:
2359 </p>
2361 <p>
2362 enables zooming out, using the mouse pointer's location as the new center of the window. If this changed to:
2365 </p>
2367 <p>
2368 in either your user's ~/gschemrc file or local 'pwd'/gschemrc file, whenever you zoom out, the zoom will NOT center on the mouse pointer but will center on the current center of the window, effectively removing the pan feature of the zoom out operation.<br/>
2370 To zoom out using the shortcut:
2371 </p>
2372 <ul>
2373 <li class="level1"><div class="li"> If the default (zoom-with-pan “enabled”) is configured in one of the gschemrc files, position the mouse pointer in the window where you want the new center</div>
2374 </li>
2376 </li>
2377 </ul>
2379 <p>
2381 Typing “<strong>Z</strong>” is particularly convenient for those that have learned to navigate the schematics using the shortcuts.
2382 </p>
2384 </div>
2385 <!-- EDIT1099 SECTION "Zoom Out (Z)" [82162-83350] -->
2389 <p>
2390 <strong>View | Zoom Full</strong> will zoom the display to the maximum possible displayable view.<br/>
2392 </p>
2394 <p>
2395 To view the maximum displayable area:
2396 </p>
2397 <ul>
2399 </li>
2400 </ul>
2402 <p>
2404 The window contents will immediately change to show the maximum possible displayable view.<br/>
2406 </p>
2408 <p>
2409 To view the maximum displayable area using the keyboard shortcut (i.e., “<strong>vf</strong>”):
2410 </p>
2411 <ul>
2413 </li>
2414 </ul>
2416 <p>
2418 The window contents will immediately change to show the maximum possible displayable view.<br/>
2420 </p>
2422 <p>
2423 <strong>View | Zoom Full</strong> is useful if you like to put your working notes outside the titleblock for you schematic, for example. Just remember, these notes would now be considered part of the windows extents, so if you were to <strong>View | Extents</strong>, the display would show the titleblock and your working notes.
2424 </p>
2426 </div>
2427 <!-- EDIT1100 SECTION "Zoom Full (vf)" [83351-84129] -->
2431 </div>
2432 <!-- EDIT1101 SECTION "Page" [84130-84148] -->
2436 </div>
2437 <!-- EDIT1102 SECTION "Manager... (pm)" [84149-84176] -->
2441 </div>
2442 <!-- EDIT1103 SECTION "Next (>)" [84177-84197] -->
2446 </div>
2447 <!-- EDIT1104 SECTION "Previous (<)" [84198-84222] -->
2451 </div>
2452 <!-- EDIT1105 SECTION "New (pe)" [84223-84243] -->
2456 </div>
2457 <!-- EDIT1106 SECTION "Revert (pr)" [84244-84267] -->
2461 </div>
2462 <!-- EDIT1107 SECTION "Close (pc)" [84268-84290] -->
2466 </div>
2467 <!-- EDIT1108 SECTION "Discard (pd)" [84291-84315] -->
2471 </div>
2472 <!-- EDIT1109 SECTION "Add" [84316-84332] -->
2476 <p>
2477 <strong>Add | Component…</strong> opens a dialog box which lets you place components from the component libraries.<br/>
2479 To place a component:
2480 </p>
2481 <ul>
2483 </li>
2485 </li>
2487 </li>
2488 <li class="level1"><div class="li"> Confirm the symbol is correct by reviewing the image in the Preview window</div>
2489 </li>
2490 <li class="level1"><div class="li"> Move the mouse into the main drawing window (you should see an outline follow the mouse pointer).</div>
2491 </li>
2493 </li>
2494 <li class="level1"><div class="li"> Position the mouse pointer, and keep pressing the first mouse button to anchor additional instances of the component</div>
2495 </li>
2496 <li class="level1"><div class="li"> When finished anchoring components, press the last mouse button or the ESC key</div>
2497 </li>
2498 </ul>
2500 <p>
2502 If a component name is already selected, hitting apply and moving the mouse into the main window will allow you to place that component again.<br/>
2504 You can rotate the component before you place it by clicking the middle button. For every button click, the component will be rotate counter-clockwise 90 degrees.<br/>
2506 Care has been taken to give components descriptive names in the libraries, though it is sometimes difficult to determine what the component really represents from its name.<br/>
2508 For example: in the analog library there are four capacitor entries:
2509 </p>
2510 <ul>
2512 </li>
2514 </li>
2516 </li>
2518 </li>
2519 </ul>
2521 <p>
2523 It helps to preview the symbol in the “Select Component” dialog box before selecting and placing the symbol.
2524 </p>
2526 </div>
2527 <!-- EDIT1110 SECTION "Component... (i)" [84333-85809] -->
2531 <p>
2534 A net is typically a contiguous set of line segments between two pins, though it is possible to draw nets between a pin and a point on another net, or between two nets.<br/>
2536 For example, the following diagram shows 3 net segments:
2537 </p>
2538 <ul>
2540 </li>
2542 </li>
2544 </li>
2545 </ul>
2548 <td class="col0"> <a href="media/geda/nets.jpg" class="media" target="_blank" title="geda:nets.jpg"><img src="media/geda/nets.jpg" class="media" alt="" /></a> </td>
2549 </tr>
2550 </table></div>
2551 <!-- EDIT1112 TABLE [86157-86179] -->
2552 <p>
2554 Note the small red segment at the end of the resistor's pins. All pins in <strong>gschem</strong> have this red segment. This is the connectivity cue for the pin. It is sometimes difficult to “grab” this attachment point when drawing nets, you may need to zoom in on the pin. To zoom in, press the “z” key. To zoom out, press the “Z” (i.e., shift-z) key.<br/>
2556 To begin drawing a net using the menu:
2557 </p>
2558 <ul>
2560 </li>
2561 <li class="level1"><div class="li"> Zoom in on the component where the net is to start, so that you can easily grab the pin's attachment point</div>
2562 </li>
2563 <li class="level1"><div class="li"> Position the mouse pointer over the pin's connectivity cue</div>
2564 </li>
2566 </li>
2567 </ul>
2569 <p>
2571 To begin drawing the net using the shortcut:
2572 </p>
2573 <ul>
2574 <li class="level1"><div class="li"> Zoom in on the component where the net is to start, so that you can easily grab the pin's attachment point</div>
2575 </li>
2576 <li class="level1"><div class="li"> Position the mouse pointer over the pin's connectivity cue</div>
2577 </li>
2579 </li>
2580 </ul>
2582 <p>
2584 To continue drawing the net segment(s):
2585 </p>
2586 <ul>
2587 <li class="level1"><div class="li"> Drag the mouse pointer in the direction of the end-point</div>
2588 </li>
2589 <li class="level1"><div class="li"> For any necessary 90º turns, single-click the mouse, and continue dragging the mouse pointer toward the end-point</div>
2590 </li>
2591 <li class="level1"><div class="li"> For any necessary non-orthogonal net segments (e.g., 45º angle), hold down the CONTROL button, single-click the mouse, and continue dragging the mouse pointer to the end-point</div>
2592 </li>
2593 <li class="level1"><div class="li"> When you reach the end-point, press the first mouse button to end the net segment</div>
2594 </li>
2596 <ul>
2597 <li class="level2"><div class="li"> If this second pin is to be connected to a third pin, continue as above</div>
2598 </li>
2599 <li class="level2"><div class="li"> If this is the end of the connections, press the last mouse button (or ESC) to end the net</div>
2600 </li>
2601 </ul>
2602 </li>
2603 </ul>
2605 <p>
2607 Press the last mouse button or ESC to cancel any net in progress.<br/>
2609 If the net is cancelled you are automatically placed in <strong>Select Mode</strong>. You must pick <strong>Add | Net</strong> again or type the shortcut to add more nets.<br/>
2611 You cannot connect a net segment to the middle of a non-orthogonal net.<br/>
2613 The boxes at the end of the nets are connectivity cues. Red boxes signify a dangling net (not connected to anything).<br/>
2615 Filled circles are midpoint connections/junctions. These cues are drawn automatically and are an indicator of electrical connectivity.<br/>
2617 See <a href="docs-20060124-gschem_ug-electrical_connectivity.html" class="wikilink2" title="docs-20060124-gschem_ug-electrical_connectivity.html">Electrical Connectivity</a> for more information.
2618 </p>
2620 </div>
2621 <!-- EDIT1111 SECTION "Net (n)" [85810-88401] -->
2625 <p>
2626 <strong>Add | Bus</strong> is basically the same as <strong>Add | Net</strong>, except that it draws buses.<br/>
2628 Buses are very new and there are many aspects which are not defined yet, so keep that in mind as you uses buses. More to be added here eventually.
2629 </p>
2631 </div>
2632 <!-- EDIT1113 SECTION "Bus (u)" [88402-88651] -->
2633 <h3 class="sectionedit1114"><a name="attribute_aa" id="attribute_aa">Attribute... (aa)</a></h3>
2636 <p>
2637 <strong>Add | Attribute…</strong> is appropriate when creating or editing symbols, to add a new attribute.<br/>
2639 <strong>Add | Attribute…</strong> brings up the “Single Attribute Editor” dialog box. This dialog box is ONLY used to add attributes. It does not display or manipulate already placed attributes.<br/>
2641 An attribute is nothing more than a text item which is in the form <code>name=value</code> (there cannot be any spaces to the left or right of the name,value pair). It can be either attached to an object, or unattached.<br/>
2643 To add an unattached attribute (e.g., “comment”, “documentation”, etc.) to the symbol:
2644 </p>
2645 <ul>
2647 </li>
2648 <li class="level1"><div class="li"> Select an attribute name off of the pulldown list, or type the attribute name into the name entry</div>
2649 </li>
2651 </li>
2653 </li>
2655 </li>
2656 </ul>
2658 <p>
2660 If you want to attach an attribute to an object, then select the desired object first and then <strong>Add | Attribute…</strong> from the pull-down menu. If you click on an object which has attached attributes, the attached attributes should be selected as well.<br/>
2662 If you select <strong>Add | Attribute…</strong> off of the pull down menus then you do not have much control as to where the attribute gets placed (it gets places either at the lower left hand corner of the object extents or at the origin of any selected object). However, if you use the hot key (i.e., “aa”) then the current mouse position is used as the anchor point for the attribute item.<br/>
2664 You cannot place an incomplete attribute (an attribute without a name and value).<br/>
2666 Please see <a href="docs-20060124-gschem_ug-components_symbols_objects_attributes.html" class="wikilink2" title="docs-20060124-gschem_ug-components_symbols_objects_attributes.html">Components/Symbols/Objects/Attributes</a> for more info on how to use attributes.
2667 </p>
2669 </div>
2670 <!-- EDIT1114 SECTION "Attribute... (aa)" [88652-90364] -->
2674 <p>
2676 To place text:
2677 </p>
2678 <ul>
2679 <li class="level1"><div class="li"> Select <strong>Options | Text Size…</strong> and select the size for the text</div>
2680 </li>
2682 </li>
2683 <li class="level1"><div class="li"> Type the text in the entry field (multiple lines may be entered by pressing Enter)</div>
2684 </li>
2686 </li>
2687 <li class="level1"><div class="li"> Move the mouse into the main window (an outline of the text should appear and follow the mouse)</div>
2688 </li>
2690 </li>
2692 </li>
2693 </ul>
2695 <p>
2697 If you leave the <strong>Add | Text…</strong> dialog box open you can place the same text item again and again by just clicking Apply (or pressing Enter) and moving the mouse into the main window.<br/>
2699 The following settings in the system-gschemrc file, the user's ~/gschemrc file, or the local 'pwd'/gschemrc file control how text is displayed:
2701 </p>
2702 <pre class="code lisp"><pre class="code lisp"><span class="co1">; text-origin-marker : Controls if the text origin markers are displayed.</span>
2704 <span class="co1">; text-caps-style : Sets the default caps style used for the display of text</span>
2705 <span class="co1">; output-text : Controls how text is rendered to postscript</span></pre></pre>
2707 <p>
2708 Text which is placed will be automatically capitalized. Please see the Resource file section below on how to control this behavior.<br/>
2710 To cancel a text place press the last mouse button or the ESC key.<br/>
2712 If you create text in the form name=value, then you are creating attributes. gEDA allows for general attributes to be free floating (or unattached). It is a good idea to change the color of these floating attributes to the current attribute color (which is also called the attached attribute color) to signify that this text item is an attribute.<br/>
2714 You can rotate the text before you place it by clicking the middle button. For every button click, the text will be rotate 90 degrees.<br/>
2716 </p>
2718 </div>
2719 <!-- EDIT1115 SECTION "Text... (at)" [90365-92168] -->
2723 <p>
2726 To draw a line:
2727 </p>
2728 <ul>
2729 <li class="level1"><div class="li"> If you want to snap the line to the grid, set the grid spacing by selecting <strong>Options | Snap Grid Spacing…</strong> and entering the grid spacing, and then selecting <strong>Options | Toggle Snap On/Off</strong> until you don't see “Snap Off” on the status-bar</div>
2730 </li>
2732 </li>
2733 <li class="level1"><div class="li"> If you want to constrain the line to 90º movements, hold the CONTROL key down while moving the mouse</div>
2734 </li>
2736 </li>
2738 </li>
2740 </li>
2741 <li class="level1"><div class="li"> When positioned at the end-point, press the first mouse button</div>
2742 </li>
2743 <li class="level1"><div class="li"> Continue placing lines, until you either press the second mouse button or type the Escape key</div>
2744 </li>
2745 </ul>
2747 <p>
2749 <strong>Add | Line</strong> draws a line in the same fashion as drawing nets with the following exceptions:
2750 </p>
2751 <ul>
2753 </li>
2755 </li>
2756 <li class="level1"><div class="li"> You keep drawing lines as long as you are in line <strong>Line Mode</strong>.</div>
2757 </li>
2758 </ul>
2760 <p>
2762 To cancel a line in progress, press the last mouse button or type the ESC key.
2763 </p>
2765 </div>
2766 <!-- EDIT1116 SECTION "Line (l)" [92169-93255] -->
2770 <p>
2772 To draw a box:
2773 </p>
2774 <ul>
2775 <li class="level1"><div class="li"> If you want to snap the box to the grid, set the grid spacing by selecting <strong>Options | Snap Grid Spacing…</strong> and entering the grid spacing, and then selecting <strong>Options | Toggle Snap On/Off</strong> until you don’t see “Snap Off” on the status-bar</div>
2776 </li>
2778 </li>
2780 </li>
2782 </li>
2784 </li>
2785 <li class="level1"><div class="li"> When positioned at the end-point, press the first mouse button again</div>
2786 </li>
2787 <li class="level1"><div class="li"> Continue placing boxes, until you either press the second mouse button or type the ESC key</div>
2788 </li>
2789 </ul>
2791 <p>
2793 To cancel a box in progress, press the last mouse button or type the ESC key.<br/>
2795 A box has no electrical significance.
2796 </p>
2798 </div>
2799 <!-- EDIT1117 SECTION "Box (b)" [93256-94008] -->
2803 <p>
2806 To draw a circle:
2807 </p>
2808 <ul>
2809 <li class="level1"><div class="li"> If you want to snap the box to the grid, set the grid spacing by selecting <strong>Options | Snap Grid Spacing…</strong> and entering the grid spacing, and then selecting <strong>Options | Toggle Snap On/Off</strong> until you don’t see “Snap Off” on the status-bar</div>
2810 </li>
2812 </li>
2814 </li>
2816 </li>
2818 </li>
2820 </li>
2821 <li class="level1"><div class="li"> Continue placing circles, until you either press the second mouse button or type the ESC key</div>
2822 </li>
2823 </ul>
2825 <p>
2827 To draw a circle (typing the shortcut), same as above except that you position the mouse pointer to the center-point of the circle before you type the shortcut.<br/>
2829 To cancel a circle in progress, press the last mouse button or the ESC key.<br/>
2831 </p>
2833 </div>
2834 <!-- EDIT1118 SECTION "Circle (ai)" [94009-94893] -->
2838 <p>
2840 To draw an arc:
2841 </p>
2842 <ul>
2843 <li class="level1"><div class="li"> If you want to snap the box to the grid, set the grid spacing by selecting <strong>Options | Snap Grid Spacing…</strong> and entering the grid spacing, and then selecting <strong>Options | Toggle Snap On/Off</strong> until you don’t see “Snap Off” on the status-bar</div>
2844 </li>
2846 </li>
2847 <li class="level1"><div class="li"> Place the mouse pointer at the center-point for the arc</div>
2848 </li>
2850 </li>
2851 <li class="level1"><div class="li"> Move the mouse to the right, to define the radius of the arc</div>
2852 </li>
2854 </li>
2855 <li class="level1"><div class="li"> Enter the Start Angle (in degrees) – 0º is the “x” axis</div>
2856 </li>
2857 <li class="level1"><div class="li"> Enter the Degrees of Sweep (for counter-clockwise sweep)</div>
2858 </li>
2860 </li>
2861 <li class="level1"><div class="li"> Continue placing arcs, until you either press the second mouse button or type the ESC key</div>
2862 </li>
2863 </ul>
2865 <p>
2867 The Start Angle can be positive or negative. The degrees are specified using the standard Cartesian coordinate system. The degrees of sweep can be positive or negative.<br/>
2869 To cancel an arc in progress (while rubberband the radius), press the last mouse button or the ESC key or press the Cancel button in the arc dialog box.
2870 </p>
2872 </div>
2873 <!-- EDIT1119 SECTION "Arc (ar)" [94894-95986] -->
2877 <p>
2880 Though you can <strong>Add | Pin</strong> while entering a schematic, it only makes sense to create pins while creating or editing symbol files.<br/>
2882 To draw a pin:
2883 </p>
2884 <ul>
2885 <li class="level1"><div class="li"> Set the grid spacing by selecting <strong>Options | Snap Grid Spacing…</strong> and entering the grid spacing, and then selecting <strong>Options | Toggle Snap On/Off</strong> until you don’t see “Snap Off” on the status-bar. The <a href="http://www.geda.seul.org/docs/current/symbols/symbols.pdf" class="urlextern" title="http://www.geda.seul.org/docs/current/symbols/symbols.pdf" rel="nofollow">gEDA/gaf Symbol Creation Document</a> specifies grid settings for pin placement in gEDA/gaf compliant symbols files.</div>
2886 </li>
2888 </li>
2890 </li>
2892 </li>
2894 </li>
2895 <li class="level1"><div class="li"> Move the mouse in the intended direction. The <a href="http://www.geda.seul.org/docs/current/symbols/symbols.pdf" class="urlextern" title="http://www.geda.seul.org/docs/current/symbols/symbols.pdf" rel="nofollow">gEDA/gaf Symbol Creation Document</a> specifies the length of pins in gEDA/gaf compliant symbol files.</div>
2896 </li>
2897 <li class="level1"><div class="li"> When positioned at the end-point, press the first mouse button</div>
2898 </li>
2899 <li class="level1"><div class="li"> Continue placing pins, until you either press the second mouse button or type the Escape key</div>
2900 </li>
2901 </ul>
2903 <p>
2905 To cancel a pin in progress, press the last mouse button or the ESC key.
2906 </p>
2908 </div>
2909 <!-- EDIT1120 SECTION "Pin (ap)" [95987-97174] -->
2913 <p>
2915 To draw a picture:
2916 </p>
2917 <ul>
2918 <li class="level1"><div class="li"> If you want to snap the picture to the grid, set the grid spacing by selecting <strong>Options | Snap Grid Spacing…</strong> and entering the grid spacing, and then selecting <strong>Options | Toggle Snap On/Off</strong> until you don’t see “Snap Off” on the status-bar</div>
2919 </li>
2921 </li>
2922 <li class="level1"><div class="li"> Select the graphic file from the “Please select a picture file” dialog box</div>
2923 </li>
2925 </li>
2927 </li>
2929 </li>
2930 <li class="level1"><div class="li"> Move the mouse in the intended direction. The outline of the picture will appear, retaining the aspect ratio of the original picture.</div>
2931 </li>
2932 <li class="level1"><div class="li"> When positioned at the end-point, press the first mouse button again.</div>
2933 </li>
2934 <li class="level1"><div class="li"> Continue placing pictures, until you either press the second mouse button or type the ESC key</div>
2935 </li>
2936 </ul>
2938 <p>
2940 To cancel a picture in progress, press the last mouse button or type the ESC key.<br/>
2942 A picture has no electrical significance.
2943 </p>
2945 </div>
2946 <!-- EDIT1121 SECTION "Picture... (ag)" [97175-98170] -->
2950 </div>
2951 <!-- EDIT1122 SECTION "Hierarchy" [98171-98193] -->
2952 <h3 class="sectionedit1123"><a name="down_schematic_hd" id="down_schematic_hd">Down Schematic (Hd)</a></h3>
2955 <p>
2956 <strong>Hierarchy | Down Schematic</strong> shifts the focus from the current schematic to a sub-schematic.<br/>
2958 Go down into a symbol, opening up any underlying schematics. Basically this will open up an underlying schematic of the selected component if it exists in the source library search path. See the Resource File section on how to define this path.<br/>
2960 There are currently two ways of specifying that a symbol has an underlying schematic or schematics:
2961 </p>
2962 <ol>
2963 <li class="level1"><div class="li"> The underlying schematic must have the same name as the symbol but have a .sch extension and must follow the _# suffix naming convention. See the Files section below on this convention.</div>
2964 </li>
2965 <li class="level1"><div class="li"> Attach an attribute to the symbol called source=filename.sch filename.sch is not a path to the symbol, but rather the basename (last file in the path specifier) of the symbol path. The underlying schematic will still be searched in the source-library path. You can specify multiple source= attributes. The underlying schematics will be opened in the order that the source= attribute is found.</div>
2966 </li>
2967 </ol>
2969 <p>
2971 If there multiple underlying schematics, they will be loaded. Movement between the schematic pages is restricted (to the same level of the same set of underlying schematics) unless the rc keyword enforce-hierarchy is modified to allow for a freer hierarchy traversal mode. See the Resource File section for more info.<br/>
2973 It is also recommend that you maintain unique names for the various levels (when using the source= attribute) to avoid possible confusion. The hierarchy mechanisms are fairly new so expect some odd behavior (and please report it)
2974 </p>
2976 </div>
2977 <!-- EDIT1123 SECTION "Down Schematic (Hd)" [98194-99806] -->
2978 <h3 class="sectionedit1124"><a name="down_symbol_hs" id="down_symbol_hs">Down Symbol (Hs)</a></h3>
2981 <p>
2982 This option will open up the symbol of the selected component.<br/>
2984 Once the symbol is open, the user can edit it and save it.<br/>
2986 At this time, the toplevel schematic will not see the symbol change unless the toplevel schematic is reloaded or File/Revert is executed. This will be fixed eventually.
2987 </p>
2989 </div>
2990 <!-- EDIT1124 SECTION "Down Symbol (Hs)" [99807-100129] -->
2994 <p>
2995 This option will move up the hierarchy (if there are pages above the currently displayed page).
2996 </p>
2998 </div>
2999 <!-- EDIT1125 SECTION "Up (Hu)" [100130-100244] -->
3000 <h3 class="sectionedit1126"><a name="documentation_ho" id="documentation_ho">Documentation (Ho)</a></h3>
3003 <p>
3004 Open any documentation available for the selected symbol/component.<br/>
3006 The job is handed over to “gschemdoc”, which makes a best-effort attempt of finding relevant documentation.<br/>
3008 The documention would normally be in <acronym title="Portable Document Format">PDF</acronym>, <acronym title="HyperText Markup Language">HTML</acronym>, text or image format, but gschemdoc tries to be as transparent as possible on this account.<br/>
3010 First and foremost, the attribute “documentation=” is assumed to point to the documentation. This attribute should either be the filename (basename) of the document, or it should be a complete <acronym title="Uniform Resource Locator">URL</acronym>.<br/>
3012 If it is a filename, and the file is found locally (in /usr/share/gEDA/documentation or otherwise), the relevant viewer will be initiated. Otherwise, a Google search for the document will be initiated.<br/>
3014 If there is no documentation attribute, the attributes “device” and possibly “value” will be consulted in much the same way as for “documentation”. File searches will be made in forms of filenames like “device-value.pdf” and “device.pdf”.<br/>
3016 Failing that, the file name for the symbol itself will be used as basis for the search.
3017 </p>
3019 </div>
3020 <!-- EDIT1126 SECTION "Documentation (Ho)" [100245-101329] -->
3024 </div>
3025 <!-- EDIT1127 SECTION "Attributes" [101330-101353] -->
3029 <p>
3030 The Attach command allows you to take a text item (in the proper form; <code>name=value</code>) and attach it to another object.<br/>
3032 To use Attributes/Attach:
3033 </p>
3034 <ol>
3036 </li>
3037 <li class="level1"><div class="li"> Select the text object(s) which will be attached to the above object</div>
3038 </li>
3040 </li>
3041 </ol>
3043 <p>
3045 The order of the sequence of selecting the object and then the text items is important; <strong>gschem</strong> will not allow you to select the text items first and then the object. After going through the above sequence the text item will turn yellow (or the current attached attribute color) signifying that the text item is an attached attribute.<br/>
3047 You cannot attach a single attribute to several different objects. You cannot attach non-text items as attributes.
3048 </p>
3050 </div>
3051 <!-- EDIT1128 SECTION "Attach (ta)" [101354-102161] -->
3055 <p>
3056 Detach allows you to deassociate attributes from objects.<br/>
3058 To deselect an object of all attributes:
3059 </p>
3060 <ol>
3062 </li>
3064 </li>
3065 </ol>
3067 <p>
3069 All the attached attributes (even if they are not selected) will be detached from the object. This behavior is probably broken and will eventually be fixed (so that only selected attributes are detached).<br/>
3071 When you detach attributes then they turn red (or the current detached attribute color). This color changes allows you to spot text which was an attribute and is now dangling (unattached).
3072 </p>
3074 </div>
3075 <!-- EDIT1129 SECTION "Detach (td)" [102162-102768] -->
3076 <h3 class="sectionedit1130"><a name="show_value_tv" id="show_value_tv">Show Value (tv)</a></h3>
3079 <p>
3080 These operations allow you to control which part of the attribute string is visible. Usually you are just interested in seeing the <code>value</code> of the attribute, but there are circumstances where seeing the <code>name</code> and <code>value</code> (or maybe just the <code>name</code>) would be useful.<br/>
3082 To use the options:
3083 </p>
3084 <ol>
3086 </li>
3088 </li>
3089 </ol>
3091 <p>
3093 The text item(s) should immediately change.<br/>
3096 </p>
3098 </div>
3099 <!-- EDIT1130 SECTION "Show Value (tv)" [102769-103307] -->
3103 <p>
3104 These operations allow you to control which part of the attribute string is visible. Usually you are just interested in seeing the <code>value</code> of the attribute, but there are circumstances where seeing the <code>name</code> and <code>value</code> (or maybe just the <code>name</code>) would be useful.<br/>
3106 To use the options:
3107 </p>
3108 <ol>
3110 </li>
3112 </li>
3113 </ol>
3115 <p>
3117 The text item(s) should immediately change.<br/>
3120 </p>
3122 </div>
3123 <!-- EDIT1131 SECTION "Show Name (tn)" [103308-103845] -->
3127 <p>
3128 These operations allow you to control which part of the attribute string is visible. Usually you are just interested in seeing the <code>value</code> of the attribute, but there are circumstances where seeing the <code>name</code> and <code>value</code> (or maybe just the <code>name</code>) would be useful.<br/>
3130 To use the options:
3131 </p>
3132 <ol>
3134 </li>
3136 </li>
3137 </ol>
3139 <p>
3141 The text item(s) should immediately change.<br/>
3144 </p>
3146 </div>
3147 <!-- EDIT1132 SECTION "Show Both (tb)" [103846-104383] -->
3148 <h3 class="sectionedit1133"><a name="toggle_visibility_tt" id="toggle_visibility_tt">Toggle Visibility (tt)</a></h3>
3151 <p>
3152 This operation allows you to toggle the visibility of attributes.<br/>
3154 To use this option:
3155 </p>
3156 <ol>
3158 </li>
3160 </li>
3161 </ol>
3163 <p>
3165 The text item(s) should change their visibility immediately.<br/>
3167 If you make an attached attribute invisible, then you can simply select the parent object and select Toggle Vis and the attribute will be come visible (likewise any visible attributes attached to that object will become invisible).<br/>
3169 If you make a free floating (unattached) attribute invisible, then the only way to make it visible (and all other invisible attributes) is to use the Edit/Show Hidden Text option.
3170 </p>
3172 </div>
3173 <!-- EDIT1133 SECTION "Toggle Visibility (tt)" [104384-105079] -->
3174 <h3 class="sectionedit1134"><a name="find_specific_text_t_shift-f" id="find_specific_text_t_shift-f">Find Specific Text... (t shift-f)</a></h3>
3177 <p>
3179 This operation allows you to find a text element in a schematic.
3180 </p>
3182 <p>
3183 To use this operation:
3184 </p>
3185 <ol>
3186 <li class="level1"><div class="li"> open the dialog and enter the substring you want to search for</div>
3187 </li>
3188 <li class="level1"><div class="li"> select whether you only want to search in the current page or in the whole hierarchy of a multipage schematic</div>
3189 </li>
3191 </li>
3192 </ol>
3194 <p>
3196 If the text is found in the schematic, gschem will zoom and pan to that element. Pressing the find button again will find the next matching text element.
3197 If no more text is found the dialog closes.
3198 </p>
3200 <p>
3201 <strong>Note:</strong> gschem will find hidden text elements, too. If you don't see the found element, try to show the hidden text.
3202 </p>
3204 </div>
3205 <!-- EDIT1134 SECTION "Find Specific Text... (t shift-f)" [105080-105740] -->
3206 <h3 class="sectionedit1135"><a name="hide_specific_text_th" id="hide_specific_text_th">Hide Specific Text... (th)</a></h3>
3209 <p>
3211 This operation allows you to hide text elements.
3212 </p>
3214 <p>
3215 To use this operation:
3216 </p>
3217 <ol>
3219 </li>
3221 </li>
3222 </ol>
3224 <p>
3226 gschem will hide all text elements that start with the given search string.
3227 </p>
3229 <p>
3230 This operation is useful if you like to hide pintype and pinseq attributes when creating symbols.
3231 </p>
3233 </div>
3234 <!-- EDIT1135 SECTION "Hide Specific Text... (th)" [105741-106102] -->
3235 <h3 class="sectionedit1136"><a name="show_specific_text_t_shift-h" id="show_specific_text_t_shift-h">Show Specific Text... (t shift-h)</a></h3>
3238 <p>
3240 This operation allows you to show hidden text elements.
3241 </p>
3243 <p>
3244 To use this operation:
3245 </p>
3246 <ol>
3248 </li>
3250 </li>
3251 </ol>
3253 <p>
3255 gschem will unhide all hidden text elements that starts with the given search string.
3256 </p>
3258 <p>
3259 This operation is useful if you like to see only one specific attribute in the whole schematic (the footprint attribute for example).
3261 </p>
3263 </div>
3264 <!-- EDIT1136 SECTION "Show Specific Text... (t shift-h)" [106103-106594] -->
3265 <h3 class="sectionedit1137"><a name="autonumber_text_tu" id="autonumber_text_tu">Autonumber Text... (tu)</a></h3>
3268 <p>
3270 This operation allows you to renumber text elements in your schematics and symbols.
3271 </p>
3273 <p>
3274 You can use it to:
3275 </p>
3276 <ul>
3277 <li class="level1"><div class="li"> renumber pinseq and pinnumber attributes when creating symbols</div>
3278 </li>
3279 <li class="level1"><div class="li"> renumber components in a schematic (the refdes attribute)</div>
3280 </li>
3282 </li>
3283 </ul>
3285 <p>
3287 To use that operation:
3289 </p>
3290 <ol>
3291 <li class="level1"><div class="li"> select or enter the text elements you like to renumber in the <em>search for</em> entry. searchtext with a ”?” at the end will match trailing ”?” and trailing numbers in the text elements you are searching for. searchtext with a “*” at the end will match the given searchtext, followed by arbitrary text and followed by a trailing ”?” or trailing numbers.</div>
3292 </li>
3293 <li class="level1"><div class="li"> the <em>autonumber text in</em> option specifies where to search for the given searchstring.</div>
3294 </li>
3295 <li class="level1"><div class="li"> the <em>skip numbers found in</em> option specifies in which region you don't want have duplicate numbers. <strong>Example:</strong> If you renumber your components you usually want uniq numbers on a page or even uniq number in the whole hierarchy of a multipage schematic. If you renumber netnames of a bus you usually want to apply the new numbers only to selected net elements. Thus you can have multiple equal netnames on a schematic sheet.</div>
3296 </li>
3297 <li class="level1"><div class="li"> the <em>overwrite existing numbers</em> option specifies whether you only want to number unnumbered elements or if you like to renumber elements too.</div>
3298 </li>
3299 <li class="level1"><div class="li"> The <em>starting number</em> entry allows you to specify the start number you like. It is common to number each schematic sheet starting with numbers like 100, 200 and so on. For bus netnames you may need numbers starting at 8, 16.</div>
3300 </li>
3301 <li class="level1"><div class="li"> The <em>sort order</em> tells in which direction you like to number your elements. For components you usually use the <em>diagonal</em>, the <em>top to bottom</em> or the <em>left to right</em> option. For bus netnames you may need <em>right to left</em> and <em>bottom to top</em> numbering. The <em>file order</em> means that the found text elements are not sorted before renumbering them. The fileorder is usually the order you have placed the objects to your sheet.</div>
3302 </li>
3303 <li class="level1"><div class="li"> the <em>remove numbers</em> options is a special option. It removes all numbers from the text elements you have selected in the <em>Scope</em> section of the dialog.</div>
3304 </li>
3305 <li class="level1"><div class="li"> the <em>automatic slotting</em> option is the second special option. When renumbering components it will add the slot attribute to slotted components like logik gates.</div>
3306 </li>
3307 </ol>
3309 <p>
3311 Pressing the apply button will start the autonumbering action.
3312 </p>
3314 </div>
3315 <!-- EDIT1137 SECTION "Autonumber Text... (tu)" [106595-109032] -->
3319 </div>
3320 <!-- EDIT1138 SECTION "Options" [109033-109053] -->
3321 <h3 class="sectionedit1139"><a name="text_size_ot" id="text_size_ot">Text Size... (ot)</a></h3>
3324 <p>
3325 <strong>Options | Text Size…</strong> pops up a dialog box which allows you to specify the text size of all text (including attributes placed with the Add/Attribute… dialog box).<br/>
3327 The text size is in points (1/72”). The default text size is 10 point text. The smallest text size is 2 points.
3328 </p>
3330 </div>
3331 <!-- EDIT1139 SECTION "Text Size... (ot)" [109054-109366] -->
3332 <h3 class="sectionedit1140"><a name="toggle_grid_on_off_og" id="toggle_grid_on_off_og">Toggle Grid On/Off (og)</a></h3>
3335 <p>
3337 </p>
3339 </div>
3340 <!-- EDIT1140 SECTION "Toggle Grid On/Off (og)" [109367-109460] -->
3341 <h3 class="sectionedit1141"><a name="toggle_snap_on_off_os" id="toggle_snap_on_off_os">Toggle Snap On/Off (os)</a></h3>
3344 <p>
3345 <strong>Options | Toggle Snap On/Off</strong> toggles the snap. Be very careful using this. Connections between pins and nets (and nets to nets) depends on being exactly connected. Turning of the grid will almost guarantee that nets/pins do not connect.<br/>
3347 Before you translate a symbol using Edit/Symbol Translate, make sure the snap is on.<br/>
3349 When snap mode is off, the text “Snap Off” will appear in the lower, righthand corner.
3350 </p>
3352 </div>
3353 <!-- EDIT1141 SECTION "Toggle Snap On/Off (os)" [109461-109912] -->
3354 <h3 class="sectionedit1142"><a name="snap_grid_spacing_os" id="snap_grid_spacing_os">Snap Grid Spacing... (oS)</a></h3>
3357 <p>
3358 <strong>Options | Snap Grid Spacing…</strong> brings up a dialog box which allows you to change the snap grid spacing (not the grid spacing). The units for this spacing are mils.<br/>
3360 Before you translate a symbol using Edit/Symbol Translate, make sure this spacing is set to 100.
3361 </p>
3363 </div>
3364 <!-- EDIT1142 SECTION "Snap Grid Spacing... (oS)" [109913-110216] -->
3365 <h3 class="sectionedit1143"><a name="toggle_outline_box_oa" id="toggle_outline_box_oa">Toggle Outline/Box (oa)</a></h3>
3368 <p>
3369 <strong>Options | Toggle Outline/Box</strong> toggles between drawing the outline of the current selection or just drawing a box when doing moves/copies/component and text places. The outline mode looks better, but tends to be significantly slower than using the box (bounding box) mode.
3370 </p>
3372 </div>
3373 <!-- EDIT1143 SECTION "Toggle Outline/Box (oa)" [110217-110526] -->
3374 <h3 class="sectionedit1144"><a name="toggle_net_rubberband_or" id="toggle_net_rubberband_or">Toggle Net/Rubberband (or)</a></h3>
3377 <p>
3378 <strong>Options | Toggle Net/Rubberband</strong> This option makes the nets stick to the pins of symbols. It is on by default. When switched off, symbols don't drag on nets when moved.
3379 </p>
3381 </div>
3382 <!-- EDIT1144 SECTION "Toggle Net/Rubberband (or)" [110527-110738] -->
3383 <h3 class="sectionedit1145"><a name="show_log_window_ol" id="show_log_window_ol">Show Log Window (ol)</a></h3>
3386 <p>
3387 <strong>Options | Show Log Window</strong> displays the log window if it has been closed or disabled from being displayed when you start up <strong>gschem</strong>.
3388 </p>
3390 </div>
3391 <!-- EDIT1145 SECTION "Show Log Window (ol)" [110739-110909] -->
3392 <h3 class="sectionedit1146"><a name="show_coord_window_oc" id="show_coord_window_oc">Show Coord Window... (oc)</a></h3>
3395 <p>
3396 <strong>Options | Show Coord Window…</strong> displays a pop-up window that displays the coordinates of the mouse pointer on the schematic. Useful for accurately placing objects.
3397 </p>
3399 </div>
3400 <!-- EDIT1146 SECTION "Show Coord Window... (oc)" [110910-111114] -->
3404 </div>
3405 <!-- EDIT1147 SECTION "Help" [111115-111132] -->
3409 <p>
3410 Every <acronym title="Graphical User Interface">GUI</acronym> application needs an <strong>Help | About…</strong> feature, to display:
3411 </p>
3412 <ul>
3414 </li>
3416 </li>
3418 </li>
3419 </ul>
3421 </div>
3422 <!-- EDIT1148 SECTION "About... (ha)" [111133-111335] -->
3426 <p>
3427 <strong>Help | Manual…</strong> brings up the “gEDA/gaf Documention” web-page installed on this computer. Very useful for accessing the various documentation available for the gEDA/gaf applications.
3428 </p>
3430 </div>
3431 <!-- EDIT1149 SECTION "Manual... (hm)" [111336-111549] -->
3435 <p>
3436 <strong>Help | Hotkeys…</strong> lists the current hotkeys (a.k.a., shortcuts, a.k.a., keyboard accellerators).
3437 </p>
3439 </div>
3440 <!-- EDIT1150 SECTION "Hotkeys... (hh)" [111550-111677] -->
3441 <h3 class="sectionedit1151"><a name="component_ho" id="component_ho">Component... (Ho)</a></h3>
3444 <p>
3445 If you select a component on the schematic, and select <strong>Help | Component…</strong>, <strong>gschem</strong> uses the gschemdoc script to do its best job finding some documentation appropriate for the component:
3446 </p>
3447 <ul>
3448 <li class="level1"><div class="li"> If the component's symbol included the <code>documentation=documentation_locator</code> attribute, this <acronym title="Uniform Resource Identifier">URI</acronym> is used to retreive the documentation. If the full <acronym title="Uniform Resource Identifier">URI</acronym> is given, the <acronym title="Uniform Resource Identifier">URI</acronym> on the internet is retrieved. If the <acronym title="Uniform Resource Identifier">URI</acronym> is not fully qualified, it is considered to be local to this computer, and is searched for and displayed.</div>
3449 </li>
3450 <li class="level1"><div class="li"> If the component's symbol does not include the <code>documentation=documentation_locator</code> attribute, a Google search is performed for <acronym title="Portable Document Format">PDF</acronym> documents, based on the <code>device=</code> attribute, the <code>value=</code> attribute, and the symbol basename.</div>
3451 </li>
3452 </ul>
3454 </div>
3455 <!-- EDIT1151 SECTION "Component... (Ho)" [111678-112460] -->
3456 <h1 class="sectionedit1152"><a name="appendix_a_--_heavy_vs_light_symbol_libraries" id="appendix_a_--_heavy_vs_light_symbol_libraries">Appendix A -- Heavy vs Light Symbol Libraries</a></h1>
3459 <p>
3460 A short discussion of Light Symbol Libraries as the default for <strong>gschem</strong>, and the option to build your own Heavy Symbol Libraries.
3461 </p>
3463 </div>
3464 <!-- EDIT1152 SECTION "Appendix A -- Heavy vs Light Symbol Libraries" [112461-112654] -->
3465 <h1 class="sectionedit1153"><a name="appendix_b_--_printing_schematics_and_symbols" id="appendix_b_--_printing_schematics_and_symbols">Appendix B -- Printing Schematics and Symbols</a></h1>
3468 <p>
3469 To be supplied…
3470 </p>
3472 </div>
3473 <!-- EDIT1153 SECTION "Appendix B -- Printing Schematics and Symbols" [112655-112733] -->
3474 <h1 class="sectionedit1154"><a name="appendix_c_--_writing_guile_scripts" id="appendix_c_--_writing_guile_scripts">Appendix C -- Writing guile Scripts</a></h1>
3477 <p>
3478 To be supplied…
3479 </p>
3481 </div>
3482 <!-- EDIT1154 SECTION "Appendix C -- Writing guile Scripts" [112734-112802] -->
3483 <h1 class="sectionedit1155"><a name="appendix_d_--_i_want_to_build_a_printed_circuit_board" id="appendix_d_--_i_want_to_build_a_printed_circuit_board">Appendix D -- I Want To Build A Printed Circuit Board</a></h1>
3486 <p>
3488 </p>
3489 <ul>
3490 <li class="level1"><div class="li"> Circuit design intended for production of Printed Circuit Boards (PCBs).</div>
3491 </li>
3493 </li>
3494 </ul>
3496 <p>
3498 The following guidelines will assist you in developing quality designs intended for use by applications that support the creation of Printed Circuit Boards:
3499 </p>
3500 <ul>
3502 </li>
3503 </ul>
3505 <p>
3507 The following on-line tutorials are an excellent method for the beginner to learn the gEDA Tools Suite design workflow resulting in a PCB:
3508 </p>
3509 <ul>
3510 <li class="level1"><div class="li"> <a href="http://www.geda.seul.org/docs/current/tutorials/gsch2pcb/gschem-warmup.html" class="urlextern" title="http://www.geda.seul.org/docs/current/tutorials/gsch2pcb/gschem-warmup.html" rel="nofollow">Bill Wilson's gschem warmup</a></div>
3511 </li>
3512 <li class="level1"><div class="li"> <a href="http://www.geda.seul.org/docs/current/tutorials/gsch2pcb/tutorial.html" class="urlextern" title="http://www.geda.seul.org/docs/current/tutorials/gsch2pcb/tutorial.html" rel="nofollow">Bill Wilson's gsch2pcb tutorial</a></div>
3513 </li>
3514 </ul>
3516 </div>
3517 <!-- EDIT1155 SECTION "Appendix D -- I Want To Build A Printed Circuit Board" [112803-113592] -->
3518 <h1 class="sectionedit1156"><a name="appendix_e_--_i_want_to_simulate_my_design" id="appendix_e_--_i_want_to_simulate_my_design">Appendix E -- I Want To Simulate My Design</a></h1>
3521 <p>
3523 </p>
3524 <ul>
3525 <li class="level1"><div class="li"> Circuit design intended for production of Printed Circuit Boards.</div>
3526 </li>
3528 </li>
3529 </ul>
3531 <p>
3533 The following guidelines will assist you in developing quality designs intended for simulation:
3534 </p>
3535 <ul>
3536 <li class="level1"><div class="li"> Discuss attributes appropriate for a SPICE model, and how these differ from attributes appropriate for a PCB.</div>
3537 </li>
3539 </li>
3540 </ul>
3542 <p>
3544 The following on-line tutorials are an excellent method for the beginner to learn the gEDA Tools Suite design workflow resulting in a SPICE simulation:
3545 </p>
3546 <ul>
3547 <li class="level1"><div class="li"> <a href="http://www.brorson.com/gEDA/SPICE/t1.html" class="urlextern" title="http://www.brorson.com/gEDA/SPICE/t1.html" rel="nofollow">"Circuit simulation using gEDA and SPICE -- HOWTO" by Stuart Brorson</a></div>
3548 </li>
3549 <li class="level1"><div class="li"> <a href="http://www-mdp.eng.cam.ac.uk/urop05/files/gedalib/starting_gEDA.pdf" class="urlextern" title="http://www-mdp.eng.cam.ac.uk/urop05/files/gedalib/starting_gEDA.pdf" rel="nofollow">Starting with gEDA at the Cambridge University Engineering Department</a></div>
3550 </li>
3551 </ul>
3553 </div>
3554 <!-- EDIT1156 SECTION "Appendix E -- I Want To Simulate My Design" [113593-114472] -->
3555 <h1 class="sectionedit1157"><a name="appendix_f_--_change_gschemdoc_user-defined_preferences" id="appendix_f_--_change_gschemdoc_user-defined_preferences">Appendix F -- Change gschemdoc User-Defined Preferences</a></h1>
3558 <p>
3559 As installed, the <strong>gschemdoc</strong> utility script is used by <strong>gschem</strong> to:
3560 </p>
3561 <ul>
3562 <li class="level1"><div class="li"> Display the “gEDA/gaf Documentation” (i.e., <strong>Help | Manual…</strong>)</div>
3563 </li>
3564 <li class="level1"><div class="li"> Display component documentation (i.e., <strong>Help | Component…</strong>)</div>
3565 </li>
3566 </ul>
3568 <p>
3570 The list of application launchers that <strong>gschemdoc</strong> uses are defined in the {binary-install-path}/bin/gschemdoc file:
3573 # these may be changed to suit local preferences
3574 #
3575 CANDIDATE_BROWSER="galeon mozilla phoenix netscape netscape-navigator opera firefox konqueror"
3578 </p>
3580 <p>
3581 To select a different application launcher, simply edit the {binary-install-path}/bin/gschemdoc file, find the above lines, and move your favorite application to the beginning of the list. For example, to use <strong>firefox</strong> as your preferred browser, move it to the beginning of the <strong>CANDIDATE_BROWSER=</strong> list, to use <strong>acroread</strong> (Adobe's Acrobat Reader) as your preferred <acronym title="Portable Document Format">PDF</acronym> reader, move it to the beginning of the <strong>CANDIDATE_PDFREADER=</strong> list, and to use <strong>locate</strong> as your preferred filesystem search utility, move it to the beginning of the <strong>CANDIDATE_LOCATE=</strong> list.
3582 </p>
3584 </div>
3585 <!-- EDIT1157 SECTION "Appendix F -- Change gschemdoc User-Defined Preferences" [114473-115689] -->
3586 <h1 class="sectionedit1158"><a name="appendix_g_--_breaking_a_large_symbol_into_smaller_symbols" id="appendix_g_--_breaking_a_large_symbol_into_smaller_symbols">Appendix G -- Breaking a Large Symbol Into Smaller Symbols</a></h1>
3589 <p>
3590 To be supplied…
3591 </p>
3593 </div>
3594 <!-- EDIT1158 SECTION "Appendix G -- Breaking a Large Symbol Into Smaller Symbols" [115690-115781] -->
3595 <h1 class="sectionedit1159"><a name="appendix_h_--_definition_of_terms" id="appendix_h_--_definition_of_terms">Appendix H -- Definition of Terms</a></h1>
3598 <p>
3599 Some terms used in the art of schematic capture:</p>
3600 <dl>
3602 <dd>A text item which is in the form <code>name=value</code>. It can be either unattached or attached.</dd>
3606 <dd>Also know as <strong>part</strong>. The equivalent of an [electronics] device, as one may place on a printed circuit board. Components are instances of a <strong>symbol</strong> placed on a schematic.</dd>
3608 <dd>Also known as “package”. The equivalent of an [electronics] device, as one may place on a printed circuit board.</dd>
3614 <dd>Also known as a <strong>land pattern</strong>. The surface space occupied by a <strong>component</strong>/<strong>package</strong>/<strong>part</strong>.</dd>
3616 <dd><strong>gschem</strong> is a component of the gEDA/gaf set of tools, which tend to integrate together in the development and maintenance of schematics and symbols. The term “gaf” stands for “<em class="u">g</em>EDA <em class="u">a</em>nd <em class="u">f</em>riends”).</dd>
3620 <dd><a href="http://www.gnu.org/software/guile/" class="urlextern" title="http://www.gnu.org/software/guile/" rel="nofollow">GNU Guile</a> is an interpreter for Scheme, a version of Lisp.</dd>
3622 <dd>Hardware Description Language (e.g., VHDL, Verilog, etc.). Used to simulate or document a device.</dd>
3624 <dd>The concept that designs can contain nested levels of schematics, so that all the circuit doesn't need to be placed on a single sheet.</dd>
3626 <dd>Also known as a <strong>footprint</strong>. The surface space occupied by a structure or device.</dd>
3630 <dd>A straight drawing element, connecting two points. On the schematic it has no electrical significance. In a symbol, a line is part of the symbol's graphic elements.</dd>
3632 <dd>A description of how a device behaves. Most often this is a SPICE model. The model is defined in <strong>gschem</strong>, but used in subsequent applications such as <strong>ngspice</strong>, <strong>gnucap</strong>, etc.</dd>
3634 <dd>A net connects two or more pins on a schematic, and is made up of segments. The net's equivalent is a “wire” or “trace” on the printed circuit board.</dd>
3638 <dd>Also known as <strong>device</strong>. The equivalent of an [electronics] device, as one may place on a printed circuit board.</dd>
3642 <dd> Also know as <strong>component</strong>. The equivalent of an [electronics] device, as one may place on a printed circuit board.</dd>
3648 <dd>A <strong>page</strong>/<strong>sheet</strong> with electronics symbols, text, and drawing elements (i.e., lines, circles, boxes, etc.) representing a diagram of an electrical or mechanical system.</dd>
3650 <dd>A collection of schematics which share a common basename (e.g., schematic_1.sch, schematic_2.sch, schematic_3.sch, etc.). The series basename ties schematics together.</dd>
3652 <dd>Also known as a <strong>slotted package</strong>. A physical [electronics] device consisting of multiple identical components (e.g., the 7400 quad NAND device consists of 4 identical NAND gates).</dd>
3654 <dd>A schematic, HDL code, or model which implements, describes, or documents some aspect of the project.</dd>
3656 <dd>A collection of <strong>objects</strong>. The objects may have <strong>attributes</strong> attatched (i.e., associated) with them. There may also be <strong>attributes</strong> attached (i.e., associated) to the <strong>symbol</strong> itself (i.e., not specifically associated with an object).</dd>
3664 <dd>The process of designing. Usually includes continuous review and re-design, until it works. In the gEDA Tools Suite design workflow, multiple applications are used. One application typically is followed by another. The flow of data collected and how this data effects the design is considered the workflow.</dd>
3665 </dl>
3666 <p>~~DISCUSSION~~
3668 </p>
3670 </div>
3672 </html>