<!DOCTYPE html PUBLIC "-//W3C//DTD XHTML 1.0 Transitional//EN"
"http://www.w3.org/TR/xhtml1/DTD/xhtml1-transitional.dtd">
<html>
<head>
<title></title>
<link rel="stylesheet" media="screen" type="text/css" href="./style.css" />
<link rel="stylesheet" media="screen" type="text/css" href="./design.css" />
<link rel="stylesheet" media="print" type="text/css" href="./print.css" />
<meta http-equiv="Content-Type" content="text/html; charset=utf-8" />
</head>
<body>
<h1 class="sectionedit27"><a name="net_attribute_mini-howto" id="net_attribute_mini-howto">net= attribute mini-HOWTO</a></h1>
<div class="level1">
<p>
by: Ales Hvezda
</p>
<p>
This document is released under <a href="http://www.gnu.org/copyleft/fdl.html" class="urlextern" title="http://www.gnu.org/copyleft/fdl.html" rel="nofollow">GFDL</a>
</p>
<p>
October 2nd, 2003
</p>
<p>
The information in this document is current as of 19991011.
</p>
</div>
<!-- EDIT27 SECTION "net= attribute mini-HOWTO" [1-216] -->
<h2 class="sectionedit28"><a name="what_is_the_net_attribute_used_for" id="what_is_the_net_attribute_used_for">What is the net= attribute used for?</a></h2>
<div class="level2">
<p>
The <strong><code>net=</code></strong> attribute is used to specify power, ground, and/or arbitrary nets in the gEDA system.<br/>
The <strong><code>net=</code></strong> attribute is used instead some of the other systems of specifying power/ground (such as having power/ground pins on symbols or power boxes). Some devices have lots of power/ground pins and having all of these pins on the symbol would increase its size and make it unmanageable. The <strong><code>net=</code></strong> attribute is the power/ground specification of choice in the gEDA system because of its simplicity and versatility.
Now having said all this, you can have power/ground pins on a symbol, but gnetlist will probably not recognize these nets connected to these pins as separate power/ground nets. Please keep this in mind as you draw symbols.
</p>
</div>
<!-- EDIT28 SECTION "What is the net= attribute used for?" [217-1022] -->
<h2 class="sectionedit29"><a name="what_is_the_format_of_the_net_attribute" id="what_is_the_format_of_the_net_attribute">What is the format of the net= attribute?</a></h2>
<div class="level2">
<p>
Attributes in gEDA are simple text items which are in the form <code>name=value</code>. All proper attributes follow this form. Attribute names are always lower case, but the value can be upper or lower case. gnetlist and friends are case sensitive. Typically net/signal names by default are upper case.<br/>
Attribute can be attached to an object or in certain cases (like the <strong><code>net=</code></strong> attribute) can be free floating (not attached to anything). The free floating attributes
are also called toplevel attributes.<br/>
The <strong><code>net=</code></strong> attribute is a text item which takes on the following form:
</p>
<pre class="code">net=signalname:pinname,pinname,pinname,...</pre>
<p>
where:
</p>
<div class="table sectionedit30"><table class="inline">
<tr class="row0">
<td class="col0"> <strong><code>net=</code></strong> </td><td class="col1"> The attribute name (always the same, lowercase) </td>
</tr>
<tr class="row1">
<td class="col0"> signalname </td><td class="col1"> The signal or net being defines (like +5V, GND, etc…) </td>
</tr>
<tr class="row2">
<td class="col0"> pinname </td><td class="col1"> The pin name (or number) which is assigned to this signal/net (or pin names/numbers) </td>
</tr>
</table></div>
<!-- EDIT30 TABLE [1725-1963] -->
<p>
The signalname cannot contain the ”:” character (since it is a delimiter). The pinname is the pin name (A1, P2, D1, etc…) or pin number (1, 2, 5, 13, etc…). The pinname cannot contain the ”,” character (since it is also a delimiter). pinnames are typically the same sort of numbers/names like the <code>pin#=#</code> attribute (if you are familiar with that attribute).<br/>
You can only have ONE signalname per <strong><code>net=</code></strong> attribute, but you can have as many pinnames/numbers as you want.
</p>
</div>
<!-- EDIT29 SECTION "What is the format of the net= attribute?" [1023-2448] -->
<h2 class="sectionedit31"><a name="how_do_you_actually_use_the_net_attribute" id="how_do_you_actually_use_the_net_attribute">How do you actually use the net= attribute?</a></h2>
<div class="level2">
<p>
You can place the <strong><code>net=</code></strong> attribute in several places. Here's the list so far:
</p>
<ul>
<li class="level1"><div class="li"> Inside a symbol either as an attached attribute or an unattached attribute (toplevel attribute). Example which creates power/gnd nets: <strong><code>net=GND:7</code></strong> or <strong><code>net=+5V:14</code></strong></div>
</li>
<li class="level1"><div class="li"> Outside a symbol (which is instantiated on a schematic) attached as an attribute to override an existing <strong><code>net=</code></strong> created net/signal. Suppose a symbol has a <strong><code>net=GND:7</code></strong> inside it already; attaching this to the symbol: <strong><code>net=AGND:7</code></strong> overrides the GND net (on pin 7) calling it AGND and connects/associates it to pin 7.</div>
</li>
<li class="level1"><div class="li"> Outside or inside a symbol to connect a net to a visible pin automatically. This is still untested and still might have some undesirable (negative) side effects. Use with caution.</div>
</li>
<li class="level1"><div class="li"> Attached to one of those special power/gnd symbol (like vcc/gnd/vdd) and you can change what that symbol represents. You could change the ground symbol to create a net called DIGITAL GND without editing the symbol (<strong><code>net=DIGITAL_GND:1</code></strong>).<br/>
In the current symbol (19991011) library there are symbols named <strong>vdd-1.sym</strong>, <strong>vcc-1.sym</strong>, <strong>vee-1.sym</strong>, etc… which do not have a <strong><code>net=</code></strong> attribute inside, so you must attach the <strong><code>net=</code></strong> attribute yourself (in the schematic).<br/>
There also symbols named 5V-minus-1.sym, 12V-plus-1.sym, 9V-plus-1.sym, etc… which have the appropriate <strong><code>net=</code></strong> attribute in them already (can be overridden though). You can use these symbol as examples of how to use the <strong><code>net=</code></strong> attribute.<br/>
</div>
</li>
</ul>
<p>
You can have as many <strong><code>net=</code></strong> attributes as you want. Just remember that <strong><code>net=</code></strong> attributes attached to the outside of a symbol override any equivalent internal (inside the symbol) <strong><code>net=</code></strong> attributes. If you run into a case where this doesn't work, please <a href="geda-howto_report_bugs.html" class="wikilink1" title="geda-howto_report_bugs.html">report a bug</a>.
</p>
</div>
<!-- EDIT31 SECTION "How do you actually use the net= attribute?" [2449-4343] -->
<h2 class="sectionedit32"><a name="caveats_bugs" id="caveats_bugs">Caveats / Bugs</a></h2>
<div class="level2">
<p>
The <strong><code>net=</code></strong> attribute/mechanism is fairly new, so there are bound to be bugs (many bugs). Here are some of the identified issues:
</p>
<ul>
<li class="level1"><div class="li"> As of 19991011 almost all of the symbols in the standard library do not have the <strong><code>net=</code></strong> attribute or any other power/ground specifiers. Hopefully this will be updated sometime (any volunteers?).</div>
</li>
<li class="level1"><div class="li"> Attach a special power symbol (vcc/gnd) to a already named net will alias (rename) that net to the signalname specified in the <strong><code>net=</code></strong> attribute (in/attached to the vcc/gnd symbol). You can override this (so the reverse is true) by playing with the “net-naming-priority”. Be careful with this. There might be other “aliasing” issues which have not been identified yet.</div>
</li>
<li class="level1"><div class="li"> Creating a <strong><code>net=</code></strong> attribute which associates a signal name with a pin which is already visible on the symbol, is probably a bad idea. This does work, but all the ramifications have not been explored yet.</div>
</li>
<li class="level1"><div class="li"> It is probably a bad idea to have the same <strong><code>net=</code></strong> attribute attached several times. Ales has not formalized what happens in this case. Just remember that the <strong><code>net=</code></strong> attribute on the outside of a symbol should override the internal one.</div>
</li>
</ul>
</div>
<!-- EDIT32 SECTION "Caveats / Bugs" [4344-5555] -->
<h2 class="sectionedit33"><a name="example" id="example">Example</a></h2>
<div class="level2">
<p>
Here's a schematic which uses standard symbols (note: the 7400 does not have the <strong><code>net=</code></strong> attribute inside yet). This schematic consists of a 7400 with the <strong><code>net=</code></strong> attributes attached for power and ground, One of the input pins grounded using a gnd symbol and the other at a logic one using the vcc symbol (with an attached <strong><code>net=</code></strong> attribute). One of the input net is named, but as you will see, the netname is replaced by the <strong><code>net=</code></strong> signal name (see above for more info on this). The output is pulled up with a pull up resistor which has power specified using the +5V symbol.<br/>
</p>
<div class="table sectionedit34"><table class="inline">
<tr class="row0">
<td class="col0"> <a href="media/geda/net.jpg" class="media" target="_blank" title="geda:net.jpg"><img src="media/geda/net.jpg" class="media" alt="" /></a> </td>
</tr>
</table></div>
<!-- EDIT34 TABLE [6176-6197] --><pre class="code">v 19991011
C 38700 58100 1 0 0 7400-1.sym
{
T 39000 59000 5 10 1 1 0
uref=U100
T 38900 59500 5 10 1 1 0
net=GND:7
T 38900 59300 5 10 1 1 0
net=+5V:14
}
N 38700 58800 37400 58800 4
{
T 37600 58900 5 10 1 1 0
netname=NETLABEL
}
N 37400 58800 37400 59200 4
N 38700 58400 37400 58400 4
N 37400 58000 37400 58400 4
C 37300 57700 1 0 0 gnd-1.sym
C 37200 59200 1 0 0 vcc-1.sym
{
T 36800 59200 5 10 1 1 0
net=+5V:1
}
N 40000 58600 41600 58600 4
{
T 41200 58700 5 10 1 1 0
netname=OUTPUT
}
C 40700 58800 1 90 0 resistor-1.sym
{
T 40800 59200 5 10 1 1 0
uref=R1
}
N 40600 58800 40600 58600 4
N 40600 59900 40600 59700 4
C 40400 59900 1 0 0 5V-plus-1.sym</pre>
<p>
<strong>gnetlist</strong> (using the geda netlist format) run using this sample schematic outputs this:
</p>
<pre class="code">START header
gEDA's netlist format
Created specifically for testing of gnetlist
END header
START components
R1 device=RESISTOR
U100 device=7400
END components
START renamed-nets
NETLABEL -> +5V
END renamed-nets
START nets
+5V : R1 2, U100 14, U100 1
GND : U100 7, U100 2
OUTPUT : R1 1, U100 3
END nets</pre>
<p>
Notice how NETLABEL was renamed (aliased to the +5V net).
</p>
</div>
<!-- EDIT33 SECTION "Example" [5556-7333] -->
<h2 class="sectionedit35"><a name="final_notes" id="final_notes">Final notes</a></h2>
<div class="level2">
<p>
If you found a bug, please <a href="geda-howto_report_bugs.html" class="wikilink1" title="geda-howto_report_bugs.html">let us know</a>.
</p>
</div>
<!-- EDIT35 SECTION "Final notes" [7334-] --></body>
</html>
distrib
>
Mageia
>
5
>
x86_64
>
media
>
core-release
>
by-pkgid
>
f2f28f61487f3042d93877451f0a311f
>
files
>
199
