1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
16
17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33
34
35
36
37
38
39
40
41
42
43
44
45
46
47
48
49
50
51
52
53
54
55
56
57
58
59
60
61
62
63
64
65
66
67
68
69
70
71
72
73
74
75
76
77
78
79
80
81
82
83
84
85
86
87
88
89
90
91
92
93
94
95
96
97
98
99
100
101
102
103
104
105
106
107
108
109
110
111
|
<html>
<head>
<title>EAGLE Help: VIA</title>
</head>
<body bgcolor=white>
<font face=Helvetica,Arial>
<hr>
<i>EAGLE Help</i>
<h1><center>VIA</center></h1>
<hr>
<dl>
<dt>
<b>Function</b>
<dd>
Adds vias to a board.
<p>
<dt>
<b>Syntax</b>
<dd>
<tt>VIA ['signal_name'] [diameter] [shape] [layers] [flags] *..</tt>
<p>
</dl>
<b>See also</b> <a href=90.htm>SMD</a>,
<a href=32.htm>CHANGE</a>,
<a href=41.htm>DISPLAY</a>,
<a href=86.htm>SET</a>,
<a href=67.htm>PAD</a>,
<a href=127.htm>Design Rules</a>
<p>
When the VIA command is active, a via symbol is attached to the cursor.
Pressing the left mouse button places a via at the current position.
When vias are added
to a signal, a short circuit test is performed. If you try to connect
different signals, EAGLE will ask you if you really want to connect
them.
<p>
<b>Signal name</b>
<p>
The <tt>signal_name</tt> parameter is intended mainly to be used in
script files that read in generated data. If a <tt>signal_name</tt>
is given, all subsequent vias will be added to that signal, and no
automatic checks will be performed.<br>
<b>This feature should be used with great care because it could result
in short circuits, if a via is placed in a way that it would connect
wires belonging to different signals. Please run a
<a href=42.htm>Design Rule Check</a> after using the VIA command
with the</b> <tt>signal_name</tt> <b>parameter!</b>
<p>
<b>Via diameter</b>
<p>
Entering a number changes the diameter of the via (in the actual
unit) and the value remains in use for further vias. Via diameters
can be up to 0.51602 inch (13.1 mm).
<p>
The drill diameter of the via is the same as the diameter set for
pads. It can be changed with
<pre>
CHANGE DRILL diameter *
</pre>
<p>
<b>Shape</b>
<p>
A via can have one of the following shapes:
<p>
Square<br>
Round<br>
Octagon
<p>
Vias generate drill symbols in the Drills layer and the solder
stop mask in the tStop/bStop layers.
<p>
Like the diameter, the via shape can be entered while
the VIA command is active, or it can be changed with the CHANGE command.
The shape then remains valid for the next vias and pads.
<p>
Note that the actual shape and diameter of a via will be determined by the
<a href=127.htm>Design Rules</a> of the board the via is used in.
<p>
<b>Layers</b>
<p>
The <tt>layers</tt> parameter defines the layers this via shall
cover. The syntax is <tt>from-to</tt>, where 'from' and 'to' are the layer numbers
that shall be covered. For instance <tt>2-7</tt> would create a via that goes from
layer 2 to layer 7 (<tt>7-2</tt> would have the same meaning). If that exact via is
not available in the layer setup of the <a href=127.htm>Design Rules</a>, the next longer via
will be used (or an error message will be issued in case no such via can be
set).
<p>
<b>Flags</b>
<p>
The following <i>flags</i> can be used to control the appearance of a via:
<p>
<table>
<tr><td valign=top><font face=Helvetica,Arial><tt>STOP</tt> </font></td><td valign=top><font face=Helvetica,Arial>always generate solder stop mask</font></td></tr>
</table>
<p>
By default a via with a drill diameter that is less than or equal to the value of
the <a href=127.htm>Design Rules</a> parameter "Masks/Limit" will not
have a solder stop mask. The above <tt>STOP</tt> flag can be used to force a solder
stop mask for a via.
<hr>
<table width=100% cellspacing=0 border=0><tr><td align=left><font face=Helvetica,Arial>
<a href=index.htm>Index</a>
</font></td><td align=right><font face=Helvetica,Arial size=-1>
<i>Copyright © 2005 CadSoft Computer GmbH</i>
</font></td></tr></table>
<hr>
</font>
</body>
</html>
|
