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
112
113
114
115
116
117
118
119
120
121
122
123
124
125
126
127
128
129
130
131
132
133
134
135
136
137
138
139
140
141
142
|
<html>
<head>
<title>EAGLE Help: PAD</title>
</head>
<body bgcolor=white>
<font face=Helvetica,Arial>
<hr>
<i>EAGLE Help</i>
<h1><center>PAD</center></h1>
<hr>
<dl>
<dt>
<b>Function</b>
<dd>
Adds pads to a package.
<p>
<dt>
<b>Syntax</b>
<dd>
<tt>PAD [diameter] [shape] [orientation] [flags] ['name'] *..</tt>
<p>
<dt>
<b>Mouse</b>
<dd>
Right button rotates the pad.
<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=62.htm>NAME</a>,
<a href=98.htm>VIA</a>,
<a href=127.htm>Design Rules</a>
<p>
The PAD command is used to add pads to a package. When the PAD command
is active, a pad symbol is attached to the cursor and can be moved
around the screen. Pressing the left mouse button places a pad at
the current position.
Entering a number changes the diameter of the pad (in the actual unit).
Pad diameters can be up to 0.51602 inch (13.1 mm).
<p>
The <tt>orientation</tt> (see description in <a href=26.htm>ADD</a>)
may be any angle in the range <tt>R0</tt>...<tt>R359.9</tt>. The <tt>S</tt>
and <tt>M</tt> flags can't be used here.
<p>
<b>Example</b>
<pre>
PAD 0.06 *
</pre>
The pad will have a diameter of 0.06 inch, provided the actual unit
is "inch". This diameter remains as a presetting for succeeding
operations.
<p>
<b>Pad Shapes</b>
<p>
A pad can have one of the following shapes:
<p>
<table>
<tr><td valign=top><font face=Helvetica,Arial>Square </font></td><td valign=top><font face=Helvetica,Arial></font></td></tr>
<tr><td valign=top><font face=Helvetica,Arial>Round </font></td><td valign=top><font face=Helvetica,Arial></font></td></tr>
<tr><td valign=top><font face=Helvetica,Arial>Octagon </font></td><td valign=top><font face=Helvetica,Arial>octagonal</font></td></tr>
<tr><td valign=top><font face=Helvetica,Arial>Long </font></td><td valign=top><font face=Helvetica,Arial>elongated</font></td></tr>
<tr><td valign=top><font face=Helvetica,Arial>Offset </font></td><td valign=top><font face=Helvetica,Arial>elongated with offset</font></td></tr>
</table>
<p>
With elongated pads, the given diameter defines the smaller side of the pad.
The ratio between the two sides of elongated pads is given by the
parameter Shapes/Elongation in the <a href=127.htm>Design Rules</a>
of the board (default is 100%, which results in a ratio of 2:1).
<p>
The pad shape or diameter can be selected while the PAD command is
active, or it can be changed with the CHANGE command, e.g.:
<pre>
CHANGE SHAPE OCTAGON *
</pre>
The drill size may also be changed using the CHANGE command. The existing
values then remain in use for successive pads.
<p>
Because displaying different pad shapes and drill holes in their real
size slows down the screen refresh, EAGLE lets you change between
real and fast display mode by the use of the SET commands:
<pre>
SET DISPLAY_MODE REAL | NODRILL;
</pre>
Note that the actual shape and diameter of a pad will be determined by the
<a href=127.htm>Design Rules</a> of the board the part is used in.
<p>
<b>Pad Names</b>
<p>
Pad names are generated by the program automatically
and can be changed with the NAME command. The name can also be defined
in the PAD command. Pad name display can be turned on or off by means
of the commands:
<pre>
SET PAD_NAMES ON | OFF;
</pre>
This change will be visible after the next screen refresh.
<p>
<b>Flags</b>
<p>
The following <i>flags</i> can be used to control the appearance of a pad:
<p>
<table>
<tr><td valign=top><font face=Helvetica,Arial><tt>NOSTOP</tt> </font></td><td valign=top><font face=Helvetica,Arial>don't generate solder stop mask</font></td></tr>
<tr><td valign=top><font face=Helvetica,Arial><tt>NOTHERMALS</tt> </font></td><td valign=top><font face=Helvetica,Arial>don't generate thermals</font></td></tr>
<tr><td valign=top><font face=Helvetica,Arial><tt>FIRST</tt> </font></td><td valign=top><font face=Helvetica,Arial>this is the "first" pad (which may be drawn with a special shape)</font></td></tr>
</table>
<p>
By default a pad automatically generates solder stop mask and thermals as necessary.
However, in special cases it may be desirable to have particular pads not do this.
The above <tt>NO...</tt> flags can be used to suppress these features.<br>
If the <a href=127.htm>Design Rules</a> of a given board specify that the
"first pad" of a package shall be drawn with a particular shape, the pad marked with
the <tt>FIRST</tt> flag will be displayed that way.<br>
A newly started PAD command resets all flags to their defaults. Once a flag is given
in the command line, it applies to all following pads placed within this PAD command
(except for <tt>FIRST</tt>, which applies only to the pad immediately following this
option).
<p>
<b>Single Pads</b>
<p>
Single pads in boards can be used only by defining a package
with one pad. Via-holes can be placed in board but they don't have
an element name and therefore don't show up in the netlist.
<p>
<b>Alter Package</b>
<p>
It is not possible to add or delete pads in packages which
are already used by a device, because this would change the pin/pad
allocation defined with the CONNECT command.
<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>
|
