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
143
144
145
146
147
148
149
150
151
152
153
154
155
156
157
158
159
160
161
162
163
164
165
166
167
168
169
170
171
172
173
174
175
176
177
178
179
180
181
182
183
184
185
186
|
<html>
<head>
<title>EAGLE Help: Design Rules</title>
</head>
<body bgcolor=white>
<font face=Helvetica,Arial>
<hr>
<i>EAGLE Help</i>
<h1><center>Design Rules</center></h1>
<hr>
<i>Design Rules</i> define all the parameters that the board layout has to follow.
<p>
The <a href=42.htm>Design Rule Check</a> checks the board against these rules
and reports any violations.
<p>
The Design Rules of a board can be modified through the Design Rules dialog, which
appears if the <a href=42.htm>DRC</a> command is selected without a terminating
<tt>';'</tt>.
<p>
Newly created boards take their design rules from the file 'default.dru',
which is searched for in the first directory listed in the "Options/Directories/Design rules" path.
If no such file is present, the program's builtin default values apply.
<p>
<b>Note</b> regarding the values for <b>Clearance</b> and <b>Distance</b>: since the internal
resolution of the coordinates is 1/10000mm, the DRC can only reliably report errors that
are larger than 1/10000mm.
<p>
<b>File</b>
<p>
The <i>File</i> tab shows a description of the current set of Design Rules and
allows you to <i>change</i> that description (this is strongly recommended if you define
your own Design Rules). There are also buttons to <i>load</i> a different set of Design
Rules from a disk file and to <i>save</i> the current Design Rules to disk.<br>
Note that the Design Rules are stored within the board file, so they will be in effect
if the board file is sent to a board house for production. The "Load..." and "Save as..."
buttons are merely for copying a board's Design Rules to and from disk.
<p>
<b>Layers</b>
<p>
The <i>Layers</i> tab defines which signal layers the board actually uses, how thick
the copper and isolation layers are, and what kinds of vias can be placed
(note that this applies only to actual <i>vias</i>; so even if no via from layer 1 to
16 has been defined in the layer setup, <i>pads</i> will always be allowed).
<p>
The layer setup is defined by the string in the "Setup" field. This string consists of
a sequence of layer numbers, separated by one of the characters <tt>'*'</tt> or
<tt>'+'</tt>, where <tt>'*'</tt> stands for <i>core</i> material (also known as <i>FR4</i>
or something similar) and <tt>'+'</tt> stands for <i>prepreg</i> (or any other kind of
isolation material). The actual <i>core</i> and <i>prepreg</i> sequence has no meaning
to EAGLE other than varying the color in the layer display at the top left corner
of this tab (the actual multilayer setup always needs to be worked out with the
board manufacturer). The vias are defined by enclosing a sequence of layers with <tt>(...)</tt>.
So the setup string
<pre>
(1*16)
</pre>
would mean a two layer board, using layers 1 and 16 and vias going through the
entire board (this is also the default value).<br>
When building a multilayer board the setup could be something like
<pre>
((1*2)+(15*16))
</pre>
which is a four layer board with layer pairs 1/2 and 15/16 built on core material
and vias drilled through them, and finally the two layer pairs pressed together
with prepreg between them, and vias drilled all the way through the entire board.<br>
Besides vias that go trough an entire layer stack (which are commonly referred to
as <i>buried</i> vias in case they have no connection to the Top and Bottom layer)
there can also be vias that are not drilled all the way through a layer stack, but
rather end at a layer inside that stack. Such vias are known as <i>blind</i> vias
and are defined in the "Setup" string by enclosing a sequence of layers with
<tt>[t:...:b]</tt>, where <i>t</i> and <i>b</i> are the layers up to which that via
will go from the top or bottom side, respectively. A possible setup with <i>blind</i>
vias could be
<pre>
[2:1+((2*3)+(14*15))+16:15]
</pre>
which is basically the previous example, with two additional outer layers that are
connected to the next inner layers by <i>blind</i> vias. It is also
possible to have only one of the <i>t</i> or <i>b</i> parameters, so for instance
<pre>
[2:1+((2*3)+(15*16))]
</pre>
would also be a valid setup. Finally, <i>blind</i> vias are not limited to starting
at the Top or Bottom layer, but may also be used in inner layer stacks, as in
<pre>
[2:1+[3:2+(3*4)+5:4]+16:5]
</pre>
A <i>blind</i> via from layer <i>a</i> to layer <i>b</i> also implements all possible
<i>blind</i> vias from layer <i>a</i> to all layers between layers <i>a</i> and <i>b</i>, so
<pre>
[3:1+2+(3*16)]
</pre>
would allow <i>blind</i> vias from layer 1 to 2 as well as from 1 to 3.
<p>
<b>Clearance</b>
<p>
The <i>Clearance</i> tab defines the various minimum clearance values between objects
in signal layers. These are usually absolute minimum values that are defined by the
production process used and should be obtained from your board manufacturer.<br>
The actual minimum clearance between objects that belong to different signals will
also be influenced by the <a href=34.htm>net classes</a> the two signals belong to.
<p>
Note that a polygon in the special signal named _OUTLINES_ will be used to generate
<a href=124.htm>outlines data</a> and as such will <b>not</b> adhere to these
clearance values.
<p>
<b>Distance</b>
<p>
The <i>Distance</i> tab defines the minimum distance between objects in signal layers
and the board dimensions, as well as that between any two drill holes.
Note that only signals that are actually connected to at least one pad or
smd are checked against the board dimensions. This allows edge markers to be drawn
in the signal layer without generating DRC errors.
<p>
For compatibility with version 3.5x the following applies:
If the minimum distance between copper and dimension is set to <tt>0</tt>
objects in the Dimension layer will not be taken into account when calculating
polygons (except for Holes, which are always taken into account). This also disables
the distance check between copper and dimension objects.
<p>
<b>Sizes</b>
<p>
The <i>Sizes</i> tab defines the minimum width of any objects in signal layers and
the minimum drill diameter. These are usually absolute minimum values that are defined by the
production process used and should be obtained from your board manufacturer.<br>
The actual minimum width of signal wires and drill diameter of vias will
also be influenced by the Net Class the signal belongs to.
<p>
<b>Restring</b>
<p>
The <i>Restring</i> tab defines the width of the copper ring that has to remain after the
pad or via has been drilled. Values are defined in percent of the drill diameter and
there can be an absolute minimum and maximum limit. Restrings for pads can be different
for the top, bottom and inner layers, while for vias they can be different for the
outer and inner layers.<br>
If the actual diameter of a pad (as defined in the library) or a via would result in a
larger restring, that value will be used in the outer layers. Pads in library packages
can have their diameter set to 0, so that the restring will be derived entirely
from the drill diameter.
<p>
<b>Shapes</b>
<p>
The <i>Shapes</i> tab defines the actual shapes for smds and pads.<br>
Smds are normally defined as rectangles in the library (with a "roundness" of 0),
but if your design requires rounded smds you can specify the roundness factor here.<br>
Pads are normally defined as octagons in the library (long octagons where this makes
sense), and you can use the combo boxes to specify whether you want to have
pads with the same shapes as defined in the library, or always square, round or
octagonal. This can be set independently for the top and bottom layer.<br>
If the "first" pad of a package has been marked as such in the library
it will get the shape as defined in the third combo box (either round, square or
octagonal, or no special shape).<br>
The Elongation parameters define the appearance of pads with shape Long or Offset.
<p>
<b>Supply</b>
<p>
The <i>Supply</i> tab defines the dimensions of Thermal and Annulus symbols used in
supply layers.<br>
Please note that the actual shape of supply symbols may be different when generating
output for photoplotters that use specific thermal/annulus apertures!
See also the notes about "Supply Layers" in the <a href=56.htm>LAYER</a> command.
<p>
<b>Masks</b>
<p>
The <i>Masks</i> tab defines the dimensions of solder stop and cream masks. They are
given in percent of the smaller dimension of smds, pads and vias and can have an
absolute minimum and maximum value.<br>
Solder stop masks are generated for smds, pads and those vias that have a drill diameter
that exceeds the given Limit parameter.<br>
Cream masks are generated for smds only.
<p>
<b>Misc</b>
<p>
The <i>Misc</i> tab allows you to turn on a grid and angle check.
<p>
<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>
|
