I believe that the File Format section of the documentation is out of
date. Attached is a patch that updates the parts that I know about and
adds an entirely new section that delves into more detail about the
Thickness, Clearance and Mask parameters.
I think that Via should have Thickness and Mask parameters just as Pin
does but I wasn't sure. If this is the case only, an additional trivial
addition is necessary.
Thanks,
David Carr
--- pcb/doc/pcb.texi 2005-01-28 18:59:08.000000000 -0600
+++ pcb.new/doc/pcb.texi 2005-06-19 20:03:03.000000000 -0500
@@ -31,7 +31,9 @@
Copyright (C) 2003, 2004 Dan McMahill
-Copyright (C) 2004 DJ Delorie
+Copyright (C) 2004, DJ Delorie
+
+Copyright (C) 2005, David Carr
This program is free software; you may redistribute it and/or modify
it under the terms of the GNU General Public License as published by
@@ -86,10 +88,29 @@
@c ---------------------------------------------------------------------
@node Copying, History, Top, Top
@unnumbered Copying
+
[EMAIL PROTECTED]
Copyright @copyright{} 1994,1995,1996,1997 Thomas Nau
[EMAIL PROTECTED]
Copyright @copyright{} 1998,1999,2000,2001,2002 harry eaton
[EMAIL PROTECTED]
+Copyright @copyright{} 1994,1995,1996, 2004 Thomas Nau
+
[EMAIL PROTECTED]
+Copyright @copyright{} 1997, 1998, 1999, 2000, 2001, 2002 harry eaton
+
[EMAIL PROTECTED]
+Copyright @copyright{} 2003, 2004 Dan McMahill
+
[EMAIL PROTECTED]
+Copyright @copyright{} 2004, DJ Delorie
+
[EMAIL PROTECTED]
+Copyright @copyright{} 2005, David Carr
+
+
This program is free software; you may redistribute it and/or modify
it under the terms of the GNU General Public License as published by
the Free Software Foundation; either version 2 of the License, or
@@ -4206,6 +4227,7 @@
chapter.
@example
+Clearance = Number
Description = Name
DeltaAngle = Number
DrillingHole = Number
@@ -4221,6 +4243,9 @@
Height = Number
LayerNumber = Number
LayoutName = Name
+Mask = Number
+MarkX = Number
+MarkY = Number
Name = quoted_string
Number = decimal | hex
PinNumber = quoted_string
@@ -4281,15 +4306,15 @@
Via = "Via(" X Y Thickness DrillingHole Name Flags ")"
Element = "Element(" Flags Description LayoutName Value \
- TextX TextY direction scale TextFlags")"
+ MarkX MarkY TextX TextY direction scale TextFlags")"
"(" @[EMAIL PROTECTED] [Mark] ")"
ElementData = @{ElementLine | Pad | Pin | ElementArc @}...
ElementArc = "ElementArc(" X Y Width Height
StartAngle DeltaAngle Thickness ")"
ElementLine = "ElementLine(" X1 Y1 X2 Y2 Thickness ")"
Mark = "Mark(" X Y ")"
-Pad = "Pad(" X1 Y1 X2 Y2 Thickness Name PinNumber Flags")"
-Pin = "Pin(" X Y Thickness DrillingHole Name PinNumber Flags ")"
+Pad = "Pad(" X1 Y1 X2 Y2 Thickness Clearance Mask Name PinNumber
Flags")"
+Pin = "Pin(" X Y Thickness Clearance Mask DrillingHole Name
PinNumber Flags ")"
Layer = "Layer(" LayerNumber Name ")"
"(" @[EMAIL PROTECTED] ")"
@@ -4422,15 +4447,15 @@
@example
File = @[EMAIL PROTECTED]
Element = "Element(" Flags Description LayoutName Value \
- TextX TextY direction scale TextFlags")"
+ MarkX MarkY TextX TextY direction scale TextFlags")"
"(" @[EMAIL PROTECTED] [Mark] ")"
ElementData = @{ElementLine | Pad | Pin | ElementArc @}...
ElementArc = "ElementArc(" X Y Width Height
StartAngle DeltaAngle Thickness ")"
ElementLine = "ElementLine(" X1 Y1 X2 Y2 Thickness ")"
Mark = "Mark(" X Y ")"
-Pad = "Pad(" X1 Y1 X2 Y2 Thickness Name PinNumber Flags ")"
-Pin = "Pin(" X Y Thickness DrillingHole Name PinNumber Flags ")"
+Pad = "Pad(" X1 Y1 X2 Y2 Thickness Clearance Mask Name PinNumber
Flags ")"
+Pin = "Pin(" X Y Thickness Clearance Mask DrillingHole Name
PinNumber Flags ")"
@end example
@table @samp
@@ -4497,6 +4522,85 @@
@end table
[EMAIL PROTECTED]
[EMAIL PROTECTED] Note about Thickness, Clearance and Mask:}
+
+Many of objects that appear in PCB Layout and Element files contain
+one or more of the parameters Thickness, Clearance and Mask. These
+parameters respectively refer to the width of line-derived object, the
+spacing between an object and any neighboring polygons and finally the
+width of soldermask relief surronding an object. While these definitions
+may seem relatively straightforward, PCB's representation of these concepts
+makes determining the appropriate value for these parameters rather more
+difficult.
+
+Pads are line-based objects, meaning that a Pad is represented by
+a line segment between points (X1, Y1) and (X2, Y2) that has a width
+given by the Thickness parameter.
+
+Recall that Pads take the following form:
[EMAIL PROTECTED]
+Pad( X1 Y1 X2 Y2 Thickness Clearance Mask Name PinNumber Flags )
[EMAIL PROTECTED] example
+
+Say that we wish to define a SMD pad that is 30mils long and is 10mils
+wide. Furthermore, we want 4mils of soldermask relief and 15mils of
+clearance between our pad and any neighboring polygons.
+
+Something like this seems appropriate:
[EMAIL PROTECTED]
+Pad( -15 0 15 0 10 15 4 "Test Pad" "1" 0x00000100 )
[EMAIL PROTECTED] example
+
+Unfourtunately, this intuitive Pad definition doesn't produce the
+desired result at all. Instead of a Pad 30mils long and 10 mils long,
+we'll get a Pad that is 40 mils long and 10 mils wide. The soldermask
+will overlap the pad by 3mils on each side and neighboring polygons
+will only have 7.5mils clearance.
+
+All of the above problems stem from three misconceptions. Firstly, we
+assumed that a pad of length 30mils and width 10mils is represented by
+a line with endpoints 30mils apart and with a thickness of 10mils.
+This assumption is half correct; a pad of width 10mils is represented
+by a line 10mils wide. However, if a pad of width 10mils is to be
+30mils long, it's underlying line needs to be only 20mils long. This
+number seems odd because so far we've only taken thickness into
+account in one dimension. In PCB, a line's thickness not only affects
+its width but also its overall length---a line extends (Thickness/2)
+past its endpoints in either direction. In other words, the a line's
+total length is the distance between its endpoints plus its Thickness.
+
+The second misconception is closely related to the first. In the
+example, we assumed that if we wanted 4mils of clearance between the
+edge of pad and the soldermask, then the Mask [clearance] would simply
+be 4mils. However, instead of 4mils relief we got 3mils of overlap.
+Once again, the problem is related to the Thickness parameter. The
+Mask parameter specifies the thickness of the region around our pad
+that the soldermask must not enter. To get 4mils of relief between
+the edge of the pad and the soldermask, Mask must be set to the sum of
+the pad's Thickness and twice our desired soldermask clearance from
+the edge, ie:
+
[EMAIL PROTECTED]
+Mask = Thickness(10mils) + 2*4mils = 10mils + 8mils = 18mils.
+
+Our last problem is a simple one. The clearance between neighboring
+polygons and the edge of our pad was only 7.5mils but we wanted
+15mils. The issue here is that the Clearance parameter specifies the sum
+of the distances between the pad edge and the polygon on both sides of
+the pad. So, to get 15mils on each side we have to multiply our
+clearance for each side by two:
+
[EMAIL PROTECTED]
+Clearance = 2*(clearance per side) = 2*15mils = 30mils
+
+To finish up, we'll take these new factors into account and fix our
+previous example. If we want a Pad 30mils long, 10mils wide, with
+15mils of polygon clearance per side, and 4mils of soldermask relief,
+then this should do it:
[EMAIL PROTECTED]
+Pad( -10 0 10 0 10 30 18 "Test Pad" "1" 0x00000100 )
[EMAIL PROTECTED] example
@node Font File, Netlist File, Element File, File Formats
@cindex font file, format of
@@ -4534,6 +4638,8 @@
@end table
+
+
@node Netlist File, Library Contents File, Font File, File Formats
@cindex netlist, file format
@cindex netlist, reading
