See below, we welcome any suggestions and feedback in preparations for
Cadsoft Support Team.
Library Management and Part Creation Standard v0.1
by Cadsoft Computer Support
Objective: The intent of this document is to provide a BASIC guideline
as to the best practices for developing user libraries. We have noticed
differing levels of quality among user contributed libraries and our
hope is that by developing this standard we will help raise the overall
quality of user contributed libraries.
Usage: This document is split up into four main sections, Library,
Symbols, Packages, and Devices. Under each main section the best
practices for that section are outlined followed by some supplemental
recommendations which are generally applicable, however they are not as
strictly recommended as the best practices.
1.Do not modify EAGLE's default libraries. They represent a known state
which support staff can rely on when assisting users. The preferred
approach is to copy elements into a user made library and then modify
them to suit your needs.
Copy procedures are discussed in the EAGLE manual section 8.12.
2.User libraries should not be stored in EAGLE's internal lib folder.
The reason being that if anything should happen to your EAGLE
installation(deletion, uninstall, viruses, hardware failure, etc.) your
libraries will be gone with it. It therefore recommended to store your
libraries in a separate location that can be easily backed up.
Recommendations for Libraries
1.In light of practice number 2 listed above, below are some suggestions
for best use of user developed libraries.
Some users like to make a separate library for each project they work on
and store it along with the board and schematic file that way everything
is together and easily accessible. A simple USE command in the
schematic/board editor will make the library active and available for
the ADD command.
Another possible scheme, is to store all of the libraries in a single
folder located outside of EAGLE's internal directory, and then include
it's path in the Library search directory. The advantage of this method
is that all of the user libraries are in one place for easy back ups.
Section 4.1 of the EAGLE manual discusses the Directories dialog.
Set a second path to your own library in Control-Panel | Options |
Directories | Libraries
1.Symbol pins must always align to a 0.1”(2.54mm) grid.
2.Symbols must always have >NAME and >VALUE place holders on layers 95
Names and 96 Values respectively.
3.Place >NAME on top, and >VALUE on bottom side of the symbol.
4.Center the symbol around the origin.
Recommendations for Symbols
1.Power pins should generally have their pin direction parameter set to Pwr.
2.Input pins should generally have their pin direction parameter set to IN.
3.Output pins should generally have their pin direction parameter set to
4.Passive pins should generally have their pin direction parameter set
5.Also IO, HIZ, NC.
6.Do not use pin direction SUP for a normal Symbols. SUP is only for
7.Any symbol notes or tips should be on layer 97 info.
8.It is better to give general names(OP AMP, DIODE, etc.) to symbols
instead of specific part numbers (LM741, 1N4007, etc.). This makes it
easy to reuse the symbol if your library is going to contain many
variations of the same type of component for example a library full of
op amps can probably make use of one op amp symbol.
9.For the >NAME and >VALUE text use a text size of 70 mils.
1.Design a package assuming that it will be placed on top of the board
(Use t layers). The MIRROR command can then be used on the board layout
to put a component on the bottom of the board.
Use tPlace for the component silkscreen which is printed on the PCB and
should not contact solder.
Use tDocu to draw leads of components leading to pads.
Use tNames for the >NAME place holder for the reference designator that
will be on the silkscreen.
Use tValues for the >VALUE place holder, which will not be part of the
Use layer 48 Document or layer 49 Reference for any artistic features or
notes that will not appear on the silkscreen.
2.Center the package around the origin.
Recommendations for Packages
1.For the >NAME and >VALUE text use a text size of 70 mils.
2.Draw outline of package in tPlace with wire width 8 mil or 4mil.
3.The ADD command in the board editor searches through the description
field, so a well setup description field can yield more fruitful
searches. Therefore a good description field for a package should include:
Standard package name(preferably in bold)
Any possible aliases for the package. For example a DIL08 package might
also be known as a DIP08.
If the package is based off of a standard document such as one of the
IPC standards, then it should be referenced in the description field if
possible as an HTML link. If a link is not possible then a reference to
the name of the document should be sufficient. Listing this information
will help in checking the package for correctness.
If applicable length x width dimension.
1.Always set a prefix, otherwise EAGLE will use U$ by default.
2.When creating multi-gated components, EAGLE will by default reference
them as G$1, G$2, etc. These names will not show up on the schematic,
therefore use the NAME command to rename the gates A, B, C, etc. A nice
way to do this is to type 'A' followed by enter when you have the gate
on your mouse cursor before placing it, EAGLE will then continue the
pattern for the other gates.
3.Use P for power symbols.
4.When naming devices use specific part numbers.
5.Always double check add levels and swap levels, otherwise your
components might not enter your schematic as you'd expect them to.
Recommendations for Devices
1.Just like packages, having a good description field can improve the
chances of the ADD command finding the component you want. A good
description field for a device should include:
Device name(preferably in bold).
Any other aliases the device might be recognized by.
A link or reference to the device's data sheet.
Short explanation of the device's function.
If applicable length x width dimension.