Enhanced Library Management Using Integrated Libraries

Schematic libraries allow you to attach footprint, simulation and other models to components. Usually, each of these model links references a file somewhere outside of the schematic library. PCB footprints will be found in PCB library files; simulation models (with some exceptions) are contained in model or sub-circuit files. So the schematic library saves a link, that is, instructions on where to find each model you attach.
Periodically, Altium Designer will need to locate these models - when you run a board update, for example, the linking instructions will be followed for all current footprints in your design. The search sequence for matching models starts with libraries in the current project, installed PCB libraries, then any files found on the project search path. The management of these separate source libraries is left entirely in your hands, meaning that Altium Designer cannot offer any guarantees that your models will find matches. These links in schematic libraries are brittle, and easily broken by everyday management tasks such as renaming folders on a hard drive, or reassigning labels to a central server.

The benefits of integrated libraries

Altium Designer has a solution: the integrated library. The integrated library includes not only the schematic library (or libraries), it also has all the associated model libraries bundled in. If a component came from an integrated library, Altium Designer is guaranteed to find the right model if it can simply locate the integrated library it came from.
Because the components and models are entirely contained within a single .IntLib file, these libraries offer portability to designers who divide their work among different workstations, or who want to share their designs with others. Simply installing the same, single file in the Libraries panel of any PC running Altium Designer will mean that component-to-model links will remain secure (assuming, again, that components were placed in the design from that integrated library).
These libraries are also checked for integrity when they are compiled. That means they are not only checked for availability, but for correct pin mappings. Even designers who want to stay with discrete library files should compile their schematics in an integrated library package, if only to ensure that the source components will map correctly to the target models. Once satisfied, they can ignore the integrated library they created, and keep placing directly from their schematic libraries.

Creating an integrated library

There is no document editor for integrated libraries. They are a product of compiling an integrated library package, which is analogous to PCB or FPGA projects. Add library files to the integrated library package, as you would add documents to any other project.
The only documents that must be added to the integrated library package are the schematic libraries you wish to include. The files containing PCB, simulation and other models can be located in any valid search location - within the project, within PCB files in the Installed Libraries list, or down the search path(s) specified for the package. That is the search order as well: left-to-right and top-to-bottom if you are viewing the lists in the Available Libraries dialog.
Whether you prefer to gather your libraries into your project or to locate them by search paths depends on your particular working style. If you are checking and editing models as you prepare the integrated library package, you may want to have the model libraries right at your fingertips, and so add them to the package itself. If you are continually adding model libraries to specific folders on your hard drive or network, then you may prefer to use the search paths, letting the compiler detect newly added libraries automatically.
Like any other project, the compiler for an integrated library package will generate a list of warning and error messages. You will be warned of any models that were not found, meaning that no matching names were found in the package or on the search paths. Additionally, you will be warned of any mapping errors, such as mapping instructions to pads 1 and 2 when the actual footprint contains pads A and K.
The integrated library file is created when the package is compiled. Remember, what you have been working on until this point is the integrated library package (.LibPkg), not the actual integrated library file (.IntLib). No integrated library exists until the package is compiled.

The Libraries panel

Opening an .IntLib file in Altium Designer will let you do one of two things. Either you can extract the source documents of the integrated library in a new integrated library package, or you can add the integrated library to the Libraries panel. This panel offers the only direct view into the integrated library file itself.
In fact, this panel was built for integrated libraries. Notice that you can browse schematic libraries only by component, and PCB libraries only by footprints. Integrated libraries, however, can be browsed by either, and browsing them by component will let you see the component to model relationship.

All models attached to a component are listed in this view of the Libraries panel. Only found models are included in this list; you should refer to the Messages panel to make sure that all of the models you attached to your components were found and validated.
Notice, however, that no editing buttons are available in the Libraries panel. Again, this is only a window for viewing the integrated library; it is not a door through which you may enter and change the things inside. This is because integrated libraries are solid - once they're generated, there's no changing them. In fact, to update an integrated library really means to replace it altogether - you must pull up the original library package, update the source documents, then recompile. If you have not changed the package name or output path, then the new integrated library will replace the old.
This is all part of the plan. An integrated library is a purposely controlled environment, and so we force you to return to the source documents to make any changes. The alternative is an exercise in juggling, where symbols and models can be modified independently at any time, without giving you any warning that they will no longer match up until you go to generate a simulation waveform, or update a board.

Placing from an integrated library

The Libraries panel contains a Place button. As this panel may contain assorted schematic, PCB and integrated libraries, you may use it in either the schematic or the PCB editor.
Any component placed from an integrated library is branded with information that will help locate the integrated library it came from later on. While a schematic library and an integrated library may contain the same component (with all the same model links), the placed components from each of these libraries will behave differently when their model information is retrieved. Those components placed from integrated libraries will look for the original integrated library to get their models, while those components placed from schematic libraries will have no access to models stored in integrated libraries.

Keeping integrated libraries available

Since integrated libraries are automatically added to the Libraries panel when they are created, and also because the Libraries panel is the only platform from which integrated components may be placed, the Libraries panel is the one and only place to be searched when integrated library model files are required. If you have uninstalled the source integrated library since placing, you will see errors in the Messages panel explaining which models couldn't be found.
This restriction to look only in the source integrated library is a setting kept at the model level, and as such, it can be changed on a model-by-model basis.
In conclusion, integrated libraries are a means of protecting the links between components and their models. Their components receive privileged status at model retrieval time, looking to the integrated library for associated models rather than embarking on a more general search.
In addition, integrated libraries offer portability and protection. They don't just maintain links; they contain the model libraries themselves. An integrated library may be taken from one design station to another, letting you sidestep the confusion of having to change your search paths from location to location. And finally, should any damage occur to the original package, including any if its links becoming broken, then Altium Designer will allow you to regenerate source documents from the integrated library.