Contact our corporate or local offices directly.
Parent page: Working with File-based Component Libraries
Integrated Libraries reflect Altium Designer's Integrated Component model. In this model, the higher-level component is modeled within the schematic symbol in a schematic library file. Other models are linked from the symbol and component parameters are added to the symbol. All source libraries – symbol and linked models – are defined within an Integrated Library Package project, which is subsequently compiled into a single file – an Integrated Library, or IntLib.
This document takes a look at the various ways in which an integrated library may be created, as well as placement from and modification to such a library.
The key benefits of compiling into an integrated library are:
An Integrated Library Package (
*.LibPkg) is a type of Altium Designer project that is used to gather together the set of design documents required to produce an integrated library. Schematic symbols are drawn in the schematic library editor, and model references/links defined for each, along with any parametric information. These are stored across one or more schematic library files. Referenced models can include PCB 2D/3D component models, circuit simulation models, and signal integrity models.
The only document that must be added to the integrated library package is the schematic library (or libraries). The files containing PCB 2D/3D component models and simulation models/sub-circuits can be located in any valid search location within the project, within files in the Installed Libraries list, or in the search path(s) specified for the package.
The library package is then compiled into a single Integrated Library file (
In summary, there are essentially four steps to creating an integrated library:
Create a new integrated library package by choosing the File » New » Library » Integrated Library command from the main menus. The new shell library package project will be added to the Projects panel and initially will not contain any documents.
Create the source schematic library (
*.SchLib) containing the components required. For each component, add the required model links and parametric information. There are two ways to create a source schematic library:
From scratch, using the File » New » Library » Schematic Library command. Create new components using the schematic library editor, or copy components across from other open schematic libraries.
With the source schematic library (or libraries) prepared, add to the library package using one of the following methods:
Create the models – referenced by the schematic components – in their corresponding files: PCB 2D/3D component models in a PCB Library (
*.PcbLib), simulation models and sub-circuits in Model (
*.Mdl) and Subcircuit (
*.Ckt) files. The most important model will, of course, be the PCB 2D/3D component model that, like its schematic library counterpart, can be created in two ways:
Using the File » New » Library » PCB Library command, create new 2D footprints (and add any 3D body information) using the PCB Library Editor, or copy components across from other open PCB libraries.
With the model files defined, they now need to be made available to the library package, so that they can easily be located when required – remember, the models are referenced by (or linked to) the schematic components. Altium Designer has a standard system for making models available, regardless of whether you are building an integrated library package, or working on a schematic design. There are three ways of making models available:
There are advantages to each, so choose the method that best suits your work practices. Different models also work better with different approaches too. For example, you may not want to see a large number of simulation models listed in the Projects panel when the library package is opened, but you might like to see the PCB 2D/3D component model libraries. In this case, define a search path to the folder where the simulation models are stored and add the PCB library to the library package.
Collectively, these three methods of model availability form the Available File-based Libraries (available to a project) and can all be defined in the Available File-based Libraries dialog, which is accessed by clicking the at the top-right of the Components panel then selecting the File-based Libraries Preferences command.
The PCB library (and other model files if required) can also be added to the library package directly using the Add Existing to Project command, which is available from the main Project menu or from the right-click menu associated with the library package's entry in the Projects panel.
Defining search paths to model files from the Search Path tab of the Available File-based Libraries dialog accesses the Search Paths tab of the Options for Integrated Library dialog (Project » Project Options). Add one or more paths as required, remembering that models are searched along these paths in order from top to bottom. Click the Refresh List button to verify that the required model files are indeed found and adjust a path if necessary.
With the source libraries added to the library package and any paths to model files defined as required, the package can now be compiled to ultimately generate the integrated library. Like any other project, the compiler for an integrated library package will generate a list of warning and/or error messages, for example, warning of any models that were not found. Additionally, pin mapping errors can be checked, such as mapping instructions to pads 1 and 2 when the actual footprint contains pads A and K.
Prior to running a compilation, it is prudent to browse through and set the error reporting conditions appropriately, on the Error Reporting tab of the Options for Integrated Library dialog.
To proceed with compilation, use the Compile Integrated Library command either from the main Project menu or from the right-click menu associated with the library package's entry in the Projects panel. The source libraries and model files are compiled into an integrated library named after the source library package (
<LibraryPackageName>.IntLib). The compiler will check for violations and any errors or warnings found will be listed in the Messages panel. Fix any problems in the source libraries then recompile.
The integrated library is saved in the output folder nominated on the Options tab of the Options for Integrated Library dialog (by default a sub-folder of the project's location:
\Project Outputs for <ProjectName>). It is automatically added to the Installed tab of the Available File-based Libraries dialog and the Data Management – File-based Libraries page of the Preferences dialog.
An integrated library can also be made directly from constituent project documents (source schematics and PCB document). Use the Make Integrated Library command, which is available from the main Design menu in either the schematic or PCB editor.
The process essentially involves:
The IntLib is added to the project (under
Libraries\Compiled Libraries in the Projects panel), added to the Installed libraries (as part of the Available File-based Libraries available to any project), and made available through the Components panel.
Related page: Working with Database Libraries
Altium Designer's Database Libraries are an ideal choice if you want your Altium Designer components to be tightly coupled to your company database. If the design needs to leave your company site, or if you prefer to have your designers work from secure integrated libraries, this can be readily achieved. Altium Designer provides the facility to compile an integrated library directly from a database library: either a standard database library (DbLib), or a version-controlled SVN database library (SVNDbLib). In this way, your CAD Librarians can still use database libraries, while your designers use regularly regenerated integrated libraries working in an 'offline' fashion as it were.
Conversion is performed using the Offline Integrated Library Maker wizard. The process is carried out on a per database table basis, with full control over which tables in the database are considered. A separate integrated library will be generated for each included table.
The process involves the following steps:
*.DbLib), or SVN Database Library file (
*.SVNDbLib) that you want to convert open as the active document, choose the Tools » Offline Integrated Library Maker command from the main menus to access the Offline Integrated Library Maker.
*.LibPkg) is created and opened in the Projects panel. The package is named using the name of the table. For a table named
Capacitor - Ceramic,for example, this would give
Capacitor - Ceramic.LibPkg.
Capacitor - Ceramic.SchLib).
Capacitor - Ceramic.PcbLib). The PCB library document is then added to the LibPkg.
Capacitor - Ceramic.IntLib), which is subsequently added to Altium Designer's Installed Libraries.
Related page: Acquiring Workspace Data Using the Content Cart
You also have the ability to acquire components from your Workspace, into an Integrated Library (
*.IntLib). And when placing components from such an Integrated Library, the actual links are back to the components in the Workspace. This gives you the ability to effectively use your company's Workspace components in an offline fashion, while ensuring the design still maintains a true connection to those components in the source Workspace.
From the Content Cart dialog, the process to acquire an IntLib is as follows:
Click on the Select target server link and choose IntLib file from the menu.
Specify the name, and location, for the generated IntLib file. By default, the file will be named in the format
Integrated_Library - <Date> - <Time>.IntLib, and generated in the location
\Users\Public\Documents\Altium\AD<Version>\Library\ExportCmpLib. Modify this as required through the Save As dialog – accessed by clicking the Change link.
Once ready, click the button to proceed with generation of the IntLib. A temporary Integrated Library Package (
*.LibPkg) will be created, with source SchLib (with symbols, parameters, and model links) and PcbLib (with footprint models) files generated and added. This is then compiled to produce the IntLib file, which is generated in the specified folder. An information dialog will confirm successful generation of the file.
After generation, the IntLib is added to the Installed Libraries list – part of the Available File-based Libraries for the software.
Placement of components from an integrated library is performed from the Components panel. Placement can be made from the active schematic document or the active PCB document. Placement can be performed in the following ways:
*.IntLibfile from the Components panel drop-down then right-click on the component to be placed and choose Place <ComponentName> from the context menu. Position the component on the schematic document then click to place.
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.
Integrated libraries are used to place components and cannot be edited directly. To make changes to an integrated library, make modifications in the source libraries first and then recompile the library package to generate a fresh integrated library that includes those changes.
To modify an integrated library:
There may be occasion where the source libraries in an integrated library need to be accessed for modification, but for whatever reason, there is no access to the original source library package project by which to do so. This is where another aspect of a single, portable integrated library file, comes into play. Although integrated libraries cannot be edited directly; they can be de-compiled back into their constituent source symbol and model libraries.
To do this:
In the Extract Sources or Install dialog that appears, click the Extract Sources button.
The source schematic and model libraries are extracted and saved in a new folder named after the integrated library's filename in the folder in which the original integrated library resides. A library package (
<IntegratedLibraryFileName>.LibPkg) is then created and the source schematic and PCB libraries are added to the project and presented in the Projects panel. Simulation model and sub-circuit files are not automatically added to the project.
Contact our corporate or local offices directly.