The central library is a database of multiple linked libraries. Included among these libraries are the Cells library, Symbols library, and PadStack library. The central library maintains the link between cells and symbols which comprises the Parts library. By having all the libraries maintained as one entity (the central library) the user is allowed to modify cells and/or symbols and not worry about having to update every part that refers to a modified cell or symbol. The central library takes care of updating all Parts to reflect the changes made to the Cell or Symbol.
NOTE: Although multiple central libraries can be created, it is only possible to link a single central library to a project. If you find yourself needing to add components to a central library that is write protected, simply create a new central library and import all components from the write-protected one. This will give you access to all components from the first central library as well as the ability to create new components or modify existing ones. In fact, early in your project development you will want to make your own central library by starting with the given ECE189 Central Library (essentially a clean slate but with built-in properly-established design rules and PCB template) and then importing padstacks, cells, symbols, and parts from other available libraries to the one that is local and writeable for your project.
This term is not defined or used uniquely within the Mentor Graphics tools but rather is a term used frequently in this document to refer to an instance of an object from a library. For instance, a component could be a part from the Parts library or could be a cell from the Cells library. The term is used rather than directly saying "part" or "cell" so that all libraries can be referenced to the action. If a particular action is limited to only a particular library or a small set of libraries then the list of libraries will be given in parentheses.
A partition is a user-defined grouping of Parts, Cells, or Symbols (within a library). These are essential to organizing your libraries. Think of partitions as folders you would create on a computer. You can create as many folders as you would like to organize your files but creating too many folders can be confusing. Partitions are more limited than folders; e.g. partitions cannot be created within partitions, though you can create as many partitions in a library as you like. Partitions also offer a limited amount of security to your library files in that only one user is allowed to modify parts in a partition. Once a user begins editing a part/cell/symbol in a partition, all others who try and access that partition will only be granted read access. Once the first user finishes editing the part/cell/symbol, then others will be able to modify a part/cell/symbol in that partition. It is recommended that if you plan on having two users working on parts using the same library that two different partitions are created so that each user will be able to modify a list of parts/cells/symbols without having to wait for the other to finish before starting work.
This topic is not covered very well in the existing documentation but is crucial to understand. The local library is used only when the Library Manager is accessed THROUGH Expedition PCB or DxDesigner. When a component, be it a Part/Cell/Symbol, is modified through this path, the component is not saved directly to the central library, but instead is saved to the local library. Having modifications of parts/cells/symbols in your local library that are not imported to the central library eventually will lead to verification errors. This happens because the design will be compared to the central library upon verification, and the part/cell/symbol will be different from the version found on the central library, thus Expedition/DxDesigner will detect an error and stop.
HOW TO AVOID VERIFICATION PROBLEMS: It is highly recommended that when a part/cell/symbol needs modification, the library manager is invoked from OUTSIDE the DxDesigner/Expedition PCB programs. This will always result in modification of the central library rather than the local library.
WHY HAVE THE LOCAL LIBRARY?: Expedition PCB maintains a local library as a safety feature to prevent a user from editing the copy in the central library and then realizing that he/she messed up such that the original copy cannot be recovered. By using the local library when editing parts through DxDesigner/Expedition PCB, users can modify components without worry that they might overwrite the original copy. This provides a possibility of restoring everything back to the original state.
HOW TO MERGE THE LOCAL LIBRARY WITH THE CENTRAL LIBRARY:
By invoking "Library Services" through the library manager, parts can be imported from the local library present in your project as well as from other central libraries. Components present in the local library that are modifications of components in the central library will require an overwrite of the older versions in the central library. If a user would wish to keep the older version then they would need to rename either of the parts to prevent the old version from being overwritten.
A "part" is a mapping between a "symbol" (which represents the connectivity within a schematic) and a "cell" (which is the device footprint on a printed circuit board). The mapping relates physical pins of the footprint with logical net names on the symbol so that the tools know how to maintain and check connectivity and usage of the part within the design. The "Parts Library" is one of the libraries present in any central library. It contains an array of linked Cells and Symbols. The Cells and Symbols are linked in this fashion so that a schematic may be designed using Symbols (where the exact footprint dimensions of the chips are not a factor) while retaining the capability to have all the connections in the schematic be placed on the board using Cells (where the exact dimensions of the chips are a factor). Though schematics can use symbols directly (rather than parts) it is highly advised to design your schematics with parts from the beginning so that they will not have to later be replaced in order to use the board routing software.
A "cell" represents the physical appearance of a device on a printed circuit board. The "Cell Library" is one of the libraries present in the central library. Each cell in this library specifies the details of the footprint of a device. What this means is that the cell has the exact dimensions of the chip package it is named after, including the geometrical patterns that must be present on each of the layers of the PCB. The cell provides the appearance that allows a chip package to be connected to the board (surface mount, through-hole, etc). In practice, "cells" are linked with a symbol in order to form a "part", and it is the "part" that is referenced in schematics and board-level manipulations.
A "symbol" is a formal representation of a component that specifies its input, output, power/ground, and other port attachments. The "Symbol Library" is one of the libraries present in the central library. Each symbol in this library is a representation of a chip that can be used in a schematic. Symbols do not contain the physical ("cell"-level) details necessary for placing the chip on a printed circuit board; in fact, a symbol need not even look like the chip it represents. The primary purpose of "symbols" are for specifying the connections within a project.
A "padstack" is a collection of geometric shapes appearing on each of mask layers surrounding a through-hole in a printed circuit board. There are also padstack-related geometries associated with surface-mounted devices. The "Padstack Library" is one of the libraries present in the central library. Each padstack in this library is a representation of a pad or through-hole to be used in a design. Padstacks are referenced in making Cells; they are very detailed. They contain exact dimensions that must precisely correspond to the description of the manufacturer's package. Our central library has most of the padstacks that we will need already defined, so once you import all of the padstacks to your project's central library, there should be no need to edit them or to create more. If you have the need to create more, access the padstack tutorial for further information.
This is one of the libraries present in the central library. Currently the library is unpopulated. However, there is room to place spice or verilog versions of chips for device emulation. Not needed for this course.
A Gerber file is a standard file format used by printed circuit board fabricators. It contains all data necessary for computer-controlled machines to create the exact mask patterns needed for PCB fab. Gerber files typically specify features such as land patterns, signal traces, and drilled holes, as well as milling and cutting information. The Gerber format in use today is also known as EIA RS-274-X.