The task of creating a component library symbol and its pin data has become an increasingly involved undertaking as components have advanced in complexity. With current large scale BGA devices requiring the placement and configuration of hundreds of pins for example, substantial time and effort is often required to create viable component symbols.
To ease the workload associated with creating component symbols, Altium Designer provides an advanced Schematic Symbol Generation Tool, based on a symbol wizard interface and pin editor dialog. This features automatic symbol graphic generation, grid pin tables and smart data paste capabilities.
The Schematic Symbol Generation Tool is provided as a software extension - Schematic symbol generation tool - which must be installed to enable the tool’s features.
Functionality is provided courtesy of the Schematic symbol generation tool extension (a Software Extension).
The Schematic Symbol Generation Tool becomes available from the Schematic Library editor by choosing the Tools » Symbol Wizard command from the main menus.
To create a new component symbol using the tool, first, add a new component to the active library document. The new symbol can then be developed through the tool's interface - the Symbol Wizard dialog - which opens when the command is launched.
This region displays a preview of the symbol graphic and dynamically represents the current settings and pin data. Use the slider bar or - and + to zoom in/out on the graphic.
While the pin data in the table can be edited to a common value for multiple cells, the dialog's Paste and Smart Paste features provide an advanced way to populate all cell data by bringing in large amounts of different data from external sources.
Within the table, standard copy and paste techniques can be used to populate data from one group of cells to another. For example, by selecting three cells in a column, copying the data (right-click - Copy), then selecting three target cells to paste into (right-click - Paste).
The same technique can be used to copy and paste a data selection from an external source, such as a spreadsheet, text file, or PDF file.
Beyond standard copy and paste techniques, Smart Paste offers the capability to populate multiple columns of data from an external source, using an automated column mapping approach.
To copy several columns of source data into matching columns in the Pin data table, right-click in the table and choose the Smart Paste command from the context menu. This opens the Pin Data Smart Paste dialog, which will be populated with the source data. A range of data delimiters are available, which can be selected to match the delimiters used in the source data.
With its settings and pin data configured as required, the symbol can then be placed into the workspace for the active library component. Placement can be in terms of a single component, or as one section of a multi-part component, using the respective commands available from the context menu associated to the dialog's Place button. Note that if the Continue editing after placement option is enabled, the Symbol Wizard dialog will remain active (allowing further editing) once the component/part has been placed.