Средство формирования схемных символов

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.

Extension Access

Functionality is provided courtesy of the Schematic symbol generation tool extension (a Software Extension).

The Schematic symbol generation tool
extension.

The Symbol Wizard functionality can only be accessed provided the Schematic symbol generation tool extension is installed as part of your Altium Designer installation. This extension is installed by default when installing the software, but in case of an inadvertent uninstall, it can be found back on the Purchased tab of the Extensions & Updates page (accessed from the  drop-down then choose Extensions and Updates). If reinstalling, you will need to restart Altium Designer once the extension has been successfully downloaded and installed.

Creating a Symbol

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.

• Number of Pins - manually type or use the up and down arrows to increase or decrease the desired number of pins.
• Layout Style - choose from a set of predefined patterns for where the pin positioning is automatically assigned. Use the drop-down to select the preferred arrangement. The Preview image to the right and the data in the Side column will be updated accordingly. Selections include:
  • Dual in-line
  • Quad side 
  • Connector zig-zag 
  • Connector 
  • Single in-line 
  • Manual
    The Manual configuration denotes that pin positions are not automatically assigned. The layout style will revert to this setting when the pin positioning of a standard style (Quad side, Connector zig-zag, and Single in-line) has been edited.

Grid

• Position – the reference position index of a symbol pin. This data is not editable.
• Group – a manually entered string used to define a collective group of pins.
• Display Name – the component pin’s display name attribute string.
• Designator – the pin’s designator attribute string. This will automatically match the pin Position by default.
• Electrical Type – use the drop-down in the field to select the electrical type for the pin. Selections include Input, I/O, Output, Open Collector, Passive, HiZ, Open Emitter, and Power.
• Description – the pin’s description string attribute.
• Side – use the drop-down in the field to select the position of the symbol. Select from Left, Bottom, Right, and Top. When this region has been changed, the Layout style setting changes to Manual.

Right-click Menu

• Move Up - use to move the selected data up one row.
• Move Down - use to move the selected data down one row.
• Copy - use to copy the selected data to the clipboard.
• Paste - use to paste the most recent data that was copied to the clipboard to the cursor position.
• Smart Paste - use to open the Pin Data Smart Paste dialog to copy several columns of external source data into matching columns in the grid. Use the dialog to configure the column data and delimiters, then click Paste.
• Clear - use to delete the pin data.

Preview

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.

Additional Controls

• Continue editing after placement - if checked, the dialog will remain active (allowing further editing) once the component has been placed.
• Place - use to place the completed symbol and pin data. Choices include:
  • Place Symbol
  • Place New Symbol
  • Place New Part

Pasting Pin Data

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.

An example of pasting data copied from an external spreadsheet, into the Pin data table.

Smart Paste

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.

Symbol Placement

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.