Altium Designer Home
...
((Dialog Reference))_AD
Dialogs((S to Z))_AD
SchLibGenerationTool_Dlg-SymbolWizardSymbol Wizard_AD
The Symbol Wizard dialog
Summary
The Symbol Wizard dialog is used to create component symbols. The dialog features automatic symbol graphic generation, grid pin tables and smart data paste capabilities.
Access
The Symbol Wizard dialog is accessed in the following ways:
- From the Schematic Library editor, by selecting Tools » Symbol Wizard from the main menus.
- From the Component Editor in its Single Component Editing mode, by clicking the drop-down icon on the button below the symbol model and selecting Wizard from the menu.
The Symbol Wizard dialog available through an Altium Designer Extension application, which is automatically installed with Altium Designer. The extension can be manually installed/removed or updated from the Altium Designer Extensions and Updates page (select the Extensions and Updates option from the system User menu – 
). The Schematic symbol generation tool extension is located within the Installed tab and within the Updates tab when a software update is available.
► See Extending & Updating Your Installation for more information on installing and managing Altium Designer Extensions.
Options/Controls
- 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
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 (presented only if the dialog was accessed from the Schematic Library editor) - use to place the completed symbol and pin data. Choices include:
- Place Symbol
- Place New Symbol
- Place New Part
Notes
- The position and size of the Symbol Wizard dialog are automatically saved. You can resize and move the during use, and the next time the dialog is opened, the size and location of the dialog remain as the previous use.
- Pin names entered with slashes in the Display Name column of the dialog's grid will be recognized as alternate pin names and added to the generated symbol's pin properties.