The NODRC_SYM_SAME_PIN property, when applied to a board, symbol instance, or symbol definition, disables pin-to-pin conductive layer checking between pins of the same symbol. Pin-to-pin checking always occurs in a symbol editor (.dra). Pin-to-pin spacing checks between different symbols remain unaffected.
This property enables you to:
- Build this property into symbols at the package level by placing the property on the symbol drawing object. It is assumed that the symbol is built correctly in the library. No pin-to-pin spacing checks occur when all symbols of that type are placed on the board. To apply this property while in the symbol drawing, select Edit > Properties from the main menu. In the Find Filter, set the Find by Name to “Drawing” and “Name”. As you select “Drawing” the Edit Property dialog box opens. Select the Nodrc_Sym_Same_Pin property and verify the value is set to “TRUE”. This requires you to update the symbol in the board design if it was already placed.
- Place this property at the design level (.brd or .mcm) on symbol instances. Choose the Symbol type in the Find by Name in the Find Filter input box. No pin-to-pin spacing checks occur on these symbols. While in the board design, select Edit > Properties from the main menu. In the Find Filter, set the Find by Name to “Symbol Type”. This will open the Find by Name or Property dialog box. Select the type of symbol(s) that you want to apply the property to and then from the list of Available Properties select the Nodrc_Sym_Same_Pin property and make sure that the value is set to “TRUE” and click the Apply and OK buttons.
- Place the property on symbol definitions. No pin-to-pin spacing checks occur on these symbols.
- Place the property at the root design level (.brd or .mcm) on the drawing object Choose Drawing in the Find by Name box in the Find Filter. All symbols on the board have pin-to-pin spacing checks disabled. While in the board design, select Edit > Properties from the main menu. In the Find Filter, set the Find by Name to “Drawing”. As soon as you selected “Drawing,” an Edit Property dialog box should have opened. Select the Nodrc_Sym_Same_Pin property and make sure that the value is set to “TRUE”.
If a symbol's pin is modified on the board, for example, you modify a padstack by instance, then the Allegro PCB Editor ignores this property and generates a normal DRC.
If you add the NODRC_SYM_SAME_PIN property to the symbol once it is placed in the board, running the Update - Symbols menu command (refresh_symbol) removes the property.
When you add the NODRC_SYM_SAME_PIN property at the end of the design cycle (recommended), Allegro PCB Editor removes the existing same component Pin-to-Pin DRC markers.
The NODRC_SYM_SAME_PIN property is not supported at the schematic level.