Issue link: https://resources.pcb.cadence.com/i/1180268
Working with IDF Best Practices: Working with IDF October 2019 10 Product Version 17.4-2019 © 1999-2019 All Rights Reserved. 4. For IDF-related objects that do not have a unique identifier or unique instance, additional rules are applied. Such objects are VIA_KEEPOUT, ROUTE_KEEPOUT and PLACE_KEEPOUT. ❑ Keepout areas without an IDF_OWNER attribute are not deleted. ❑ IDF keepouts that exactly match Allegro PCB Editor keepouts are ignored. ❑ IDF keepouts that do not match existing Allegro PCB Editor keepouts are imported as is. This may create overlapping keepouts. 5. Because Allegro allows the user to add geometry and text to BOARD GEOMETRY/ OUTLINE, when an IDF file is imported, all items on BOARD GEOMETRY/OUTLINE tagged with IDF_OWNER = MCAD will be deleted. Any other items remain. This occurs regardless of the ownership of the incoming board outline in the IDF file. If any items exist on BOARD GEOMETRY/OUTLINE after the MCAD items are deleted, the following message appears in the log file: WARNING(SPMHXL-48): There is existing geometry on Board Geometry / Outline. This geometry may conflict with the IDF data. Review the board outline in Allegro after idf_in is complete. This conservative approach is necessary because of the relaxed rules about defining a board outline in Allegro. User interaction is needed to correctly resolve the conflict. Component Placement The MCAD/ECAD flow indicates that you import a netlist into the Allegro PCB Editor database prior to importing an IDF file. The database contains components with reference designators. As a result, you can take advantage of the reference designator field in the PLACEMENT section of the IDF file. For example, an Allegro PCB Editor database contains a connector with the reference designator P100 referencing the conn100p_2r_50mm symbol in the netlist. The component itself is not placed. The statements in the PLACEMENT section of an IDF file (shown below) and the rules the enhanced IDF translator applies place the connector P100 at the location specified, using the footprint referenced in the database. .PLACEMENT 500-9999-00 CONN100 P100 3300.00000 3500.00000 0.00000 270.00000 TOP MCAD 600-0000-00 CONN50 P200 3300.00000 1500.00000 0.00000 270.00000 TOP MCAD .END_PLACEMENT P200,however, is placed using the string "500-9999-00" as the name of the footprint. You can control the package name field by changing the value of the ECAD_NAME parameter on