Issue link: https://resources.pcb.cadence.com/i/1180284
Electrical Design, Mechanical Design Incremental Data Exchange in Allegro PCB Editor October 2019 9 Product Version 17.4-2019 © 1999-2019 All Rights Reserved. Recommended Flow Steps MCAD initiation This section outlines the preferred flow for establishing the first steps in defining a baseline with the MCAD tool as the initiator. This flow assumes that board outline, restricted areas, mounting holes and components locations are to be defined. 1. The MCAD designer creates the initial board with the following items: a. Board outline – the physical board outline with routed cut-outs. b. Mounting holes – Drill holes, such a mounting and tooling-holes not associated with any physical part, placed by the ECAD tool. c. Component boundary areas – One component keep-in area. Usually, this area is within the bounds of the board outline but may extend beyond the board outline. Various package keep out areas may be defined where component placement and component height restrictions may apply for top, bottom, and all other layers. Definitions such as, external layers apply only, and any internal layer, which are valid for an ECAD tool, may be ignored or converted to "ALL" in the MCAD tool. d. Conductor boundary Areas – Only one conductor keep-in area (ROUTE_KEEPIN) may be defined. Various conductor keep-out (ROUTE_KEEPOUT) areas where placement of conductor material is not allowed may be defined. Restrictions may apply for top, bottom, and all layers. Definitions such as, external layers apply only, and any internal layer, which are valid for an ECAD tool, may be ignored or converted to "ALL" in the MCAD tool. e. Via Keep out Area – Areas where via locations are restricted. Restrictions may apply for top, bottom and all layers. External layers apply only, any internal layer definition may be ignored or converted to "ALL" in the MCAD tool. f. Key parts or components that do not require reference designators may be placed at this time. A mapping file may be required in the MCAD tool, to map the MCAD part model name with the Allegro symbol model name. Any component or part that requires a reference designator should not be placed at this time. 2. The MCAD designer exports an IDX baseline. The newly generated baseline is passed to the Allegro PCB Designer. 3. The Allegro PCB Designer imports the IDX baseline. 4. The Allegro PCB Designer places parts that require a reference designator within the board outline. The Allegro designer exports the new placement data (selecting only those placed parts as incremental export data) as an incremental IDX file. The incremental IDX file is then sent to the MCAD designer.