Issue link: https://resources.pcb.cadence.com/i/1180288
Allegro/OrCAD Rigid Flex Design Creation Best Practices _______________________________________________________________________ Learn more at Cadence Online Support - https://support.cadence.com Page 24 © 2016 Cadence Design Systems, Inc. All rights reserved worldwide. Cro ss -Sectio n Tab le Exa m ple Creating Multi-Stackup Zones in the Design Drawing This section of the document focuses on how to create multi-stackup zones in a design. Overview Positioning of different stackups for a rigid-flex design is accomplished by defining Stackup Zones. The user creates the boundary (a shape) of the Zone, then assigns a stackup definition previously created in Cross Section Editor to the zone. Zones are not required for every stackup definition in the design. Any area within the DESIGN_OUTLINE that does not have a zone is defaulted to the Primary Stackup. When creating stackup zones in the design, each stackup zone requires a unique name and be assigned a stackup definition. Options for a constraint set and Room name are available. If either of these two options is selected, a constraint region or room geometry is created for the optional object. The optional geometries are copies of the zone boundary and are grouped with the zone so that when any boundary changes are made to a zone, the associated constraint region and room are also updated. If the zone is deleted, so are the constraint region and the room. IMPORTANT NOTE: In the 17.2 QIR 1 release, there are specific rules and processes that must be followed to correctly define zones. 1. The DESIGN_OUTLINE is used for the outer extents of the design. Zone trimming will only apply to the DESIGN_OUTLINE or another ZONE boundary. 2. Zones cannot be overlapped or nested. If a zone is added and intersects/overlaps with an existing zone, the newer zone will be trimmed to the existing zone boundary. 3. When a zone is first defined with pre-existing symbols, traces, vias, or conductor shapes within the boundary, the stackup assignment for that zone may fail. The symbols, traces, vias, conductor shapes must be moved out of the area where the zone will be defined, and the stackup reassigned. After that the moved or deleted objects can be replaced. Traces and shape placement within a zone will fail if the layer they are defined on no longer exists. 4. If any symbols, traces, vias, and/or conductor shapes are placed on the design within a zone, and the zone stackup assignment is altered, the modification will fail. The symbols, traces, vias, conductor shapes must be moved out of that zone prior to the new stackup assignment. After the modifications are complete, the objects can be replaced. Traces and shape placement within a zone will fail if the layer they are defined on no longer exists. Creating a Zone A zone is created in the Zone Creation tool. To create a zone, perform the following steps: 1. In PCB Editor, choose the Setup - Zones - Create menu. The Options Tab displays the parameters for the Zone definition. 2. Specify the zone name and the stackup definition to be assigned to that zone.