Routing is the process of converting the ratsnest, “connection guides”, to real connections whilst following the required design rules. The connections can be made automatically, or manually. Whilst autorouting can be effective in some applications, routed connections are commonly made manually.

Etch Grids

Routing is done on the Etch Grids, defined in Setup>Grids. The Etch Grids can be: regular, a single value, like 0.1mm; irregular, multiple values, like 0.1 0.15 0.1; or repeated values, like 0.1 0.1 0.1 0.1 0.1, which will cause every 5th “grid dot” to be highlighted. The Grid will be switched to the Etch Grids when routing and whenever the Etch Class is the Active Class. A “mix” of pin spacings may mean that a small value for the Etch Grids is required to complete routing between all of the components.

Making Connections

Connections can be added from the Route>Connect menu, by hovering over a “connectable” object and right-clicking>Add Connect (the object type needs to be enabled in Find), or by left-clicking a “connectable” object in Etch Edit Application Mode (again, the object type needs to be enabled in Find). “Connectable” objects are Pins, Vias, existing Connect Lines, shapes and ratsnest lines.

When adding connections, it is important to check the Active and Alternate Layers. The Active Layer is the one that the connections will be added to and the Alternate Layer is the one that will be switched to when a Via is added, at which point the Active and Alternate Layers will swap. If a Pin, or an existing Connect Line, is the selected “connectable” object for the start of a connection, PCB Editor will set the Active Layer to the Layer that the selected “connectable” object is on. For designs with complex cross sections, multiple routing layers and multiple Via types to choose from, using Working Layer can be an advantage since it will issue a prompt when adding a Via to which Layer and which Via should be used to make the connection.

Adding Vias

Vias are added with a right-click>Add Via, or double-click, once the connection has been started. The Via added is determined from the Options settings, Vias that can make connections between the Active and Alternate Layers will be listed, unless in Working Layer connection mode.

Vias can be: “Through”, all routing Layers; “Blind”, exposed on an outer Layer and connecting to inner routing Layers; or “Buried”, connecting two inner routing Layers. Blind and Buried Vias do not block routing channels on all layers and may not cause impedance changes in the same way that Through Vias can. Blind and Buried Vias can be defined in the Padstack Editor and added to the Padstack Library, or defined manually, or automatically, within the PCB board file itself. (Setup>(Auto)Define B/B Vias). Constraint Manager controls which vias can used on nets and is controlled by the Physical Constraint Set. The Auto Define B/B Vias function can create the B/B Vias and assign them to Net Classes but note that automatically creating B/B Vias may result in Via combinations that cannot be manufactured if “all” layers are selected.

Working Layer

When routing the default option is to use the “Active / Alternate” option, routing is added on the Active Layer and switched to the Alternate Layer when a Via is added. This is fine if there are two routing layers and limited Via selection but, for multiple routing layers and Via types, changing to Working Layer mode allows for the “target” Layer and Via to be selected. This can be enabled from the Options pane whilst in an active routing command. Change the Alt drop down to WL then activate the required working layers.

Auto-routing

PCB Editor using any OrCAD PCB Designer license has the ability to autoroute a design using PCB Router, the autorouter. This allows you to run routing modes such as fanout or bus routing as well as a complete autoroute. The autorouter can be run as a standalone tool, requires OrCAD PCB Designer license or above, or directly from inside PCB Editor, any PCB Editor license. There are some things that must be done prior to autoroute which are:-

Check/define etch grids if required. (Coarse grids, >1mm for example, may cause unexpected results from the autorouter)

Check/define cross section (layer stackup).

Check/define appropriate constraints and properties.

Check for NO_ROUTE, FIXED, and NO_GLOSS properties.

Set “through” pins to “full contact” for Shapes.

You may want to save your design before starting any automatic routing.

All content Copyright 2022 Parallel Systems Ltd.