Added Net Classes for PCB

CircuitStudio 1.4 introduces the ability to add Net Classes to PCB designs. This feature allows designers to manage names and primitive memberships when creating a new, or editing an existing net class. Classes are a way of gathering design primitives in a logical manner, and are often priceless when used to target their member objects through specific design rule scoping.

Net Classes are now also retained when importing Eagle files.

User Defined Net Classes can be created on the Schematic for collections of nets which are not automatically added to a Net Class(Buses and Harnessed Signals are added to a class automatically) through the use of a Net Class Directive(See below), however it is important to mention that if a Net Class Definition exists in PCB only, the ECO process by default will try to remove them to synchronize Schematic and PCB.   If you want to create classes on the PCB, or you have pre-existing classes and the ECO process is trying to remove them change the ECO Generation Options for your project and set the entry for Remove Net Classes in the Modifications Associated With Nets section of the ECO Generation Tab to Ignore Differences

This will allow the Project to detect differences, so it can still add and modify classes as needed, but will prevent the ECO from removing any classes defined in PCB.  Alternatively, you can define all classes on the Schematic through the use of Net Class Directives. 

Place the Directive and Name the class within the Parameter

Net Classes can be easily viewed and managed from the Nets mode of the PCB panel. The top section lists Net Classes, the middle section lists Nets within a selected Net Class(es), and the bottom section lists primitives within a selected Net(s).

Right-clicking on a Net Class entry and choosing Properties from the menu (or double-clicking on the entry directly) opens the Edit Net Class dialog for that class. From this dialog you can view/modify the net membership of the class, rename it, or add additional classes.

As you type within one of the mask fields (Name, Non-Members, Members) above a list, the list is filtered to only show strings that match the mask string. You can use the ? (any single character) and * (any characters) wildcards in the mask string -for example, "*" to display all primitives, or "D?" to display all primitives that start with the letter D. The middle buttons can be used to moveprimitives quickly between the two lists.

Net Classes can also be managed from the Object Class Explorer (Home | Design Rules | Classes) which allows designers to browse and manage the defined object classes for the current PCB document

Click on the entry for a specific Net Class in the folder-tree pane (or double-click on its entry in a summary list) to access controls for managing the object membership of that class.

Net Classes can also be used to define rules within the PCB Rules and Constraints Editor.

The clearance rules from net classes in Eagle are used in all objects within that class of different signals.
You are reporting an issue with the following selected text and/or image within the active document: