Tutorial - Setting Up the Design Constraints in Altium Designer

Parent page: Tutorial - A Complete Design Walkthrough with Altium Designer

Main page: Defining Design Requirements Using the Constraint Manager

Altium Designer's PCB editor is a rules-driven environment, meaning that as you perform actions that change the design, such as placing tracks, moving components, or autorouting the board, the software monitors each action and checks to see if the design still complies with the design constraints. If it does not, then the error is immediately highlighted as a violation. Setting up the design constraints before you start working on the board allows you to remain focused on the task of designing, confident in the knowledge that any design errors will immediately be flagged for your attention.

Design constraints are configured in the Constraint Manager (Design » Constraint Manager)

Command not in the menus?

accessible from both the schematic and PCB sides of the design. In this tutorial, the design constraints will be defined from the schematic side and then transferred to the PCB, along with other design data (components and nets).

All design requirements are configured as constraints in the Constraint Manager.

Defining the Clearance Constraint

The first step is to define how close electrical objects that belong to different nets can be to each other.

This requirement is handled by the clearance design constraints. The Constraint Manager includes the Clearances view that presents the clearance matrix where clearances between net classes in the design can be defined. For the tutorial, a clearance of 0.25mm between all objects is suitable.

Note that entering a value into a cell in the clearance matrix or into the Clearance field will automatically apply that value to all of the fields in the grid region at the bottom of the Constraint Manager when a cell in the clearance matrix is selected. You only need to edit in the grid region when you need to define a clearance based on the object type.

Defining the Width Constraints

The width of the routing is controlled by the applicable width design constraint, which is automatically selected when you run the Interactive Routing command and click on a net.

When you are configuring the constraints, the basic approach is to set the generic constraint to target the largest number of nets and then add specific constraints to target nets with special width requirements, such as power nets. Constraint priority applies automatically based on the natural hierarchy of design objects.

For example, the tutorial design includes a number of signal nets and two power nets. The net constraint for all nets can be configured at 0.25mm. Even though the All Nets scope also targets the power nets, these nets can be specifically targeted by adding a specific constraint.

Defining the Via Style Constraint

As you route and change layers, a via is automatically added. In this situation, the via properties are defined by the applicable via style design constraint. If you place a via from the Place menu, its values are defined by the default primitive settings. For the tutorial, you will configure the via style design constraint.