Getting ready to route

Once the components are positioned on the board, you are ready to start routing. Before launching into Altium Designer's routing features, let's cover the features that will help you manage the routing process.

Is it Ready to Route?

There is a saying that PCB design is 90% placement and 10% routing. While you could argue about the percentage of each, it is generally accepted that good component placement is the most important aspect to good board design. Keep in mind that you may need to tune the placement as you route too, perhaps running a test autoroute on a dense area first, tweaking the placement to improve routability.

Prioritizing the Routing

Where to begin, you ask? An autorouter typically routes connections one by one, whereas a human can consider the impact of many connections simultaneously. For the autorouter to have any hope it must do a good job of ordering the connections for routing. It will use factors such as connection length, density of connections, assignment of direction to routing layers, alignment of the connection direction to routing directions, and so on. And if it is any good, it will review the order constantly as it routes. A human will consider these factors as well, but will also use higher-order skills, such as will this set of 16 routes pass between those two components, should these noisy nets be routed on a separate pair of layers from these sensitive nets, and so on.

Finding that Net

An unrouted board can appear intimidating - a mass of connection lines criss-crossing all over the board. Controlling the display of the connection lines and setting their color will help you manage the routing process.

Using the PCB Panel

A valuable feature is the PCB Editor's ability to mask, or filter objects in the workspace. This feature will fade out everything except the object(s) of interest. To explore this, set the mode of the PCB panel (upper dropdown list) to Nets, this will display a list of nets on the board. As you click on a net name in the panel the workspace display will change, zooming to show the nodes in the net, and fading out everything except the pads and connection lines in the net - effectively pulling out that net from the rest of the board. Note that even when you click in the workspace the mask remains, the chosen net remains clearly visible, making it easy to examine or route. Click the Clear button at the bottom right of the workspace to clear the mask and restore the entire workspace to normal brightness.

Note that as well as an individual net, you can mask a class of nets (if any classes are defined), and also multiple nets (by holding the CTRL key as you click in the PCB panel to select a net name).

Changing the Connection Line Color

Main article: Controlling the Color of Connection Lines

When the design is transferred from the schematic into the PCB workspace, a view configuration that controls the workspace environment and visibility of many elements is applied. View configurations are available for use in both 2D and 3D workspaces and are defined and edited in the View Configurations dialog (Design » Board Layers & Colors [shortcut L]) and can be saved and re-used. An easy way to make important nets stand out is to change the color of their connection lines. To do this, double-click the net name in the PCB panel to open the Edit Net dialog, where you can edit the connection line color. You can also highlight the display of connection lines using their layer colors, for more information refer to Controlling the Color of Connection Lines.

Hiding/Displaying Connection Lines

As an alternate to masking, you can completely hide one, many, or all of the connection lines. There are a number of commands to control the display of connection lines in the View - Connections submenu. You can also access these commands while you are working by pressing the N shortcut key.

Are the Design Rules Defined?

Before you start routing you need to configure the applicable routing design rules. Select Design - Rules from the menus to display the PCB Rules and Constraints Editor dialog. The tree on the left of the dialog shows the 10 rule categories (Electrical, down to Signal Integrity). In each category there are a number of rule types, for example, there are eight different types of routing rules you can define.

Selecting a rule type will display all the rules of that type that are currently defined. The image below shows the four routing width rules defined for a board. Note rule priority, this defines the precedence of the rules, with 1 being the highest.

Routing width rules defined for a board.

Click on an individual rule name in the tree on the left of the dialog to display the settings for that rule. There are two distinct parts to every design rule, the constraint - what are my requirements, and the scope - what do I want this rule to target. Using the routing width design rule as an example, let's look at this in more detail.

The Rule Constraints

Rule constraints specify the settings or limits you want applied to the objects targeted by this rule.

For the Width rule, constraints are for minimum, preferred and maximum widths of the track segments that make up the routing. Note that the min / preferred / max settings can also be defined for each of board layer, giving you complete control over how the board is routed. A handy feature to know is that you can increase and decrease the routing width as you route, between the minimum and maximum settings, read about this in the Changing the Track Width while Interactively Routing section.

The rule constraints define the requirements of that rule. This rule specifies that the routing width must be between 0.2mm and 0.6mm.

The Rule Scope

Altium Designer has a powerful and flexible rule definition system, making it possible to exactly specify the design requirements, however complex they might be. Rather than defining routing requirements as attributes of the objects, design rules are defined separately, and then target the objects they apply to via the rule's scope along the lines of 'I want this rule to apply to those objects'.

The scope of the rule is specified by entering a query that defines what objects this rule will target.

It is this ability to exactly scope each rule, in combination with the ability to assign each rule's priority that gives you complete control over the PCB design requirements. The rule constraint image shows the scope of a routing width design rule that is targeting the GND net. If the scope (Full Query) of the rule had been set to All, then it would apply to All nets on the board. Rules are scoped by writing a query. The query is written automatically if you select from the options on the left of the dialog, like All, Net, Net Class, and so on. If you are new to writing queries then try the Query Builder, it will walk you through the process and write the query for you.

The Width Rule

The most basic routing rule is the Routing Width rule, which determines the width that the nets will be routed at. As a minimum, your design will have one width rule, targeting all nets on the board.

It is not good design practice to have only one width rule for a board, with the minimum width set to the smallest routing width you need on the board, and the maximum set to the widest route you need. A better approach is to have one rule that targets the largest number of nets, with a scope of All . You then add extra rules that target individual nets or classes of nets, such the GND net, or the PowerNets net class (if such a class has been created). These rules will have a higher priority, so whenever you start to route one of these nets the higher priority rule will override the All nets rule, giving you the correct routing width. Suitable Width rules need to be defined before you start routing.

The Clearance Constraint

The partner to the width rule is the clearance constraint, which defines how close the net you are routing is allowed to get to other objects on that layer of the board. Again you can define multiple clearance constraints, to keep higher voltage nets or differential pair nets away from other routing, to keep polygon pours a specific distance from routing, and so on. Suitable Clearance Constraints need to be defined before you start routing.

Setting Up the Routing Layers

Routing layers, also referred to as signal layers, are set up in the Layer Stack Manager dialog (Design - Layer Stack Manager) shown below. Use the dialog controls to add layers and set their location in the layer stack.

Electrical layers are added in the Layer Stack Manager dialog.

The display of all layers, and the addition of mechanical layers, is controlled in the View Configurations dialog (shortcut L)\ shown below.

The display of all layers is controlled in the View Configurations dialog.

See Also