Working with a Track Object on a PCB in Altium Designer

Parent page: PCB Objects

Track objects are used for routing and for general purpose drawing lines. There are 4 placed track segments in
the image above, and another in the process of being placed.

Summary

A Track segment is a primitive design object, a straight line of a defined width. Use tracks to define a straight line in the PCB workspace. Tracks are placed on a signal layer to form the electrical interconnections, or routing, between component pads. Tracks placed on a non-electrical layer are called Lines, where they are used as general-purpose drawing elements to create component outlines, instructional information, keepout boundaries, and so on. Tracks are also used in group design objects, such as dimensions and coordinates.

Availability

Tracks are available for placement in both PCB Editor and the PCB Library Editor.

PCB Editor

In the PCB Editor different commands are used for placing tracks, depending on whether you wish to place the track on a signal layer to route a connection, or place it on a non-electrical layer as a drawing-type line. Although tracks and lines are actually the same object, the difference is how the software behaves during their placement, which is why there are different commands. When a track placement command is run, such as Interactive Routing, the software monitors the click location and automatically adopts the net name of an existing object (such as a pad) under the click location. It also monitors and obeys any applicable design rules. When a line placement command is run, these monitoring behaviors do not occur. 

• To place a Track object:
  • Click Place » Interactive Routing from the main menus.
  • Place » Keepout » Track from the main menus.
  • Click the button  in the Wiring toolbar.

• To place a Line object:
  • Click Place » Line [P, L] from the main menus..
  • Click the button  from Utilities toolbar, then click the  button from drop down list.

PCB Library Editor

To place a Line object, click Place » Line [P, L] or click the button from the PCB Lib Placement toolbar.

Placement

Regardless of which command is used (routing or line placement), the basic placement behavior is the same. After launching the command, the cursor will change to a crosshair and you will enter track placement mode. Placement is made by performing the following sequence of actions:

1. Click or press Enter to anchor the starting point for the first track segment. If a routing-type placement command is being run and you click to start placement on an existing object, the track will adopt the net name of that object. The width will be determined by the applicable Routing Width design rule, but this can be overridden by certain interactive routing options, which are described in more detail below.
2. Move the cursor to define the track segment and click or press Enter to anchor the end point for this first segment, which is also the start point for the next connected segment.
3. Continue to position the cursor and click or press Enter to anchor a series of vertex points that define the series of connected track segments.
4. Right-click or press Esc to end the current series of connected track segments.

Additional actions that can be performed during placement include:

• Press the * key to cycle through the available signal layers. If performing track placement a via is automatically added at each signal layer change, in accordance with the defined drill pairs and the applicable Routing Via Style design rule. Alternatively, use the Shift+Ctrl+Wheel Roll combination to move through the routing layers, each notch of the mouse wheel will move to the next (or previous) available signal layer.
• Press the + and - keys on the numeric keypad to cycle forward and backward through all layers currently visible in the design.
• Press the Tab key to access an associated properties dialog, from where properties for the track can be changed on-the-fly:
  • Track placement - the Interactive Routing dialog will appear.

• Line placement - the Line Constraints dialog will appear.

Placement Modes

While placing track segments there are 5 available corner modes, 4 of which also have corner direction sub-modes. During placement:

• Press Shift+Spacebar to cycle through the 5 available corner modes: 45 degree, 45 degree with arc, 90 degree, 90 degree with arc, and Any Angle.
• Press Spacebar to toggle between the two corner direction sub-modes.
• When in either of the arc corner modes, hold the  or  keys to shrink or grow the arc. Hold the Shift key as you press to accelerate arc resizing.
• Press the 1 shortcut key to toggle between placing 1 segment per click (the first 5 images just below), or 2 segments per click (the last image in the set just below). In the first mode the hollow track segment is referred to as the look-ahead segment.
• Press the Backspace key to remove the last vertex.

Press Shift+Spacebar to cycle through the 5 available corner modes, press Spacebar to toggle the corner direction, press the 1 shortcut to
toggle placement between 1 segment or 2 segments.

Placing a Track as a Keepout

Using the Place » Keepout » Track command Track can be placed as a layer-specific keepout object or an all-layer keepout to act, for example, as a placement or routing barrier. Objects defined as keepouts are ignored during output generation, such as photo plotting and printing.

Keepout properties and restrictions can be assigned using the Keepout - Line dialog.

To access the Keepout - Line dialog, press Tab during placement. After placement, access the dialog by double-clicking on the Keepout Track or right-click and select Properties from the context menu.

Interactive Routing and the Applicable Design Rules

During Interactive Routing the default behavior is for the software to ensure the track segments are placed in accordance with the applicable Electrical and Routing design rules. That means the software will not allow a new track segment to be placed so that it violates an existing track segment that belongs to a different net, instead it will clip the track segment to meet the design rules. This interactive routing behavior is known as the Routing Conflict Resolution mode. The default mode is Stop at First Obstacle (the current mode is displayed on the Status bar), press Shift+R to cycle through the available modes.

The term applicable design rules means all those rules that apply to the object being placed. The design rules engine works on a system where the designer scopes exactly which objects they want each rule to apply to. During placement the design rules engine is queried to determine the highest priority rule that applies in the current placement situation. Rules that apply during Interactive Routing include:

• Electrical Clearance
• Routing Width
• Routing Via Style

The animation below demonstrates routing in action. The net GND is being routed in accordance with a defined, and applicable Routing Width design rule. Note that when the cursor is moved over the via associated to the +12V net, the route is automatically being clipped to ensure the applicable Electrical Clearance Constraint design rule is being met.

The applicable routing width and clearance design rules are automatically obeyed during interactive routing.

How the Routing Width is Determined

Unless the rules engine is disabled, the overriding behavior of the software is to always ensure that the routing width is within the range allowed by the applicable Routing Width design rule. A common approach is to allow a range of widths to be used for a net, to give the designer flexibility in fitting in the route, while satisfying the current carrying requirements of that net. Supporting this, the Routing Width design rule has Min, Preferred and Max settings which can be configured to allow a range of widths, or can be set the same to require a specific width. The width can also be configured as an Impedance, and can also have a different range specified for each signal layer.

The default Routing Width design rule that is applied to all nets for a new PCB.

As the designer, you have a number of options that can help select the most appropriate routing width when you commence routing, these are configured on the PCB Editor — Interactive Routing page of the Preferences dialog, as shown below.

Interactive Routing preferences, note the Interactive Routing Width Sources options, these
determine what size is used when you start a route.

Note the Track Width Mode, this is set to Rule Preferred in the image above, so when the route commences on an existing net object, such as a pad, this is the width that will be used. WHowever, if the route commences on an existing track, then the Pickup Track Width From Existing Routes option will override the Track Width Mode, and set the new width to match the existing width.

As the designer, you can also press the Shift+W shortcut while routing to access the a variation of the Favorite Interactive Routing Widths dialog (shown below), where a different width can be selected, or you can press Tab and open the Interactive Routing for Net dialog, and type in a new width value. The value chosen or entered must lie between the Min and Max settings defined in the applicable rule, if it does not it is automatically clipped back to the nearest of these. Note that pressing Shift+W will also switch the Track Width Mode to User Choice, reflecting that you have chosen to override the rule settings and manually select a width.

Press Shift+W to open this dialog and select a different width
from your list of preferred sizes.

Interactive Routing Shortcuts

While you are routing, there are a number of shortcuts that are available, for example you can press Shift+R to cycle through the available conflict resolution modes, or press Backspace to rip up the last placed vertex (corner). To display a list of shortcuts while you are routing, press Shift+F1, or ~ (Tilda). A list of available interactive shortcuts will be displayed, either select the required shortcut, or press Esc to close the menu and then use the shortcut key sequence.

Graphical Editing

This method of editing allows you to select a placed track object directly in the workspace and change its size, shape or location, graphically.

When an track object is selected, the following editing handles are available:

A selected Track.

• Click and drag A to reposition the end points of the track.
• Click and drag B to change the shape of the track.

The PCB editor includes sophisticated algorithms for moving track segments on the board, so that the neat arrangement of the routing can be maintained. This sliding of track segments can be invoked interactively, either by clicking to first select the track segment and then clicking and holding when the special cursor appears to slide the segment, or by simply clicking and holding on a track segment and sliding it. Sliding behavior can be configured using the Dragging options on the PCB Editor - Interactive Routing page of the Preferences dialog. These options allow you to assign the Move action to a track, useful if you want to be able to freely move an individual track segment.

Control track sliding behavior with dragging options set at the preferences level.

If the Move action is assigned through these options, the track segment can be rotated or mirrored during the move:

• Press the Spacebar to rotate the segment anti-clockwise or Shift+Spacebar for clockwise rotation. Rotation is in accordance with the value for the Rotation Step, defined on the PCB Editor – General page of the Preferences dialog.
• Press the X or Y keys to mirror the segment along the X-axis or Y-axis respectively.

Non-Graphical Editing

The following methods of non-graphical editing are available:

Via an Associated Properties Dialog

Dialog page: Track

This method of editing uses the following to modify the properties of a track object.

Individual track segments can be edited in the Track dialog.

After placement, the dialog can be accessed in one of the following ways:

• Double-clicking on the placed track object.
• Placing the cursor over the track object, right-clicking and choosing Properties from the context menu.
• Run command Edit » Change, then click an existing object.

Editing via an Inspector Panel

Panel pages: PCB Inspector, PCBLIB Inspector, PCB Filter

An Inspector panel enables the designer to interrogate and edit the properties of one or more design objects in the active document. Used in conjunction with appropriate filtering - by using the PCB Filter panel or the Find Similar Objects dialog - the panel can be used to make changes to multiple objects of the same kind, from one convenient location.

Editing via a List Panel

Panel pages: PCB List, PCBLIB List, PCB Filter

A List panel allows the designer to display design objects from one or more documents in tabular format, enabling quick inspection and modification of object attributes. Used in conjunction with appropriate filtering - by using the PCB Filter panel or the Find Similar Objects dialog - it enables the display of just those objects falling under the scope of the active filter – allowing the designer to target and edit multiple design objects with greater accuracy and efficiency.