Contact our corporate or local offices directly.
Parent page: PCB Objects
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.
Tracks are available for placement in both PCB Editor and the PCB Library 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.
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:
Additional actions that can be performed during placement include:
While placing track segments there are 5 available corner modes, 4 of which also have corner direction sub-modes. During placement:
A 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. A layer-specific keepout track is simply a Track object with its Keepout property enabled, an all-layer keepout is a Track that has been placed on the Keepout layer.
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:
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.
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.
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.
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.
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.
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:
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.
If the Move action is assigned through these options, the track segment can be rotated or mirrored during the move:
The following methods of non-graphical editing are available:
Dialog page: Track
This method of editing uses the following to modify the properties of a track object.
After placement, the dialog can be accessed in one of the following ways:
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.
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.
Contact our corporate or local offices directly.