Altium Designer Documentation

Track

Created: July 28, 2015 | Updated: June 19, 2017

The Track Dialog.

Summary

The Track dialog allows the designer to modify the properties of a track object. Note that a line is also a track object, the term line is used to indicate that the object is intended to be a non-net object, so it will not automatically inherit the net name of a touching object. A line also presents a different dialog if Tab is pressed during placement.

Access

The Track dialog can be accessed prior to entering placement mode, from the PCB Editor – Defaults page of the Preferences dialog. This allows the default properties for the track object to be changed, which will be applied when placing subsequent tracks.

During placement, the dialog can be accessed by pressing the Tab key.

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

  • Double-clicking on a track object.
  • Placing the cursor over a track, right-clicking and selecting the Properties command from the context menu.
  • Using the Edit » Change command and clicking once over a placed track object.

Options/Controls

  • Start X/Y - Shows the current X/Y coordinate of the track start point, relative to the current origin.
  • End X/Y - Shows the current X/Y coordinate of the track end point, relative to the current origin.
  • Width - Shows the current width of the track. Edit this field to change the track width, within the range 0.001mil to 10000mil.

Values can be defined in either mm or mil units. When entering a value in units other than the current units, add the mm or mil suffix to the value.

Properties

  • Layer - Define which layer the track is on.
  • Net - Select the Net that this track is to belong to. Note that if track placement commences at the same location as an existing object that is already connected to a Net, then the Net property of the new object is automatically assigned to that Net.
  • Locked - Lock the object so that it cannot be edited graphically.
    If attempting to graphically modify an object that has its Locked property enabled, a dialog will appear asking for confirmation to proceed with the edit. If the Protect Locked Objects option is enabled on the PCB Editor – General page of the Preferences dialog, and the Locked option for that design object is enabled as well, then that object cannot be selected or graphically edited. Double click on the locked object directly and disable the Locked property, or disable the Protect Locked Objects option, to graphically edit the object.
  • Keepout - Check this box to set the object to act as a layer-specific Keepout object. A Keepout object is displayed in the layer color, outlined in the Keepout color. A keepout object is used on a signal layer to create a layer-specific keepout. Layer-specific keepouts are not included during output generation.
  • Solder Mask Expansion - this field allows you to enable and control the expansion to be used with respect to the track on the Solder Mask layer, to create the required opening in the mask. This opening can be larger (a positive expansion value) or smaller (a negative expansion value) than the track itself. The following options are available:
    • No Mask - no opening in the solder mask.
    • Expansion value from rules - choose this option to have the solder mask expansion for the track follow the defined value in the applicable Solder Mask Expansion design rule.
    • Specify expansion value - choose this option to override the applicable design rule and specify the solder mask expansion value for the track.
  • Paste Mask Expansion - this field allows you to enable and control the expansion to be used with respect to the track on the Paste Mask layer, to create the required opening in the mask. This opening can be larger (a positive expansion value) or smaller (a negative expansion value) than the track itself. The following options are available:
    • No Mask - no opening in the paste mask.
    • Expansion value from rules - choose this option to have the paste mask expansion for the track follow the defined value in the applicable Paste Mask Expansion design rule.
    • Specify expansion value - choose this option to override the applicable design rule and specify the paste mask expansion value for the track.
Paste and Solder masks are shown in the negative, that is, when you see an object on one of those layers it is actually a hole or opening in that layer.

Quickly change the units of measurement currently used in the dialog between metric (mm) and imperial (mil) using the Ctrl+Q shortcut. This affects the dialog only and does not change the actual measurement unit employed for the board, as determined by the Measurement Unit setting in the Board Options dialog (Design » Board Options).

Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.

お問合せ

お近くの営業所にお問合せください。

We're sorry to hear the article wasn't helpful to you.
Could you take a moment to tell us why?
200 characters remaining
You are reporting an issue with the following selected text
and/or image within the active document: