Altium Designer Documentation

Configuring PCB Region Object Properties in Altium Designer

Created: 15.06.2017 | Updated: 14.03.2018
Полное содержание

Parent page: Region

PCB Editor object properties are definable options that specify the visual style, content and behavior of the placed object. The property settings for each type of object are defined in two different ways:

  • Pre-placement settings – most Region object properties, or those that can logically be pre-defined, are available as editable default settings on the PCB Editor - Defaults page of the Preferences dialog (accessed from the  button at the top-right of the workspace). Select the object in the Primitive List to reveal its options on the right.
  • Post-placement settings – all Region object properties are available for editing in the Properties panel when a placed Region is selected in the workspace.

The Region default settings in the Preferences dialog and the Region mode of the Properties panel   The Region default settings in the Preferences dialog and the Region mode of the Properties panelThe Region default settings in the Preferences dialog and the Region mode of the Properties panel

In the below properties listing, options that are not available as default settings in the Preferences dialog are noted as "Properties panel only".

Net (Properties panel only)

This region is available only when Copper is selected as the Kind in the Properties region.
  • Net - use to choose a net for the region. All nets for the active board design will be listed in the drop-down list.
  • Net Class - displays the net class. Ths field is dependent upon the net selected in the Net field and is not editable.
  • Net Length - displays the net length. Ths field is dependent upon the net selected in the Net field and is not editable.

Properties

  • ​​​Layer - this field is available only when Kind is set to Copper, Polygon Cutout, or Cavity. Use it to specify the layer on which the region is placed. For Copper and Polygon Cutout, all defined (and enabled) layers for the active board design are listed in the drop-down list. For Cavity, only enabled mechanical layers are listed.
Note that the Cavity Kind is only available when in the PCB Library Editor.
  • Kind - use the drop-down to select the function of the region:
    • Copper - a solid, positive area that can be placed on any design layer, such as a signal (copper) layer.
    • Polygon Cutout - functions as a polygon cutout defining a negative or no-copper area within a polygon. Repour the polygon after placing a Cutout.
    • Board Cutout - functions as a board cutout defining a negative area or hole within the board shape.
    • Cavity - used to define an embedded cavity within which a component will reside 'inside the board'. A region of this kind only can be placed on a suitable mechanical layer and must completely enclose the 3D body of the component with sufficient clearance on each side. Check with the fabricator to find out how much clearance is required.
Note that the Cavity Kind is only available when in the PCB Library Editor.
  • Cavity Height - enter the cavity height. This option is available only when Kind is set to Cavity.
  • Locked (Properties panel only) - enable to protect the region from being graphically edited.

Outline Vertices (Properties panel only)

This region is used to modify the individual vertices of the currently selected region object. You can modify the locations of existing vertices, add new vertices or remove them as required. Arc connections between vertex points can be defined and support is also provided for exporting vertex information to and importing from a CSV-formatted file. You also can adjust the position of the region object by globally applying delta-x/delta-y values to all vertex points.

  • Vertices Grid - lists all of the vertex points currently defined for the region in terms of:
    • Index - the assigned index of the vertex (non-editable).
    • X - the X (horizontal) coordinate for the vertex. Click to edit.
    • Y - the Y (vertical) coordinate for the vertex. Click to edit.
    • Arc Angle (Neg = CW) - the angle of an arc that is drawn to connect this vertex point to the next. By default, connections are straight line edges with this field remaining blank. Click to edit then enter an arc angle as required. Entry of a positive value will result in an arc drawn counterclockwise. To draw a clockwise arc, enter a negative value.
Straight line edges are used to connect one vertex point to the next. If you would rather have an arc connection, enter a value for the required Arc Angle. Entry is made in the field associated to the source vertex point with the arc being from this vertex to the subsequent vertex below in the list.
  • Add - click to add a new vertex point. The new vertex will be added below the currently focused vertex entry and will initially have the same X,Y coordinates as the focused entry. Click the  to remove the currently selected vertex.
Paste Mask Expansion
  • Rule/Manual - select the desired paste mask expansion configuration. When Manual is selected, you can enable and enter the desired measurement.

Solder Mask Expansion

  • Rule/Manual - select the desired solder mask expansion configuration. When Manual is selected, you can enable and enter the desired measurement.
Обнаружили проблему в этом документе? Выделите область и нажмите Ctrl+Enter, чтобы оповестить нас.

Связаться с нами

Связаться с нашими Представительствами напрямую

We're sorry to hear the article wasn't helpful to you.
Could you take a moment to tell us why?
200 characters remaining
Вы сообщаете о проблеме, связанной со следующим выделенным текстом
и/или изображением в активном документе: