Search In: Doc:Documentation: Altium CircuitStudio
Altium DesignerAltium 365Altium MCAD CoDesignerAltium On-Prem Enterprise ServerAltium CircuitMakerCompany DashboardAltium Infrastructure Server
Close
Search Search on Documentation
Documentation Altium CircuitStudio ... PCB Dialogs

Board Options

Created: December 16, 2024 | Updated: August 14, 2018
Other Related Resources
Project Options (Dialog)

Parent page: PCB Dialogs

The Board Options dialog

Summary

The Board Options dialog provides a range of options, including measurement units, sheet display, and snap settings, that affect only the active PCB document. They can, therefore, collectively be thought of as local-level options rather than global options (that are set for all PCB documents in the Preferences dialog).

Access

The dialog can be accessed from both the PCB Editor and PCB Library Editor:

  • PCB Editor - click Home | Board | from the main menus or right-click in the workspace then use the Options » Board Options command from the context menu.
  • PCB Library Editor - click Home | Board | from the main menus or right-click in the workspace then use the Options » Library Options command from the context menu.

Options/Controls

Measurement Unit

  • Unit - select the default measurement units for the current PCB document. Click to select from either metric (mm) or imperial (mil) units. Default units are used to display any distance related information on screen or in reports.
The default units are always used if a unit suffix (mm or mil) is not entered when specifying any distance related information in any dialog editing fields. Quickly change the units of measurement currently used in a 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.

The measurement unit employed for the board can also be changed directly from the Ribbon menus using the 

and  buttons in the Home | Grids and Units region.

Designator Display

It can be difficult to position the designator strings in a multi-channel design since they can end up being quite long. As well as choosing a naming option that results in a short name, another option is to display just the original, logical component designation instead. For example, C30_CIN1 would display as C30. This would, of course, necessitate some other notation being added to the board to indicate the separate channels, such as a box being drawn around each channel on the component overlay. Use this field to determine how designators are to be displayed. The following options are available:

  • Display Physical Designators - choose this option to display the physical designators. These are the designators displayed on the compiled tab views of the schematic source documents. For multi-channel designs, designator format is determined by the Designator Format field on the Multi-Channel tab of the Options for Project dialog. Physical designators are unique, e.g., R1_CH1.
  • Display Logical Designators - choose this option to display the logical designators. These are the designators displayed on the Editor tab views of the schematic source documents. Logical designators are not unique, for example the R1_CH1 physical designator will become R1.
If you choose to display the logical designators for components in a multi-channel design, these will be displayed on the PCB and in any output generated, such as prints and Gerber's. The unique physical designators, however, are always used when generating a Bill of Materials.

Route Tool Path

  • Layer - use this field to choose the mechanical layer (from those currently enabled for use in the design) on which to define the route tool path for the board. Controlling the display of this path when viewing the board in 3D is performed using the Show Route Tool Path option on the Physical Materials tab of the View Configurations dialog (accessed by pressing the L key when in 3D viewing mode).

Sheet Position

This region provides controls relating to the PCB Sheet. The PCB Sheet is a special drawing feature used to represent the printed page in 2D Layout Mode. The sheet is not a design object, but rather is a display feature designed to work with objects placed on a mechanical layer (such as dimensions, notes, and title blocks). When you create a new PCB file, a default sheet is automatically created. It is not shown initially, but when enabled, appears as the white shape behind the design objects present in the workspace.

  • X - use this field to enter the X (horizontal) coordinate for the bottom-left corner of the sheet.
  • Y - use this field to enter the Y (vertical) coordinate for the bottom-left corner of the sheet.
The coordinates are measured in relation to the absolute origin, which is the bottom-left corner of the workspace. The distance can be defined in either metric or imperial units regardless of the default units for the board. To specify the units when entering a size, add the mm or mil suffix to the value.
The position of the PCB (the board shape) does not change with sheet position since the PCB position is referenced from the absolute origin. To see the absolute origin reference point, enable the Origin Marker option on the View Options tab of the View Configurations dialog.
  • Width - use this field to enter a custom width for the sheet.
  • Height - use this field to enter a custom height for the sheet.
  • Display Sheet - enable this option to display the sheet in the workspace. The sheet can be hidden at any time by disabling this option. All linked mechanical layers will also be hidden.
  • Auto-size to linked layer - with this option enabled, you can use the Home | Board |  » Auto-Position Sheet command to automatically resize the Sheet to exactly enclose the objects on any linked mechanical layers.
CircuitStudio's \Templates sub-folder includes a variety of template PCB files that include sheet borders for different paper sizes. Open the appropriate sized template and copy the contents of the relevant mechanical layers into your current PCB design.

UniqueID

The current unique identifier for the board. The Unique ID (UID) is a system-generated value that uniquely identifies this board. A new UID value can be entered directly into this field.

  • Reset - click this button to have the system generate a new UID for the board.

Snap Options

  • Snap To Grids - enable this option to allow the cursor to snap to the default cartesian grid defined for the board.
  • Snap To Linear Guides - enable this option to allow the cursor to snap to manually placed linear Snap Guides.
  • Snap To Point Guides - enable this option to allow the cursor to snap to manually placed point Snap Guides.
  • Snap To Object Axis - enable this option to allow the cursor to snap to dynamic alignment guides created through proximity to the hotspot(s) of placed objects<.
    • Advanced/Simple - use this control to accessed advanced options for this feature.
  • Snap To Object Hotspots - use this option to toggle whether the cursor can snap to the hotspot(s) of placed objects when it is simultaneously close (on both the X and Y axes) to such a hotspot.
    • Range - use this field to define the electrical grid range. This value determines how close you need to get to an electrical object's hot-spot before the cursor will snap to it, even if the object is not on the Snap Grid. In general, you would set the Electrical Grid range to a setting somewhat less than the Snap Grid. For example, if the Snap Grid is set to 50mil, an appropriate Electrical Grid range would be 30mil. Enter a value directly or choose one of the predefined values available from the field's drop-down.
    • Snap On All Layers - enable this option to allow the cursor to snap to any electrical object on any visible layer. When this option is disabled, the cursor will only recognize and snap to objects placed on the currently selected layer.
When in Single Layer mode, the Electrical Grid will only apply to electrical objects on the current layer.
  • Snap To Board Outline - enable this option to allow the cursor to snap to the board outline. This option can be useful for dimensioning a PCB, particularly when the board corners or vertices are off the Snap Grid.
  • Snap To Arc Centers - enable this option to allow the cursor to snap to the centers of placed arc objects.

Advanced Options - Snap To Object Axis

  • Near Range - use this field to specify the distance the cursor can be from an enabled object, inside which that object's hotspot will cause the cursor to snap to a system-generated dynamic alignment guide.
  • Near Objects - when this option is enabled, the required design objects are used as snap point sources as the cursor is moved near to them.
  • Far Objects - when thi open is enabled, the required design objects are used as snap point sources when the cursor is further away from an object, beyond the specified Near Range. An enabled object's hotspot will continue to cause the cursor to snap to a system-generated dynamic alignment guide at this greater distance.

Additional Buttons

  • Grid - click this button to access the Cartesian Grid Editor dialog, from where you can manage the default snap grid for the board.
  • Guides - click this button to access the Snap Guide Manager dialog, from where a range of manual snap guides and snap points for the board can be defined and managed.
If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.
Content