Parent page: Laying out Your PCB
A logical step after creating and checking the schematic document is creating and designing the PCB. Use the File » New » PCB command to create a new PCB document. It is a good idea to configure the PCB by defining the origin, units, grid size, as well as the color display and visibility of the required layers.
Many aspects of the PCB environment setup are configured through the Properties panel in its Board mode described below. To learn more about other features for the configuration of the PCB environment, refer to the following pages:
- Colors & Visibility Control – the PCB editor can display the PCB document in 2D or 3D modes with definitions for layers, 3D colors, visibility and other items, known as view configurations, available from the View Configuration panel.
- Working with the Cursor-Snap System – the PCB editor is a grid-based design environment - design objects are placed on what is referred to as the placement, or snap grid. As well as the snap grid, the software includes a number of additional snap features, designed to help you accurately position and align design objects. Together, these features are referred to as the Unified Cursor-Snap System.
- Working with Mechanical Layers – even the simplest board needs design detail beyond the tracks and pads that implement the circuit. It might be the component courtyards or it might be the 3D component models. In Altium Designer, this type of additional information is detailed on Mechanical Layers.
- Your View of the PCB – modern PCBs are multi-layer entities that require their clear representation in the PCB editor design space. Altium Designer features a comprehensive set of tools facilitating the display of the objects, layers, and nets that you need right now, in both 2D and 3D modes.
- PCB Panel – the PCB panel allows you to browse the current PCB design using a range of filter modes to determine which object types or design elements are listed, highlighted, or selected.
The Properties panel in its Board mode (active when no design object is currently selected in the PCB editor design space) contains options and controls for the basic configuration of the current PCB document.
The following collapsible sections contain information about the options and controls available under the panel's General tab:
The options in this section of the panel determine which PCB objects may be selected in the design space.
- All - On button – select to remove object filtering so that all types of objects may be selected.
- Object buttons – toggle each object button to enable/disable the ability to select that object type.
- Grids – used to toggle whether the cursor will snap to the active design space grid. When this option is enabled the cursor will pull, or snap, to the nearest snap grid location. The active snap grid is displayed on the Status bar, and in the PCB editor Heads Up display.
- Guides – used to toggle whether the cursor will snap to manually placed linear or point Snap Guides. A Snap Guide will override the Snap Grid.
- Axes – used to toggle whether the cursor will axially align (in either the X or Y direction) to the enabled Objects for snapping. The Axis Snap Range defines the distance within which X or Y axial alignment will occur. A dynamic alignment guide line is displayed when alignment is achieved, from the current cursor location to the axially-aligned object snap point (hotspot).
- Snapping – select directly or use the Shift+E shortcut to select whether you want to snap to objects on:
- All Layers – enable this option to allow the cursor to snap to any electrical object on any visible layer.
- Current Layer – enable this option to allow the cursor to only recognize and snap to objects placed on the currently selected layer.
- Off – enable this option to turn off snapping to hotspots.
- Objects for snapping
- On/Off – check to enable snapping for the desired objects.
- Objects – a list of the available objects.
- Snap Distance – when the cursor is within this distance from an enabled object snap point (and snapping is enabled for the active layer), the cursor will snap to that point.
- Axis Snap Range – when the cursor is axially-aligned and within this distance from an enabled object snap point (and the Axes feature is enabled), a dynamic guide line will display to indicate that alignment has been achieved.
- Board Size
- Components/Layers/Nets/Primitives and Others – displays information for each listed category such as the total number of the listed item.
- Reports – click to open the Board Report dialog in which you can specify the content to be included when generating a detailed report for the board.
- Units – use to select the default measurement units for the current PCB document. Default units are used to display any distance-related information on screen or in reports. The default units are always used if a unit's suffix (mm or mil) is not entered when specifying any distance-related information.
- Polygon Naming Scheme – select a naming system from the drop-down menu. There are four choices of naming templates:
NET NAME_LAYER NAME_PXXX
LAYER NAME_NET NAME_PXXX
NET NAME – name of the net to which the polygon is connected. If the polygon is not connected to a net, the name
NONET is used.
LAYER NAME – user-defined name of that layer from the Layer Stack.
LXX – system assigned copper layer number based on the current order of layers in the Layer Stack where Top Layer is
L01. This value is updated whenever the order of copper layers is changed.
PXXX – system-assigned numerical index; unique for each polygon on the board.
- Designator Display – use this field to determine how designators are to be displayed. It can be difficult positioning the designator strings in a multi-channel design, as 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. The following options are available:
Physical – choose 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 Project Options dialog. Physical designators are unique, e.g.,
Logical – choose 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 simply
- Sheet Settings – use this region to configure the PCB sheet.
- X/Y – enter the X and Y coordinates for the bottom left corner of the sheet. This distance is measured from the absolute origin, which is the bottom left corner of the design space. The distance can be defined in either metric or imperial units regardless of the default units (which are determined by the Units setting). To specify the units when entering a size, add the mm or mil suffix to the value.
- Width – enter a width for the sheet here. The sheet provides an area that emulates the traditional drawing sheet and is useful for placing information such as dimensions, notes and title blocks. Information placed on mechanical layers can be linked to the sheet so that they only display when the sheet is being displayed. Sheet size can be defined in either metric or imperial units regardless of the default units (which are determined by the Units setting). To specify the units when entering a size, add the mm or mil suffix to the value.
- Height – enter a height for the sheet here. The sheet provides an area that emulates the traditional drawing sheet and is useful for placing information such as dimensions, notes and title blocks. Information placed on mechanical layers can be linked to the sheet so that they only display when the sheet is being displayed. Sheet size can be defined in either metric or imperial units regardless of the default units (which are determined by the Units setting). To specify the units when entering a size, add the mm or mil suffix to the value.
- Get Size From Sheet Layer – enable this option to size the sheet from the sheet layer.
The following collapsible section contains information about the options and controls available under the panel's Parameter tab:
- Buttons – toggle each button to show/hide related parameters in the grid table below.
- Grid – lists the Name and Value of the parameters associated with the current PCB document. The grid lists both system parameters (e.g., the PCB file name) and the parameters calculated from the PCB (e.g., the number of components on the PCB and the board thickness).
- Place – click to place the currently selected parameter as a special string. The special string will be placed on the layer defined as the default layer for Text objects on the PCB Editor - Defaults page of the Preferences dialog.
The panel's Health Check tab provides an interface to the PCB Health Check Monitor. To learn more about this functionality, see PCB Health Check Monitor.
When a design object is selected, the panel will present options specific to that object type. The following table lists the object types available for placement within a PCB document – click a link to access the properties page for that object.