Applied Parameters: UpdateCaption=False
This command is used to place a Via object onto the active document. A via is a primitive design object. It is used to form a vertical electrical connection between two or more electrical layers of a PCB. A via is a 3-dimensional object having a barrel-shaped body in the Z-plane (vertical) with a flat ring on each (horizontal) copper layer. The barrel-shaped body of the via is formed when the board is drilled and through-plated during fabrication. In the X and Y planes, vias are circular, like round pads. The key difference between a via and a pad is that as well as being able to span all layers of the board (top to bottom), a via can also span from a surface layer to an internal layer or between two internal layers.
For detailed information about this object type, see Via
This command can be accessed from the PCB Editor and the PCB Library Editor by:
- Choosing the Place » Via command from the main menus.
- Locating and using the Via command () on the Active Bar.
- Clicking the button on the Wiring toolbar (PCB Editor) and the PCB Lib Placement toolbar (PCB Library Editor).
- Right-clicking in the workspace then choosing the Place » Via command from the context menu (PCB Editor only).
After launching the command, the cursor will change to a cross-hair and you will enter via placement mode. A via will appear "floating" on the cursor:
- Position the cursor then click or press Enter to place a via.
- Continue placing further vias or right-click or press Esc to exit placement mode.
Press the Tab
key to access the Properties panel
, from where properties for the via can be changed on-the-fly. Pressing Tab
pauses placement, allowing you to interact with the panel (or other area of the software) directly. To resume, click the pause symbol that appears over the workspace, or press Esc
While attributes can be modified during placement (Tab
to bring up the Properties
panel), keep in mind that these will become the default settings for further placement unless the Permanent
option on the PCB Editor – Defaults page
of the Preferences dialog
is enabled. When this option is enabled, changes made will affect only the object being placed and subsequent objects placed during the same placement session.
- Vias can be multi-layer (passing from the Top layer to the Bottom layer through all other layers) or confined to any two signal layers - known as blind or buried vias. A blind via connects from the surface of the board to an internal signal layer, a buried via connects from one internal signal layer to another internal signal layer. Vias use layer colors to indicate which layers are connecting.
- If blind, buried or build-up type vias are to be used, the Drill pairs must be configured with a drill pair for each layer-pair that a via spans. Consult your board fabricator if you are designing a multi-layer board that is going to include blind or buried vias to ensure the optimal layer stack up and layer-pairing are achieved.
- A via will adopt a net name if it is placed over an object that is already connected to a net.
- Typically vias are not placed manually, they are placed automatically as part of the interactive routing process. When you change layers during manual, interactive routing, a via is automatically inserted to preserve the electrical conductivity.
- A selected via template - in the PCB Pad Via Templates panel - can be reused in the current board as a new via instance by dragging it onto the layout or by choosing Place from the panel's right-click context menu.
- A via template that is stored as part of a Pad Via Library can also be placed in the PCB design directly from the PCB panel when configured in Pad & Via Templates mode. Choose the required template library then select the required via template within that library and click the Place button (in the Templates region of the panel).