Altium NEXUS Documentation

Via

Modified by Tania Mashkoory on Aug 15, 2019

Parent page: PCB Objects

A via that spans and connects from the top layer (red) to the bottom layer (blue), and also connects to one internal power plane (green).

Summary

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. Vias are a three-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.

Via definitions can also be stored in Pad and Via Template libraries, refer to the Pad & Via Templates and Libraries page to learn more.

Availability

Vias are available for placement in both the PCB editor and the PCB Library editors in the following ways:

  • Click Place » Via from the main menus.
  • Click the  button on the Wiring toolbar.
  • Click the Via button () in the drop-down on the Active Bar located at the top of the workspace. (Click and hold an Active Bar button to access other related commands. Once a command has been used, it will become the topmost item on that section of the Active Bar.)
  • Right-click in the workspace then choose the Place » Via command from the context menu. 

Placement

After launching the command, the cursor will change to a crosshair and you will enter via placement mode:

  1. Position the cursor and click or press Enter to place a via.
  2. Continue placing further vias or right-click or press Esc to exit placement mode.

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.

Auto-placement of Vias During Routing

When a net is being interactively routed, you can cycle through the available signal layers by pressing the * key on the numeric keypad. Alternatively, use the Ctrl+Shift+Roll Mouse Wheel combination to move through the signal layers. When this is done, the software will automatically place a via in accordance with the applicable Routing Via Style design rule. Note that multiple Via Style design rules can be defined allowing different via sizes to be assigned to different nets.

Default Settings versus Design Rules

When a via is placed in free space, it is not possible for the software to apply a routing style design rule during placement. In this situation the default via will be placed.

Graphical Editing

Vias cannot have their properties modified graphically other than their location.

  • To move a via and also move the connected tracks, click and hold then move the via. The connected routing will remain attached to the via as it is moved.
  • To move a via without moving the connected tracks in the PCB Editor or PCB Library Editor, select the Edit » Move » Move command, then click, hold and move the via.

If a via is being moved with the routing to create more routing or component space, it can be more efficient to re-route than move routing. The software includes a feature called Loop Removal. With this feature enabled, you route along a new path (starting and ending somewhere along the original routing), as soon as you right-click to exit the interactive routing mode the old routing (loop) is removed, including any redundant vias.

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. Click the locked object to select it then disable the Locked property in the List panel or disable the Protect Locked Objects option to graphically edit the object.

Non-Graphical Editing

The following methods of non-graphical editing are available:

Via the Properties Panel

Properties page: Via Properties

The properties of a Via can be edited in the PCB editor's Properties panel, which allows editing of all item(s) currently selected in the workspace.

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

To access the properties of a placed Via :

  • Double-click on the Via.
  • Right-click on the Via then select Properties from the context menu.
  • If the Properties panel is already active, click once on the Via to select it.

Editing Multiple objects

The Properties panel supports editing multiple objects, where the property settings that are identical in all currently selected objects may be modified. When multiples of the same object type are selected manually, via the Find Similar Objects dialog or through a Filter or List panel, a Properties panel field entry that is not shown as an asterisk (*) may be edited for all selected objects.

Quickly change the units of measurement currently used in the panel between metric (mm) and imperial (mil) using the Ctrl+Q shortcut. This affects the panel only and does not change the actual measurement unit employed for the board.

Working with Vias

Vias are a key element of the routing. This section provides valuable information on working with vias.

Thru-hole, Blind and Buried Vias

The default is for a via to span from the Top Layer through to the Bottom Layer; this is known as a thru-hole via. In a multi-layer board, a via can also span other layers. The possible layers that a via can span depends on the fabrication technology used to fabricate the board. The traditional approach to manufacture a multi-layer board is to make it as a set of thin double-sided boards, which are then sandwiched together under heat and pressure to form a multi-layer board.

The image below shows a six layer board, as shown by the layer names on the left side of the image. This board would first be fabricated as three double-sided boards (Top-Plane1, Mid1-Mid2, Plane2-Bottom) as indicated by the hatched core layers.

These double-sided boards can have via sites drilled, if required, forming what are known as blind vias (via number 1) when the via spans from a surface layer to an inner layer; and buried vias, when a via spans from one internal layer to another internal layer (via number 2). After the layers are pressed together into a single multi-layer board, thru-hole vias are drilled (via number 3).


The three types of vias that can be created: blind (1), buried (2) and thru-hole.

Another type of multi-layer board fabrication technology is called Build-up technology, where layers are added one after the other, often over a double-sided or traditional multi-layer board. When this technology is used, vias can be drilled with a laser after each layer is added during the build up process, resulting in a large number of possible layer-pairs that can be spanned. The layer-pairs used for each via are defined by the Start Layer and End Layer settings for the via.

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.

Microvias 

The definition of a microvia (or build-up via) (µVia), according to IPC-2226A, is a blind structure with a maximum aspect ratio of 1:1 when measured in accordance with the image below, terminating on or penetrating a Target Land, with a total depth (X) of no more than 0.25 mm [9.84 mil], measured from the structure's Capture Land foil to the Target Land.

µVias (microvias) are used as the interconnects between layers in high density interconnect (HDI) designs, to accommodate the high input/output (I/O) density of advanced component packages and board designs. Sequential build-up (SBU) technology is used to fabricate HDI boards. The HDI layers are usually built up onto a traditionally manufactured double-sided core board or a multilayer PCB. As each HDI layer is built on to each side of the traditional PCB, µVias can be formed using: laser drilling, via formation, via metallization, and via filling. Because the hole is laser drilled, it has a cone shape.

If a connection required a path through multiple layers, the original approach was to stagger a series of µVias using a step-like pattern. Improvements in technology and processes now allow µVias to be stacked directly on top of each other.

Buried µVias are required to be filled, while blind µVias on the external layers do not require filling. Stacked µVias are usually filled with electroplated copper to make electrical interconnections between the multiple HDI layers and provide structural support for the outer level(s) of the µVia.

Supported Types of µVias

  • The software supports a µVia that traverses from one layer to an adjacent layer.
  • The other type of µVia that is supported is referred to as a Skip µVia, this type skips the adjacent layer, landing on the next copper layer after that.
  • The Via Type is detected automatically based on the defined layer span in the Layer Stack Manager, as shown in the image below.
  • µVias are automatically stacked when traversing multiple layers.

Solder Mask Expansions

An opening in the solder mask is automatically created by the software the same shape as the via. This opening can be larger (a positive expansion value) or smaller (a negative expansion value) than the via itself as defined by the Mask Expansion settings. The expansion is measured from the outer edge of the copper. Solder mask openings over a via can be slightly larger than the via copper area, smaller to cover the copper area but not the drill hole, or they can be completely closed, which is called tented. The default is for the via to use the Expansion value from the Solder Mask Expansion rule. This can be overridden and manual values defined directly in the Properties panel, if required.

The term tenting means to close off. If a tenting option is enabled, then the settings in the applicable Solder Mask Expansion design rule will be overridden resulting in no opening in the solder mask on that solder mask layer for this via. 

Solder mask layers are shown in the negative, i.e. when you see an object on a mask layer, it is actually a hole or opening in that layer. The solder mask can also be shown in the positive, more about this below.

Testpoint Settings

Use the Testpoint region to define this via as a testpoint for Fabrication and/or Assembly. A testpoint is a location where a test probe can make contact with the PCB to check for correct function of the board. Any pad or via can be nominated as a testpoint.

Configuring the Display of Vias

There are a number of display features available to help you work with vias.

Via Colors

Via colors are configured in the View Configuration panel. The copper ring of the via is shown in the current Multi-Layer setting in the Layers section. The via hole color is shown in the Via Holes setting in the System Colors section. You can also disable the display of holes by toggling the  for the desired setting(s).

A thru-hole via is shown on the left. The via on the right is a blind via; the hole is shown in the start and end layer colors.

Vias and the Solder Mask

The default presentation of layers in the PCB editor is to always show the Multi-Layer as the top most layer. That can make it difficult to accurately view the contents of the solder mask layers especially when a pad or via uses a negative mask expansion since the solder mask layer contents will disappear under the multi-layer object. You can change this by changing the layer drawing order on the PCB Editor — Display page of the Preferences dialog. Set the current layer to be drawn as the top-most layer.

By changing the layer drawing order to show the Current Layer on top, when you make the Top Solder the current layer the mask openings are accurately presented as shown in the image below. The green arrows show the size of the solder mask opening for a via on the left, a pad where the mask opening is contracted in the center, and a pad where the opening is expanded on the right.


Configure the display settings to be able to examine the solder mask openings.

Other Via Display Settings

To display the via net name, enable the Via Nets option in the Additional Options region on the View Options tab of the View Configuration panel.

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

联系我们

联系原厂或当地办公室

You are reporting an issue with the following selected text
and/or image within the active document:
Altium Designer 免费试用
Altium Designer Free Trial
我们开始吧!首先,您或者您的公司已经在使用Altium Designer了吗?

如果您有任何需求,请点击这里联系获取当地办公室销售代表联系方式。.
Copyright © 2019 Altium Limited

既然您在使用Altium Designer,为何仍需要试用?

如果您有任何需求,请点击这里联系获取当地办公室销售代表联系方式。.
Copyright © 2019 Altium Limited

好的,实际上您无需下载一个试用版本。

点击下方按钮下载最新版本的Altium Designer安装包

下载Altium Designer 安装包

如果您有任何需求,请点击这里联系获取当地办公室销售代表联系方式。.
Copyright © 2019 Altium Limited

填写下方表格,获取Altium Designer最新报价。

点击[获取免费试用],并同意我们的隐私政策。您会接收到来自Altium的资讯,并允许其改变您的通知首选项。

如果您是Altium维保期内客户,您不需要下载试用版本。

如果您不是Altium维保客户,请填写下方表格免费试用。

点击[获取免费试用],并同意我们的隐私政策。您会接收到来自Altium的资讯,并允许其改变您的通知首选项。

您为何想要试用Altium Designer?

如果您有任何需求,请点击这里联系获取当地办公室销售代表联系方式。.
Copyright © 2019 Altium Limited

那您来对地方了!请填写下方表格申请试用吧。

点击[获取免费试用],并同意我们的隐私政策。您会接收到来自Altium的资讯,并允许其改变您的通知首选项。

Great News!

Valid students can get their very own 6-month Altium Designer Student License for FREE! Just fill out the form below to request your Student License today.

点击[获取免费试用],并同意我们的隐私政策。您会接收到来自Altium的资讯,并允许其改变您的通知首选项。

好的,您可以下载免费的Altium Designer Viewer查看文档,有效期6个月。

请填写下方表格申请。

点击[获取免费试用],并同意我们的隐私政策。您会接收到来自Altium的资讯,并允许其改变您的通知首选项。

好棒!创作是一件超酷的事情,我们可以为您提供完美的设计软件。

Upverter是一个社区导向的交流平台,专为您这样的创客量身定做。

点击这里看看吧!

如果您有任何需求,请点击这里联系获取当地办公室销售代表联系方式。.
Copyright © 2019 Altium Limited

好的,您可以下载免费的Altium Designer Viewer查看文档,有效期6个月。

请填写下方表格申请。

点击[获取免费试用],并同意我们的隐私政策。您会接收到来自Altium的资讯,并允许其改变您的通知首选项。