Altium Designer Documentation

Via Properties

Modified by Susan Riege on Jan 11, 2019
All Contents

Parent page: Via

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 Via 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 Via object properties are available for editing in the Properties panel when a placed Via is selected in the workspace.

      The Via default settings in the Preferences dialog and the Via 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)

  • Net - use the drop-down to select the net to which this via belongs. All nets for the active board design will be listed in the drop-down list. Note that if via placement commences at the same location as an existing object that is already connected to a Net, then the Net property of the new object is automatically assigned to that Net. Select No Net to specify that the via is not connected to any net. The Net property of a primitive is used by the Design Rule Checker to determine if a PCB object is legally placed. 
  • Net Class - displays the net class. This field is dependent upon the net selected in the Net field and is not editable.
  • Net Length - displays the net length. This field is dependent upon the net selected in the Net field and is not editable.

Via Template

Template - displays the current template for the via. Use the drop-down to select another template. If there is an associated Library, that library will be displayed. 

Location (Properties panel only) 

The  icon to the right of this region must be displayed as  (unlocked) in order to access the below fields. Toggle the lock/unlock icon to change its lock status. 
  • (X/Y)
    • X (first field) - this field shows the current X position of the center of the via relative to the current origin. Edit the value in the field to change the position of the via relative to the current origin. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. Default units (metric or imperial) are determined by the Units setting in the Other region of the Properties panel in Board mode (accessed when no objects are selected in the workspace), and are used if the unit is not specified. 
    • Y (second field) - this field shows the current Y position of the center of the via relative to the current origin. Edit the value in the field to change the position of the via relative to the current origin. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. Default units (metric or imperial) are determined by the Units setting in the Other region of the Properties panel in Board mode (accessed when no objects are selected in the workspace), and are used if the unit is not specified. 

Properties

  • Drill Pair - use the drop-down to select the desired layer on which this via starts and ends.
  • Drill Pairs - click to open the Drill-Pair Manager dialog in which you can configure the required drill pairs for the active layer stack.

Hole Information

  • Hole Size - this field displays the current hole size for the via. The value specifies the diameter of the hole (as a round, square or slotted shape) in mils or mm to be drilled in the via during fabrication. The hole size can be set from 0 to 1000mil and can be set larger than the via to define (copper free) mechanical holes. Edit the value in this field to change the via hole size. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. Default units (metric or imperial) are determined by the Units setting in the Other region of the Properties panel in Board mode (accessed when no objects are selected in the workspace), and are used if the unit is not specified. 
  • Tolerance - setting hole tolerance attributes can help determine the fits and limits of your board. Specify the minimum (-) and maximum (+) tolerances for the hole. There is no default hole tolerance value in Altium Designer.
Component datasheets list a tolerance with plus/minus to accommodate variations in aging, wear, temperature, plating, material, machining, and so forth. As holes are drilled, drill bits wear and get smaller, or the drill may vibrate or wiggle slightly in a hole, causing a slightly larger hole. Mounting holes are then plated, and the plating may be thicker or thinner for each batch or position on the board. You also have to account for thermal expansion or shrinkage of the Printed Circuit Board PCB substrate as it is being processed. Therefore, hole tolerance is critical in the design process to accommodate all tolerance, drill wear or wobble, and plating variations.

Size and Shape

  • Simple - select to choose a simple via.  
    • Diameter - enter the desired diameter of the via. The via diameter is the same on all layers.
  • Top-Middle-Bottom - select to choose different diameters for the top layer, all internal signal layers, and Bottom Layer. 
    • Displayed Layer(s) - click on a displayed layer to configure vias for that layer. The selected layer is highlighted.
    • Diameter - click the drop-down then enter the required diameter of the via for the selected layer.
  • Full Stack ​- select to choose a Full Stack via object. 
    • Displayed Layer(s) - click on a displayed layer to configure vias for that layer. The selected layer is highlighted.
    • Diameter - click the drop-down then enter the required diameter of the via for the selected layer.

Solder Mask Expansion

  • Rule - select to have the solder mask expansion for the via follow the defined value in the applicable Solder Mask Expansion design rule.
    • Top
      • Tented - check if it desired for any solder mask settings in the solder mask expansion design rules to be overridden, which results in no opening in the solder mask on the top layer of this via and is therefore tented. Disable this option and this via is affected by a solder mask expansion rule or specific expansion value.
    • Bottom
      • Tented - check if it desired for any solder mask settings in the solder mask expansion design rules to be overridden, which results in no opening in the solder mask on the bottom layer of this via and is therefore tented. Disable this option and this via is affected by a solder mask expansion rule or specific expansion value.
  • Manual - select to override the applicable design rule and specify the solder mask expansion value for the via. 
    • Top - enter the top layer solder mask expansion value. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. Default units (metric or imperial) are determined by the Units setting in the Other region of the Properties panel in Board mode (accessed when no objects are selected in the workspace), and are used if the unit is not specified. This field is accessible only if Tented is not enabled.
      • Tented - check if it desired for any solder mask settings in the solder mask expansion design rules to be overridden, which results in no opening in the solder mask on the top layer of this via and is therefore tented. Disable this option and this via is affected by a solder mask expansion rule or specific expansion value.
    •  - you can enter Bottom measurement and Tented options if Bottom layer Solder Mask Expansion values are required. Click  to disable Bottom layer options if they are not required.
    • Bottom - enter the bottom layer solder mask expansion value. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. Default units (metric or imperial) are determined by the Units setting in the Other region of the Properties panel in Board mode (accessed when no objects are selected in the workspace), and are used if the unit is not specified. This field is accessible only if the link icon is set to  and the Tented option is not enabled.
      • Tented - check if it desired for any solder mask settings in the solder mask expansion design rules to be overridden, which results in no opening in the solder mask on the bottom layer of this via and is therefore tented. Disable this option and this via is affected by a solder mask expansion rule or specific expansion value.
      • From Hole Edge - when enabled, the Solder Mask opening will follow the shape of the via. The mask is therefore independent of via shape and size, and is scaled from both the hole size and shape. For example, a via with a square hole will create a square mask opening that matches the hole dimensions, as well as the assigned expansion value. Also note that a via's expansion mask opening size will track any changes in the hole size.

Notes on Tenting

Partial and complete tenting of vias can be achieved by defining an appropriate value for Solder Mask Expansion. This expansion constraint can either be defined on a via-by-via basis in the Properties panel, or by defining appropriate Solder Mask Expansion design rules. By setting the expansion value to a suitable value, you can achieve the following:

  • To partially tent a via - covering the land area only, set the Expansion to a negative value that will close the mask right up to the via hole.
  • To completely tent a via - covering the land and hole, set the Expansion to a negative value equal to or greater than the via radius.
  • To tent all vias on a single layer, set the appropriate Expansion value and ensure that the scope (Full Query) of a Solder Mask Expansion rule targets all vias on the required layer.
  • To completely tent all vias in a design, in which varying via sizes are defined, set the Expansion to a negative value equal to or greater than the largest via radius. When tenting an individual via, options are available to follow the expansion defined in the applicable design rule, or to override the rule and apply a specified expansion directly to the individual via in question.

Testpoint

  • Fabrication/Assembly - these options allow you to specify vias to be used as testpoint locations in fabrication and/or assembly testing. Enable Top for this via to be defined as a top layer testpoint. Enable Bottom for this via to be defined as a bottom layer testpoint.
Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.

お問合せ

お近くの営業所にお問合せください。

We're sorry to hear the article wasn't helpful to you.
Could you take a moment to tell us why?
You are reporting an issue with the following selected text
and/or image within the active document:
Altium Designer 無償評価版
Altium Designer 無償評価版
Altium Designerを使用していますか?

弊社の営業担当より詳細情報をご案内しますので、アルティウムジャパン までお問い合わせください。.
Copyright © 2019 Altium Limited

評価版ライセンスが必要な理由を下記から選択してください。

弊社の営業担当より詳細情報をご案内しますので、アルティウムジャパン までお問い合わせください。.
Copyright © 2019 Altium Limited

その場合、評価版ライセンスは不要です。

ボタンをクリックして、最新のAltium Designerインストーラをダウンロードしてください。

Altium Designerインストーラをダウンロードする

弊社の営業担当より詳細情報をご案内しますので、アルティウムジャパン までお問い合わせください。.
Copyright © 2019 Altium Limited

Altium Designerの新規ライセンスのお見積もりをご希望の場合、下記のフォームに入力してください。

プライバシーポリシーに同意の上、[ダウンロード]をクリックしてください。ご登録いただきましたメールアドレスにメールマガジンが送信されます。メール配信の停止は、メール内の​通知設定​​でお手続きいただけます。

Altium Designerサブスクリプションをご利用中の場合、評価版ライセンスは不要です。

お客様がAltium Designerサブスクリプションの有効なメンバーではない場合、下記のフォームに入力して無償評価版をダウンロードしてください。

プライバシーポリシーに同意の上、[ダウンロード]をクリックしてください。ご登録いただきましたメールアドレスにメールマガジンが送信されます。メール配信の停止は、メール内の​通知設定​​でお手続きいただけます。

Altium Designerを評価する理由を下記から選択してください。

弊社の営業担当より詳細情報をご案内しますので、アルティウムジャパン までお問い合わせください。.
Copyright © 2019 Altium Limited

無償評価版を使用するには、下記のフォームに入力してください。

プライバシーポリシーに同意の上、[ダウンロード]をクリックしてください。ご登録いただきましたメールアドレスにメールマガジンが送信されます。メール配信の停止は、メール内の​通知設定​​でお手続きいただけます。

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.

プライバシーポリシーに同意の上、[ダウンロード]をクリックしてください。ご登録いただきましたメールアドレスにメールマガジンが送信されます。メール配信の停止は、メール内の​通知設定​​でお手続きいただけます。

その場合、Altium Designerビューワーの無償ライセンス(有効期間6か月)をダウンロードできます。

下記のフォームに入力してライセンスをリクエストしてください。

プライバシーポリシーに同意の上、[ダウンロード]をクリックしてください。ご登録いただきましたメールアドレスにメールマガジンが送信されます。メール配信の停止は、メール内の​通知設定​​でお手続きいただけます。

素晴らしいですね。アルティウムではモノづくりに最適なプログラムを提供しています。

Upverterは、コミュニティ主導型の無償プラットフォームで、お客様のような作り手の要求に合わせて設計されています。

試してみる場合、こちらをクリック してください。

弊社の営業担当より詳細情報をご案内しますので、アルティウムジャパン までお問い合わせください。.
Copyright © 2019 Altium Limited

その場合、Altium Designerビューワーの無償ライセンス(有効期間6か月)をダウンロードできます。

下記のフォームに入力してライセンスをリクエストしてください。

プライバシーポリシーに同意の上、[ダウンロード]をクリックしてください。ご登録いただきましたメールアドレスにメールマガジンが送信されます。メール配信の停止は、メール内の​通知設定​​でお手続きいただけます。