Altium NEXUS Documentation

Routing Via Style

Modified by Tania Mashkoory on Dec 5, 2019
All Contents

Rule category: Routing

Rule classification: Unary

Summary

This rule specifies the style of vias that can be used when routing. You have the option to define specific Min/Max/Preferred values for the via's diameter and hole size - defined as part of the rule's constraints - or use via templates available to the board design.

Via templates can be local (for vias that are saved with the PCB design file), or can be sourced from one or more Pad Via Template Libraries (*.PvLib), installed as part of the available libraries set.
All design rules are created and managed within the PCB Rules and Constraints Editor dialog. For a high-level view of working with the design rules system, see Constraining the Design - Design Rules. For detailed information regarding how to target the objects that you want a design rule to apply to, see Scoping Design Rules.

Constraints

Default constraints for the Routing Via Style rule. Roll the mouse over the image to compare the two modes available. 

  • Mode - use the drop-down to choose from the following two modes:
    • Min/Max preferred - choose this mode to set the permissable values (Minimum/Maximum/Preferred) for the via's diameter and hole size as part of the rule itself.
    • Template preferred - choose this mode to be able to use via styles defined through via templates available to the board.

Mode = Min/Max preferred

When this mode is chosen, the constraints region changes to present the following options:

  • Via Diameter - specifies constraint range values to be adhered to with respect to the diameters of vias placed when routing the board. The following individual values are definable:
    • Minimum - the minimum permissible value for the via diameter.
    • Maximum - the maximum permissible value for the via diameter.
    • Preferred - the preferred value for the via diameter.
  • Via Hole Size - specifies constraint range values to be adhered to with respect to the hole sizes of vias placed when routing the board. The following individual values are definable:
    • Minimum - the minimum permissible value for the via hole size.
    • Maximum - the maximum permissible value for the via hole size.
    • Preferred - the preferred value for the via hole size.

Mode = Template preferred

When this mode is chosen, the constraints region changes to present the following options:

  • Templates List - lists the available via templates that can be used with the rule. These are via templates (local or defined in Pad Via Template Libraries) that are made available to the board design as part of the Local Pad & Via Library (accessed through the PCB Pad Via Templates panel). For each available template the following information is presented:
    • Template Name - the read-only name of the template. For a local template, auto-generated naming is used, in compliance with IPC standards, For a template sourced from a PvLib, this naming can be customized as part of template configuration within that library.
    • Description - the read-only description written for the template.
    • Library - the library from which the template is sourced. This can be <Local> (where the via is defined and saved with the PCB document) or the name of the external Pad Via Template Library (<LibraryName>.PvLib) which has been made available to the PCB document.
    • Enabled - enable this option to have the template made available for via placement during Interactive Routing.

How Duplicate Rule Contentions are Resolved

All rules are resolved by the priority setting. The system goes through the rules from highest to lowest priority and picks the first one whose scope expression matches the object(s) being checked.

Rule Application

Online DRC, Batch DRC, during autorouting, during interactive routing.

When the mode of the rule is set to Min/Max preferred, the following considerations apply:

  • The Preferred via attributes are used by the Autorouter.
  • The Minimum and Maximum via attributes are obeyed by the Online DRC and Batch DRC.
  • The Maximum and Minimum via attributes also determine the range of permissible values that can be used during interactive routing - when you press the + (or *) key on the numeric keypad to toggle routing signal layers and drop a via, press the / key on the numeric keypad to place a fanout via, or press the 2 shortcut key to place a via without changing layer.
  • Press the Tab key while routing to access the Properties panel, from where you can change a value within its defined range. If a value is entered outside of its range, it will automatically be clipped.

When the mode of the rule is set to Template preferred, the following considerations apply:

  • When a routing via is placed, you can cycle through the available via options by pressing the 4 key. In this case, the options will toggle through the via templates that have been enabled as part of the applicable rule.
  • Press the Tab key while routing to access the Properties panel, from where you can change the via template currently applied.

Tips

  1. In order to control the size of blind and buried vias, individual rules can be set up targeting the different layer pairs. For example, to control the via size for blind vias between the top layer and mid layer 1, the following scope (Full Query) can be used:

(StartLayer = 'Top Layer') and (StopLayer = 'Mid-Layer1')

To control the via size for buried vias between mid layer 2 and mid layer 3, the following scope would be used:

(StartLayer = 'Mid-Layer2') and (StopLayer = 'Mid-Layer3')

Alternatively, instead of creating individual rules, you can expand the one rule query using ORs as follows:

((StartLayer = 'Top Layer') and (StopLayer = 'Mid-Layer1')) or((StartLayer = ' Mid-Layer2') and (StopLayer = 'Mid-Layer3'))

 

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。

听上去很棒!您知道我们为学生提供了特殊折扣么?欲知详情,请点击这里。.

同时,请填写下方表格申请免费试用吧。

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。

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。