Altium NEXUS Documentation

Working with the Board Outline Clearance Design Rule on a PCB in Altium NEXUS

Modified by Susan Riege on Apr 7, 2021
All Contents

Rule Category: Manufacturing

Rule classification: Unary

Summary

This rule defines the minimum clearance allowed from design objects that are fabricated, to edges of the board. Either a single clearance value can be specified for all object-to-edge possibilities, or different clearances for different pairings can be defined, through the use of a dedicated Minimum Clearance Matrix. The terms Board Outline and Board Edge are general names used interchangeably to describe the outer edge of the board. The term edge is defined in the table below the image. The Board Outline Clearance design rule checks object-to-edge clearances on the electrical and overlay (silkscreen) layers.

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 Board Outline Clearance rule.

Edge Type Definition
Outline Edge The outer-most (exterior) edge of the board
Cavity Edge The edge of a user-defined cavity
Cutout Edge The edge of a user-defined cutout
Split Barrier When a Split Line defines the edge of the board on this layer, this edge is referred to as a Split Line Barrier
Split Continuation When this layer continues beyond a Split Line, this edge is referred to as a Split Line Continuation (a permeable boundary). To allow an object-kind to cross a Split Continuation, set the clearance value to zero. Zero indicates that for these object-kinds, this is a continuation layer, and the objects are allowed to violate (pass over) the split line. Use this technique to allow routed tracks, for example, to travel across from one Layer Stack Region to another.
  • Minimum Clearance - the value for the minimum clearance required. A value entered here will be replicated across all cells in the Minimum Clearance Matrix. Conversely, when a different clearance value is entered for one or more object pairings in the matrix, the Minimum Clearance constraint will change to N/A, to reflect that a single clearance value is not being applied across the board.
  • Minimum Clearance Matrix - provides the ability to fine tune clearances between the various object-to-edge clearance combinations in the design.
The default Board Outline Clearance rule for a new PCB document will default to use 10mil for all object-to-edge clearance combinations. When creating a subsequent new rule, the matrix will be populated with the values currently defined for the lowest priority Board Outline Clearance rule.
To allow an object-kind to cross an edge, set the clearance value to zero. Zero indicates to the software that an object-kind is allowed to violate (pass over) this edge type. Use this technique to allow routed tracks, for example, to travel across from one Layer Stack Region to another.

Working with the Clearance Matrix

Definition of clearance values in the matrix can be performed in the following ways:

  • Single cell editing - to change the minimum clearance for a specific object pairing.
  • Multi-cell editing - to change the minimum clearance for multiple object pairings:
    • Use Ctrl+Click, Shift+Click, and Click+Drag to select multiple cells in a column.
    • Use Shift+Click, and Click+Drag to select multiple contiguous cells in a row.
    • Use Click+Drag to select multiple contiguous cells across multiple rows and columns
    • Click on a row header to quickly select all cells in that row.
    • Click on a column header to quickly select all cells in that column.

With the required selection made (either a single cell or multiple cells), making a change to the current value is simply a case of typing the new value required. To submit the newly entered value, either click away on another call, or press Enter. All cells in the selection will be updated with the new value.

To set a single clearance value for all possible object pairings, simply set the required value for the Minimum Clearance constraint. On clicking Enter, this value will be replicated across all applicable cells of the matrix. Alternatively, click the blank grey cell at the top-left of the matrix, or use the Ctrl+A shortcut. This selects all cells in the matrix, ready to accommodate a newly-entered value.

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, interactive routing, and autorouting.

 

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

We're sorry to hear the article wasn't helpful to you.
Could you take a moment to tell us why?
200 characters remaining
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。