Altium Designer Documentation

Matched Lengths

Modified by Jason Howie on Sep 26, 2019
此文档页面引用了不再受支持的产品 Altium Vault, Altium Vault 及其组件管理功能已迁移到 Altium Concord Pro
All Contents

Rule Category: High Speed

Rule Classification: Unary

Summary

This rule specifies the allowable difference in net lengths. This rule is essential in a high-speed design, where the challenge is not just about how long it takes the signals to arrive (which is determined by their overall length), but how important it is that the specified signals arrives at the same time. Depending on the signal switching speeds, the function of the signal, and the materials used in the board, the allowed difference could be as much as 500mils, or as little as 1mil.

The set of nets being targeted is defined by the scope of the rule (as defined by its full query), with the reference length (the longest net in the set) being determined by the rule scope, in combination with the Constraints settings. Other targeted nets will pass the rule if their Current Length is:

(LongestLength - tolerance) ≤ CurrentLength ≤ LongestLength

Those nets that are found to be outside of a specified tolerance (i.e. are too short) can be quickly lengthened by running the Equalize Net Lengths command. Alternatively, you can take full control by interactively tuning the lengths of nets, or differential pair nets, using the Interactive Length Tuning, and Interactive Diff Pair Length Tuning commands, respectively.
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 Matched Lengths rule. Roll the mouse over the image to compare the two modes of
operation available.

  • Tolerance - specifies a length tolerance when comparing each net with the longest net in the set. Any net whose length does not lie within the specified tolerance is deemed to be too short and will have track added to it should the Equalize Net Lengths command be run.
  • Group Matched Lengths - choose this option to check lengths between all nets targeted by the rule scope.
  • Within Differential Pair Length - choose this option to check lengths between the nets in each differential pair targeted by the rule scope. Refer to the Tips section to learn more.

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, the Equalize Net Lengths feature, interactive length tuning.

Tips

  1. The PCB Editor can add "accordion" sections to nets to equalize their lengths. Having defined the Matched Lengths rule, from the PCB document select Tools » Equalize Net Lengths . The matched lengths rule will be applied to the nets specified by the full query of the rule and accordion sections will be added to those whose length falls outside the permissible tolerance. The underlying algorithm that adds the accordion sections will only do so on vertical and horizontal tracks. If a net has been predominantly routed using 45° track segments, the possibility of successful equalization will be greatly reduced, depending upon the availability and extent of horizontal and vertical track on which to add the equalizing accordion lengths. If nets with such routing do exist, reroute them using short 45° track lengths and more orthogonal sections. The degree of success depends on the amount of space available for the accordion sections and the accordion style being used. The 90° style is the most compact and the 45° style is the least compact. Alternatively, use the Interactive Length Tuning command instead.
  2. When scoping a Matched Net Length rule for interactive tuning purposes:
    1. For individual nets - define a class containing the nets that you wish to tune (Net, Differential Pair or xSignal class), and scope the rule to target that class. The length tuning tool will then find the longest net in that set of target nets and give you a valid range for the target nets of: (LongestLength - tolerance) ≤ CurrentLength ≤ LongestLength.
    2. For differential pair nets - if there are multiple differential pairs and the design requires pair-to-pair matched net lengths, you will create two Matched Net Length rules. The first rule defines the pair-to-pair length matching requirements, and has the Constraint set to Group Matched Lengths. The second rule is to ensure the nets within each differential pair are within tolerance, and has the Constraint set to Within Differential Pair Length. When this Constraint option is used, the software will detect all differential pairs targeted by the rule scope, and then compare the +ve and -ve members of each pair against each other.

Refer to the Length Tuning article to learn more about interactively tuning route lengths.

Refer to the Differential Pair Routing article to learn more about routing differential pairs.

 

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。