Altium NEXUS Documentation

Width

Modified by Phil Loughhead on Aug 24, 2020
All Contents

Rule category: Routing

Rule classification: Unary

Summary

This rule defines the width of tracks placed on the copper (signal) 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


Constraints for the Width rule, which apply to all layers. Enter layer-specific values in the grid (hover the cursor over to show).

  • Preferred Width - specifies the preferred width to be used for tracks when routing the board.
  • Min Width - specifies the minimum permissible width to be used for tracks when routing the board.
  • Max Width - specifies the maximum permissible width to be used for tracks when routing the board.
  • If the values for Preferred Width, Min Width, and Max Width are specified in the fields above the image, they will apply to all signal layers. To define layer-specific values, enter them into the Layer Attributes Table (the grid) below the image. Hover the cursor over the image to show the difference.
  • Press the 3 shortcut key during interactive routing to change which value is being used. Use the shortcut to cycle between Min Width, Preferred Width, Max Width, and User Width - the current mode is displayed in the Heads-Up display and on the Status bar.
    Learn more about Interactive Routing
  • Check Tracks/Arcs Min/Max Width Individually - checks individual widths of tracks and arcs fall within the minimum and maximum range.
  • Check Min/Max Width for Physically Connected - checks the width of routed copper formed by a combination of tracks, arcs, fills, pads, and vias falls within the minimum and maximum range.
  • Use Impedance Profile - this option becomes available when there is at least one impedance profile defined in the Layer Stack Manager. When enabled, use the drop-down to select the impedance profile desired. When the rule is configured in this mode, the Preferred Width required on each routing layer is calculated as part of the specified impedance profile. Once the rule is defined, as you route a net that falls under the scope of the rule, the track width will automatically be set to the width required to meet the specified impedance for that layer. When this option is enabled the Preferred Width cannot be edited in the rule, but the Min Width and Max Width values can.
    Learn more about Configuring the Layer Stack for Controlled Impedance Routing
  • Show values for layer stack - this option appears in the dialog when there are multiple layer stacks defined in the Layer Stack Manager. If the board includes multiple layer stacks then the Width Constraints must be configured for each of the layer stacks, using either the all-layer fields above the image or the layer-specific fields in the Layer Attributes Table.
    Learn more about Defining and Configuring Substacks

Configure the Constraints for each layer stack in the design (hover the cursor over the image to show a different stack).

  • Layer Attributes Table - the grid region at the bottom of the dialog displays all signal layers defined in the layer stack, unless the Use Impedance Profile option is enabled. If this option is enabled, then only the layers available as part of the selected impedance profile will be displayed. The minimum, maximum and preferred routing widths are displayed, as well as other layer-specific information. The routing width fields can be set globally by defining the values in the constraint fields above the image, or individually by typing values directly into the table. When the Use Impedance Profile option is enabled, the required width entries will be automatically calculated and entered for each layer in the table. In this mode the Preferred Width values cannot be edited, but the Min Width and Max Width values can.

When defining values for the minimum, maximum and preferred routing widths, the Layer Attributes Table will highlight any invalid entries by using red text. This could happen, for example, when you specify a minimum constraint value that is greater than the maximum constraint value. The incorrect rule definition is further highlighted by the rule name becoming red in both the folder-tree pane and the respective summary lists, in the PCB Rules and Constraints Editor dialog.

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

The Preferred Width setting is obeyed by the Autorouter.

The Min Width and Max Width settings are obeyed by the Online DRC and Batch DRC. They also determine the range of permissible values that can be used during interactive routing (press Tab key while routing to change the trace width within the defined range, through the Properties panel). If a value is entered outside of this range, it will automatically be clipped.

Tips

  1. The width of each net in a differential pair is monitored by the applicable Differential Pairs Routing rule.
 
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?
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。