Altium Designer Documentation

Width

Modified by Jason Howie on Sep 26, 2019
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

Default constraints for the Width rule.

  • Min Width - specifies the minimum permissible width to be used for tracks when routing the board.
  • Preferred Width - specifies the preferred 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.

The values specified for Min Width, Preferred Width, and Max Width will apply to all signal layers.

  • 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 Copper (tracks, arcs, fills, pads & vias) - checks the width of routed copper formed by a combination of tracks, arcs, fills, pads & vias falls within the minimum and maximum range.
  • Characteristic Impedance Driven Width - if the design needs to be routed to strict impedance requirements, ensure that this option is enabled. When the rule is configured in this mode, the routing width required on each routing layer is calculated based on the specified impedance, using the appropriate equation (Microstrip or Stripline) and the physical parameters of the layer stack. 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. The Min/Preferred/Max Width constraints change to the following impedance-based incarnations:
    • Min Impedance - specifies the minimum permissible impedance to be observed when routing the board (default = 50 ohms).
    • Preferred Impedance - specifies the preferred impedance to be observed when routing the board (default = 50 ohms).
    • Max Impedance - specifies the maximum permissible impedance to be observed when routing the board (default = 50 ohms).
  • Layers in layerstack only - allows you to display and edit the width constraints for just the defined signal layers in the layer stack. When enabled, only the layers in the stack will be displayed in the Layer Attributes Table. When disabled, all signal layers will be displayed.
  • Layer Attributes Table - displays all signal layers or only those defined in the layer stack, as controlled by the Layers in layerstack only option. 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 a value in the individual width constraint fields, or individually by typing a width value directly into the table. When the Characteristic Impedance Driven Width option is enabled, the required width entries will be automatically calculated and entered for each layer in the table. They can not be defined on an individual basis while in this mode.

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.
  2. The impedance equations used for calculating the impedance and trace width are accessed from the Layer Stack Manager dialog, by pressing the Impedance Calculation button. The subsequent dialog that appears - the Impedance Formula Editor dialog - contains impedance calculators for both Microstrip and Stripline impedance calculations. Default equations are in place to calculate the impedance and the required trace width in order to satisfy that impedance when routing (as shown below). These equations can be modified if required.
  • Calculated Impedance - the default formula is:

(60/SQRT(Er*(1-EXP(-1.55*(0.00002+TraceToPlaneDistance)/TraceToPlaneDistance))))*LN(5.98*TraceToPlaneDistance/(0.8*TraceWidth+TraceHeight))

  • Calculated Trace Width - the default formula is:

((5.98*TraceToPlaneDistance)/EXP(CharacteristicImpedance/(60/SQRT(Er*(1-EXP(-1.55*(0.00002+TraceToPlaneDistance)/TraceToPlaneDistance)))))-TraceHeight)/0.8

Note that if the plane layer is not adjacent to the signal layer then the nearest plane layer will be used in the calculations.
  • Calculated Impedance - the default formula is:

(80/SQRT(Er))*LN((1.9*(2*TraceToPlaneDistance+TraceHeight)/(0.8*TraceWidth+TraceHeight)))*(1-(TraceToPlaneDistance/(4*(PlaneToPlaneDistance-TraceHeight-TraceToPlaneDistance))))

  • Calculated Trace Width - the default formula is:

((1.9*(2*TraceToPlaneDistance+TraceHeight))/(EXP((CharacteristicImpedance/(80/SQRT(Er)))/(1-(TraceToPlaneDistance/(4*(PlaneToPlaneDistance-TraceHeight-TraceToPlaneDistance))))))-TraceHeight)/0.8

Note that if the plane layers are not adjacent to the signal layer then the nearest plane layers will be used in the calculations. Note also that an offset stripline configuration is not supported.

 

 

 

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。