Altium NEXUS Documentation

Fanout Control

Modified by Jason Howie on Sep 26, 2019
All Contents

Rule category: Routing

Rule classification: Unary

Summary

This rule specifies fanout options to be used when fanning out the pads of surface mount components in the design that connect to signal and/or power plane nets. Fanout essentially turns an SMT pad into a thru hole pad, from a routing point of view, by adding a via and connecting track. This greatly increases the probability of successfully routing the board, as a signal is made available to all routing layers instead of just the top or bottom layer. This is particularly needed in high-density designs where routing space is very tight.

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 Fanout Control rule (Fanout_Default).

  • Fanout Style - specifies how the fanout vias are placed in relation to the SMT component. The following options are available:
    • Auto - chooses the style most appropriate for the component technology and in order to give optimal routing space results.
    • Inline Rows - fanout vias are placed within two aligned rows.
    • Staggered Rows - fanout vias are placed within two staggered rows.
    • BGA - fanout occurs in accordance with the specified BGA Options.
    • Under Pads - fanout vias are placed directly under SMT component pads.
  • Fanout Direction - specifies the direction to use for the fanout. The following options are available:
    • Disable - do not allow fanout with respect to the SMT components targeted by the rule.
    • In Only - fanout in an inward direction only. All fanout vias and connecting track will be placed within the component's bounding rectangle.
    • Out Only - fanout in an outward direction only. All fanout vias and connecting track will be placed outside of the component's bounding rectangle.
    • In Then Out - fanout all component pads in an inward direction to begin with. All pads that cannot be fanned out in this direction should be fanned out in an outward direction (if possible).
    • Out Then In - fanout all component pads in an outward direction to begin with. All pads that cannot be fanned out in this direction should be fanned out in an inward direction (if possible).
    • Alternating In and Out - fanout all component pads (where possible) in an alternating fashion, first inward then outward.
  • Direction From Pad - specifies the direction to use for the fanout. When a BGA component is fanned out, its pads are sectioned into quadrants, with fanout applied to the pads in each quadrant simultaneously. The following options are available:
    • Away From Center - fanout for pads in each quadrant is applied following a 45° angle away from the component's center.
    • North-East - all pads, in each quadrant, are fanned out in a North-Easterly direction (45° anti-clockwise from the horizontal).
    • South-East - all pads, in each quadrant, are fanned out in a South-Easterly direction (45° clockwise from the horizontal).
    • South-West - all pads, in each quadrant, are fanned out in a South-Westerly direction (135° clockwise from the horizontal).
    • North-West - all pads, in each quadrant, are fanned out in a North-Westerly direction (135° anti-clockwise from the horizontal).
    • Towards Center - fanout for pads in each quadrant is applied following a 45° angle toward the component's center. In most cases, uniformity of direction will not be possible due to required fanout space already taken by another pads' fanout via. In these cases, fanout will occur in the next available direction (North-East, South-East, South-West, North-West).
  • Via Placement Mode - specifies how the fanout vias are placed in relation to the pads of the BGA component. The following options are available:
    • Close To Pad (Follow Rules) - fanout vias will be placed as close to their corresponding SMT component pads as possible, without violating defined clearance rules.
    • Centered Between Pads - fanout vias will be centered between the SMT component pads.

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

During interactive routing and autorouting.

Tips

  1. The following default Fanout Control design rules are automatically created, covering the typical component package types available (listed in descending order of priority). These rules can be edited or others defined, in accordance with your individual design requirements.
    1. Fanout_BGA – with a query of IsBGA.
    2. Fanout_LCC - with a query of IsLCC.
    3. Fanout_SOIC - with a query of IsSOIC.
    4. Fanout_Small - with a query of (CompPinCount < 5).
    5. Fanout_Default - with a query of All.
  2. The style used for the fanout vias will follow the applicable Routing Via Style design rule(s). Additional track laid down as part of the fanout process from pad to via will follow the applicable Routing Width design rule(s).

 

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。