Altium NEXUS Documentation

Working with a Connection Object on a Multi-board Schematic Document in Altium NEXUS

Modified by Phil Loughhead on Jul 27, 2021
All Contents

Parent page: Multi-board Schematic Objects

A placed Wire type Connection between Module Entries.

Summary

A Connection is a graphical object that is placed between Module Entries in a multi-board Design document to interconnect Modules. Multi-board Connections represent the physical connections (wires, plugs and sockets, cables, or harnesses) that are used between the child board designs.

Types

The Multi-board system editor offers two broad types of Connections that can be placed between Module Entries:

  • Simple – the connection between the Module Entries is through a collection of wires, or as a direct PCB plug-in via mated connectors.
    • Wire – the connection is represented as individual wires between the pins of each Module Entry connector.
    • Direct Connection – the connection is represented as a direct mating between the pins of each Module Entry connector.
  • Grouped – the connection between Module Entries is through a collected set of Nets that are terminated by a physical connector part (plug, socket, header, etc.,) at each end.
    • Cable – the connection is represented by a physical cable with terminating connectors that mate to the (board) connectors at each Module Entry.
    • Harness – the connection is represented by a physical harness with terminating connectors that mate to the (board) connectors at each Module Entry.

Availability

Connections are available for placement in the multi-board schematic editor as follows:

  • Choose the Place » <connection type> command from the main menus, where connection type is a Wire, Direct Connection, Cable, or Harness.
  • Select a Connection type on the Active Bar located at the top of the design space. Click and hold an Active Bar button to access other connection commands.
  • Right-click in the drawing design space then select Place » <connection type> from the context menu.

Placement

After launching the command, the cursor will change to a cross-hair, indicating connection placement mode. For all types of Connections, placement is made by performing the following actions:

  1. Hover the cursor over a Module Entry's connection indicator (orange circle), which will change to a green circle to indicate a valid connection point.
  2. Click to confirm the Connection line's starting point.
  3. Reposition the cursor then click to place a series of vertex points that define the path of the wire.
  4. Position the cursor over the destination Module Entry connection point then click to complete the Connection line path.
  5. Continue placing further Connections between other Module Entry pairs, or right-click or press Esc to exit placement mode.
The default settings for the types of Connection objects are available in the Multi-board Schematic - Defaults page of the Preferences dialog.

After Placement

After placing a Connection, the individual connections within it can be examined in the Properties panel. To edit the individual connections within a Connection, use the Connection Manager (Design » Connection Manager). Changes made in the Connection Manager can be pushed back to the child PCB projects, using the Design » Update Child Projects command.

Note that there is an additional step required if the Connection type is Cable or Harness. These Connection types must have a cable/harness connector component assigned before the individual connections will appear in the Properties panel or the Connection Manager. The cable/harness connectors are assigned in the Properties panel, as shown below.

  • Cable and Harness connectors are assigned in the Multi-board schematic editor and can be included in the Multi-board Bill of Materials.
  • The other elements that make up the cable or harness assembly cannot be included on the Multi-board schematic, but can be included directly in the BomDoc by creating Manual Solutions in ActiveBOM.
  • Alternatively, there are resources available that demonstrate how cable design can be achieved in the schematic editor. For example, this video created by the team at Nine Dot Connects shows how to create the elements in a cable and design the cable in the schematic editor.

Graphical Editing

This method of editing allows a placed Connection object to be selected in the design space and graphically edit its path or terminating points.

Once selected, a Connection line is highlighted (green) and can be manipulated as follows:

  • Click and drag a line segment in its perpendicular plane to alter the connection line path.
  • Click and drag a Connection terminating point (at a Module Entry) to reposition its location, then click to confirm. Normally, the connection end would be moved to another Module Entry, but it also can be positioned in free space where it adopts a nominal end point identifier.

A selected Wire Connection being graphically manipulated.

A placed and terminated Connection is automatically assigned a Designator (W_PS in the example above) as an object identifier, which is editable in the Properties panel. Its terminating ends are identified by their connection target information in the format <TargetModuleDesignator>-<TargetEntryDesignator>.

Non-Graphical Editing

Properties page: Connection Properties

The non-graphical method of editing a Connection is available in the multi-board Properties panel, which provides editable property fields for the item that is currently selected in the design space.

The Properties panel when a Wire Connection object is selected.

To open the Properties panel and access the properties of a placed Connection:

  • Double-click on the Connection object.
  • Right-click on the Connection then select Item Properties from the context menu.

If the Properties panel is already active:

  • Click on the Connection to access its properties in the panel.
To manually open the Properties panel, select View » Panels » Properties from the main menu or click the button at the bottom right of the design space then select Properties from the pop-up menu.
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。