Altium Designer Documentation

PlacePort

Created: June 8, 2017 | Updated: January 30, 2019

Parent page: Schematic Commands

The following pre-packaged resource, derived from this base command, is available:


Applied Parameters: None

Summary

This command is used to place a Port object onto the active document. A port is an electrical design primitive. It is used to make an electrical connection between one schematic sheet and another sheet, or sheet symbol (through a corresponding sheet entry), in a design using multiple sheets (both flat and hierarchical designs). The name of the port defines the connection (i.e. a port on a schematic sheet connects to ports or sheet entries with the same name on other sheets in the project).

For detailed information about this object type, see Port.

Access

Ports are available for placement in the Schematic Editor only, by:

  • Choosing Place » Port from the Schematic Editor main menu.
  • Locating and using the Port command () on the Active Bar.
If the command has been recently used from the Active Bar, it will become the active/visible button. Where other commands are available, this is indicated by a triangle at the bottom-right corner of the button. Click and hold on the active button to access a menu of all associated commands for that grouping.
  • Clicking the  button on the Wiring toolbar.
  • Right-clicking in the workspace and choosing Place » Port from the context menu.

Use

After launching the command, the cursor will change to a cross-hair and you will enter port placement mode. Placement is made by performing the following sequence of actions:

  • Click or press Enter to anchor the left-hand edge of the port.
  • Move the cursor to adjust the length of the port as required, then click or press Enter to complete placement of the port.
  • Continue placing further ports or right-click or press Esc to exit placement mode.
At any time during placement, press the Tab key to access the Properties panel, from where properties for the port can be changed on-the-fly. Pressing Tab pauses placement, allowing you to interact with the panel (or other area of the software) directly. To resume, click the pause symbol that appears over the workspace.

Additional actions that can be performed during placement - while the port is still floating on the cursor, and before its left-hand edge is anchored - are:

  • Press the Alt key to constrain the direction of movement to the horizontal or vertical axis, depending on the initial direction of movement.
  • Press the Spacebar to rotate the port counterclockwise or Shift+Spacebar for clockwise rotation. Rotation is in steps of 90°.
  • Press the X or Y keys to mirror the port along the X-axis or Y-axis respectively.

Tips

  1. When compiling a schematic or generating a netlist, the relationship between ports and sheet symbols is determined by the Net Identifier Scope chosen for the project. This scope is defined by setting the Net Identifier Scope option, on the Options tab of the Options for Project dialog (Project » Project Options). When set to Flat or Global, all ports with the same name, within the same or different schematic documents, are considered to be electrically connected. When set to Hierarchical or Strict Hierarchical, ports only connect vertically to their corresponding sheet entries. They do not connect horizontally to other ports of the same name.
  2. The I/O Type field in the Properties panel allows you to define the port's electrical type. Choose from either Input, Output, Bidirectional, or Unspecified.
  3. To negate (include a bar over the top of) a port name, use one of the following methods:
    1. Include a backslash character after each character in the name (e.g. E\N\A\B\L\E).
    2. Enable the Single '\' Negation option on the Schematic - Graphical Editing page of the Preferences dialog, then include one backslash character at the start of the name (e.g. \ENABLE).
  4. Port names are not used for naming nets. This means a system-generated net name will be used if no net label or power object is associated with that net.
  5. When a Port is connected to a Signal Harness, the Port becomes a Harness object. By default, the Port will change color to match the color of the Signal Harness.
  6. By default, the font used for the port's Name follows the global document-level font. This is set using the Document Font field, in the General section of the Properties panel (when no object is selected). This can be overridden at the individual port-level, using the control below the port's Name field (again, edited through the Properties panel) - allowing you to fully control the textual presentation of ports as needed.
  7. For information on how a placed port object can be modified graphically, directly in the workspace, see Graphical Editing.
  8. While attributes can be modified during placement (Tab to bring up the Properties panel), bear in mind that these will become the default settings for further placement unless the Permanent option on the Schematic - Defaults page of the Preferences dialog is enabled. When this option is enabled, changes made will affect only the object being placed and subsequent objects placed during the same placement session.

 

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。