Altium Designer Documentation

Working with a Part Object on a Schematic Sheet in Altium Designer

Modified by Tania Mashkoory on Dec 11, 2020

Parent page: Schematic Objects

The Part represents the actual physical electronic component.

Summary

A part is an electrical design primitive. It is a schematic symbol that represents an electronic device, such as a resistor, a switch, an operational amplifier, a voltage regulator, etc. Parts are stored within components in schematic component libraries. Note that each component can contain one or more parts. Along with a symbolic representation of the component, the part also includes links to models, such as the PCB footprint, and also parameters that are used to document details such as component parameters and supplier information. How the model links and parameters are added to the part depends on the type of library storage being used.

The terms Part and Component are both used to describe the symbol that represents the actual electronic device. The term Part is used because some components contain multiple parts. For example, a quad Op Amp component contains four separate Op Amps, or a resistor network can contain eight independent resistors. For these types of devices, you can create a separate schematic symbol to represent each Part during the component definition and place each of these parts independently. The terms Part and Component are used interchangeably on this page unless a multi-part component is being discussed.

Availability

Parts are available for placement in both the schematic and schematic library editors.

  • In the schematic editor, click Place » Part.
  • Right-click in the workspace then choose Place » Part from the context menu.
  • From the Components panel, right-click Place <ComponentName>
  • Dragging and dropping a component from the Components panel.
  • Select the Place button in the Details pane of the Components Panel, or by use the Enter hotkey.
  • From the SCH Library panel when in the schematic library editor, select a component, then click Place

Placement from the Components Panel

In the schematic editor, the part selection and placement process may be done from the Components panel.

  • The panel displays the contents of the currently selected library. Use the drop-down next to the library name to choose another library.
  • Use the mask field below the currently selected library field to filter the list and speed the searching process or scroll and select the required part.
  • Click Place, double-click, or click and drag to place the selected component onto the active schematic sheet. While the part is floating on the cursor, it can be rotated (press Spacebar), mirrored along an axis (press X or Y), or edited (press Tab) before placement.
  • The columns shown in the list of components in the currently selected library can be reorganized (click and drag) or reconfigured (right-click then choose Select Columns).

On the left, an iteration of the Components panel when signed into a managed content server. On the right, an iteration of the Components panel when not signed into a server.

Searching for a Component

The file-based (non-managed) library menu options provides you the ability to set preferences, perform searches, and migrate filed-based library content. To access these options, select the library menu  button at the top right of the Components panel.

Select the File-based Libraries Preferences command to open the Available File-based Libraries dialog, where you may view controls to add or remove libraries, install libraries, and specify library search paths.

The current listing of file-based library components may be filtered by entering a search phase in the Components panel Search field. To access more advanced search capabilities for component Libraries, select the File-based Libraries Search option from the panel’s  menu (top right), which opens the File-based Libraries Search dialog. The dialog offers flexible search options including query-based filter constraints, and the ability to search through all available file-based libraries or those within a specified path.

  • The default search Scope is to search for Components in the Available File-based Libraries.
  • Alternatively, the dialog also supports searching through Libraries on path stored in folders on a drive. To do this, enable the Libraries on path option then configure the Path options as required.
  • The Filters use "AND" and, therefore, it is better to start with a simple filter and if there are many results, use the Refine last search mode to search within the results.
  • Query search results are presented in the File-based Libraries Search dialog when selecting Helper.

Placing from the Schematic Library Editor

A part also can be placed directly from a library that is open in the schematic library editor from the SCH Library panel. Note that:

  • Clicking the Place button in the panel will place the selected part (component) in the last active schematic sheet.
  • While the part is floating on the cursor, it can be rotated (press Spacebar), mirrored along an axis (press X or Y), or edited (press Tab) before placement. The action can also be performed during dragging of the object. Rotation is in increments of 90°.
  • If a part is placed directly from a library, that library does not need to be added in the Available File-based Libraries dialog first.

A Part can also be placed directly from an open Schematic Library using the SCH Library panel.

While attributes can be modified during placement (Tab to access the Properties panel), keep 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.

Graphical Editing

Graphical editing for a part is limited to moving, rotating and mirroring. When a part is selected in the workspace, a dashed selection box will appear around it. To graphically manipulate a selected component:

  • Press Delete to remove the selected part from the design.
  • Click and hold to move the selected part. The cursor will jump to the nearest electrical hotspot (the wiring end of the nearest pin).
  • Press the Spacebar to rotate the arc counterclockwise or Shift+Spacebar for clockwise rotation. The action can also be performed during dragging of the object. Rotation is in increments of 90°.
  • While a part is moving on the cursor, press the X or Y key to mirror it along that axis.

A selected Part

When a component is rotated, its text strings are automatically repositioned to suit the new orientation. This behavior can be disabled if required. To do this, edit the string then clear the Autoposition checkbox in the Parameters Properties panel. Note that manually positioned text strings are denoted by a dot. These dots can be hidden if required by clearing the Mark Manual Parameters option on the Schematic - Graphical Editing page of the Preferences dialog.

If attempting to graphically modify an object that has its Locked property enabled, a dialog will appear asking for confirmation to proceed with the edit. If the Protect Locked Objects option is enabled on the Schematic - Graphical Editing page of the Preferences dialog and the Locked option for that design object is enabled as well, then that object cannot be selected or graphically edited. Double-click on the locked object directly and disable the Locked property or disable the Protect Locked Objects option to graphically edit the object.

Working Between the Schematic Component and the PCB Component

The software includes tools to help work between the component on the schematic and that same component on the PCB. These tools include Cross Probing, Cross Selection, and Selecting the PCB Components from the schematic.

Cross Probe

As the name implies, Cross Probe allows you to click on a component in one editor and jump to that component in the other editor. To Cross Probe:

  • Click Cross Probe located on the schematic or PCB editor menu on the Tools menu.
  • When you click the component in the schematic editor, it will be centered and zoomed in the PCB editor. The zoom level is set on the System - Navigation page of the Preferences dialog.
  • The default behavior is to remain in the same editor, ready to cross probe another component. To switch to the other editor as you Cross Probe, hold the Ctrl key. 

Cross Select Mode

Cross Select Mode selects the same component in the other editor. Note that it does not zoom and center. Cross Selection is either on or off. Click Tools » Cross Select Mode to toggle the mode on/off. Select multiple components by holding the Shift key as you click to select.​

Selecting the PCB Components

This feature allows you to select multiple schematic components in a specific order, then place those same components in the PCB editor in the same order. To use this feature:

  • Select the components on the schematic one by one (hold Shift as you click to select multiple components).
  • Switch to the PCB editor then press the I, C shortcut to launch the Reposition Selected Components command. The Reposition Selected Components command is also available on the right-click menu after pressing the I shortcut. 
If attempting to graphically modify an object that has its Locked property enabled, a dialog will appear asking for confirmation to proceed with the edit. If the Protect Locked Objects option is enabled on the Schematic – Graphical Editing page of the Preferences dialog, and the Locked option for that design object is enabled as well, then that object cannot be selected or graphically edited. Click the locked object to select it then disable the Locked property in the List panel or disable the Protect Locked Objects option to graphically edit the object.

Non-Graphical Editing

Via the Properties Panel

Properties page: Part Properties

This method of editing uses the associated Component dialog and the Properties panel mode to modify the properties of a part object.

 The Part dialog, on the left, and the Part mode of the Properties panel on the right

After placement, the Component dialog can be accessed by:

  • Double-clicking on the placed component object.
  • Placing the cursor over the component object, right-clicking then choosing Properties from the context menu.

During placement, the Component mode of the Properties panel can be accessed by pressing the Tab key. Once the component is placed, all options appear.

After placement, the Component mode of the Properties panel can be accessed in one of the following ways:

  • If the Properties panel is already active, by selecting the component object.
  • After selecting the arc object, select the Properties panel from the Panels button in the bottom right section of the workspace, or by selecting View » Panels » Properties from the main menu.
If the Double Click Runs Interactive Properties option is disabled (default) on the Schematic - Graphical Editing page of the Preferences dialog, when the primitive is double-clicked or you right-click on a selected primitive then choose Properties, the dialog will open. When the Double Click Runs Interactive Properties option is enabled, the Properties panel will open. 
While the options are the same in the dialog and the panel, the order and placement of the options may differ slightly. 

Editing Multiple Objects

The Properties panel supports multiple object editing, where the property settings that are identical in all currently selected objects may be modified. When multiples of the same object type are selected manually, via the Find Similar Objects dialog or through a Filter or List panel, a Properties panel field entry that is not shown as an asterisk (*) may be edited for all selected objects.

Via a List Panel

Panel pages: SCH List, SCHLIB List, SCH Filter, SCHLIB Filter

List panel allows you to display design objects from one or more documents in tabular format enabling quick inspection and modification of object attributes. Used in conjunction with appropriate filtering - by using the applicable Filter panel, or the Find Similar Objects dialog - it enables the display of just those objects falling under the scope of the active filter – allowing you to target and edit multiple design objects with greater accuracy and efficiency.

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。