Altium Designer Documentation

PCB - Nets

Modified by Susan Riege on Aug 7, 2018
此文档页面引用了不再受支持的产品 Altium Vault, Altium Vault 及其组件管理功能已迁移到 Altium Concord Pro
All Contents

Parent page: PCB Panel

The Nets mode of the PCB panel


The PCB panel allows you to browse the current PCB design using a range of filter modes to determine which object types or design elements are listed, highlighted or selected. The panel also has editing modes for specific object types or design elements that provide dedicated controls for editing procedures. Note that you can access the properties for any element listed in the panel.

In Nets mode, the two main list regions of the panel will change to reflect an object hierarchy in order from the top:

  1. Net Classes, as defined by the board.
  2. Individual member Nets within a class.
  3. Individual items (Primitives) within a Net (pads, vias, tracks, and fills).

While the middle sections change between the various modes of the PCB panel, the top and bottom portions of the panel remain the same. For a panel overview and information on those sections, please see the PCB panel page.

Panel Access

When the PCB Editor is active, click the Panels button at the bottom-right corner of the workspace then select PCB from the context menu. Alternatively, you can access the panel through the View » Panels » PCB command.

Panels can be configured to be floating in the editor space or docked to sides of the screen. If the PCB panel is currently in a group of panels, use the PCB tab located at the bottom of the panels to bring it to the front.

Once the PCB panel has been opened, select the Nets option from the drop-down menu at the top of the PCB panel to enter Nets mode.

Browsing Nets

Net Classes

In the top region of the panel (Net Classes), right-click on a net or net item entry then choose Properties from the subsequent menu (or double-click on the entry directly) to access the Edit Net Class dialog in which you can view or edit the net membership of the class, rename it, or add additional classes.


The middle region of the panel displays nets from the Net Class(es) selected in the region above.

The following information is listed with each Net by default:

  • - this feature has two functions:
    • color background - the color assigned to the net. This color is always applied to the net's connection lines. It can also be applied to that net's routing using the net color display override feature. Double-click to edit the color for this net, or right-click to edit the color for all currently selected nets.
    • checkbox - check this to apply the color to the routing (enable the net color display override feature) for this net. Right-click to enable (or disable) the display override feature for all currently selected nets. Press F5 to enable/disable net color display override in the workspace.
      See Net Color Override - Displaying the Net Color on Routed Nets to learn more.
  • Name - name of the net.
  • Node Count - the total number of pads in this net.
  • Routed Length - the sum of the lengths of the placed track and arc segments that form the routing, plus the vertical distance traversed through vias (see note below). The routed length calculator does not attempt to resolve overlapping track segments or routing wiggles inside pads.
  • Signal Length - accurate calculation of the total node-to-node distance. The following notes apply to Signal Length calculations:
    • Resolves overlaps and wiggles inside pads.
    • Handles routing paths created with objects other than tracks and arcs (e.g., a region or a fill).
    • Includes vertical distances through vias (see note below).
    • Includes the Total Pin/Package Length for this net.
    • Includes the Un-Routed (Manhattan) Length for this net.
    • Failure to comply with applicable Length/Matched Length design rules is flagged by the signal length being displayed on a colored background: signal lengths that are too short in yellow, signal lengths that are too long in red.
      See Length Tuning to learn more about how the Length and Matched Length design rules are applied.
    • A signal is a point-to-point entity; for this reason, only nets with two nodes will show a Signal Length in the Nets mode of the panel (nets with other Node counts will display n/a). For nets with more than two nodes, define xSignals to calculate their signal length.
      See the PCB - xSignals panel page.
      See Defining High Speed Signal Paths with xSignals to learn more about xSignals.
  • Total Pin/Package Length - the sum of all the Pin Package Length values in all pads in that net. This value is defined as a property of the PCB pad and can also be specified in the schematic pin.
  • Un-Routed (Manhattan) Length - the vertical plus horizontal (X+Y) distance of all unrouted sections.

Right-click in the region then use the Columns sub-menu to add the following columns:

  • Min/Max - settings from the applicable Length and Matched Length design rules. If there is no applicable rule(s) defined, the internal defaults of Min=0mil and Max=99999mil are used.
    See Length Tuning to learn more how the Min and Max settings are derived from the Length and Matched Length design rules.
  • Estimated Length - this is the Routed Length plus the length of connection lines for any section still to be routed. It does not use the Manhattan length for the unrouted portion; instead it uses the direct point to point distance.

Vertical distance through a via - the vertical distance a signal travels through a via is the sum of all layer thicknesses (copper and dielectric) between the start and stop layers copper layers, plus half the thickness of the start layer and half the thickness of the stop layer. Layer thicknesses are defined in the Layer Stack Manager.


The display/inclusion of each net item type in the bottom Primitives region of the panel is dependent on whether the corresponding option for each has been enabled on the right-click menu, accessed from either the Nets or Primitives regions.

Right-click on a net or net item entry to select the included items.

Note that the Primitives list right-click context menu also offers the option to create an xSignal between two selected items. See the PCB - xSignals panel page for more information.

In summary, as you click on an entry in the panel's list, a filter will be applied based on that entry. The visual result of the selection (in the design editor window) is determined by the highlighting methods enabled (Dim, Zoom, etc.,). Multiple entries can be selected in each region using standard Shift+Click and Ctrl+Click features.

Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.



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?

Copyright © 2019 Altium Limited

既然您在使用Altium Designer,为何仍需要试用?

Copyright © 2019 Altium Limited


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

Copyright © 2019 Altium Limited

填写下方表格,获取Altium Designer最新报价。





您为何想要试用Altium Designer?

Copyright © 2019 Altium Limited



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.


好的,您可以下载免费的Altium Designer Viewer查看文档,有效期6个月。






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。