Altium NEXUS Documentation

ManualRoute

Modified by Susan Riege on Jul 13, 2018

Parent page: PCB Commands

The following pre-packaged resources, derived from this base command, are available:


Applied Parameters: mode= line|Keepout=True|UpdateCaption=False

Summary

This command is used to place a Line object onto the active document. In truth, a line is actually a Track object that is not net-aware. Tracks are typically placed as 'lines' on a non-electrical layer where they are used as general-purpose drawing elements to create component outlines, instructional information, and so on.

Although tracks and lines are actually the same object, the difference is how the software behaves during their placement, which is why there are different commands. When a track placement command is run, such as Interactive Routing, the software monitors the click location and automatically adopts the net name of an existing object (such as a pad) under the click location. It also monitors and obeys any applicable design rules. When a line placement command is run, these monitoring behaviors do not occur.
For detailed information about this object type, see Track.

Access

This command can be accessed from the PCB Editor and PCB Library Editor by:

  • Choosing the Place » Line command from the main menus.
  • Locating and using the Line 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.
  • Right-clicking in the workspace then choosing the Place » Line command from the context menu.
In addition, from the PCB Editor the command can be accessed by clicking the  button on the Utility Tools drop-down () of the Utilities toolbar. In the PCB Library Editor, access can be made by clicking the  button on the PCB Lib Placement toolbar.

Use

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

  1. Click or press Enter to anchor the starting point for the first track segment.
  2. Move the cursor to define the track segment then click or press Enter to anchor the end point for this first segment, which is also the start point for the next connected segment.
  3. Continue to position the cursor then click or press Enter to anchor a series of vertex points that define the series of connected track segments.
  4. Right-click or press Esc to end the current series of connected track segments.
Press the Tab key to access the Properties panel, from where properties for the line (its width and layer) 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 or press Esc.

Additional actions that can be performed during placement include:

  • Press the * key on the numeric keypad to cycle through the available signal layers. Alternatively, use the Shift+Ctrl+Wheel Roll combination to move through the routing layers; each notch of the mouse wheel will move to the next (or previous) available signal layer.
  • Press the + and - keys on the numeric keypad to cycle forward and backward through all layers currently visible in the design.

Placement Modes

While placing track segments there are five available corner modes, four of which also have corner direction sub-modes. During placement:

  • Press Shift+Spacebar to cycle through the five available corner modes: 45 degree, 45 degree with arc, 90 degree, 90 degree with arc, and Any Angle.
  • Press Spacebar to toggle between the two corner direction sub-modes.
  • When in either of the arc corner modes, hold the  or  keys to shrink or grow the arc. Hold the Shift key as you press to accelerate arc resizing.
  • Press the 1 shortcut key to toggle between placing one segment per click (the first five images below), or two segments per click (the last image in the set below). In the first mode, the hollow track segment is referred to as the look-ahead segment.
  • Press the Backspace key to remove the last vertex.

Press Shift+Spacebar to cycle through the five available corner modes, press Spacebar to toggle the corner direction, press the 1 shortcut to
toggle placement between one segment or two segments.

Tips

  1. While attributes can be modified during placement (Tab to open the Properties panel), keep in mind that these will become the default settings for further placement unless the Permanent option on the PCB Editor – 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.


Applied Parameters: mode= line|Keepout=True

Summary

This command is used to place a Keepout Track object onto the active document. A Keepout in PCB design is a user defined area or perimeter placed in the layout that copper objects cannot intersect. Typically included to control the area used by automated copper placement actions, such as polygon pours and interactive routing, a Keepout also represents an invalid location when manually placing copper objects. 

As specified ‘no go’ areas during design layout, Keepout objects use the existing Clearance Constraint Rules to control routing and detect placement violations, but unlike other placed objects, cannot be assigned to a Net and are not shown in generated Outputs or printouts. In its simplest sense, a Keepout acts as an ‘interference’ object that prevents other copper objects from intersecting its area as specified by the global Clearance Rule.

Access

This command is accessed from the PCB Editor and the PCB Library Editor by choosing the Place » Keepout » Track command from the main menus.

Keepouts can be placed on all (copper) signal layers, excluding copper planes. When the currently active board layer is not compatible with Keepouts, the command is not available (grayed out).

Use

After launching the command, the cursor will change to a crosshair and you will enter keepout track placement mode. Placement is made by performing the following sequence of actions:

  1. Click or press Enter to anchor the starting point for the first keepout track segment.
  2. Move the cursor to define the track segment then click or press Enter to anchor the end point for this first segment, which is also the start point for the next connected segment.
  3. Continue to position the cursor then click or press Enter to anchor a series of vertex points that define the series of connected keepout track segments.
  4. Right-click or press Esc to end the current series of connected keepout track segments.
Press the Tab key to access the Properties panel, from where properties for the keepout track (its width and layer) 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, or press Esc.

Additional actions that can be performed during placement include:

  • Press the * key on the numeric keypad to cycle through the available signal layers. Alternatively, use the Shift+Ctrl+Wheel Roll combination to move through the routing layers; each notch of the mouse wheel will move to the next (or previous) available signal layer.
  • Press the + and - keys on the numeric keypad to cycle forward and backward through all layers currently visible in the design.

Placement Modes

While placing keepout track segments there are five available corner modes, four of which also have corner direction sub-modes. During placement:

  • Press Shift+Spacebar to cycle through the five available corner modes: 45 degree, 45 degree with arc, 90 degree, 90 degree with arc, and Any Angle.
  • Press Spacebar to toggle between the two corner direction sub-modes.
  • When in either of the arc corner modes, hold the  or  keys to shrink or grow the arc. Hold the Shift key as you press to accelerate arc resizing.
  • Press the 1 shortcut key to toggle between placing one segment per click or two segments per click. In the first mode, the hollow track segment is referred to as the look-ahead segment.
  • Press the Backspace key to remove the last vertex.

Tips

  1. To place an all-layer keepout, make the Keepout layer the active layer then place keepout track on that layer. Alternatively, after placement, select the keepout track and set its Restricted for Layer field (in the Properties section of the Properties panel) to Keep-Out Layer. Keepouts are indicated by the current Keep-Out layer color. Keepout objects set to a specific signal layer are outlined by the Keep-Out color, whereas Keepouts on the Keep-Out Layer show as solid color.
  2. When editing the properties of the placed keepout track, the associated Keepout Restrictions options determine which object types will be restricted by the Keepout. Deselecting an object type will cause the Keepout to allow transgressions by that type of object (not kept out) by not imposing the applicable Clearance Rule.
  3. Keepouts are automatically restricted to the Layer on which they are placed, so Keepouts applied directly to the Keep-Out layer will become All Layer Keepouts. When the Keepout Layer is changed, the Keepout will be limited to and appear on the specified Layer. Note that a conventional (non Keepout) object cannot be placed on the Keep-Out Layer.
  4. While attributes can be modified during placement (Tab to open the Properties panel), keep in mind that these will become the default settings for further placement unless the Permanent option on the PCB Editor – 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.

Contact Us

Contact our corporate or local offices directly.

You are reporting an issue with the following selected text
and/or image within the active document:
ALTIUM DESIGNER FREE TRIAL
Altium Designer Free Trial
Let’s get started. First off, are you or your organization already using Altium Designer?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

In that case, why do you need an evaluation license?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Got it. You actually don’t need an evaluation license for that.

Click the button below to download the latest Altium Designer installer.

Download Altium Designer Installer

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Please fill out the form below to get a quote for a new seat of Altium Designer.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

If you are on Altium Subscription, you don’t need an evaluation license.

If you are not an active Altium Subscription member, please fill out the form below to get your free trial.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Why are you looking to evaluate Altium Designer?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

You came to the right place! Please fill out the form below to get your free trial started.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

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.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Got it. You can download a free Altium Designer Viewer license which is valid for a 6 months.

Please fill out the form below to request one.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

That’s great! Making things is awesome. We have the perfect program for you.

Upverter is a free community-driven platform designed specifically to meet the needs of makers like you.

Click here to give it a try!

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Got it. You can download a free Altium Designer Viewer license which is valid for a 6 months.

Please fill out the form below to request one.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.