PCB_Cmd-ManualRouteManualRoute_AD

Applied Parameters: mode= line

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, keepout boundaries, and so on.

Access

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

• PCB Editor - the following methods of access are available:
  • Choose the Place » Line command from the main menus.
  • Click the  button on the Utility Tools drop-down () of the Utilities toolbar.
• PCB Library Editor - the following methods of access are available:
  • Choose the Place » Line command from the main menus.
  • Click the  button on the PCB Lib Placement toolbar.
  • Right-click in the workspace and choose the Place » Line command from the context menu.

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 and 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 and 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.

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.
• Press the Tab key to access the Line Constraints dialog, from where properties for the track (its width and layer) can be changed on-the-fly.

Placement Modes

While placing track segments there are 5 available corner modes, 4 of which also have corner direction sub-modes. During placement:

• Press Shift+Spacebar to cycle through the 5 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 1 segment per click (the first 5 images just below), or 2 segments per click (the last image in the set just 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 5 available corner modes, press Spacebar to toggle the corner direction, press the 1 shortcut to
toggle placement between 1 segment or 2 segments.

Tips

1. A Track can be placed as a layer-specific keepout object, or an all-layer keepout to act, for example, as a placement or routing barrier. Objects defined as keepouts are ignored during output generation, such as photo plotting and printing. A layer-specific keepout track is simply a Track object with its Keepout property enabled, an all-layer keepout is a Track that has been placed on the Keepout layer.
2. While attributes can be modified during placement (Tab to bring up associated properties dialog), bear 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: None

Summary

This command is used to interactively route the connections on your board. Routing is the process of connecting the nodes in each net by placing a series of track segments and vias to define a path from one node to the next. The Interactive Routing tool helps maximize routing efficiency and flexibility in an intuitive way, including following cursor path for laying route sections, pushing obstacles, and automatically following existing connections, all in accordance with applicable design rules.

Access

This command is accessed from the PCB Editor by choosing the Tools » Legacy Tools » Interactive Routing command, from the main menus.

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. If you click to start placement on an existing object, the track will adopt the net name of that object.
2. Move the cursor to define the track segment and 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 and 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.

When you start interactive routing, the PCB Editor will not only let you start placing track objects, it will:

• Monitor cursor position and mouse-clicks, applying all applicable design rules.
• Follow your cursor path, minimizing the number of actions required to place sections of routing.
• Monitor the connectivity and update connection lines as soon as you finish a route.
• Supports routing-specific shortcuts, for example pressing the * key on the numeric keypad to push to the next signal layer, inserting a via in accordance with the routing via style design rule.

As you route the net, the standard conflict resolutions modes are available: Push Obstacles, Ignore obstacles, and Stop at First Obstacle. Use Shift+R to cycle through the modes.

The following basic keyboard shortcuts can be used at any time:

• Click or Enter - commits the routing up to the current cursor position and places the tracks.
• Right-click or Esc - terminates the current route. Any routing that has been committed before calling the termination is retained.
• Backspace - unwinds the last committed route back to its starting point. If any objects had been pushed through placing the last segment, they are moved back to their original positions. This feature is not available after using Auto-Complete.
• 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.

Placement Modes

While placing track segments there are 5 available corner modes, 4 of which also have corner direction sub-modes. During placement:

• Press Shift+Spacebar to cycle through the 5 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 1 segment per click (the first 5 images just below), or 2 segments per click (the last image in the set just 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 5 available corner modes, press Spacebar to toggle the corner direction, press the 1 shortcut to
toggle placement between 1 segment or 2 segments.

Loop Removal

Altium Designer provides support for Loop Removal when interactively routing your nets. As you route there will be many instances where you need to change some of the existing routing. Rather than attempting to change the existing routing using a drafting type approach of clicking and dragging track segments, you re-route. To do this, launch the Interactive Routing command, click on the existing routing to start, and then route the new path, coming back to meet the existing routing. This will create a loop with the old path and the new path - no need to worry though, as soon as you right-click or press Esc to terminate the route, the redundant segments are automatically removed, including any redundant vias.

Tips

1. Tracks on a PCB are made from a series of straight segments. Each time there is a change of direction, a new track segment begins. Also, by default, the PCB editor constrains tracks to a vertical, horizontal or 45° orientation, allowing you to easily produce professional results. This behavior can be customized to suit your needs.
2. Interactive routing preferences are defined on the PCB Editor - Interactive Routing page of the Preferences dialog. These preferences can be accessed while routing by using the Tab shortcut.
3. For a high-level overview on interactively routing nets in Altium Designer, see Interactive Routing.

Applied Parameters: mode=SMART|TARGET=DIFF_PAIR

Summary

This command is used to place differential pair track objects onto the current document and is useful for quickly routing connections manually. Differential pair routing is a design technique employed to create a balanced transmission system able to carry differential (equal and opposite) signals across a printed circuit board. Typically this differential routing will interface to an external differential transmission system, such as a connector and cable.

Access

This command is accessed from the PCB Editor by choosing the Tools » Legacy Tools » Differential Pair Routing command, from the main menus.

Use

Differential pairs are routed as a pair - that is, you route two nets simultaneously. After launching the command, you will be prompted to select one of the nets in the pair. Click on either to start routing. It doesn't matter if the positive or negative trace in a pair is selected as the system will automatically select the other trace too.

As you route, the Smart Router attempts to completely route the chosen connections along the shortest path, using horizontal, vertical and diagonal segments, while automatically walking around any obstacle along the path. The Smart Router will automatically complete the entire connection if both the start and end nodes are on the same layer, while maintaining any applicable design rules.

Tips

1. Differential pairs need to be defined first either through the schematic design (through placement of Differential Pair Directives), or manually via the PCB panel (configured in its Differential Pair Editor mode). You also need to have defined applicable rules prior to using this command. These are: Routing Width, Differential Pairs Routing, and Electrical Clearance.
2. Interactive routing preferences are defined on the PCB Editor - Interactive Routing page of the Preferences dialog. These preferences can be accessed while routing by using the Tab shortcut.

Applied Parameters: mode=SMART|TARGET=SINGLE

Summary

This command is used to place track objects onto the current document and is useful for quickly routing short connections.

Access

This command is accessed from the PCB Editor by choosing the Tools » Legacy Tools » Smart Interactive Routing command, from the main menus.

Use

After launching the command, the cursor will change to a crosshair and you will enter track placement mode.

As you route, the Smart Router attempts to completely route the chosen connection along the shortest path, using horizontal, vertical and diagonal segments, while automatically walking around any obstacle along the path. The Smart Router will automatically complete the entire connection if both the start and end nodes are on the same layer, while maintaining any applicable design rules.

Tips

1. Interactive routing preferences are defined on the PCB Editor - Interactive Routing page of the Preferences dialog. These preferences can be accessed while routing by using the Tab shortcut.

Applied Parameters: mode= line|Keepout=True

Summary

This command is used to place a layer-specific keepout Track object onto the active document. A keepout track is simply a standard track object that has its Keepout property enabled. It can be used to designate a 'no-go' area for autorouting. Objects defined as keepouts are ignored during output generation, such as photo plotting and printing.

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.

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 and 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 and 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.

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.
• Press the Tab key to access the Line Constraints dialog, from where properties for the track (its width and layer) can be changed on-the-fly.

Placement Modes

While placing track segments there are 5 available corner modes, 4 of which also have corner direction sub-modes. During placement:

• Press Shift+Spacebar to cycle through the 5 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 1 segment per click, or 2 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 a standard Track object on that layer.
2. While attributes can be modified during placement (Tab to bring up associated properties dialog), bear 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.