PCB_Cmd-ManualRouteManualRoute_AD

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.

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.

• 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.

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.

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.

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.