The Quick Routing command (accessed from the main menu and the Active Bar) offers lighter routing with less settings and capabilities, suitable for simpler designs. Its general behavior and shortcuts is the same as the standard Interactive Routing command.
Capabilities include:
-
A number of routing modes, such as: stop at first obstacle, walkaround, and push and shove.
-
Powerful dragging capabilities that maintains track angles and orthogonality.
-
A loop removal feature that makes re-routing a quick and easy process.
The Quick Routing tool helps maximize routing efficiency and flexibility in an intuitive way, including following cursor path for laying route sections, single-click routing completion, pushing or walking around obstacles, and automatically following existing connections, all in accordance with applicable design rules.
This router is referred to as Quick because it offers a reduced feature-set. Features that are not included in the Quick Router include:
-
No turn smoothing
-
Little support for Any Angle routing
-
No pushing of T-junctions
-
Simple Push&Shove support
-
No Miter Ratio, Min Arc, or Pad Entry Stability
-
Simple Gloss Effort, with no support for Gloss Neighbor
If you need any of these features, use the Interactive Routing tool.
The PCB editor also includes the Quick Differential Pair Routing tool -
learn more.
The following collapsible sections contain information about the Quick Interactive Routing options and controls available:
Net Information
-
Net Name – displays the name of the net to which the interactive routing is connected.
-
Net Class – displays the net class that the interactive routing belongs to (if it is a member of a net class).
-
Length – the total Signal Length. The Signal Length is the accurate calculation of the total node-to-node distance. Placed objects are analyzed to resolve stacked or overlapping objects and wandering paths within pads, and via lengths are included.
-
Delay – the total delay of the selected segments, including those unrouted.
Select the clickable links of the
Net Name,
Net Class,
Length, and
Delay from the
Interactive Routing mode of the
Properties panel to be redirected to the
PCB – Nets panel, where you may view and change details of the nets associated.
Properties
-
Layer – use the drop-down to specify on which layer the routing is located.
-
Via – if the via is associated with a template, the template name is displayed here.
-
Via Diameter – specify the via diameter.
-
Via Hole Size – specify the via hole size.
-
Width – use the drop-down to specify the width.
-
Min – signifies that the design rule minimum width defined for the current net will be used
-
Preferred – signifies that the design rule preferred width defined for the current net will be used.
-
Max – signifies that the design rule maximum width defined for the current net will be used.
Interactive Routing Options
-
Routing Mode – use the drop-down or use the Shift+R shortcut to cycle through the desired routing modes. The following choices are available:
-
Ignore Obstacles – select to ignore existing objects (routing can be freely placed). Violations are highlighted.
-
Walkaround Obstacles – select to have the Interactive Router route around existing tracks, pads, and vias. If this mode cannot walk around an obstacle without causing a violation, an indicator appears to show that the route is blocked.
-
Push Obstacles – select to have the Interactive Router move existing tracks out of the way. This mode can also push vias to make way for the new routing. If this mode cannot push an obstacle without causing a violation, an indicator appears to show that the route is blocked.
-
HugNPush Obstacles – select to have the Interactive Router hug existing tracks, pads, and vias as closely as possible and where necessary, push obstacles to continue the route. If this mode cannot hug or push an obstacle without causing a violation, an indicator appears to show that the route is blocked.
-
Stop At First Obstacle – in this mode, the routing engine will stop at the first obstacle that gets in the way.
-
AutoRoute Current Layer – select to enable auto-routing only on the current layer.
-
AutoRoute MultiLayer – select to enable auto-routing on multiple layers.
-
Corner Style – select the desired routing corner style or use the Shift+Spacebar shortcut to cycle through the corner styles.
-
Gloss Effort (Routed) – select the desired gloss level directly from the panel or use the Shift+Ctrl+G shortcut to cycle through the following choices:
-
Off – in this mode, glossing is essentially disabled. Note, however, that cleanup is still run after routing/dragging occurs to eliminate, for example, overlapping track segments. This mode is typically useful at the end stage of board layout when the ultimate level of fine-tuning is required (for example, when manually dragging tracks, cleaning pad entries, etc.).
-
Weak – in this mode, a low level of glossing is applied with the Interactive Router considering only those tracks directly connected to or in the area of the tracks that you are currently routing (or tracks/vias being dragged). This mode of glossing is typically useful for fine-tuning track layout or when dealing with critical traces.
-
Strong – in this mode, a high level of glossing is applied with the Interactive Router looking for shortest paths, smoothing out tracks, etc. This mode of glossing is typically useful in the early stages of the layout process when the aim is to get a good amount of the board routed quickly.
-
Gloss Effort (Neighbor) – select the desired gloss level to apply to traces being pushed by the net currently being routed directly from the panel through the following choices:
-
Off – in this mode, glossing is essentially disabled. Note, however, that cleanup is still run after routing/dragging occurs to eliminate, for example, overlapping track segments. This mode is typically useful at the end stage of board layout when the ultimate level of fine-tuning is required (for example, when manually dragging tracks, cleaning pad entries, etc.).
-
Weak – in this mode, a low level of glossing is applied with the Interactive Router considering only those tracks directly connected to or in the area of the tracks that you are currently routing (or tracks/vias being dragged). This mode of glossing is typically useful for fine-tuning track layout or when dealing with critical traces.
-
Strong – in this mode, a high level of glossing is applied with the Interactive Router looking for shortest paths, smoothing out tracks, etc. This mode of glossing is typically useful in the early stages of the layout process when the aim is to get a good amount of the board routed quickly.
-
Automatically Remove Loops – enable to automatically remove any redundant loops that are created during manual routing. This allows you to re-route a connection without having to manually remove redundant tracks. However, there are times when you need to route nets such as power nets and you need loops. You can toggle this option for a selected net by using the Shift+D shortcut to override this global setting for the same net.
-
Remove Loops With Vias – enable to automatically remove loops with vias. Disable this option for vias to remain during loop removal.
-
Remove Net Antennas – enable this option to remove any track or arc end that is not connected to any other primitive and forms an antenna.
-
Display Clearance Boundaries – enable to have the no-go clearance area defined by the existing objects and the applicable clearance rule displayed as shaded polygons within a local viewing circle or use the Ctrl+W shortcut to toggle on or off during routing. This option is not available in the Ignore Obstacles routing mode.
-
Reduce Clearance Display Area – enable to use a smaller clearance boundary. This option is available only when the Display Clearance Boundaries option is enabled.
-
Show Length Gauge – enable to display the length gauge, which shows the current routed length. The gauge settings are calculated from the set of constraints defined by the applicable design rules. Use the Shift+G shortcut to toggle the display on or off during routing.
Rules
Constraints defined by the applicable design rules will be listed under the Rules section of the Properties panel.
-
Via Constraint – click to open the Edit PCB Rule dialog in which you can define PCB rules for a via.
-
Width Constraint – click to open the Edit PCB Rule dialog in which you can define PCB rules for routing width.
