Interactively Routing Your PCB in Altium Designer

Created: December 19, 2023 | Updated: September 27, 2024 | Applies to version: 24

Now reading version 24. For the latest, read: Interactively Routing Your PCB in Altium Designer for version 25

Routing is the process of defining a connective path between the nodes in each net. This path is defined by placing PCB design objects, such as tracks, arcs, and vias, on the copper layers to create a continuous connection between the nodes. Rather than placing these objects one by one to build up the connective path, you interactively route the connection.

In the PCB editor, interactive routing is an intelligent process. After launching the command, click on a pad to select a connection to be routed. The interactive router then attempts to define a route path from that pad, all the way to the current cursor location.

The size of the track that is placed is controlled by the applicable Routing Width design rule, and the clearance from other net objects is controlled by the applicable electrical Clearance design rule. How the interactive router responds to existing objects, such as pads and routing on other nets, depends on the current Routing Conflict Resolution mode. The mode determines whether the router will Walkaround the obstacle, or attempt to Push it, or Stop, or Ignore it.

Cursor guided routing makes complex manual routing around obstacles fast, easy and intuitive. In other words, you create the path of the route with your mouse and the Interactive Router attempts to place the tracks according to that path. This works in accordance with design rules and also with various constraints for track placement and corner types.

Interactive routing can be performed on:

A single net – Route » Interactive Routing
Two nets configured as a differential pair – Route » Interactive Differential Pair Routing – learn more
A set of selected nets – Route » Interactive Multi-Routing – learn more

Interactively routing a connection - after launching the command and clicking on a connection line, the Interactive Router finds a path from the net object to the current cursor location, weaving around existing objects. A click of the mouse button will place all hatched track segments, Ctrl+Click to auto-complete the route.

Interactive Routing Tips

Run the Route » Interactive Routing command (the button on the Active Bar, shortcut: Ctrl+W) then click on an object that has a net attribute to start routing. This can be a pad, a connection line, an existing via, a track end on a partially routed net, in fact, any object that belongs to the net.
The PCB editor will jump to the nearest electrical object on that net, such as the center of a pad or the end of a track segment, and then attempt to define a route path from there to the current cursor location.
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.
- Support routing-specific shortcuts, such as pressing the * key on the numeric keypad to push to the next signal layer or inserting a via in accordance with the routing via style design rule.
As you route, click to place the tracks up to the cursor, then continue moving your cursor, and so on. This is so that the software can accurately maintain the path you have chosen—if you go too far before committing the tracks, portions of your path may be altered.
If you prefer working in a panel to using shortcuts, press Tab to pause routing and open the Interactive Routing mode of the Properties panel.
Many of the settings, such as the current routing mode, width, gap, and via size, are displayed on the Status bar or the Heads Up Display (Shift+H to toggle it on/off).
The Interactive Router's ability to reach the current cursor location depends on the current Routing Conflict Resolution mode, which is displayed on the Status bar () and the Heads Up Display when the Interactive Routing command is running.
Press Shift+R to cycle through the available conflict resolution modes. You can configure which modes are available on the Interactive Routing page of the Preferences dialog.
If the mode is set to Walkaround, Push and Hug or Push, the Interactive Router will attempt to find a path around and between existing objects, as shown in the video below.
Potential route path segments are displayed as hatched (placed on the next click) or hollow (the look-ahead segment; use this to work out where the previous segment should end).
Click or press Enter to place all hatched segments.
Right-click or Esc to terminate the current route. Any routing that has been committed before calling the termination is retained.
Press Spacebar to toggle the corner direction.
Press Shift+Spacebar to cycle through the available corner modes (learn more).
Press Backspace to "rip up" the last-placed segment(s). 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.
To switch routing layer and insert a via:
- Press the * key on the numeric keypad to switch the next available signal layer, or
- Press + and - keys on the numeric keypad, or
- Use the Ctrl+Shift+Wheel Scroll shortcut combination, or
- Press the 8 key to select a Via Type from those available (learn more).
Press L when you click to start routing on a through-hole pad or via and realize you are on the wrong layer, each press will step to the next available signal layer.
Press / on the numeric keypad to insert a via and release that connection (use this for fanouts).
Press 2 to insert a via and not switch layers (continue routing on the same layer).
Ctrl+Click to instruct the interactive router to attempt to automatically complete the current route. If it does not auto-complete, it does not mean the connection cannot be routed. It could be that the distance is too far or it could be that the termination point is on another layer.
The Quick Routing and Quick Differential Pair Routing commands offer lighter routing with fewer settings and capabilities, suitable for simpler designs.
This page describes the process of interactively routing a single net and the settings that control that process. If you are looking for information on specialized routing techniques, such as differential pair or controlled impedance routing, refer to the links on Routing the PCB page.
Press Shift+F1 while routing to display a menu of available in-command shortcuts. You can select a command from the menu or use the shortcut keystrokes displayed next to each command.

Monitoring Connectivity during Interactive Routing

The PCB editor includes a net analyzer that constantly monitors the location of all objects in the design space and updates the connection lines when any net-type object is edited. The net analyzer monitors all the objects attached to a net. For example, when a connection is routed, the connection line between those two pads is automatically removed by the net analyzer. If a net is partially routed, then a shorter connection line will be displayed between the two closest route points on the net.

It does not matter if you choose to ignore the connection line and route the net from/to a different location. As soon as routing is terminated, the net-analyzer runs and removes the connection line if it is no longer required, as shown in the video below.

Even though the connection line connects the pad centers, you are free to route wherever you choose. The net analyzer constantly monitors the routing progress and updates the connection line.

Because the arrangement of connection lines is determined by the routing topology design rule, it is possible that the connection line will not attach to the end of the track and instead attach to some other point in the net that is closer to another point in the net. If preferred, connection lines can be forced to the track ends by enabling the Smart Track Ends option on the PCB Editing – General page of the Preferences dialog. The video below demonstrates this. Note that you can force the net analyzer to run and update the connection lines, by performing an edit action on an object belonging to that net. Edit actions include: moving an object, clicking and holding on an object, or double-clicking to display that object's properties.

Note how the GND net connection line is attached to pad 1 instead of the end of the route. Once Smart Track Ends has been enabled and an edit performed, the connection line jumps to the end of the route.

To learn more about the connectivity in the PCB design space, refer to the Understanding Connectivity on Your PCB page.

How the Routing is Located in the Design Space

The PCB editor is a grid-based editing environment, the default behavior is for your interactive routing to be placed on the current snap grid. As well as the snap grid, the software includes a number of additional snap features, designed to help you accurately position and align design objects. Together, these features are referred to as the Unified Cursor-Snap System.

The key elements of this system include:

User-Definable Grids – available in both Cartesian and Polar formats.
Object Snapping – enabling placed objects to pull the cursor into position, based on cursor proximity to that object's snap points (hotspots). Use this to pull the cursor to the center of an off-grid pad, for example.
Snap Guides – that can be freely placed and provide a handy visual cue for object alignment.
Axis Snapping – a feature to pull the cursor, in either the X or Y direction, so that it axially aligns with a nearby object's hotspot.

Demonstration of the cursor-snap features.

The Snap System options are configured:

In the Properties panel, when there are no objects selected, or
By pressing Ctrl+E during routing to display the floating controls (as shown in the video above).

Learn more about Working with the Cursor-Snap System

The Basics of Interactive Routing

When you launch the interactive routing command and click on a connection line, the interactive routing engine will add a chain of connected track segments from the nearest existing net object, such as a pad or existing track, along the shortest available path to the current cursor location.

Those track segments will be hatched, to show that they are proposed segments that have not yet been placed (uncommitted). When you left-click to place those segments, they will become solid. These solid segments are referred to as soft commits – meaning the software recognizes them as segments you wish to retain, but the interactive routing engine may remove them or convert them back to uncommitted (hatched) if your routing path makes them redundant or creates an illegal shape. This behavior is demonstrated in the first video on this page.

Interactively routing a simple board.

When you click on a connection line to start routing, the software will jump to the nearest existing net object. To change which object on that net that has been chosen:

Press 9 to switch to the net object at the other end of the connection line. If the location of the object being switched to is not in the current window, the view jumps and centers around the new cursor position.
When there are two or more connection lines attached, press 7 to switch to another connection line, leaving the same net object.
Press Shift+F1 for a list of in-command shortcuts.

Configuring the Interactive Router

The default settings for interactive routing are configured:

In the PCB Editor – Interactive Routing page of the Preferences dialog (), or
During interactive routing, in the Properties panel, press Tab to display the panel as you route. Click the Pause icon ( ) displayed on the screen to return to routing.

The following collapsible sections contain information about the Interactive Routing options and controls:

Net Information

Net Name – the name of the net being interactively routed.
Net Class – the net class that the net being routed 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 can 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 Terminate Routing – when enabled, when you complete a route to the target pad, the routing tool does not continue in routing mode from the target pad but rather resets and is ready for you to click on the next source pad from which to route. If this option is disabled, after you route to the target pad, the tool will remain in routing mode and use the previous target pad as the source for the next route.
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.
Allow Via Pushing – check this option to allow pushing a Via when in Push Obstacles or HugNPush Obstacles mode.
Pin Swapping – check this option to enable pin swapping or use the Shift+C shortcut.
Auto Shrinking – check this option to automatically shrink the routing width to a value that would allow routing in locations where the trace cannot be routed between obstacles with the currently chosen routing width. Learn more about Routing Auto-shrinking.
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.
Pad Entry Stability – protects centered pad entries. Use the slider bar to configure the level of protection:
- Off = no protection
- Max = maximum protection
Apply Trace Centering – enables the trace centering functionality. When enabled, an additional clearance is added between the net being routed and existing pads/vias where possible and the following options are available to configure the functionality:
- Adjust Vias – when the option is enabled, vias will be pushed to maintain the additional clearance where possible.
  To prevent vias from being pushed by trace centering, you can either:
  - disable the Adjust Vias option. In this case, centering will not be applied between unlocked vias, or
  - disable the Allow Via Pushing option. In this case, vias will not be pushed (even to ensure the minimum clearance from the Clearance constraint).
- Added Clearance Ratio – a multiplier of the applicable clearance, which is then added to the clearance. For example, if the applicable clearance is 0.15mm, setting the option to 2 would instruct the routing engine to clear existing pads and vias by 0.15 + 2*0.15 = 0.45mm where possible. The routing engine can then reduce this clearance down to the specified clearance if required.
Learn more about Trace Centering.
Miter Ratio – controls the minimum corner tightness. The Miter Ratio multiplied by the current track width equals the separation between walls of the tightest U-shape that can be routed for that ratio. Enter a positive value equal to or greater than zero (the x multiplier is added automatically). Learn more about Mitered Corners.
Subnet Jumper Length – specify the desired length of a subnet jumper placed during interactive routing – learn more.

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.

Controlling the Corner Style

During interactive routing, the shape formed by the tracks and arcs that create a corner is referred to as the corner style. Diagonal corners are the most common, but curved corners (created by placing arcs), are also popular. There are 5 available corner styles, 4 of which also have corner direction sub-modes.

Press Shift+Spacebar during routing to cycle through the corner styles, the current style is displayed on the Status bar () and in the Heads Up display.
Press the Spacebar to toggle the corner direction.
Alternatively, press Tab to open the Interactive Routing mode of the Properties panel and change the corner style there.
Press the 1 shortcut key to toggle between routing with a look-ahead segment or placing all visible segments when you click. In the look-ahead mode, the last segment is displayed as hollow. This segment is referred to as the look-ahead segment and is not placed when you click. It allows you to work out where the previous segment needs to terminate without committing to placing that last segment.
Press the Backspace key to remove the last vertex.

Corner Style	Initial Corner Direction	Alternate Corner Direction	Notes
Track 45
Line 45/90 With Arc			Use the `,` & `.` keys to interactively change the arc radius, hold Shift to accelerate the radius change.
Track 90
Line 90/90 Vertical Start With Arc			Use the `,` & `.` keys to interactively change the arc radius, hold Shift to accelerate the radius change.
Any Angle			Use this mode in conjunction with Strong Glossing to perform snake routing.

Miter or Curve the Corners

Corners can be defined using short, straight track segments, or they can be created using one or more arcs. The images below show the two most popular corner styles; Track 45 and Any Angle.

Examples of two of the corner styles, Track 45 and Any Angle, click to enlarge an image.

Note how in the first image the interactive router is maintaining an overall orthogonal/diagonal pattern for the flow of the routing. In the Any Angle style the interactive router is finding the shortest path between the start location and the cursor location – this style of routing is called Snake Routing.

Mitered Corners

The most common routing corner shape is 45 degree mitered (diagonal) corners. Switch to the Track 45 corner mode to route diagonal corners. To ensure that it is not possible to inadvertently create right or acute corners during routing, both interactive routing and interactive sliding include a Miter Ratio option. Enter a positive value equal to or greater than zero. Some examples of the same trace routed with different values of the Miter Ratio option are shown below.

❯ ❮

~~Javascript~~ ID: InteractiveRouting_MiterRation_AD24_5

The Miter Ratio multiplied by the current track width equals the separation between the walls of the tightest U-shape that can be routed for that miter ratio, as shown below.

Set the Miter Ratio to zero to create a right- or acute-angle corner with tracks being routed or dragged. In this case, a miter is not created (true zero mitering, as it were) – show example. This feature is in Open Beta and available when the PCB.ZeroMitersRemoving option is enabled in the Advanced Settings dialog. When the option is disabled, a short miter fully covered by adjacent traces is created if Miter Ratio = 0.

The Miter Ratio value defined in the Properties panel is used during interactive routing, interactive sliding, glossing and retracing.
The default Miter Ratio value used during interactive routing and sliding is configured in the PCB Editor – Interactive Routing page of the Preferences dialog.
The default Miter Ratio value used during glossing and retracing is configured in the PCB Editor – Gloss and Retrace page of the Preferences dialog.

Arcs in Corners

Many designers require curved corners. Curved corners can be routed with either the Line 45/90 With Arc corner mode or the Line 90/90 With Arc corner mode. The Line 90/90 With Arc corner mode will force a 90-degree corner though, so use the Line 45/90 With Arc corner mode if the route needs to continue at 45 degrees. The arc can be interactively resized during routing using the and keys (hold Shift to accelerate the resizing process).

When a curved corner style is selected during interactive routing, the glossing engine will favor a tangential path around existing curved objects. That is, the arc placed to create the corner is located and radially sized to exactly curve around the existing object. This is designed to form smooth routing through a sea of curved shapes, for example, the escape via pattern under a BGA. If the Routing Gloss Effort is set to Strong it can result in the straight track segments between the arcs being placed at an angle other than horizontal or vertical.

If you require all of the straight track segments to placed exactly horizontal or vertical, with curved corners, it can be more efficient to route with diagonal corners and then gloss the routing to curve the corners. This is achieved by setting the Hugging Style set to Rounded, and then running the Retrace Selected command. Retrace is used rather than the Gloss Selected because Retrace does not attempt to shorten the route path and reduce the number of corners, instead it focuses on glossing along the same path, in accordance with the current design rule settings. Glossing is discussed below.

Curving the corners of existing routing.

Snake Routing

As well as using the arc corner modes as just discussed, a style of smooth flowing, point-to-point routing can also be achieved by setting the corner style to Any Angle and the Routing Gloss Effort to Strong. This creates what is referred to as Snake Routing. Use this when the routing requires any angle routes to flow through multiple curved objects, as shown in the example video below.

Snake routing, with the corner style set to Any Angle.

Automatic Connection Completion

The Interactive Router is able to attempt automatic completion (Auto-Complete) of connections to the target pad, hold Ctrl and Left Click to instruct the Interactive Router to attempt to complete the current connection. This can make routing much faster than placing individual track segments, however, there are some limitations to the Auto-Complete feature, as follows:

The start point and target pad must reside on the same layer.
The route can be completed in accordance with design rules (provided that routing conflicts are not being ignored).

Auto-Complete is available at any time, and you can even Ctrl+click directly on a pad or connection line to route it, there is no need to select it first. You can use Auto-Complete on connections that are partially routed as well. To do this, Ctrl+click on the end of the last track segment, or the remaining connection line, to complete it to the target.

If a connection cannot be auto-completed, the tool will return to the last used interactive routing mode.

Subnet Jumpers

One of the great strengths of an FPGA-based design is that the routing challenge can be resolved in both the PCB and the FPGA, potentially resulting in fewer routing layers and a simpler PCB. For this to be a reality, the design system must support both PCB-driven and FPGA-driven pin swaps. Altium Designer supports pin swapping in the PCB editor, from simple 2-pin components through to high pin-count FPGAs.

To support pin swapping at any stage of the design process, including on the routed PCB, the PCB editor can add and remove small routing connectors, called subnet jumpers. A subnet jumper is a short segment of track that the software recognizes as an element that can be easily placed and removed; either manually via the Add and Remove Subnet Jumper commands in the Route menu, or automatically by the routing engine if you route to a swappable pin during interactive routing.

❯ ❮

~~Javascript~~ ID: SubnetJumpers

Incoming routing approaches a high pin-count FPGA.

The PCB editor's Automatic Net/Pin Optimizer is used to find the best pin swaps, de-tangling the connection lines.

The Add Subnet Jumpers command is used to complete the routing.

Manually Placed Subnet Jumpers

When nets still include a short length of connection line, the routing can be completed by running the Route » Add Subnet Jumpers command. When this command is executed, the Subnet Connector dialog appears, as shown below. After a value is entered into the dialog and the Run button clicked, every connection line on the board is examined, and any whose length is no greater than the Maximum Subnet Separation length is replaced by a track segment. This track segment will have the same width as the narrower of the two segments being joined. Note that the angle that the subnet jumper is placed at is defined by the locations of the connection line end-points.

Specify the maximum length allowed for subnet jumpers.

Run the Route » Remove All Subnet Jumpers command to remove all existing subnet jumpers from the board.
To support the Add and Remove Subnet Jumpers commands, the Edit » Slice Tracks command can be used to slice existing routing.

Subnet Jumpers Placed during Interactive Routing

If the net being routed is configured to be swappable, the routing engine will recognize and highlight all potential routing targets. If you are routing toward an existing track segment (rather than a pad) and you elect to route to a swappable track segment rather than the same-net track segment, the Interactive Routing engine automatically adds a subnet jumper, as demonstrated in the video below.

A subnet jumper is automatically added during interactive routing if the target is the swappable route, rather than the same-net route.

To perform pin swapping, the Pin Swapping option must be enabled. Press Tab while routing to display the Interactive Routing mode of the Properties panel, and configure the option.
The length of a subnet jumper placed during interactive routing is defined by the Subnet Jumper Length option in the Properties panel for interactive routing.

Resolving Subnet Jumpers into Standard Tracks

To convert a subnet jumper to a regular track segment, click and hold on it briefly, then release the mouse button (without moving the mouse). The subnet jumper will be replaced by a standard track segment, as shown towards the end of the video above. To use the same approach to convert multiple subnet jumpers in a single action, select the subnet jumpers first and then click and hold on one of the selected subnet jumpers. To select all subnet jumpers on the board, run the query IsSubnetJumper in the PCB Filter panel with the Select checkbox enabled.

Interactive Routing and Interactive Sliding Options

Whether you're interactively routing a connection or dragging an existing route to make way for more routing, the same set of routing technologies are applied. This section summarizes the options available in the Interactive Routing and the Interactive Sliding modes of the Properties panel. The default settings for many of these options are configured in the PCB Editor – Interactive Routing page of the Preferences dialog.

Interactive Routing and Interactive Sliding Options

Gloss Effort (Routed)

During a route event, such as interactive routing, interactive sliding, or ActiveRouting, the software runs the glossing engine. The glossing engine constantly reviews all of the segments placed or impacted by the current route event, attempting to improve the quality of the results. Measures of quality include: reducing the number of corners, reducing the number of segments, removing acute angles and reducing the overall route length.

Glossing has three settings; Off, Weak and Strong. These settings are discussed in the Glossing – Smoothing the Routes section.

Gloss Effort (Neighbor)

Gloss Effort (Neighbor) configures the amount of glossing applied to adjacent routes that are impacted by the current interactive routing or sliding. It also has three settings; Off, Weak and Strong.

Hugging Style

This option controls how corner shapes are to be managed during interactive sliding and will affect both the tracks being slid and the tracks being pushed. During sliding use the Shift+Spacebar shortcut to cycle through the three modes.

45 Degree – always use straight orthogonal/diagonal segments to create corners during sliding (use this mode for traditional orthogonal/diagonal routing behavior).
Mixed – use straight track segments when the objects being moved/pushed against are straight, use arcs when they are curved.
Rounded – use arcs at each vertex involved in the move/push. Use this mode for snake routing, and to use arcs + any angle routes when glossing (during interactive routing and manual glossing).

Existing corners that are impacted by track movement during interactive sliding, will be converted (45 Degree to Rounded, or Rounded to 45 Degree) based on the current Hugging Style.

Conflict Resolution

This option determines how you want the routing/sliding objects to react when they encounter an existing object. Use the Shift+R shortcut to cycle through the available modes during routing or sliding.

These are the modes that are referred to as the Routing Conflict Resolution modes in the PCB Editor – Interactive Routing page of the Preferences dialog.

Vertex Action

To better support the designer's need to easily manipulate and re-shape the existing routing, there are specific options that are applied when you click and drag on a vertex rather than a track or arc (the vertex is the corner location where two segments meet). Use the Spacebar shortcut to cycle through the available modes during sliding.

Deform – break or lengthen the track segments attached to the moving vertex so that the vertex follows the cursor movement.
Scale – hold the corner shape and resize and move the incoming track segments, keeping the vertex attached to the cursor.
Smooth – reshape the corner smoothly, inserting arcs to create a curved corner when dragging inward (in Mixed or Rounded Hugging Style), at every vertex impacted by the sliding process. Also add arcs when dragging outward in Rounded Hugging Style.

Checkbox Options

Automatically Terminate Routing – when the current connection being routed reaches the target pad, automatically stop routing that net but remain in the Interactive Routing command, ready to start routing another net.
Automatically Remove Loops – when this option is enabled you can route a new path for an existing route – when the new route path comes back to meet the existing path the redundant loop is automatically removed. Learn more about Modifying Existing Routes.
Remove Net Antennas – a net antenna is a short, unterminated track (arc) segment. These are automatically removed if the current routing impacts on an object that the antenna is touching.
Allow Via Pushing – during routing/sliding in Push or Hug & Push modes, allow existing vias to also be pushed.
Display Clearance Boundaries – display the no-go area around existing objects, defined by the applicable Clearance design rule(s).
- Reduce Clearance Display Area – reduce this display to a circular zone around the current cursor location.
Show Length Gauge – the length gauge indicates how well the current route is meeting applicable Length and Matched Length design rules. Learn more about Length Tuning.

Pad Entry Stability

The Pad Entry Stability slider protects centered pad entries, preventing Glossing from un-centering a centered track (it holds a centered track on-center, it does not center an un-centered track). Use the slider bar to configure the level of protection:

Off = no protection
Max = maximum protection

Trace Centering

The trace centering functionality adds an additional clearance between the net being routed or dragged and existing pads/vias where possible when the Apply Trace Centering option is enabled. When the option enabled, the following options are available to configure the functionality:

Adjust Vias – when the option is enabled, vias will be pushed to maintain the additional clearance where possible.
To prevent vias from being pushed by trace centering, you can either:
- disable the Adjust Vias option. In this case, centering will not be applied between unlocked vias, or
- disable the Allow Via Pushing option. In this case, vias will not be pushed (even to ensure the minimum clearance from the Clearance constraint).
Added Clearance Ratio – a multiplier of the applicable clearance, which is then added to the clearance. For example, if the applicable clearance is 0.15 mm, setting the option to 2 would instruct the routing engine to clear existing pads and vias by 0.15 + 2*0.15 = 0.45 mm where possible. The routing engine can then reduce this clearance down to the specified clearance if required.

To disable trace centering when interactively sliding a trace, you can use the Disable Trace Centering When Dragging option in the Dragging region of the PCB Editor – Interactive Routing page of the Preferences dialog or in the Properties region of the Properties panel for interactive sliding. When this option is enabled, trace centering does not apply during the interactive sliding of traces even if the feature's main Apply Trace Centering option is enabled.

Learn more about Trace Centering.

Miter Ratio

The Miter Ratio controls the minimum corner tightness. The Miter Ratio multiplied by the current track width equals the separation between walls of the tightest U-shape that can be routed for that ratio, as shown in the Mitered Corners description, earlier on this page. Enter a positive value equal to or greater than zero (the x multiplier is added automatically).

Min Arc Ratio

The Min Arc Ratio is applied during any angle interactive routing and also during interactive sliding with Mixed Hugging Style. The ratio is used to determine the minimum radius arc allowed, when the arc radius falls below this minimum the arc is replaced by track segments, where:

Min Arc Radius = Min Arc Ratio x Arc Width

This setting is not applied during any arc in corner routing or interactive sliding with Rounded Hugging Style, as these modes do not use segmented arcs.
Set the Minimum Arc Ratio to 0 (zero) to always use arcs.

Learn more about Modifying Existing Routes

Glossing – Smoothing the Routes

To help produce neat routing with the minimum number of corners, the PCB editor includes a Glossing tool. Glossing is a sophisticated set of algorithms developed specifically to produce cleaner routing and pad entries, that respect the intent of the applicable design rules. Glossing attempts to reduce the path length, improve the shape of corners and reduce their number, generally resulting in neater routing created from fewer segments. Glossing also leaves sub-net jumpers as they were, and when there are room-based width rules, width changes at the boundary are respected. As you move the cursor around and define a new interactive route path, all of the yet-to-be-committed routing is also automatically glossed.

The Glossing engine also includes a Retrace Selected command. Use this when you need to update selected routes to the changes you have made to settings in the routing rules. With Retrace, you can "fatten up" selected power routing, or update the selected differential pair to new width and gap settings.

Glossing is applied during: Interactive Routing, Interactive Sliding, and by running the Gloss Selected or Retrace Selected commands.

Glossing has three settings: Off, Weak, and Strong. Use the Ctrl+Shift+G shortcut to cycle through the settings during interactive routing or interactive sliding, or press Tab to open the Properties panel and select the setting:

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). In other words, the geometry of the trace is mainly preserved, just locally smoothed. This mode of glossing is typically useful for fine-tuning track layout or when dealing with critical routes.
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. Note that when Strong glossing is combined with one of the arc in corner modes, it also allows any-angle traces. The assumption here is that since the designer is curving the corners they will be comfortable with non-orthogonal routing between corners.

Along with the current Gloss Effort setting, Glossing also obeys these settings:

Corner Style
Hugging Style (during Interactive Sliding and also when the Gloss Selected or Retrace Selected commands are run)
Miter Ratio
Min Arc Ratio

Using these options, Glossing controls how tightly a corner is created and how the curved shape is formed in the route around a curved obstacle.

To control glossing effort during interactive routing or sliding, there are two options: Gloss Effort (Routed) for the route being placed or dragged and Gloss Effort (Neighbor) for the adjacent routes that are impacted by the current interactive routing or sliding. Examples of different gloss effort modes for these options are shown below.

❯ ❮

~~Javascript~~ ID: InteractiveRouting_GlossEffortRouted_AD24

❯ ❮

~~Javascript~~ ID: InteractiveRouting_GlossEffortNeighbor_AD24

Existing routing can be glossed by running the Route » Gloss Selected command. Use this to your advantage to perform design changes, such as converting mitered corners to arcs, by configuring the Corner Style before running the command.

Learn more about Glossing & Retracing of Existing Routes

Temporarily Inhibit Glossing – Glossing is a core feature for interactive routing and sliding, but there will be situations where it prevents you from achieving the route shape you desire. Glossing can be temporarily inhibited during routing by holding the Ctrl+Shift shortcut keys; when they are released, glossing will be re-enabled at the current setting.

Performing a Gloss

The glossing tool is run:

During Interactive Routing – in accordance with the current gloss settings, defined in the PCB Editor – Interactive Routing page of the Preferences dialog or the Interactive Routing mode of the Properties panel.
During Interactive Sliding – in accordance with the current gloss settings, defined in the PCB Editor – Interactive Routing page of the Preferences dialog or the Interactive Sliding mode of the Properties panel.
On the currently selected routing – choose the Route » Gloss Selected command from the menus or press the Ctrl+Alt+G keyboard shortcuts, to gloss in accordance with the gloss settings defined in the PCB Editor – Gloss and Retrace page of the Preferences dialog or the Gloss And Retrace panel.
After ActiveRoute – by enabling the Gloss Results option in the PCB ActiveRoute panel.

Inhibit Glossing During Routing and Sliding

There may be times when you want to temporarily turn off glossing. Glossing can be inhibited by pressing and holding the Ctrl+Shift shortcut keys – as soon as the keys are released glossing resumes at the current Routing Gloss Effort setting. Note that the status bar will not reflect this state; it will continue to display the last selected state.

Glossing Options