Glossing & Retracing of Existing Routes

Parent page: Routing the PCB

Routing a printed circuit board is a detailed, iterative process. Rarely are you able to simply route, or ActiveRoute, all of the nets in a single pass. More often you will be routing a set of nets and as you move on to the next set of nets, you are continually adjusting and moving existing routes, perhaps manually dragging them, or perhaps pushing and shoving them as you interactively route more nets.

The end result is that your finished routing can end up looking like it was autorouted, with lots of unnecessary jigs and corners.

Re-routing & Rearranging Existing Routes

Routing a board can be a complex and time-consuming process as you work to position the components and complete the routing - move that component slightly, shove that routing, re-route those critical nets to avoid potential cross-talk, now see if that bus can be routed through that area, and so on. As you route your board, you will be constantly modifying routing that you have already done.

There are two approaches to modifying the routing; you can either reroute or re-arrange.

Rerouting is ideal when the new route path is more complex than simply moving a few track segments. Rerouting is performed in the same way as the initial routing using the Interactive Routing (or Interactive Differential Pair Routing) command - when you complete the new route path the old loop of redundant track segments is removed.

Alternatively, you can re-arrange the routing. To re-arrange existing routing, click and hold on a track segment then drag it to its new location. Connected track segments will remain connected at the angle they were previously connected - a behavior called interactive sliding. Interactive sliding also supports the Conflict Resolution Modes, including Push, Hug and Push, and Ignore.

Reroute an Existing Route

• There is no need to un-route a connection to redefine its path; simply click the Interactive Routing button on the Active Bar ( ) and start routing the new path.
• The Loop Removal feature will automatically remove any redundant track segments (and vias) as soon as you close the loop and right-click to indicate you are done.
• You can start and end the new route path at any point, swapping layers as required.
• You can also create temporary violations by switching to Ignore Obstacle mode (as shown in the video below), which you later resolve.

A simple animation showing the Loop Removal feature being used to modify existing routing.

Rearrange Existing Routes

• To interactively slide or drag track segments across the board, click, hold and drag as shown in the video below.
• The default dragging behavior is configured on the PCB Editor - Interactive Routing page of the Preferences dialog.
• The PCB editor will automatically maintain the 45/90 degree angles with connected segments, shortening and lengthening them as required.

A demonstration of interactive sliding being used to modify the existing routing.

Interactive Sliding Tips

• While sliding a route you can move the cursor and hotspot snap it to an existing, non-moving object such as a pad. Use this to help align the new segment location with an existing object and avoid very small segments being added.
• During sliding, one of the Routing Conflict Resolution modes applies. Press Shift+R to cycle through the modes as you drag a track segment.
• To convert a 90-degree corner to a 45-degree route, start dragging on the corner vertex.
• The interactive sliding engine includes algorithms specifically for dragging a vertex (corner), configure the Vertex Action in the Preferences dialog, or in the Interactive Sliding mode of the Properties panel. Press the Spacebar to cycle through the modes as you drag a vertex.
• To break a single segment, select the segment first, then position the cursor over the center vertex to add in new segments.
• Existing pads and vias will be jumped, or vias will be pushed if necessary and possible when the Allow Via Pushing option is enabled.   
• Interactive sliding supports non-orthogonal routing.
• The default behavior is to drag (slide) tracks (selected or unselected). If you need to move a segment without maintaining its connection to the attached segments, change the default dragging behavior using either the Unselected via/track or the Selected via/track options on the PCB Editor - Interactive Routing page of the Preferences dialog.

Modifying T-Junctions

There is specific support for interactively modifying a T-junction - click and drag on the junction point to modify a T-junction.

Examples of the T-Junction dragging capabilities.

Interactive Via Dragging

PCB designers can spend a lot of time adjusting the routing, perhaps due to a late design change, or to achieve completion of their design. This can mean pushing and shoving existing routing, dragging vias, and nudging components.

Adjust the via dragging behavior in the Properties panel.

Complimenting the support for glossing of neighbor routes, via dragging is also supported. Via dragging supports Neighbor Glossing, configured through the Interactive Via Dragging mode of the PCB editor's Properties panel. Press Tab during via dragging to access the panel and adjust the settings.

Press Tab as you drag to configure the Via Dragging options.

Differential Pair Dragging

To recognize the members in a differential pair, the concept of Coupling is used. When the software recognizes objects that belong to a differential pair it will attempt to drag the pair's partner track or via if the Keep Coupled option is enabled in the Interactive Sliding or the Interactive Via Dragging modes of the Properties panel.

Press X as you drag a via-pair to rotate the pair by 90 degrees.

To confirm that the partner objects are coupled, the software checks that the objects:

• For via pairs - belong to the pair, and are closer than 2 * Preferred Gap
• For track pairs - belong to the pair, are on the same layer, are separated by no more than the Preferred Gap

Options that Affect Routing, Rerouting and Interactive Sliding

There are a number of options that impact the rerouting behavior, these options are configured in the PCB Editor - Interactive Routing page of the Preferences dialog.

• The Automatically Remove Loops option must be enabled to perform rerouting. There are situations when you may want to create loops, for example, power net routing. If necessary, Loop Removal can be disabled for an individual net by editing that net in the PCB panel. To access the option, set the panel to Nets mode, then double-click on the net name in the panel to open the Edit Net dialog.
• As with Interactive Routing, the Current Routing Conflict Resolution mode will be used.
  • Use the checkboxes to enable only those modes you want to be available in the Current Mode list.
  • Press Shift+R to cycle through the enabled modes as you reroute.
• The Automatically Terminate Routing option is useful. If it is enabled, as soon the new route connects to the existing routing, the redundant loop is removed (as shown in the video above). If this option is disabled, the loop is removed when you right-click to release the current route. The option can work against you when you need to place new routing on top of the existing routing (perhaps overlapping), in this situation it can be better to disable it.
• The Glossing Effort options control how strongly the routing engine attempts to smooth or gloss the routing being modified, and it does this based on the Hugging Style, Arc Ratio, Miter Ratio, and Pad Entry Stability settings. Learn more about glossing in the, Improving the Quality of the Routing section below.

Interactive Routing and Interactive Sliding Panels

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. Press Tab as you work to open the Properties panel in the relevant mode. After changing the settings, click the  icon in the middle of the screen to return to routing or sliding. The default settings for these options are configured in the PCB Editor - Interactive Routing page of the Preferences dialog.

Interactive Routing and Interactive Sliding Options

Routing 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 - 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 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.

Routing 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).

Routing Mode / Sliding Mode

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 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.
• Remove Net Antennas - a net antenna is a short, unterminated track (arc) segment. These are automatically removed if the current routing impacts 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

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.

Routing-Aware Move Component

While routing the board, it is not uncommon for the designer to need to adjust the location of a routed component to create space for new routing. To help with this, the PCB editor includes a routing-aware move component feature. The feature is enabled via the Component Re-route checkbox, in the PCB Editor - Interactive Routing page of the Preferences dialog. Essentially, the feature will break the routing at the component pads, fanouts or escape routes, and then attempt to re-route those broken connections once the moving component(s) has been placed. 

A key requirement of the feature is to preserve fanouts and escape routing. To support this, the Shift+Tab shortcut is used to cycle through the possible sets of objects being moved, as detailed below.

During the move process, the options can be controlled using the following shortcuts:

• Component Re-route Mode (Shift+R) - toggles the re-route mode on and off. After the moving set has been released, the software will attempt to re-route the component(s) to reconnect any broken nets. Use the Shift+R shortcut to disable the Component re-route option in Interactive Routing page of the Preferences dialog. The current Component Re-route status is displayed in the Heads Up display and on the Status bar. 
• Change Component Selection (Shift+Tab) - while dragging, the set of objects being moved can still be changed. Press Shift+Tab to cycle through the following selection sets:
  • Components only, then
  • Components +Via Fanouts +Escapes +Interconnects, then
  • Initial selection set (if different from the previous two), then
  • Back to Components only.
• The Move component with relevant routing option behaves as follows:
  • Enable the option to start the move component action with the relevant routing (Components +Via Fanouts +Escapes +Interconnects), use the Shift+Tab shortcut to cycle the selection set as described above. 
  • Disable the option to start the move component action with components only selected. Because the set of relevant routing objects is detected prior to the move commencing, it is not possible to use Shift+Tab to cycle through the selection set when the option is disabled.

When the Component Re-route option is enabled, connected routes are restored after the moving component is placed.

For better control of how pads of the component being moved should be connected with the objects of the same nets, you can use the N key to cycle through net line connect modes. The following modes are supported:

• Pad to Pad - during the move, connection lines displayed between pads of the component being moved and the nearest pads of the same nets on the board.
• Breaks - during the move, connection lines displayed between pads of the component being moved and the track breaks of the same nets on the board.
• Hidden - connection lines hidden.

Current net line connect mode is shown in the Heads Up Display (HUD) when a component is moved.

Improving the Routing

To help produce neat routing with the minimum number of corners, the PCB editor also 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 and also 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 as you 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" that existing power routing, or update that differential pair to new width and gap settings.

• Glossing focuses on improving the trace geometry, where Retrace assumes the overall geometry is satisfactory, focusing instead on satisfying the design rules.
• Glossing preserves the existing trace width and differential pair gap, while Retrace changes them to Preferred.
• Glossing runs whenever ActiveRoute finishes, if the Gloss Results option is enabled in the PCB ActiveRoute panel.
• Glossing also runs during interactive routing, on all track segments that are yet to be committed (all segments placed since the Interactive Routing command was launched and you started routing a net).

Glossing - Improving the Quality of the Routing

The PCB editor includes powerful tools for improving the quality of existing routing. Whenever you move the cursor to define a new route path, all of the proposed routing is automatically glossed. Glossing will attempt to reduce the path length, and also improve the shape of corners and reduce their number, generally resulting in neater routing created from fewer segments.

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. Along with the current Gloss Effort settings, 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.

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.

Existing routing can also be retraced (Route » Retrace Selected). Retrace assumes the overall geometry is satisfactory, focusing instead on verifying that the routing meets the design rules. Where Gloss preserves the existing trace width and pair gap, Retrace changes them to Preferred. Retrace is an excellent tool to use when a design rule has changed, and that change needs to be applied to existing routing.

Summary of Glossing Behavior

To summarize:

• Flexible approaches to selection can be used, supporting partial glossing of a routed net:
  • To gloss only a section of a routed net you can select a track segment at either end of the section or select a pin or a via to signify the end of the desired section.
• Glossing attempts to repair dangerous pad entries:
  • Gloss does not automatically comply with the SMT rules (SMD Entry & SMD To Corner) if it detects that they are encouraging unnecessary jogs and circuitous routing.
  • If SMT rules rules are present the gloss engine tries to recognize dangerous situations, such as the potential for solder bridging, and adjusts its behavior based on these rules.
  • For this to occur, the Corner option must be disabled in the SMD Entry rule, and the SMD To Corner rule must have a suitable setting.
  • Rule deviations: Gloss will keep the track segment orthogonal with the pad edge being exited from, but will not necessarily keep it centered within that edge. Gloss will also allow the track segment to exit from the side of the pad if the SMD to Corner distance and other applicable rules can be satisfied.
• Glossing differential pairs:
  • When applied to differential pair routes, Gloss attempts to zip-up the pair, reducing the lengths of the unzipped portions. The corresponding unzipped portions from opposite sides are made equal in length, if possible, but Gloss does NOT add meanders to the shorter side of the pair. If length balancing is not achieved naturally, the pair is left unbalanced.
  • Particular attention is applied to differential pair pad entries to improve their quality, but Gloss does not attempt to match the lengths of the entry routes.
  • Where differential pair routes cross a room boundary and change width, Gloss gives preference to synchronous width change of the pair members. This means it does not change the width/gap of both routes right on the boundary, instead it focuses on keeping the pair matched, so when a width change occurs, it happens to both segments at the same time. So if the routing enters the room at an angle, one route in the pair will change width on the room boundary, and the second route in the pair will change width at a location adjacent to the first route. (show image)
• Support for Subnet Jumpers:
  • Gloss treats Subnet Jumper tracks as fixed.
• Support for room-based rules:
  • Gloss adheres to Clearance and Diff Pair Routing rules scoped to rooms.
  • Gloss allows the route to change width as it enters a room; it will attempt to preserve the original widths used both outside and within the room.
  • If there is a width change at a room boundary, Gloss will maintain the width change.
• Exclusions:
  • To exclude routes from glossing or retracing, lock the track segments.
  • Tracks at non-45 degree angle increments are not glossed; it is assumed these have been placed intentionally to satisfy a design requirement.
• Feedback:
  • Command and progress information is displayed on the Status bar.
  • Info and Warning messages are displayed in the Messages panel. Details are in the Information and Warnings section below.

Options that Control Glossing Behavior during Interactive Routing

Gloss Effort (Routed)

How strongly a route is glossed is controlled by the current Gloss Effort (Routed) setting. Configure the option in the Interactive Routing page of the Preferences dialog, or use the Ctrl+Shift+G shortcuts to cycle through the three modes. The current setting is displayed on the Status bar. (show image)

• 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 a strong emphasis on the shortest path. This mode of glossing is typically useful in the early stages of the layout process when the aim is to get a large portion of the board routed quickly.

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 glossing. Glossing applies to all track segments that are impacted by the current editing action, so can also affect surrounding tracks. For example, during interactive routing or interactive sliding in push mode both the tracks being slid and the tracks being pushed will be glossed, according to the current Hugging Style setting.

• 45 Degree - always use straight orthogonal/diagonal segments to create corners (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 being glossed. Use this mode for snake routing, and to use arcs + any angle routes when glossing (during interactive routing and manual glossing).

Minimum Arc Ratio

The Minimum 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

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 below. Enter a positive value equal to or greater than zero.

Pad Entry Stability

The Pad Entry Stability slider protects centered pad entries. It applies during glossing to protect an already-centered pad entry (exit), it does not attempt to re-center an existing off-center pad entry.

• 0 (Off) = no protection
• 10 (Max) = maximum protection

Demonstration of the Pad Entry Stability feature.

Performing a Gloss

The glossing tool is run:

• On selected routing - by choosing the Route » Gloss Selected command from the menus or pressing the Ctrl+Alt+G keyboard shortcuts.
• After ActiveRoute - by enabling the Gloss Results option in the PCB ActiveRoute panel.
• During Interactive Routing - in accordance with the current gloss settings, defined in 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 Preferences dialog or the Interactive Sliding mode of the Properties panel.

Retrace - Modifying the Properties of Existing Routing

A common task facing the board designer is needing to modify the properties of the existing routing. Perhaps you need to change the routing width because of a change in the design specifications, or perhaps the layer stackup had to be modified, so the impedance-controlled routing widths and gaps need to be changed to suit the updated impedance requirements.

The interactive routing engine includes a feature specifically developed to help with this challenge, called Retrace. The Retrace feature assumes the overall geometry of the routing is satisfactory, focusing instead on checking and updating the routing to the current design rule settings. With Retrace, you can "fatten up" that existing power routing, or update that differential pair to new width and gap settings.

Retrace works exactly as its name implies, running along the selected routes, updating them to the current rule specifications. Because it does this on an individual net or pair level, it will attempt to maintain clearances, but is not able to push surrounding routes if more room is required. In this situation, the rule updates are applied only to those route segments that do not create a violation.

Select the required net(s) and run the Retrace Selected command from the Route menu.

An example of Retrace being used to change the routing corners to curved with arcs.

Notes about Retracing:

• Retrace obeys the Preferred setting in the applicable Routing Width or Differential Pairs Routing rule.
• Retrace is applied to the currently selected tracks/arcs. An easy way to select the routing is to select a single segment in the net, then press Tab to select all touching track segments on that layer. If the routing traverses multiple layers, press Tab a second time to select the routing on the other layers.
• The Retrace command follows the existing route path, focusing on rule compliance rather than the shortest path or least number of corners.
• Retrace will not place a track/arc segment that creates a violation. If a track/arc of the preferred width will not fit, the largest width that does not create a violation is used.
• Retrace does not change vias to suit changes in the Routing Via Style design rule.
• Retrace obeys the current settings configured in the PCB Editor - Gloss And Retrace of the Preferences dialog or in the Gloss And Retrace panel. See the Options that Control Glossing and Rerouting Behavior on Selected Routing section to learn more.

Summary of Retrace Behavior

To summarize:

• Retrace is similar to Gloss (and uses the same engine internally). The differences are:
  • Gloss preserves the width; Retrace changes it to the Preferred value.
  • Gloss produces the shortest possible result, often radically deviating from the original; Retrace approximately follows the original.
• Use the same selection principles as Gloss to select the routes to be Retraced.
• Use Retrace to update the selection and apply the applicable preferred Width rule.
• Modifies selected routes as needed to avoid poor quality corners and pad entries while preserving the general route geometry.
• Use Retrace to update the diff pair gap:
  • Will update the zipped portion of the pair (where the sides are at Max Gap or less from each other), changing the gap to Preferred.
  • To reduce the gap in a routed pair, change the Diff Pair Routing rule so that the Preferred Gap is the desired gap, and the Max Gap is the old Preferred Gap value, then run Retrace. Caveat: Retrace does not handle an unreasonably large Max Gap.
  • Retrace can also be used to increase the gap in a routed pair; set the Preferred Gap in the Diff Pair Routing rule to the required value.
  • Note: if the new Preferred settings are larger than the current width/gap, Retrace may fail to reach its goal without creating violations. In such cases it will use smaller values to avoid creating violations. No pushing of obstructions is performed.
• Exclusions:
  • Retrace requires both ends of the selected routing to connect to a pad or via, it does not work on dangling routes.
• Feedback:
  • Command and progress information is displayed on the Status bar.
  • Info and Warning messages are displayed in the Messages panel. Details are in the Information and Warnings section below.

Performing a Retrace

The retrace tool can be accessed in the PCB Editor by choosing the Route » Retrace Selected command from the main menus.

Options that Control Glossing and Retracing Behavior on Selected Routing

The PCB Editor – Gloss And Retrace page of the Preferences dialog and the Gloss And Retrace panel provide numerous controls relating to the functionality of the Gloss Selected and Retrace Selected features within the PCB design space.

 

Gloss & Retrace Parameters

• Hugging Style – controls how corner shapes are to be managed during glossing or retracing.
  • 45 Degree – always use straight orthogonal/diagonal segments to create corners during glossing or retracing (use this mode for traditional orthogonal/diagonal routing behavior).
  • Rounded – use arcs at each vertex involved in the glossing or retracing. Use this mode to use arcs + any angle routes when glossing.
• Avoid polygons – when this option is enabled, existing polygons will be respected when the Gloss Selected or Retrace Selected command is run. If the option is disabled existing polygons will be ignored (routed across), affected polygons can then be repoured.
• Avoid rooms – when this option is enabled, existing rooms will be respected when the Gloss Selected or Retrace Selected command is run. If a room scoped by specific routing width requirements is defined in the design and the routing to be glossed/retraced does not cross the room, the resulting routing will not cross this room either when the option is enabled. If the option is disabled, existing rooms will be routed across, and the width to be used within such rooms will be that is defined in constraints of the room-based rule.
• Pad Entry Stability – protects centered pad entries. Enter the desired level (the preferences) or use the slider bar (the panel) to configure the level of protection. '0'/'Off' gives no protection; '10'/'Max' gives maximum protection. This option is only applicable/available when the 45 Degree option is selected for Hugging Style.
• 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.

Gloss Parameters

• Effort – select the desired gloss level from the following choices:
  • Weak – in this mode, a low level of glossing is applied. 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 a strong emphasis on the shortest path. 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.

Retrace Parameters

These controls are applicable/available when the 45 Degree option is selected for Hugging Style.

• Set Width – use the drop-down to select one of the rule-based width options (Min / Max / Preferred) of an applicable Width or Differential Pairs Routing design rule when the Retrace Selected command is run, or select the Current width of tracks to be retraced. Alternatively, enter a desired custom width value directly in the field.
• Set Diff Pair Gap – use the drop-down to select one of the rule-based gap options (Min / Max / Preferred) of an applicable Differential Pairs Routing design rule when the Retrace Selected command is run, or select the Current gap between differential pair tracks to be retraced. Alternatively, enter a desired custom gap value directly in the field.

Information and Warning Messages

Info	Reason
Skipped immovable + <Descriptor>	An object is protected from Gloss/Retrace: for example, locked or belonging to a component. Max count 20, clickable.
Skipped subnet jumper + <Descriptor>	Subnet jumpers are left alone, user informed in each case. Max count 20, clickable.
Skipped reflex angle + <Descriptor>	Arcs greater than 180 degrees are not glossed. Max count 20, clickable.
Skipped objects in user-defined Union	Objects belonging to a union are not glossed (does not apply to Length Tuning unions). Issued once per union involved. Max count 20, clickable, zooming to the Union bounding rectangle.
Command does not apply to arcs (Retrace only)	Retrace does not support arcs. Max count 1, clickable, zoom to the first arc encountered.

Warning	Reason
Applicable Diff Pair Routing rule not found for some object(s) + <Descriptor>	Some of the Gloss / Retrace targets belong to a diff pair net, but there is no applicable Diff Pair Routing rule. In such cases, the command treats the target as a non-diff pair object, meaning the two sides of the pair may be Glossed away from each other. Max count 1, clickable.
Applicable Width rule not found for some object(s) + <Descriptor>	Retrace uses Min to Preferred Width rule settings. If there is no applicable Width rule found, the current width is preserved. Max count 1, clickable.
Pre-existing Min Width violation(s) detected + <Descriptor>	Retrace uses Min to Preferred Width rule settings, using preferred if it causes no DRC violations, or smaller if needed to avoid DRC violations. Thus, a DRC-free track will stay DRC-free if it was at least at Min Width to begin with. If it was narrower, setting it to Min width may result in a DRC violation. This message warns of such occurrences, whether or not it resulted in an actual DRC violation. Note that the original thin object will have been widened and possibly moved by the time you have a chance to click on the message. You may need to Undo to understand what has happened. Max count 1, clickable.

See Also

• Routing the PCB (parent article)
• Interactive Routing
• ActiveRoute
• Topological Autorouting
• Differential Pair Routing
• Controlled Impedance Routing
• Length Tuning