Routing is the process of defining a connective path between the nodes in each net, 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 interactive routing command, you click on a pad to select a connection to be routed. As you move the cursor away from the pad, the interactive router attempts to define a route path from that pad, all the way to the current cursor location. The path that the router defines is controlled by various properties, including the current corner style and the gloss settings.
The properties of the tracks/arc being placed are controlled by the Routing Width design rule, and the clearance from other net objects by the electrical Clearance design rule.
How the interactive router responds to objects that already exist on the board, such as component 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 Hug the object and Push it if required, or Push it, or Stop , or Ignore it.
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 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
Building routing proficiency requires a good understanding of how the objects are located in the PCB design space , the following section gives an overview of this. It is also important to understand how to control the display of the routes , to easily see what you are working on within the densely packed design space, there is an overview of this in the second section. The third skill that builds your routing proficiency is to learn how to control the properties of the tracks and vias as you route .
If you have these skills and have come to this page to learn more about the process of routing, then jump down to the working with the interactive router section.
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
There are two core aspects to the cursor-snap system, what the cursor snaps to, and when it will snap.
What - the points in space that the cursor snaps to include: user-defined Grids , work Guides, and snap points on the existing Objects .
When - the cursor snaps to a snap point: it snaps when it is within the Snap Distance , and snapping is allowed on that Layer .
Demonstration of the cursor-snap features: configure the options in the Properties panel, or by pressing Ctrl+E .
What you snap to
Snap to grids Grids are available in both Cartesian and Polar formats ( Multiple grids can be defined within the same area, with the highest priority grid (lowest numerical value) being applied ( Grids can also be configured to target: all objects, just component objects, or not component objects, use this to define a higher priority component placement grid ( Learn more about grids .
Snap to objects Placed objects will pull the cursor into position when it moves within the Snap Distance , based on cursor proximity to that object's snap points (hotspots). Use this to pull the cursor to the center of a track or an off-grid pad, for example. Object snapping can be applied on: all layers, only the current layer, or disabled. Use the Shift+E (
Snap to guides Horizontal, vertical, diagonal, and point guides can be placed and used for object alignment, as shown in the video above. Learn more about guides .
Snap to object axes A feature that pulls the cursor, in either the X or Y direction, so that it axially aligns with a hotspot on a placed object that is within the Axis Snap Range (
Controlling the snapping
Before you start – configure the snap options in the Properties panel ( (with nothing selected in the design space).
During routing – Press Ctrl+E Esc
Inhibit snapping – all snapping is temporarily inhibited by holding down the Ctrl
Snapping to the Grid
Snapping to Objects
Snap to objects The cursor snaps to: enabled Objects for snapping (1), that are on the enabled Snapping layers (2), when the cursor is within the Snap Distance (3)(
When to snap Object snapping has three states, Off, Current Layer, or All Layers. Press Shift+E Snapping buttons in the Properties panel. The current snapping state is displayed on the Status bar (
Snapping to Guides and Axes
The printed circuit board design is often very dense and crowded with objects. There are a number of features in the software to help manage object visibility, including: layer visibility, masking and dimming, object visibility and transparency, along with a number of other features.
Use the highlighting, object and layer control features to help interpret the design.
Single layer mode Press Shift+S PCB Editor – Board Insight Display page of the Preferences dialog ( Each press of Shift+S
Layer sets Pre-defined sets of visible layers can be configured and then selected using the Manage Layer Sets button down the bottom left of the editing window ( New sets are defined in the View Configuration panel, this is demonstrated in the video above.
Dim or Mask to fade To quickly highlight an object of interest, such as a component, a net, a differential pair, or any type of class, browse the object in the PCB panel and enable the Dim or Mask mode ( Both of these modes fade all objects except those you are interested in, making the objects of interest stand out. The Dim and Mask levels are configured in the View Configuration panel (
Clearance boundaries Enable this to display the required clearance around electrical objects. ( The clearance is shown as white shading, configured to show the distance specified by the electrical clearance constraint that is applicable to the object being routed (or slid). You use the Ctrl+W Ctrl+W
More about controlling the display of the clearance boundaries .
Object transparency The transparency level of each object type can be configured in the Object Visibility section of the View Configuration panel ( Use the All Objects slider at the top of the set to adjust all objects simultaneously.
The visibility of objects Hiding objects that are not of interest is a convenient way of de-cluttering the design space ( Note that the objects are still tested by the constraint system, to hide polygons from visibility and from the constraint system, Shelve them instead.
Displaying net names Configure the options to control the display of net names on pads, vias and tracks In the View Configuration panel ( Note that net names are always shown at the center of each track segment, but can be repeated if required. The display font properties are configured in the PCB Editor – Board Insight Display page of the Preferences dialog (
You have configured the clearance , routing width and routing via style design constraints – you are ready to route. When you click to start routing, how does the router know what track width to use, and what via size to use when you switch layers?
Simple demonstration of setting up to route, then selecting the routing width and via style during routing.
Starting a Route
Launch the interactive router... Use any of these techniques to start interactive routing:
Select the Route » Interactive Routing command from the menus.
Click on the Interactive Routing button on the Active Bar (
Press the Shift+W
A crosshair will appear on the cursor; you are ready to start routing.
...then click on a connection line If you click on a connection line after launching the Interactive Routing command, the Interactive Router will jump to the object at the nearest end of the connection line and add track segments from the click location up to the current cursor location. It will also switch to the layer that the object is on if it not the current layer.
Press the 9
Press the 7
...or click on an object If you click on an object that belongs to a net the Interactive Router will switch to the layer the object is on and add track segments from the click location to the current cursor location.
...or click in free space If you click in free space, you start routing, except this time it will be a no-net route. As a no-net route it will use the PCB editor default track width.
The initial style of the route The starting width of the route is described in the collapsible section just below. How the interactive router forms a corner as you move the cursor around is referred to as the corner style . Diagonal corners are the most common, but curved corners (created by placing arcs), are also popular.
More about corner style settings .
It is also possible to manually edit the values during routing. Press Tab Properties panel ( , and edit the:
routing layer,
routing via diameter and hole size,
routing width (between the min and max settings defined in the Width constraint either select or type in a value).
Changing the Routing Width (0:29)
Starting width The starting width is determined by the setting of the Track Width Mode in the Interactive Routing Width Sources options (
More about default track width mode settings .
Min & max widths The minimum and maximum width of the route are defined by the Min Width and Max Width settings in the applicable routing Width constraint ( The PCB editor will attempt to keep the width within this range.
Press the 3Shift+W Choose Width dialog ( The last state is retained as the current Track Width Mode . The current track width mode is displayed on the Status bar and in the heads-up display (
More about the favorite width settings .
Routing defaults Configure the default interactive routing settings in the PCB Editor – Interactive Routing page of the Preferences dialog ( Alternatively, press Tab Interactive Routing panel ( , or as you move an existing routing in the Interactive Sliding panel (
More about the interactive routing options .
Changing the Routing Layer (1:14)
Default layer Routing defaults to the currently active signal layer. Before launching the interactive routing command, click the required layer tab at the bottom of the design space to start routing on that layer ( If you click to start routing on an object on another layer, that layer automatically becomes the active signal layer.
Press Ctrl+Shift+Wheelroll
Press Ctrl+L (
On the numeric keypad, step through the signal layers with the +-*1 9
Click on a connection line If you launch the Interactive Routing command and click on a connection line (or an existing route object), the Interactive Routing will jump to the nearest end of the connection line and switch to the layer that the object is on. Press the 9 7
Changing the Via (1:22)
Routing via If you switch layers during routing, a via is automatically added, in accordance with the applicable Routing Via Style design constraint.
Default routing via The size of the via that is used during a layer change is determined by the setting of the Via Size Mode in the Interactive Routing Width Sources options ( This can be changed as you route, as described below.
Cycle available via sizes Press 4Via Size Mode . The current via size mode is displayed on the Status bar and in the heads-up display (
Alternatively, press Shift+V Choose Via Size dialog ( Only a via whose size is between the Minimum and Maximum size defined by the applicable Routing Via Style design constraint can be chosen.
Cycle the via span The layers that a via spans is determined by the current Via Type , with the available via types being defined in the Layer Stack Manager ( When there is a via floating on the cursor during routing, press the 6 ( Alternatively, press the 8 ( Note that suitable vias can include a stack of multiple vias, if suitable via types can be stacked to achieve the current layer change. The current via type is displayed on the Status bar and in the heads-up display (
Learn more about vias .
Learn more about defining the via types .
Each click of the mouse places (commits) all of the hatched track segments from their start location, up to the cursor. Press Backspace
How does the route leave an SMD pad? How does the routing react when an obstacle is encountered, does it walk around that obstacle, push it, or ignore it? What shape does the corner take, and how does it pass between the pads on other components? Where the previous section outlined how to control the properties of the route itself, this section summarizes the features you have to control the route as it moves through the routing space.
Working with the Interactive Router
Hatched/solid/hollow track/arc segments Hatched tracks/arcs are unplaced, solid track/arcs are placed ( Note that for the connection currently being routed, solid track/arcs are classified as soft-commits , meaning the routing engine recognizes that they are placed but retains the ability to gloss them and to remove them if you move the cursor to a location where they are no longer appropriate (demonstrated in the video at the start of this page).
When the track attached to the cursor is hollow (not hatched or solid), it is referred to as the look-ahead segment , it will not be placed when you next click. Use this feature to position the end point of the previous segment, without committing to placing the last segment ( Press the 1
How the router forms the corners 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 (
Press the Spacebar to toggle the corner direction.
Alternatively, press Tab to open the Properties panel and change the corner style there (
How the routing leaves a pad How the interactive routing engine exits or enters a pad is controlled by:
SMD Pad Entry constraint – defines which edges of the pad that the routing can exit or enter (
SMD to Corner constraint – defines the route exit distance from the edge of the pad to the first allowed corner vertex (
Pad Entry Stability setting – defines how hard the interactive routing engine should attempt to hold the track to the center of the pad edge during exit (
More about pad entries .
How the route reacts to an existing object This is determined by the current setting of the Conflict Resolution Mode. The current conflict resolution mode is displayed on the Status bar ( , in the heads-up display ( , and on the Properties panel during routing or sliding.
More about the conflict resolution mode .
The smoothness of the new routing As you move the cursor away from the initial click location the routing re-shapes to find the best path around objects, to reach the current cursor location. The neatness, or quality of that path is determined by the current glossing setting . Glossing is a suite of tools that improve the quality of the routing, attempting to reduce the path length, improve the shape of corners, and reduce their number. It also attempts to avoid right-angles, and prevent acute angles at T-junctions and pads. Glossing also supports differential pairs and will attempt to improve the amount of pair that is balanced in length and separation.Glossing has three settings; Off, Weak and Strong. During interactive routing or interactive sliding use the Ctrl+Shift+G Tab Properties panel and select the required setting.
More about glossing during routing .
Auto-complete the connection As you interactively route a net, hold Ctrl Left Click auto-complete the current connection. To be able to auto-complete:
If a connection cannot be auto-completed, the tool will return to the last used interactive routing mode.
Center the routes between pads / vias The interactive router obeys the design constraints, automatically routing through a pair of pads at the minimum allowed clearance from the nearest pad. If you prefer the routes to be moved away so that it is spaced between the pads then configure the Apply Trace Centering option . To support the ability to achieve this between any pair of pads, or vias, or pad/via pair, the feature uses a clearance multiplier that it can intelligently adjust the routing clearance up to.
More about centering the routes between pads .
Auto-narrow the route Necking the route to fit through a narrow gap is sometimes the only way to route that net. The Auto Shrinking feature can achieve this, automatically narrowing the route down to just fit through the gap, with the allowed minimum being defined by the routing width constraint.
More about the auto shrink feature .
Route selection strategies Selecting the routes to be worked on is a key aspect of routing. It could be selecting routes to un-route them, to gloss them, to check their properties, or delete them.
More about strategies for selecting the routing .
Responding to Obstacles – Conflict Resolution Mode
You launch the interactive routing command and click on a pad. As you move the cursor away from the pad the interactive routing engine lays a path of hatched track segments from the pad you clicked on up to the current cursor location, and as you move the cursor around it updates the hatched segments to best define the route path, in accordance with the design constraints and the current glossing settings.
How the interactive router responds to objects already in the PCB workspace, such as pads or routing on other nets, depends on the current routing conflict resolution mode. The routing conflict resolution mode determines if the interactive routing engine will attempt to push those obstacles, or walk around them, or simply ignore them and route over the top of them.
Simple demonstration of the different behaviors of the conflict resolution modes.
Routing Conflict Resolution Mode
Current mode The current routing conflict resolution mode is displayed in the heads-up display ( and on the status bar ( It is also displayed in the Properties panel during interactive routing ( , interactive sliding ( , and interactive via dragging (
Changing modes To change modes during interactive routing (or interactive sliding or via dragging), press the Shift+R
Available modes Individual conflict resolution modes can be enabled / disabled in the PCB Editor – Interactive Routing page of the Preferences dialog ( If a mode is disabled in the preferences, it will not be available in the dropdown list in the Preferences panel or when the Shift+R
More about each of the conflict resolution modes .
Glossing during Routing
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 while defining a new interactive route path, all of the yet-to-be committed routing is also automatically glossed.
As well as applying glossing to the net being routed, the interactive routing engine can also gloss the adjacent (neighbor) nets that are being impacted by the net under route.
Simple demonstration of the different results achieved with glossing off and glossing on.
Understanding Glossing
When does glossing run The glossing tool runs:
How strong is glossing How strongly a route is glossed is controlled by the current Gloss Effort (Routed) setting. Configure the option ( Ctrl+Shift+G shortcuts to cycle through the three gloss strengths. The current setting is displayed on the Status bar (
Off – 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 – 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 – 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 (routed) settings
Glossing the neighbors During Push or Hug & Push interactive routing or sliding, the adjacent routes, or neighbors, will be impacted. These neighbors can also be glossed, based on the Gloss Effort (neighbor) setting (Gloss effort (neighbor) settings
How the glossing engine wraps the route around other objects and forms the corners is referred to as hugging . The available Hugging Style settings include:
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).
Hugging style settings
Controlling the properties of the corner If corners are being formed with straight track segments, the default behavior is for the glossing engine to apply a small miter to a 90 degree corner, with the size controlled by the Miter Ratio setting. Miter ratio settings
If corners are being formed with arcs, the minimum arc size is controlled by the 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. Minimum arc ratio settings
Inhibit glossing during routing and sliding There may be times when you want to temporarily turn off glossing. Glossing can be inhibited during routing 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.
More about the interactive routing options .
The slides below show simple examples of the different Gloss Effort (Routed) and Gloss Effort (Neighbor) settings.
Miter or Curve the Corners
Corners can be defined using short, straight track segments (miters), 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 .
The most common routing corner shape is 45 degree mitered (diagonal) corners. Switch to the Track 45 corner mode to route diagonal corners. Complimenting this, the interactive routing engine also includes a miter ratio feature that ensures that tight corners retain a miter, making it impossible to inadvertently create right angle or acute corners during routing.
The Miter Ratio is defined as:
Miter Ratio x current track width = separation between the walls of the tightest U-shape that can be routed for that miter ratio
The miter ratio controls the minimum sized miter that is automatically added to the corner.
Both interactive routing and interactive sliding include a Miter Ratio option. Enter a positive value equal to or greater than zero. Examples of the same trace routed with different values of the Miter Ratio option are shown below.
The Miter Ratio value defined in the Properties panel is used during interactive routing, interactive sliding, glossing and retracing.
Press Tab Miter Ratio value during interactive routing ( or sliding ( , or configure the value in the Preferences dialog (
If you are running the Gloss Selected or Retrace Selected commands from the Route menu, the Miter Ratio value used for these commands is configured in the PCB Editor – Gloss and Retrace page of the Preferences dialog ( or the Gloss and Retrace panel (
When the Miter Ratio is set to zero, the inside edge of the corner created by the two track segments forms a right-angle, but there is still a short diagonal segment in the corner that creates a chamfer on the outside edge of the corner ( To intentionally create a right- or acute-angle corner with tracks being routed or dragged, enable the PCB.ZeroMitersRemoving option in the Advanced Settings dialog (feature currently in Open Beta), and set the Miter Ratio = 0. In this case, a miter is not created, giving true zero mitering (
Many designers require curved corners. Curved corners can be placed as you route – 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 Shift
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 , the Gloss Effort to Weak , and then running the Gloss Selected command, with the routing selected.
To curve the corners of existing routing, set the Hugging Style to Rounded, Gloss Effort to Weak, and then select the routing and run the Route » Gloss Selected command.
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 – the corner style is set to Any Angle.
Routing Pad Entries
The interactive routing engine leaves and enters surface mount pads according to the applicable SMD pad entry design constraints. As you route or (slide the route), the exit / entry is constantly being glossed, according to the current gloss strength setting. 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. The glossing engine also includes the Pad Entry Stability feature, which enables the designer to instruct the glossing engine to favor the pad centerline.
The SMT Design Constraints control how the interactive router exits and enters surface mount pads, these should be configured before starting the routing process. Open the PCB Rules and Constraints Editor dialog (click Design » Rules from the main menus) to create and configure these design rules.
SMD to Corner This constraint defines the distance from the edge of the pad to the center of the vertex where the first corner is located. The value should be greater than the width of the track or the applicable clearance rule (whichever is greater). If it must be less than that, there are three ways you can approach this:
Press the Spacebar while performing the pad entry. This can help align the last track segment along the pad center.
Commit the routing close to the pad then perform the pad entry without glossing (glossing can be temporary disabled by holding down Ctrl+Shift ).
If performing the pad entry with more than one possible entry, move the mouse inside the pad. That allows you to choose where you want your SMD entry.
SMD Entry The constraint defines where the route is allowed to enter the pad. For this constraint, the Side of the pad is the longer edge.
Note that the Side option in the design rule is only applied when the pad SideLength > 2 * EndLength. This is done because most SMD discretes have almost-square pads, and for these devices it is often desirable to route into any edge of the pad.
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
Use the Pad Entry Stability feature to help keep the route in the center of the pad.
Notes:
Pad entry stability works independently of the SMD to Corner and SMD Entry constraints, so will still function when they have not been applied.
Depending on the sizes of the objects, maximum protection can result in an acute angle at the pad edge.
Center Routes Between Pads
The Apply Trace Centering option does this. To allow the centering algorithm to be flexible and to be applied between any two pads, any two vias, or any pad and any via, the desired centering distance is specified as a multiple of the applicable clearance constraint, where:
Distance = Clearance + Added Clearance Ratio x Clearance
The interactive routing engine will attempt to route around the target pad/via at this Distance, automatically reducing (and centering) it when the distance from the other edge of the trace to the nearest pad or via becomes less than Distance.
Where possible, adds an additional clearance between the net being routed or dragged and existing pads/vias.
Pad Entry Stability
Apply trace centering When the Apply Trace Centering option is enabled, trace centering is applied during interactive routing and interactive sliding. When the routing engine detects that a route is passing between pads / vias it attempts to center the route, up to a maximum distance of the applicable clearance constraint plus the applicable clearance constraint multiplied by the Added Clearance Ratio. Use the Disable Trace Centering When Dragging option to disable centering during interactive sliding.
Center between what? The trace centering feature does not require the pads to belong to the same component, it is able to center between any two pads, any two vias, or any pad and any via. Use the Adjust Vias option to enable/disable centering between via-via or via-pad combinations.
Where is the center? Rather than attempting to identify the center between the relevant pads/vias, the feature uses 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.
This feature is available when the PCB.EnableTraceCentering option is enabled in the Advanced Settings dialog (feature currently in Open Beta).
Auto-Shrinking during Routing
Auto Shrinking feature .
This feature is available when the PCB.Routing.EnableAutoShrinking option is enabled in the Advanced Settings dialog (feature currently in Open Beta).
BGA components use an array of small, closely located pads. This makes them challenging to route, often requiring the routing width to be reduced to route to the inner rows of pads. This can be achieved manually during interactive routing using the techniques described on this page. You can also automate this width-switching behavior by adding a placement room and a room-based routing width constraint. Because the interactive router obeys these constraints, tracks will automatically neck and expand as the room is entered or exited.
The routing width and clearances are automatically adjusted within the room.
Shrink the Routing within an Area
Define the area The area where the routes need to be reduced in width is identified by defining a placement room constraint ( Learn more about working with rooms .
A Placement Room Definition constraint is normally scoped to target one or more components. In this situation where it is ultimately being used to control the routing within the area defined by the room, you do not actually have to scope it to target specific components. For example, the scope of the rule (Full Query ) could be set to All and the routing would still behave as required. The advantage of scoping it to target the component(s) within the room is that if the component(s) needs to be moved, the Design » Rooms » Move Room command can be used to move the room and the components together.
Define the width The routing width is defined by the applicable Routing Width Constraint ( Target the routes outside of the room with a lower priority constraint. The routing width within the room is reduced by adding another higher-priority Routing Width Constraint that specifies that routing that touches the room have a narrower width, using the TouchesRoom scope . The interactive routing engine will automatically terminate the current track segment and start a new segment at the room boundary to satisfy a constraint such as this. This technique can be used for both single-sided nets and differential pairs.
Learn more about defining constraints within a room .
Follow mode – Tracing an Existing Shape
A challenging requirement is to place a route so that it follows an existing shape or contour. The contour could be an obstacle, a cutout or the board edge, or an existing route.
Rather than having to route against the contour using careful and accurate mouse movements and click actions to ensure the new route hugs the contour, in Follow mode, you click to nominate the contour that you want to follow, then move the cursor to define the route direction. The interactive router will add track and arc segments so that the new route follows the contour in compliance with applicable design rules. This feature is particularly useful when placing curved routes.
Use Follow mode to exactly route along an existing shape.
Route to Follow a Contour
First step Launch the Interactive Routing command and click on the net to be routed, in the usual way.
Enable Follow mode With the route started, press Shift+F next object detected under the cursor will be followed. Move the cursor to define the direction that the new route should follow the contour, but do not click as the follow route is formed along the way.
In the video above the board cutout is followed for the first route, then the previous route is followed for each of the other routes.
To place the follow route The next left-click of the mouse is interpreted as the termination point for the follow route, after clicking you revert back to regular interactive routing.
To abort Follow mode Press Backspace Esc
Differential pairs Follow mode also supports differential pairs (
For a complex shape, Follow mode creates the route out of many track and arc segments. If you need to remove some of the follow routing, rather than carefully selecting and deleting tracks and arcs to remove a section, click once on the last segment to select it and then press Backspace Backspace
Intentionally shorting different nets
It is not uncommon to need to intentionally connect two different nets. An example could be when you need to connect an Analog ground and a Digital ground in a controlled way. This is achieved by connecting the two nets through a Net Tie component. A Net Tie component is nothing more than a controlled short circuit, allowing you to decide the location on the board where the nets connect.
The challenge with routing towards a Net Tie pad is the rules engine will see that a violation is about to occur and prevent you from routing to the Net Tie pad. This will not occur if you start routing from the Net Tie pad. Alternatively, you can temporarily switch the Routing Mode to Ignore Obstacle.
To route a Net Tie, route out from from the Net Tie pads.
Learn more about Intentionally Connecting Two Nets .
Fanout and Escape Routes
Altium Designer includes surface mount component fanout tools, which also support BGA escape routing. The escape routing engine attempts to route each pad out to just beyond the edge of the device - making routing connections to them much easier. Fanout is designed to be run prior to interactive or auto-routing, and will only attempt to fanout unrouted components.
Fanout and escape routing is launched from the Route » Fanout sub-menu of the main menus or using the Component Actions » Fanout Component command from the component's right-click menu.
Fanout Options dialog opens. The dialog includes controls that let you specify fanout and escape routing options, as well as options for using blind vias. The blind via option is only available if there suitable blind Via Types defined in the Via Types tab of the Layer Stack Manager .
A fanned out BGA, the pads are shown solid and the fanout tracks and vias semi-transparent. The fanout is based on the settings in the dialog, in accordance with the Fanout Control constraint.
Fanout Options (
Fanout Pads Without Nets Enable this option to fanout pads from the component even if they have no nets assigned to them. When this option is disabled, only pads with nets assigned will be fanned out.
Fanout Outer 2 Rows of Pads Enable this option to also fanout pads from the outer two rows (which are usually easily routed).
Fanning out a component will drop vias as required to enable connection. If drill-pairs have been configured for layers and the Update fanout using Blind Vias option is enabled, blind vias will be dropped, otherwise, through-hole vias will be used.
Include escape routes after fanout completion Enable this option to add escape routing to each fanout. Escape routing places tracks onto the fanout vias and component pads, bringing them out to the edges of the component.
Update fanout using Blind Vias (BGA escape routing only) Enable this option to drop blind vias between configured drill-pair layers in the layer stack. When this option is disabled, only through-hole vias will be dropped regardless of drill-pair layer settings. If there are no drill layer pairs defined to be able to use blind vias, this option will appear as Cannot Fanout using Blind Vias (no layer pairs defined) .
If there are no drill layer pairs defined to be able to use blind vias, this option will appear as Cannot Fanout using Blind Vias (no layer pairs defined) .
Escape differential pair pads first if possible (same layer, same side) Enable this option to fanout and escape route any assigned differential pair nets together, before performing other fan out operations, effectively keeping their routes together. The fanout will place escape routing tracks on to the same layer and as adjacent as possible.
Used inner pads are fanned out first using the traditional dog-bone (a short route with a via on the end) to access another layer, and then from the via they are escape-routed out just beyond the edge of the device, working through the available routing layers until all pads have been escape routed. A report of all pads that could not be escape routed is generated and opened, click on an entry in the report to cross probe to the PCB and examine that object.
Example of fanout and escape routes for a 1mm pitch BGA.
Performing a Fanout
Running a fanout Select the required fanout command from the Route » Fanout submenu. Regardless of which menu command is chosen, the Fanout Options dialog will open. When it has been configured and you click OK, the chosen fanout will be performed.
What controls the fanout process? As well as the settings in the Fanout Options dialog, fanout and escape routing is done in accordance with the applicable design constraints, including the Fanout Control , Routing Width , Routing Via Style (for fanout vias), Routing Layers , and the Electrical Clearance constraints.
Why does nothing happen when I run a fanout command? This could be due to:
The component is already routed, or partially routed. A fanout can only be performed on an unrouted surface mount component.
The design constraints (mentioned above) do not allow the tracks / vias to be placed. Test this by attempting to manually interactively route from one of the pads, switching layers to drop a via. If it cannot be done manually, then it cannot be done by any of the fanout commands.
There is a Fanout Control design constraint that targets the device that does not permit the fanouts to be placed. First confirm that the design constraint you have configured to target the device, does in fact target that device. This can be done by copying the query from the Object Match field of the constraint, such as IsBGA, into the PCB Filter panel, and applying it to see that it targets the device correctly. If it does, then confirm that the constraint settings are configured appropriately. For example, if the Fanout Direction option is set to Disable , no fanouts can be placed.
Why do some of the fanouts show violations as soon as they have been placed?
If the Fanout Pads Without Nets option is enabled, each track that touches a no-net pad will fail the Short-Circuit constraint.
The fanout algorithms do not respect width changes at the boundary of a room, so escape routes that extend beyond the edge of the room will be routed at the width required within the room, showing a violation of the Width constraint because the route extends beyond the edge of the room. This can be resolved by selecting the fanouts (Edit » Select » Component Connections ) and running the Route » Retrace Selected command. More about the retrace command .
All of the fanout commands are available in the Route » Fanout submenu. You can also fanout the component currently under the cursor, right-click on a component and select Fanout Component from the context menu.
Fanout Commands (
Fanout » All Fanout the pads of all surface mount components in the current design that connect to both signal and power plane nets. This procedure can be particularly useful in determining whether a design - especially a complex, high-density design - is likely to be successfully routed when passed to the Autorouter.
Fanout » Power Plane Nets Fanout the pads of all surface mount components in the current design that connect to power plane nets.
Fanout » Signal Nets Fanout the pads of all surface mount components in the current design that connect to signal nets.
Fanout » Net Fanout all SMT component pads connected to a chosen net.
If you do not know the location of a pad on the net, or one of its connection lines, click in free space and the Net Name dialog will pop up, prompting for the net name. If you are unsure of the net name, type ? then click OK to launch the Nets Loaded dialog, which lists all loaded nets for the design. The SMT component pads for the net you choose in the dialog will be fanned out (where possible) when you click OK .
Fanout » Connection Fanout all SMT component pads in a chosen connection.
Fanout » Component Fanout the pads of the chosen surface mount component that connect to both signal and power plane nets. If a component contains pads that are not connected to any nets, a dialog will appear asking if you wish to fanout these pads as well.
If you do not know the location of a component, click in free space and the Component Designator dialog will pop up, prompting for the component name. If you are unsure of the component name, type ? then click OK to launch the Components Placed dialog, which lists all components for the design. The pads for the SMT component you choose in the dialog will be fanned out (where possible) when you click OK .
Fanout » Selected Components Fanout the pads of the selected surface mount components that connect to both signal and power plane nets. If a component contains pads that are not connected to any nets, a dialog will appear asking if you wish to fanout these pads as well.
Fanout » Pad Fanout the chosen SMT component pad that connects to either a signal or power plane net.
Fanout » Room Fanout the pads of all surface mount components in the chosen room that connect to both signal and power plane nets.
Component Actions » Fanout Component Right-click on a surface mount component in the design space to access the Component Actions menu of the required component (selected or not) is used to fanout the pads of the currently under the cursor, that connect to both signal and power plane nets. If a component contains pads that are not connected to any nets, a dialog will appear asking if you wish to fanout these pads as well.
If you use any of the fanout commands before autorouting the board, there is no need to lock the preroutes unless you have additional manual routing or have modified the fanout routing in some way.
To fanout the pads of a component, make sure that there is no polygon pours under this component on any layer. Polygons can be shelved before creating fanouts and restored afterward.
Interactive Multi-Routing
There are often groups of signals that need to be routed together along the same path on the PCB, such as the Address and Data busses. To help with this, the interactive router includes an interactive multi-routing command. The multi-route process is configured in the multi-routing Properties panel (
Multiple selected nets can be simultaneously multi-routed.
During interactive multi-routing, press Tab to open the Properties panel and configure the settings.
Choose the connections to route Before launching the command, select the source pad of each net to be included in the route. Shift+click to select individual pads, Ctrl+click and drag to draw a selection rectangle and sub-select multiple child pads in a component.
Start multi-routing The Interactive Multi-Routing command is accessed from the Route menu or the Active Bar (
Controlling the track spacing Use the B shortcut to decrease the bus spacing and the (Shift+B ) shortcut to increase it, in increments of the current snap grid. Press C to converge the bus spacing to the minimum allowed by the applicable Routing Width design constraint.
Changing the route properties Use the same shortcuts as for the Interactive Routing to perform other actions, such as cycle through the conflict resolution modes , switch routing layers , change via options , and so on.
More about the interactive routing options .
Layer The layer that the multi-route is being placed on. Use the drop-down to select a different layer, vias will be added automatically. Alternatively, use the layer-change shortcuts .
Via Template If the via is associated with a template the template name is displayed here and can be changed using the dropdown.
Learn more about pad and via templates .
Via Hole Size Displays the via hole size that will be used. The value can be edited directly, within the range allowed by the applicable routing via style design constraint.
More about selecting the via size and via type during routing .
Via Diameter Displays the via diameter that will be used. The value can be edited directly, within the range allowed by the applicable routing via style design constraint.
More about selecting the via size and via type during routing .
Routing width selector Use the slider to set the routing width to the Min/Preferred/Max value defined in the applicable routing width constraint.
Pickup From Existing Routes When this option is enabled and you are routing from an existing track, the existing track width is used (overriding the width chosen in the sliding selector).
Bus Spacing Enter the desired bus spacing or use the Shift+BB
From Rule Click the button (or use the C
More about the interactive routing options .
( Applicable routing and via constraints will be listed under the Rules section of the Properties panel.
More about the applicable design constraints .
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.
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.
Working with Subnet Jumpers
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 ( 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.
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.
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.
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.
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 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 (
Quick Routing Tools
quick routing commands. 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.
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 are the same as the standard Interactive Routing command.
Summary of Capabilities
Includes Capabilities include:
A number of routing modes, such as: stop at first obstacle, walkaround, and push and shove.
Dragging capabilities that maintains track angles and orthogonality.
A loop removal feature that makes re-routing a quick and easy process.
Does not support 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 .
Net Information (
During interactive routing and interactive sliding, the net under edit is detailed in the Net Information section of the Properties panel.
More about the net information .
Quick Routing Properties (
Layer The layer that the route is being placed on. Use the drop-down to select a different layer, vias will be added automatically. Alternatively, use the layer-change shortcuts .
Via If the via is associated with a template the template name is displayed here and can be changed using the dropdown.
Learn more about pad and via templates .
Via Diameter Displays the via diameter that will be used. The value can be edited directly, within the range allowed by the applicable routing via style design constraint.
More about selecting the via size and via type during routing .
Via Hole Size Displays the via hole size that will be used. The value can be edited directly, within the range allowed by the applicable routing via style design constraint.
More about selecting the via size and via type during routing .
Width selector Use the dropdown to set the routing width to the Min/Preferred/Max value defined in the applicable routing width constraint, or type in a new value (between the Min and Max defined in the routing width constraint).
Interactive Routing Options (
Available interactive routing options are listed under the Interactive Routing Options section of the Properties panel.
More about the interactive routing options .
Design Constraints (
Applicable routing and via constraints are listed under the Rules section of the Properties panel.
More about the applicable design constraints .
Routing is an interactive process, requiring the designer to constantly adjust, update, or even remove the existing routing, as they complete the board design.
The simplest way to change the routing is to click, hold, and drag that route to a new location. Sometimes sliding is not the solution, you need to reroute a section instead. The interactive routing engine supports this, using a feature called Loop Removal . This feature monitors the interactive routing process, and if it detects that a new path has been routed in parallel to an existing path, it automatically removes the old redundant segments.
Dragging existing routes is called Interactive Sliding , with the controls for this displaying in the Properties panel during sliding ( During sliding, the interactive routing engine will attempt to maintain the quality of the routing, while complying with the applicable design constraints. Key features that control the sliding process include: the routing conflict resolution mode (response to obstacles), the gloss strength (effort in tidying the results), and hugging (wrapping around obstacles and forming corners). There are a number of features that support interactive sliding, including T-junction and vertex dragging, via dragging, as well as differential pair dragging support.
There are also features to support dragging routed components.
Strategies for Selecting the Routing
One of the great challenges with interactive software tools is interfacing those tools to the designer's fingertips so they can easily and fluidly move between the various tasks, such as creating, reshaping and cleaning the routing. For this to happen, it must be easy to select the routes of interest.
Perhaps the easiest way to select a route is to click once on any object in the net of interest, and then press the Tab
Demonstration of route selection techniques using the Tab
When you press Tab
The first time – select all connected routing objects on the same layer
The second time – select all connected routing objects on all layers
The third time – select all objects on that net in the design space (skipped if there are no unconnected net objects)
The fourth time – return to the initial selection set
Route Selection Techniques
What can be selected? All of the graphical editors in Altium Designer include a selection filter . The filter defines what object-types are currently available for selection, it can be accessed in the Properties panel ( , and also on the Active Bar ( An object-type must be enabled in the Selection Filter to be able to select it.
Learn more about working with the selection filter and the active bar .
Left Mouse Click Click to select the object under the cursor. If there are multiple objects under the cursor only one will be selected, based on an order of priority . If the mouse is not moved, each subsequent click of the mouse will select the next object in the stack, based on its priority.
Selection rectangle – everything touched Click in free space and drag left, a green selection rectangle is formed ( Any object touched by the green rectangle is selected ( (if allowed by the selection filter).
Selection rectangle – objects within Click in free space and drag right, a blue selection rectangle is formed ( Any object that is completely enclosed by the blue rectangle is selected ( (if allowed by the selection filter).
Select a connection line Alt+Left click and drag left ( All visible connection lines that are touched by the green selection rectangle are selected.
Select existing routes Left click and drag left ( All unlocked track segments that are touched by the green selection rectangle are selected. Use the Tab key to select additional track segments in those nets.
Select routes under a component Shift+Left click and drag left ( All unlocked track segments that are touched by the green selection rectangle are selected. Without Shift , the click and drag can be interpreted as Move Object; if it is the component above the routes will move. The component will also be selected, however when you press Tab to select connected track segments, the component will be deselected. Alternatively, use the selection filter to disable the selection of large objects, such as components and polygons.
Select component pads Ctrl+Left click and drag left ( All unlocked component pads that are touched by the green selection rectangle are selected.
Adding to the selection Hold Shift
Selecting from the PCB panel If you know the object that you want to select but do not know where it is, the PCB panel can be used to locate and select: nets, differential pairs, components and more. Not only can you select from the panel, you can configure it to zoom to the objects and fade (mask or dim) all other objects (
Learn more about the PCB panel .
Accessing all of the selection commands Select the Edit » Select menu to access all of the PCB editor selection commands ( Note that the Select sub-menu can also be accessed directly at any time by pressing the S
For example, press S C Select Physical Connection command. Certain commands also include a direct shortcut, for example use the Ctrl+H Select Connected Copper command without opening any menus.
This section summarizes routing selection techniques, learn more about all of the PCB editor object selection commands .
Cleaning and Clearing the Routes
Delete
Use the Backspace key to remove a segment and then select the last-touching segment.
Unwinding existing routing
Backspace to unwind a route The Backspace Backspace Backspace Backspace
Note that if the selected object has more than one object touching it, the object will be deleted when Backspace Delete
Unwind the route in both directions To unwind the route in both directions, select a track segment then press the Ctrl+Delete Ctrl+Delete
(
Remove all routed tracks/arcs and vias. The connectivity analyzer will detect this and replace them with their logical connections. If any of the routing is locked a confirmation dialog will appear, allowing to exclude or include this routing.
Un-route all physical connections in a specified net. After launching the command, the cursor will change to a crosshair, position the cursor over a routed connection (or pad) belonging to the net you wish to un-route, then click or press Enter .
If you do not know the location of a pad or routed connection in the net, click in free space and the Net Name dialog will pop up prompting for the net name. If you are unsure of the net name, type ? into the dialog and click OK to launch the Nets Loaded dialog, which lists all loaded nets for the design. All physical connections for the net you choose in the dialog will be un-routed when you click OK .
Un-route the physical connection between two pads. After launching the command, the cursor will change to a crosshair. Position the cursor over a segment of track that you wish to un-route (or a pad or via that it is connected to) then click or press Enter . If opting to un-route a connection by clicking on the associated pad, the following behavior is observed when there are multiple connections to the pad: current layer track will be un-routed first, followed by track in layer stack-up order (from the top layer down).
Un-route all physical connections emanating from the pads of the specified component. After launching the command, the cursor will change to a crosshair. Position the cursor over the component whose physical connections you wish to un-route then click or press Enter .
If you do not know the location of a component, click in free space and the Components Designator dialog will pop up, prompting for the component's designator. If you are unsure of the designator, type ? then click OK to launch the Components Placed dialog, which lists all components in the design. The physical connections for the component you choose in the dialog will be un-routed when you click OK . Each connection will un-route to the next pad detected on that connection. Track segments beyond that pad will not be removed.
Component Actions » Unroute Component command from the context menu.
Un-route all physical connections associated with the specified room. After launching the command, the cursor will change to a crosshair and you will be prompted to choose a room. Position the cursor over the room whose physical connections you wish to un-route then click or press Enter . A dialog will appear asking whether you wish to un-route connections that extend outside of the room. If you click Yes , all tracks (and vias) that reside in or cross the boundary of the room will be removed and replaced by the logical connections. If you click No , only the pad-to-pad connections that are contained wholly within the room will be un-routed.
If you click Yes to un-route the connections that cross the boundary of the room, the connection is un-routed from the component pad within the room to the next destination pad along the connection outside of the room. Tracks on the other side of this destination pad will remain routed.
Room Actions » Unroute Room command from the context menu.
If any track or via primitives to be un-routed are locked, a confirmation dialog will appear asking whether you want to allow the un-route of locked primitives. If you select No , only track and via primitives that are not locked will be un-routed.
Cleaning Nets (
Clean a net To clean individual routed nets for undesired duplicate (stacked) track segments, use the Design » Netlist » Clean Single Nets command. When you launch the command a crosshair cursor will appear, click on an object in the net you wish to clean. The net will be analyzed, and all instances of stacked redundant track segments will be removed. Note that the command only removes stacked track segments that are identical in their properties (i.e. same layer, same width, etc.).
Clean all nets To clean all routed nets for stacked track segments, use the Design » Netlist » Clean All Nets command. All nets will be analyzed, and all instances of stacked track segments will be resolved, with the redundant segments being removed. Note that the command only removes stacked track segments that are identical in their properties (i.e. same layer, same width, etc.).
Reroute and Remove Loops
Automatic Loop Removal feature.
This feature monitors the interactive routing process, and if it detects that a new path has been routed in parallel to an existing path, it automatically removes the old redundant segments. The option is on by default ( , applying to all nets. It can be disabled for selected nets, or it can be temporarily disabled during interactive routing to allow a specific loop to be created. The loop just created will be retained if loop removal is re-enabled for this net.
Automatic Loop Removal is enabled, when the new route path comes back to meet the existing route the old loop is automatically removed.
Rerouting with Loop Removal
Disable for selected nets Certain nets may require loops (multiple paths to the same point), such as a power or ground net. Loop removal can be disabled for these nets in the PCB panel (in Nets mode), either double-click on the net name to open the Edit Net dialog ( , or right-click on the net name and use the commands in the context menu (
Toggle on / off during routing Loop removal can be toggled on / off during interactive routing by pressing the Shift+D Shift+D
Starting and stopping When you are placing a new route, it is handy if the routing engine drops the connection (terminates) when you reach the target pad. However, during rerouting you might want to re-join an existing route path, but then continue laying the new path over the existing route. In this situation, you can temporarily disable the Automatically Terminate Routing option in the Properties panel (
Remove Net Antennas A route that is unterminated is called a net antenna . To prevent the loop removal feature from removing these, disable the Remove Net Antennas sub-option in the Properties panel ( Note that an antenna that terminates in a via is always preserved during automatic loop removal.
Remove Loops with Vias Use the Remove Loops with Vias sub-option to remove / prevent removal of loops that include one or more vias (
Preserve wider routes Note that if the new route path consists of tracks narrower than the existing path, the existing path will not be removed by the automatic loop removal feature.
Loop removal in a differential pair Rerouting a differential pair presents a challenge to the loop removal algorithm, because it needs to initially allow track crossovers before resolving loops (
Moving the Routing
interactive sliding. The controls for interactive sliding are available in the Preferences dialog ( , and can also be accessed in the Properties panel by pressing Tab
Key features that control the sliding process include: the routing conflict resolution mode (response to obstacles), the gloss strength (effort in tidying the results), and hugging (wrapping around obstacles and forming corners). There are a number of features that support interactive sliding, including T-junction and vertex dragging, via dragging, as well as differential pair dragging support.
A demonstration of interactive sliding being used to modify the existing routing.
Interactive Sliding (Dragging)
To slide (drag) a track Click and hold on the track segment, then move the mouse to start sliding the route. The PCB editor will automatically maintain the 45/90 degree angles with connected segments, shortening and lengthening them as required. Interactive sliding also supports non-orthogonal routing.
If the route does not move, it could be that the route is locked (an icon appears to indicate this (
To change the sliding behavior Press Tab during sliding to access the Properties panel, where you can change any of the interactive sliding settings (Hugging Style should be 45 Degree if your routing has diagonal corners. Press the Shift+Spacebar shortcut keys to cycle through the Hugging Style modes during sliding.
How the sliding routes are impacted The extent to which the moving tracks are reshaped as you slide them is controlled by the current Gloss Effort (Routed) setting ( , press the Ctrl+Shift+G shortcuts to cycle through the modes during sliding. Note that during interactive sliding glossing is automatically reduced to Weak , to avoid the glossing engine from fighting the designer in their attempts to relocate the routing. If you find that the routing will still not slide how you want, try setting the Gloss Effort (Routed) to Off .
How the sliding route responds to existing objects
During sliding, one of the Routing Conflict Resolution modes (Ignore, Push, HugNPush) applies ( Press Shift+R to cycle through the modes as you drag a track segment.
How neighboring routes are impacted The impact that the moving tracks have on the adjacent routing is controlled by the current Gloss Effort (Neighbor) setting ( , press Tab while sliding to change the setting.
Hugging - how glossing wraps around other objects and forms corners How the glossing engine wraps the route around other objects and forms the corners is referred to as hugging . The available Hugging Style settings include:
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).
Hugging style settings
The interactive sliding engine includes algorithms specifically for dragging a vertex (corner).
The Vertex Action option ( Spacebar
To convert a 90-degree corner to a 45-degree route, start dragging on the corner vertex with the Vertex Action setting in Deform mode.
Move a segment instead of dragging 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, either hold Ctrl Unselected via/track or the Selected via/track options in the Preferences dialog (
What you snap to during sliding The routing you are sliding will not only snap to the current snap grid, but can also snap other objects depending on the object snapping settings, the layer snapping setting, and if the snap guides and axes snapping settings are enabled (
Ctrl key. There is a summary of cursor-snap behavior at the start of this page.
There are specific algorithms included to support interactively modifying a T-junction - click and drag on the junction point to modify a T-junction (
Complementing the support for glossing of neighbor routes, via dragging is also supported. Via dragging supports Neighbor Glossing (
Tab during via dragging to access the panel and adjust the settings (
To recognize the members in a differential pair, the concept of coupling is used (
Keep Coupled option is enabled (
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
Push or jump Existing pads and vias will be jumped, or vias will be pushed if necessary and possible when the Allow Via Pushing option is enabled (
Break a track segment To break a single track segment, select the segment first, then position the cursor over the center vertex and click and drag, adding in new segments.
Object visibility To more easily see the objects that make up the current routing, adjust the Transparency of the routing objects in the View Configuration panel (
More about the interactive routing options .
Moving a Routed Component
There are two aspects to this tool, one is that it attempts to restore the routing to the component pads to suit the new location. The second is that it identifies fanouts, escape routes, and between-pin routes - collectively referred to as relevant routing - and can attempt to exactly maintain the pattern of this routing during the component move (if enabled).
When the Component re-route option is enabled, connected routes are restored after the moving component is placed.
Reroute a Moved Component
Enable rerouting of moved component(s) Enable the Component re-route option in the Preferences dialog ( , or use the Shift+R
When does rerouting happen? Essentially, the feature breaks 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.
Include relevant routing Fanouts, escape routes, and between-pin routes are collectively referred to as relevant routing. These can be moved as if they were part of the component footprint by enabling the Move component with relevant routing option ( The feature includes the up to xx pins field, if the moving component has more pins than specified in this field, the Move component with relevant routing option will ignore the selected component. Note that this feature is only available when a single component is being moved.
The slides below show how to control each function of the move component with routing feature.
To make the Move Component behavior routing friendly, the software detects and fixes violations in both the moving routing and the pre-existing routing. The default handling of violations is to visualize them while moving and attempt to resolve them on drop. Violations are resolved by pushing the pre-existing routing. Violations that cannot be resolved are left.
Glossing and Retracing Existing Routes
This section focuses on glossing as a post process, glossing existing routes. Once the routes of interest have been selected, configure the gloss settings in the Gloss and Retrace panel ( and then run the Route » Gloss Selected command.
retrace feature. Use this when you need to update selected routes to suit changes you have made to the design constraints, such the routing width, or the differential pair gap. 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 while preserving the existing trace width and differential pair gap.
Retrace focuses on satisfying the design constraints, updating the widths and differential pair gaps to suit the current constraint settings.
What does Gloss Selected do? Glossing analyzes the selected routes, reducing the number of corners, and neatening and shortening them. It also repairs poor quality pad entries, and also attempts to improve the quality of differential pair routing.
What is Glossed?
Gloss Selected 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. More about selection strategies .
Flexible approaches to selection can be used, supporting partial glossing of a routed net. To gloss a section of a routed net, simple 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), then run the Gloss Selected command (shortcut Ctrl+Alt+G
Note that if only tracks/arcs on one side of a pair are selected, this side will be glossed as a single-ended trace. Select tracks/arcs on both sides to enter differential pair mode glossing.
What options control Gloss Selected? Gloss Selected obeys the current settings configured in the PCB Editor - Gloss and Retrace page of the Preferences dialog (Gloss and Retrace panel (
More about the Gloss Selected options .
Glossing a differential pair
When applied to differential pair routes, the tool recognizes "zipped" portions of the routes - where the pair is already at the defined diff pair gap from each other. Its goal is 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. Glossing is applied to each unzipped and zipped portion, trying to make it short and smooth but without sacrificing the parallel routing and length balance. 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 (
When glossing a differential pair, Gloss will attempt to will attempt to preserve the dominant gap of the selected portion of the pair, where possible:
It will, however, narrow it down as needed to ensure DRC-free passage in tight zones and balanced pad entries at the ends.
This behavior is applied to the zipped portion of the pair (where the sides are at Max Gap or less from each other).
Caveat: Gloss does not handle an unreasonably large Max Gap.
Dominant gap – gloss finds the distance between the selected traces that is most common along the selected length and uses this wherever possible.
Support for room-based rules
Gloss adheres to Clearance and Diff Pair Routing constraints 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.
Support for Subnet Jumpers Gloss treats Subnet Jumper tracks as fixed.
Exclusions
To exclude routes from glossing or retracing, lock the track segments.
Arcs are currently not glossed.
Tracks at non-45 degree angle increments are not glossed; it is assumed these have been placed intentionally to satisfy a design requirement.
Gloss Selected feedback
What does Retrace Selected do?
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, more on this below.
What is Retraced?
Retrace Selected 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. More about selection strategies .
Flexible approaches to selection can also be used, supporting partial retracing of a routed net. To retrace a section of a routed net, simple 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), then run the Retrace Selected command. All of the routing between the end points will be retraced. In a differential pair, perform the selection on both sides of the pair.
What options control Retrace Selected? Retrace obeys the current settings configured in the PCB Editor - Gloss And Retrace of the Preferences dialog or in the Gloss And Retrace panel.
More about the Retrace options .
Updating the vias in Retraced routes Retrace updates the widths of tracks and arcs according to the applicable Routing Width design constraint or the value entered into the Set Width field in the Gloss and Retrace panel. It does not update the routing vias to reflect changes in the Routing Via Style design constraint. To resolve via-size changes:
Select the nets, the Properties panel will load all selected tracks, arcs and vias.
Use the Post Selection Filter at the top of the panel to exclude all objects except vias (
Modify the via size to match the updated Routing Via Style design rule. If you do a single via before starting this bulk-edit process a new Via Template will be created, which you can then select when you are updating all the other vias.
Run the Retrace command on the selected routing to update the routing widths.
Resolve any design violations that might have occurred because of the via size change. The Retrace command will not update routing widths if it creates a violation; confirm that the width changes satisfy your design requirements.
Retracing a differential pair 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 constraint so that the Preferred Gap is the desired gap, and the Max Gap is the old Preferred Gap value, then run Retrace. Alternatively, a new gap value can be typed directly into the Set Diff Pair Gap field in the Gloss and Retrace panel. Please note that 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 or enter a new gap value in the Set Diff Pair Gap field in the Gloss and Retrace panel.
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.
Retrace feedback
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
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 or retracing.
More about the hugging style settings .
Avoid polygons When 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 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 .
More about pad entry stability .
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.
More about the miter ratio .
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.
More about the gloss effort settings .
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 constraint when the Retrace Selected command is run, or retrace using the Current width. 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 constraint when the Retrace Selected command is run, or retrace using the Current gap between the differential pair tracks. Alternatively, enter a desired custom gap value directly in the field. Note that this option is available only when the 45 Degree option is selected for Hugging Style .
Preserve route path Enable to preserve the exact trace geometry during Retrace. When this option is enabled, the Retrace algorithms will not modify the centerline of the trace. Tracks may change width and be split into segments of different widths, but the trajectory will not be changed.
This option will narrow down a track to avoid a DRC violation, while, with this option disabled, it is possible to shift a trace a bit.
This option will not remove defects that existed before retrace, or that were created by widening the trace.
This option works only for single-ended routes because preserving the path for differential pairs is impossible without breaking the pair. When retracing a differential pair its path will be changed if needed, regardless of the state of the option.
Information Messages (
Skipped immovable + <Descriptor>An object is protected from Gloss/Retrace: for example, locked or belonging to a component.
Skipped subnet jumper + <Descriptor>Subnet jumpers are left alone, user informed in each case.
Skipped reflex angle + <Descriptor>Arcs greater than 180 degrees are not glossed.
Max count 20, clickable.
Skipped objects in user-defined UnionObjects 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 Messages
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.
( , Interactive Sliding (( options available in the Properties panel. The default settings for these capabilities are configured in the PCB Editor section of the Preferences dialog (
Press Tab Properties panel, press Tab Properties panel, or press Tab Properties panel.
The routing action will be paused to give you access to the panel – to return to the interactive process press Esc on the keyboard, or click the Pause icon (
This option determines how you want the routing/sliding objects to react when they encounter an existing object. Press the Shift+R Tab Properties panel and select the required setting.
More about the conflict resolution mode during interactive routing , or during interactive sliding .
The color of the row reflects when a capability is available.
In this mode the interactive router can place tracks anywhere, including over existing objects, displaying but allowing potential violations.
Attempt to find a path, from the last click location to the current cursor location, around existing objects such as tracks, pads and vias. The clearance to other objects is defined by the applicable Clearance design rule. If this mode cannot walkaround an obstacle without causing violation, an indicator appears to show the route is blocked.
Push existing tracks and vias to make room for the new route. If this mode cannot push an obstacle without causing violation, an indicator appears to show the route is blocked. Via pushing is controlled by the Allow Via Pushing option.
The routing will closely follow existing objects and only push them when there is insufficient room for the track being routed. If this mode cannot hug or push an obstacle without causing violation, an indicator appears to show the route is blocked.
The routing will stop at the first obstacle that gets in the way.
Apply auto-router intelligence to the interactive router, automatically selecting between pushing and walking around to give the shortest overall route length, on the current layer.
Apply auto-router intelligence to the interactive router, automatically selecting between pushing, walking around or switching layers to give the shortest overall route length.
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.
Press Shift+Spacebar Spacebar Tab Properties panel.
More about controlling the corner style during interactive routing , or during interactive sliding .
Gloss Effort .
Measures of glossing quality include: reducing the number of corners, reducing the number of segments, removing acute angles and reducing the overall route length. Use the Ctrl+Shift+G Tab Properties panel and select the required setting.
More about gloss effort during interactive routing , during interactive sliding , and during glossing or retracing of selected routing .
The color of the row reflects when a capability is available.
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 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 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.
During interactive sliding, glossing is temporarily reduced to Weak, to avoid the glossing engine from fighting the designer in their attempts to relocate the routing.
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 .
Press Tab Properties panel and select the required setting.
More about gloss effort during interactive routing and during interactive sliding .
The color of the row reflects when a capability is available.
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 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 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.
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. 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. The current Hugging Style is also applied during glossing or retracing of selected routes .
Use the Shift+Spacebar shortcut to cycle through the three modes.
More about hugging during interactive sliding , and during glossing or retracing of selected routing .
The color of the row reflects when a capability is available.
Always use straight orthogonal/diagonal segments to create corners during sliding (use this mode for traditional orthogonal/diagonal routing behavior).
Use straight track segments when the objects being moved/pushed against are straight, use arcs when they are curved. The minimum arc size is controlled by the Min Arc Ratio option .
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).
Options that are applied when you click and drag on a vertex rather than along a track or arc segment (the vertex is the corner location where two segments meet). Use the Spacebar shortcut to cycle through the available modes during sliding.
The color of the row reflects when a capability is available.
Break or lengthen the track segments attached to the moving vertex so that the vertex follows the cursor movement.
Hold the corner shape and resize and move the incoming track segments, keeping the vertex attached to the cursor.
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.
If there is a shortcut available for an option, it is detailed on the right-hand side of the Properties panel. Each description includes an image of where that option can be configured.
The color of the row reflects when a capability is available.
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 click and start routing another net.
More about when to use this option during re-routing .
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.
More about automatic loop removal during re-routing .
↳ Remove Loops with Vias
When there is a direct via-to-pad connection, the via will be removed if deemed no longer needed after loop removal.
↳ Remove Net Antennas
A net antenna is a section of routing that is unterminated at one end. These are automatically removed if the current routing impacts on an object that the antenna is touching.
Keep Coupled Check this option to ensure objects that belong to a differential pair will be dragged with the pair's partner track or via.
More about dragging a differential pair .
Include Miters Check this option to include miters while dragging track segments.
Merge Parallel Check this option to allow a track segment being dragged to be merged with an existing stationary segment once the dragged segment became aligned to the stationary segment.
Allow Via Pushing
Check this option to allow pushing a Via when in Push Obstacles or HugNPush Obstacles modes.
Pin Swapping Check this option to enable pin swapping for this net.
Learn more about setting up for pin swapping .
Auto Shrinking
Check this option to automatically shrink the routing width to a value that would allow routing in locations where the track cannot be routed between obstacles with the currently chosen routing width. Note that the width can be reduced down to the minimum allowed by the applicable Routing Width design constraint.
More about auto shrinking .
This feature is available when the PCB.Routing.EnableAutoShrinking option is enabled in the Advanced Settings dialog (feature currently in Open Beta).
Display Clearance Boundaries
Display the no-go area around existing objects ( , defined by the Clearance design rule that is applicable to those objects.
More about controlling the display of routes .
↳ Reduce Clearance Display Area
Reduce the display of clearance boundaries 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 .
The 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.
More about routing pad entries .
Apply Trace Centering
When enabled, the interactive routing engine detects when a route is passing between pads and attempts to center the route, up to a maximum distance of the applicable clearance constraint multiplied by the Added Clearance Ratio specified below. Trace centering can also be applied between via-via and via-pad if the Adjust Vias sub-option is enabled. This feature can be disabled during track sliding , if required.
More about trace centering .
This feature is available when the PCB.EnableTraceCentering option is enabled in the Advanced Settings dialog (feature currently in Open Beta).
↳ Adjust Vias
This option serves two purposes:
Enable for the trace centering feature to also center between via-via or via-pad. Disable if centering between via-via or via-pad is not required. To prevent vias from being pushed by trace centering, you can disable the Allow Via Pushing option. In this case, vias will not be pushed (even to ensure the minimum clearance from the Clearance constraint). More about trace centering .
If vias should be pushed when in Push or HugNPush modes .
To exclude vias disable the Adjust Vias option.
↳ 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 to precisely center the routes, if required.
More about trace centering .
↳ Disable Trace Centering when Dragging
Enable this option to switch off trace centering when interactively sliding a route. When this option is enabled, trace centering does not apply during interactive sliding of a route, even if the main Apply Trace Centering option is enabled.
More about trace centering .
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 ( Enter a positive value equal to or greater than zero (the x multiplier is added automatically).
More about mitering corners .
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.
Subnet Jumper Length
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 into swap-enabled nets, 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. This value defines the length of the subnet jumper that is added to a swappable net during interactive routing.
More about subnet jumpers .
During interactive routing, the Routing Width and Routing Via Style design constraints that apply to the route being performed, are displayed in the Properties panel. These are live links, click to open the relevant design constraint for review or editing, if required.
The color of the row reflects when a capability is available.
Via Constraint
The Routing Via Style design constraint that is applicable to the net(s) currently being routed.
Width Constraint
The Routing Width design constraint that is applicable to the net(s) currently being routed.
During interactive routing and interactive sliding, the net(s) under edit are detailed at the top of the Properties panel.
The color of the row reflects when a capability is available.
Name & Class
The Name of the Net or Differential Pair under edit is displayed, along with the Class it belongs to (if any). The Name and Class are live links, click to open the PCB panel displaying the relevant net or pair details.
Length & Delay
The Signal Length and the calculated Delay are detailed, the displayed values are valid when the initial routing/sliding click occurs. The Length and Delay are live links, click to open the PCB panel displaying the relevant net or pair details, which will update in real-time as the routing or sliding is performed.
Defines the behavior to be applied when you click and drag on an object.
Apart from Vertex Actions, these options are only available in the Preferences dialog.
When enabled the software will attempt to preserve the angle when dragging, in accordance with the current Interactive Sliding settings in the Properties panel (Re-route and Break Track commands are run from the Edit » Move menu ( :
Ignore Obstacles - obstacles will be ignored to preserve angle during dragging.
Avoid Obstacles (Snap Grid) - based on the snap grid, the software will try to avoid obstacles while preserving angles.
Avoid Obstacles - software will try to avoid obstacles during dragging.
Disable Trace Centering When Dragging Detailed earlier on this page
Vertex Actions Detailed earlier on this page
Defines the default behavior when dragging an unselected via or track to be either a Move or Drag action. To access the mode not chosen, hold the Ctrl
Defines the default behavior when dragging a selected via or track to be either a Move or Drag action. To access the mode not chosen, hold the Ctrl
This field defines the current Component Conflict Resolution mode when moving components within the design space. For this feature, components are identified by their selection bounding box . The following modes are supported:
Ignore – this is the default behavior, where the component can be moved even if it creates a violation with neighboring component(s).
Push – the component will push other components away to provide compliance with clearances between components. Components in unions can be pushed and the location of components in the union may change but the union will not break. Locked components cannot be pushed.
Avoid – the component will be forced to avoid violating component clearance rules between other components.
When enabled, after moving component(s) to a new location and releasing, the software will attempt to re-route the component(s) to reconnect any broken nets. During movement, the Shift+R shortcut can be used to toggle the re-route behavior off/on. Note that component re-routing is not applied to a moved component if that component is a member of a union.
More about moving components with routing .
Enable this 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. 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.
More about moving components with routing .
Stores the last-used routing width and via size selected during interactive routing. During interactive routing, cycle though the modes by pressing the 3
These options are only available in the Preferences dialog.
If enabled, the interactive router will set the width of the new route to match the track under the cursor when you click to commence interactive routing, instead of using the Track Width Mode selected below. If there is no track segment below the click location when you commence interactive routing, then the current Track Width Mode is used.
There are four possible widths that a connection can be routed at: Constraint Minimum, Constraint Preferred, Constraint Maximum, and User. This option holds the last-selected mode, which is used the next time you launch the Interactive Routing command. Press the 3
More about selecting the track width mode during routing .
There are four possible via sizes that can be used for a layer change during interactive routing: Constraint Minimum, Constraint Preferred, Constraint Maximum, and User. This option holds the last-selected mode, which is used the next time you launch the Interactive Routing command. Press the 4
More about selecting the via size and via type during routing .
Stores the user-defined list of routing widths that are presented when the Shift+W (
These options are only available in the Preferences dialog.
Favorite Interactive Routing Widths Click the button to open the Favorite Interactive Routing Widths dialog, where you configure the list of pre-defined widths that the Shift+W
