PCB_Dlg-EditRoutingConstraintsInteractive Routing_AD

The two incarnations of the Interactive Routing For Net dialog. As opened while placing Multiple Traces (back) and while routing a net (front).

SUMMARY

The Interactive Routing For Net dialog provides controls related to routing settings, including routing width, via size, conflict resolution etc.

ACCESS

This dialog can be accessed in the following ways:

• Press Tab while routing a net.
• Press Tab while placing Multiple Traces.

If accessed using the latter method (Multiple Traces), this dialog appears in a truncated form.

OPTIONS/CONTROLS

Bus Routing

This section is available only when the dialog has been accessed while placing Multiple Traces.

• Bus Spacing - Manually specify the bus routing.
• From Rule - Assign bus spacing based on the existing design rule. 

Properties

This section is available only when the dialog has been accessed while routing a net.

• User preferred Width - Choose the preferred value from drop-down list. Both mm and mil options are listed.
• Apply to all layers - Enable this option to apply the chosen width for all layers.
• Via Hole Size - Specify the via hole size in this field.
• Via Diameter - Specify the via hole diameter in this field.
• Layer - Specify which layer the routing is on.
• Template - If the via is associated with a template, the template name is viewable here.

Routing Width Constraints

This section is available only when the dialog has been accessed while routing a net.

• Edit Width Rule - Click to open the Edit PCB Rule - Max-Min Width Rule dialog, in which the designer can define PCB rules for routing width.

Via Style Constraints

This section is available only when the dialog has been accessed while routing a net.

• Edit Via Rule - Click to open the Edit PCB Rule - Routing Via-Style Rule dialog, in which the designer can define PCB rules for via.

Pin Swapping

This section is available only when the dialog has been accessed while routing a net.

• Enabled - Check this option to enable pin swapping.
• Compile Project - This button appears only when project compilation is out of date, click this button to compile project.
• Preferred Subnet Jumper Length - Specify the desired Subnet Jumper length.

Routing Conflict Resolution

Certain options in this section are only available if the dialog has been accessed while routing a net.

• Ignore Obstacles - Enable this option to ignore existing objects (routing can be freely placed). Violations are highlighted. 
• Push Obstacles - Select to have the Interactive Router move existing tracks out of the way while routing. This mode can also push vias to make way for the new routing. If this mode cannot push an obstacle without causing violation, an indicator appears to show that the route is blocked.
• Walkaround Obstacles - Enable this option to have the Interactive Router route around existing tracks, pads and vias while routing. If this mode cannot walkaround an obstacle without causing violation, an indicator appears to show that the route is blocked. 
• Stop At First Obstacle - In this mode, the routing engine will stop at the first obstacle that gets in the way.
• Hug And Push Obstacles - Enable this option to have the Interactive Router hug existing tracks, pads and vias as closely as possible while routing and, where necessary, push obstacles to continue the route. If this mode cannot hug or push an obstacle without causing a violation, an indicator appears to show that the route is blocked.
• Current Mode - Choose current routing mode from drop-down list.
• AutoRoute On Current Layer - Enable to AutoRoute only on the current layer.
• AutoRoute On Multiple Layers - Enable to AutoRoute on multiple layers.

Interactive Routing Options

• Restrict to 90/45 - Enable to restrict the routing to 90 degrees and 45 degrees only.
• Follow Mouse Trail - Enable this option to activate routing through the mouse trail.
• Automatically Terminate Routing -  Enable so when you complete a route to the target pad, the routing tool does not continue in routing mode from the target pad but resets, ready for you to click on the next source pad to route from. If this option is disabled, after you route to the target pad the tool will remain in routing mode, using the previous target pad as the source for the next route.
• Automatically Remove Loops -  Enable to automatically remove any redundant loops that are created during manual routing. This allows you to re-route a connection without having to manually remove redundant tracks.
  However, there are times when you need to route nets such as power nets and you need loops, thus you can toggle the Remove Loops option for a selected net by editing its net property from the Edit Net dialog via the PCB panel. The Remove Loops local setting for the specified net overrides this global setting for the same net.
  • Remove Net Antennas - Enable this option to remove any track or arc end that is not connected to any other primitive and thus forms an antenna.
• Allow Via Pushing - Check this option to allow pushing Via when you're in Push Obstacles or Hug and Push Obstacles mode.
• Display Clearance Boundaries - Enable this option to have the no-go clearance area defined by the existing objects and the applicable clearance rule displayed as shaded polygons, within a local viewing circle. This option is not available in the Ignore Obstacles routing mode.
  • Reduce Clearance Display Area - Enable this option to use a smaller clearance boundary.

Routing Gloss Effort

• Off - In this mode, glossing is essentially disabled. Note, however, that cleanup is still run after routing/dragging occurs to eliminate overlapping track segments for example. This mode is typically useful at the end stage of board layout, where the ultimate-level of fine-tuning is required (for example when manually dragging tracks, cleaning pad entries, etc).
• Weak - In this mode a low level of glossing is applied, with the Interactive Router considering only those tracks directly connected to, or in the area of, the tracks that you are currently routing (or tracks/vias being dragged). This mode of glossing is typically useful for fine-tuning track layout, or when dealing with critical traces.
• Strong - In this mode a high level of glossing is applied, with the Interactive Router looking for shortest paths, smoothing out tracks, etc. This mode of glossing is typically useful in the early stages of the layout process, when the aim is to get a fair bit of the board routed quickly.

Interactive Routing Width / Via Size Sources

• Pickup Track Width From Existing Routes - Enable to use the existing track width when routing from an placed track. That is, even if the current routing width is different to the existing track, the existing track width will be adopted when you continue the route from it.
• Track Width Mode -  - Choose a track width mode for interactive routing. The available modes are:
  • User Choice - With this mode enabled the width is determined from the width selected in the Choose Width dialog - accessed by pressing Shift + W while routing.
  • Rule Minimum - With this mode enabled the design rule minimum width defined for the current net will be used.
  • Rule Preferred - With this mode enabled the design rule preferred width defined for the current net will be used.
  • Rule Maximum - With this mode enabled the design rule maximum width defined for the current net will be used.
• Via Size Mode - Choose one of the via size modes for interactive routing. The available modes are:
  • User Choice - With this mode enabled the via size is determined from the size selected in the Choose Via Sizes dialog - accessed by pressing Shift + V while routing.
  • Rule Minimum - This mode uses the minimum via size rule.
  • Rule Preferred - This mode uses the preferred via size rule.
  • Rule Maximum - This mode uses the maximum via size rule.

Favorites

• Favorite Interactive Routing Widths - Click to open the Favorite Interactive Routing Widths dialog.

Buttons

• Menu - Click to access the following context menu options:
  • Edit Width Rule - Click to open the Edit PCB Rule - Max-Min Width Rule dialog, in which the designer can define PCB rules for routing width.
  • Edit Via Rule - Click to open the Edit PCB Rule - Routing Via-Style Rule dialog, in which the designer can define PCB rules for via.
  • Add Width Rule - Click to open the Edit PCB Rule - Max-Min Width Rule dialog, in which the designer can define PCB rules for routing width.
  • Add Via Rule - Click to open the Edit PCB Rule - Routing Via-Style Rule dialog, in which the designer can define PCB rules for via.
  • Net Properties - Click to open the Edit Net dialog, in which allows designers to edit nets, including changing the net name, adding or removing physical pins for the specified net, and specifying track length for the net.