Altium NEXUS Documentation

AutoRoute

Modified by Susan Riege on Jul 13, 2018

Parent page: PCB Commands

The following pre-packaged resources, derived from this base command, are available:


Applied Parameters: Action=Start

Summary

This command is used to route the entire board using the Situs Autorouter. Situs is a Topological Autorouter. A topological autorouter uses a different method of mapping the routing space - one that is not geometrically constrained. Rather than using workspace coordinate information as a frame of reference (dividing it into a grid), a topological autorouter builds a map using only the relative positions of the obstacles in the space, without reference to their coordinates. It does this by triangulating the space between adjacent obstacles. This triangulated map is then used by the routing algorithms to "weave" between the obstacle pairs from the start route point to the end route point. The greatest strengths of this approach are that the map is shape independent (the obstacles and routing paths can be any shape) and the space can be traversed at any angle - the routing algorithms are not restricted to purely vertical or horizontal paths, as with a rectilinear expansion routers.

For a high-level look at this approach to auto-routing, see Topological Autorouting.

Access

This command is accessed from the PCB Editor by choosing the Route » Auto Route » All command from the main menus.

Use

After launching the command, the Situs Routing Strategies dialog will open. The Autorouter conducts its own pre-routing analysis and presents the results as a report in the dialog. The report provides information including:

  • Design rules currently defined for the design that will be adhered to by the Autorouter (and the number of design objects - nets, components, pads - affected by each rule).
  • Routing directions defined for all signal routing layers.
  • Drill layer pair definitions.

The report lists potential problems that could affect router performance. Where possible, hints are provided in order to advise how the design could be better prepared prior to autorouting. Any errors/warnings/hints that are listed should be scrutinized and, if needed, the corresponding routing rules adjusted before proceeding to route the design.

It is essential that any routing-related rule violations are resolved before starting the Autorouter. Not only can violations prevent routing at the location of the violation, they can also greatly slow the router as it continually attempts to route an unrouteable area.

The Autorouter comes pre-configured with a number of Routing Strategies that have been found to be useful for different applications, but you can create your own strategies based on experimentation and the sorts of boards with which you are working. A new routing strategy can be added from the dialog by clicking the Add button, which opens the Situs Strategy Editor dialog. Use this latter dialog to define the strategy as required by including the routing passes you need.

In general, the default routing strategies for two layer and multi-layer boards are fine for most routing situations. It is important, however, to ensure that any relevant routing design rules are set up prior to running the Autorouter.

With a clean pre-routing analysis, and the chosen routing strategy selected, proceed to start the Autorouter by clicking the Route All button.

Tips

  1. Pre-route critical nets and, if it is essential that they are not changed by the routing process, lock them by enabling the Lock All Pre-routes option in the Situs Routing Strategies dialog. Avoid unnecessary locking though; a large number of locked objects can make the routing problem much more difficult.
  2. Differential pair nets cannot be autorouted and must be manually routed and locked before using the Autorouter. If differential pairs are not locked prior to auto routing, it is very likely that they will be altered by the Autorouter and signal integrity of the differential pair could be adversely effected.
  3. Do not be afraid to experiment. If the results of running the Autorouter are not acceptable, do something to change the router's approach. Add intermediate cleanup and straighten passes, make more room around dense areas, or change layer directions. Experiment with the router by creating new strategies to control the order of passes, changing the number of vias that can be dropped by the Autorouter, changing the routing layer directions, constraining the router to orthogonal routes only, and so on. Keep notes of the combinations that have been tried use this information to identify and reuse which configurations work best on particular designs.
  4. All Autorouter event and routing information will appear as messages in the Messages panel.


Applied Parameters: Action=NetClass

Summary

This command is used to route all connections in the specified net class(es).

Access

This command is accessed from the PCB Editor by choosing the Route » Auto Route » Net Class command from the main menus.

Use

After launching the command, the Choose Net Classes to Route dialog will open. Select one or more net classes that you wish to route using the Autorouter then click OK - the Autorouter will attempt to autoroute all connections for all nets in the chosen net class(es) using the Main routing strategy.

After routing is complete, the dialog will re-open. Choose further net classes to route or click Cancel to exit.

Tips

  1. It is important to ensure that any relevant routing design rules are set up prior to running the Autorouter.
  2. Select multiple net classes for routing using standard multi-select techniques (Ctrl+click, Shift+click).
  3. All Autorouter event and routing information will appear as messages in the Messages panel.
>


Applied Parameters: Action=ComponentClass

Summary

This command is used to route all connections emanating from the pads of components in the specified component class(es).

Access

This command is accessed from the PCB Editor by choosing the Route » Auto Route » Component Class command from the main menus.

Use

After launching the command, the Choose Component Classes to Route dialog will open. Select one or more component classes that you wish to route using the Autorouter, specifiy the Connections Routing Mode then click OK - the Autorouter will attempt to autoroute all connections that emanate from the pads of all components in the chosen component class(es) using the Main routing strategy.

After routing is complete, the dialog will re-open. Choose further component classes to route or click Cancel to exit.

Tips

  1. It is important to ensure that any relevant routing design rules are set up prior to running the Autorouter.
  2. Select multiple component classes for routing using standard multi-select techniques (Ctrl+click, Shift+click).
  3. All Autorouter event and routing information will appear as messages in the Messages panel.


Applied Parameters: Action=Net

Summary

This command is used to route all connections in a specified net.

Access

This command is accessed from the PCB Editor by choosing the Route » Auto Route » Net command from the main menus.

Use

After launching the command, the Autorouter will initialize and the cursor will change to a cross-hair. Position the cursor over any connection line (or pad) in the net you wish to route then click or press Enter. The Autorouter will attempt to autoroute all connections in the net using the Main routing strategy.

Continue routing connections associated with other nets or right-click, or press Esc to exit.

Tips

  1. It is important to ensure that any relevant routing design rules are set up prior to running the Autorouter.
  2. All Autorouter event and routing information will appear as messages in the Messages panel.


Applied Parameters: Action=Component

Summary

This command is used to route all connections emanating from the pads of a specified component.

Access

This command is accessed from the PCB Editor by choosing the Route » Auto Route » Component command from the main menus.

Use

After launching the command, the Autorouter will initialize and the cursor will change to a cross-hair. Position the cursor over the component you wish to route then click or press Enter. The Autorouter will attempt to autoroute all connections emanating from pads of the chosen component, up to the next encountered pad in each case using the Main routing strategy.

Continue routing connections associated with other components or right-click or press Esc to exit.

Tips

  1. It is important to ensure that any relevant routing design rules are set up prior to running the Autorouter.
  2. All Autorouter event and routing information will appear as messages in the Messages panel.


Applied Parameters: Action=OnSelectedComponents

Summary

This command is used to route all connections emanating from the pads of currently selected components in the main design workspace.

Access

This command is accessed from the PCB Editor by choosing the Route »  Auto Route » Connections On Selected Components command from the main menus.

Use

First, ensure that all components whose associated connections you wish to autoroute, are selected in the main design workspace.

After launching the command, the Autorouter will attempt to autoroute all connections emanating from pads of the selected components, up to the next encountered pad in each case using the Main routing strategy.

Tips

  1. It is important to ensure that any relevant routing design rules are set up prior to running the Autorouter.
  2. All Autorouter event and routing information will appear as messages in the Messages panel.


Applied Parameters: Action=BetweenSelectedComponents

Summary

This command is used to route all connections running between the currently selected components in the main design workspace.

Access

This command is accessed from the PCB Editor by choosing the Route » Auto Route » Connections Between Selected Components command from the main menus.

Use

First, ensure that all components whose associated connections you wish to autoroute are selected in the main design workspace.

After launching the command, the Autorouter will attempt to autoroute all connections running between the pads of the selected components using the Main routing strategy.

Tips

  1. It is important to ensure that any relevant routing design rules are set up prior to running the Autorouter.
  2. All Autorouter event and routing information will appear as messages in the Messages panel.


Applied Parameters: Action=SingleComponent|ContextObject=Component

Summary

This command is used to route all connections emanating from the pads of the component under the cursor.

Access

This command is accessed from the PCB Editor by right-clicking over a component and choosing the Component Actions » Autoroute Component command from the context menu.

Use

After launching the command, the Autorouter will attempt to autoroute all connections emanating from pads of the component, up to the next encountered pad in each case using the Main routing strategy.

Tips

  1. It is important to ensure that any relevant routing design rules are set up prior to running the Autorouter.
  2. All Autorouter event and routing information will appear as messages in the Messages panel.


Applied Parameters: Action=Area

Summary

This command is used to route all connections that are fully contained (start and end) within a specified area.

Access

This command is accessed from the PCB Editor by choosing the Route » Auto Route » Area command from the main menus.

Use

After launching the command, the Autorouter will initialize and the cursor will change to a cross-hair. Position the cursor then click to anchor the first corner of the routing area. Move the cursor to size the routing area then click to anchor the second corner. The Autorouter will attempt to autoroute all connections starting and ending within the designated area using the Main routing strategy.

Continue routing connections within another defined area or right-click or press Esc to exit.

Tips

  1. It is important to ensure that any relevant routing design rules are set up prior to running the Autorouter.
  2. All Autorouter event and routing information will appear as messages in the Messages panel.


Applied Parameters: Action=Room

Summary

This command is used to route all connections that reside completely within the boundaries of a selected room.

Access

This command is accessed from the PCB Editor by choosing the Route » Auto Route » Room command from the main menus.

Use

After launching the command, the Autorouter will initialize and the cursor will change to a cross-hair. Position the cursor over the room you wish to route then click or press Enter. The Autorouter will attempt to autoroute all connections that reside completely within the room boundaries using the Main routing strategy.

Continue routing connections associated with other rooms or right-click or press Esc to exit.

Tips

  1. It is important to ensure that any relevant routing design rules are set up prior to running the Autorouter.
  2. All Autorouter event and routing information will appear as messages in the Messages panel.


Applied Parameters: Action=SingleRoom|ContextObject=Room

Summary

This command is used to route all connections that reside completely within the boundaries of the room under the cursor.

Access

This command is accessed from the PCB Editor by right-clicking over a room then choosing the Room Actions » Autoroute Room command from the context menu.

Use

After launching the command, the Autorouter will attempt to autoroute all connections that reside completely within the room boundaries using the Main routing strategy.

Tips

  1. It is important to ensure that any relevant routing design rules are set up prior to running the Autorouter.
  2. All Autorouter event and routing information will appear as messages in the Messages panel.


Applied Parameters: Action=Setup

Summary

This command is used to run the Situs Routing Strategies dialog, from where you can interrogate a pre-routing analysis report for the design and choose the strategy to be used when routing. The routing strategy is the intelligence of the Router, defining which of the various routing algorithms to use and when in order to turn the 'virtual' routing paths identified in the topological map into high-quality, highly efficient, real routing on the board.

The Situs Autorouter is a Topological Autorouter. A topological autorouter uses a different method of mapping the routing space - one that is not geometrically constrained. Rather than using workspace coordinate information as a frame of reference (dividing it into a grid), a topological autorouter builds a map using only the relative positions of the obstacles in the space without reference to their coordinates. It does this by triangulating the space between adjacent obstacles. This triangulated map is then used by the routing algorithms to "weave" between the obstacle pairs from the start route point to the end route point. The greatest strengths of this approach are that the map is shape independent (the obstacles and routing paths can be any shape) and the space can be traversed at any angle - the routing algorithms are not restricted to purely vertical or horizontal paths as with a rectilinear expansion routers.

Access

This command is accessed from the PCB Editor by choosing the Route » Auto Route » Setup command from the main menus.

Use

After launching the command, the Situs Routing Strategies dialog will open. The Autorouter conducts its own pre-routing analysis and presents the results as a report in the dialog. The report provides information including:

  • Design rules currently defined for the design that will be adhered to by the Autorouter (and the number of design objects - nets, components, pads - affected by each rule).
  • Routing directions defined for all signal routing layers.
  • Drill layer pair definitions.

The report lists potential problems that could affect router performance. Where possible, hints are provided in order to advise how the design could be better prepared prior to autorouting. Any errors/warnings/hints that are listed should be scrutinized and, if needed, the corresponding routing rules adjusted before proceeding to route the design.

It is essential that any routing-related rule violations are resolved before starting the Autorouter. Not only can violations prevent routing at the location of the violation, they can also greatly slow the router as it continually attempts to route an unrouteable area.

The Autorouter comes pre-configured with a number of Routing Strategies that have been found to be useful for different applications, but you can create your own strategies based on experimentation and the sorts of boards with which you are working. A new routing strategy can be added from the dialog by clicking the Add button, which opens the Situs Strategy Editor dialog. Use this latter dialog to define the strategy as required by including the routing passes you need.

In general, the default routing strategies for two layer and multi-layer boards are fine for most routing situations. It is important, however, to ensure that any relevant routing design rules are set up prior to running the Autorouter.

After the required routing strategy has been chosen/defined and any warnings investigated/resolved, click the OK button. The chosen strategy will be selected the next time you use the Autorouter to route the entire board.

Tips

  1. Pre-route critical nets and, if it is essential that they are not changed by the routing process, lock them by enabling the Lock All Pre-routes option in the Situs Routing Strategies dialog. Avoid unnecessary locking though; a large number of locked objects can make the routing problem much more difficult.


Applied Parameters: Action=Stop

Summary

This command is used to terminate the autorouting process at the completion of the current routing pass.

Access

This command is accessed from the PCB Editor by choosing the Route » Auto Route » Stop command from the main menus.

Use

After launching the command, the Autorouter will stop and no further routing of the board will take place. Any connections on the board that have already been routed will remain routed.

Tips

  1. All Autorouter event and routing information will appear as messages in the Messages panel.


Applied Parameters: Action=Reset

Summary

This command is used to reset the Autorouter - initializing the memory needed by the autorouter before it attempts to route. It allows you to effectively modify the existing routing strategy, or change to a different routing strategy, on-the-fly, when routing the entire board.

Access

This command is accessed from the PCB Editor by choosing the Route » Auto Route » Reset command from the main menus.

Use

After launching the command, the Situs Routing Strategies dialog will open. Use the dialog to make changes to the current routing strategy (where available) or switch to a different one then click the Route All button. The Autorouter will initialize for routing based on the modified/different strategy.

Tips

  1. All Autorouter event and routing information will appear as messages in the Messages panel.


Applied Parameters: Action=Pause

Summary

This command allows you to pause the current Autorouting operation.

Access

This command is accessed from the PCB Editor by choosing the Route » Auto Route » Pause command from the main menus.

Once the command has been used, the entry on the menu will change to Resume.

Use

After launching the command, progress of the Autorouter will be temporarily halted. To continue again, run the command again (which now appears as the Route » Auto Route » Resume command).

Tips

  1. To stop the autorouting process completely, use the Route » Auto Route » Stop command.
  2. All Autorouter event and routing information will appear as messages in the Messages panel.

 

Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.

Contact Us

Contact our corporate or local offices directly.

You are reporting an issue with the following selected text
and/or image within the active document:
ALTIUM DESIGNER FREE TRIAL
Altium Designer Free Trial
Let’s get started. First off, are you or your organization already using Altium Designer?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

In that case, why do you need an evaluation license?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Got it. You actually don’t need an evaluation license for that.

Click the button below to download the latest Altium Designer installer.

Download Altium Designer Installer

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Please fill out the form below to get a quote for a new seat of Altium Designer.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

If you are on Altium Subscription, you don’t need an evaluation license.

If you are not an active Altium Subscription member, please fill out the form below to get your free trial.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Why are you looking to evaluate Altium Designer?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

You came to the right place! Please fill out the form below to get your free trial started.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Great News!

Valid students can get their very own 6-month Altium Designer Student License for FREE! Just fill out the form below to request your Student License today.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Got it. You can download a free Altium Designer Viewer license which is valid for a 6 months.

Please fill out the form below to request one.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

That’s great! Making things is awesome. We have the perfect program for you.

Upverter is a free community-driven platform designed specifically to meet the needs of makers like you.

Click here to give it a try!

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Got it. You can download a free Altium Designer Viewer license which is valid for a 6 months.

Please fill out the form below to request one.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.