Automated Board Layout using the Situs Topological Autorouter

Parent page: The Routing

Routing the connections on a printed circuit board is a complex and time-consuming activity. On large or dense boards, the process of routing can take a designer considerable time, something that an autorouter can assist with.

Altium NEXUS's Situs™ autorouter uses a topological-analysis technique to map the board space, which, unlike geometric or shape-based mapping, is not dependent on obstacle shape or coordinates. Topological mapping provides greater flexibility in route path determination and unrestricted routing direction.

Autorouting the Board

The Situs Topological Router brings a new approach to the autorouting challenge. It uses advanced topological mapping first to define the routing path, then calls on a variety of proven routing algorithms to convert this 'human-like' path to a high-quality route. As an integral part of the PCB Editor, it follows the PCB electrical and routing rule definitions.

Board Setup

While Situs is straightforward to set up and run, there are certain points you should be aware of to produce optimal routing.

Component Placement

Ultimately, the component placement has the most significant impact on routing performance. Altium NEXUS's PCB Editor includes a number of tools, such as dynamically optimized connection lines, that allow you to fine tune component placement. The optimal component placement is when the connection lines are as short and least 'tangled' as possible.

Other good design practices include placing components so their pads are on a regular grid (to maximize the amount of free space between the pads for routing), placing similar sized surface mount components exactly opposite each other on double sided boards, and consulting device manufacturers datasheets for decoupling placement guidelines. This is not a complete list of placement considerations, simply a few suggestions.

Keepouts

The router requires a closed boundary, made up of placed keepout objects. Typically, this boundary follows the edge of the board. Placed objects will obey the applicable clearance rule to ensure that they remain a suitable distance away from this boundary, to satisfy any mechanical or electrical clearance requirements that the design may have. The router will also obey keepouts within this outer boundary, as well as layer-specific keepouts.

You can create a closed boundary that follows the edge of the board shape, using the Line/Arc Primitives from Board Shape dialog. For more information about keepouts, see Object Specific Keepouts.

Polygon Pours

Polygon (or copper) pours can be either solid (filled with one or more copper regions) or hatched (constructed from tracks and arcs). A medium to large hatched polygon pour includes a large number of tracks and arcs. While the router can route a board that includes such polygon pours, the sheer number of objects they introduce increases the complexity of the routing process.

Typically you should only place polygon pours prior to routing if they are required, for example, they are being used to construct unusually shaped pre-routing, perhaps the incoming mains routing or a critical ground region. Otherwise it is preferable that polygon pours be added to the design once routing is complete.

Is it Routable?

An autorouter is a human attempt to understand and model the routing process, then replicate that process automatically. If the board contains an area that can not be routed by hand, then it will not be autorouted either. If the router is continually failing on a component or a section of the board then you should attempt to route it interactively. It may be that there are placement or rule configuration issues that make it impossible to route at all.

Pre-routing

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.

Differential pairs nets must be manually routed and locked before using the autorouter. If you do not so this, the routing is very likely to change and alter the signal integrity of the differential pair.

Configuring the Design Rules

Make sure the routing design rules are appropriate to the board technology you are using. Poorly targeted or inappropriate design rules can lead to very poor autorouting performance. Note that the router obeys all Electrical and Routing design rules, except the Routing Corners rule.

Rules are defined in the PCB Rules and Constraints Editor dialog (Design » Rules), which can be accessed directly from the Situs Routing Strategies dialog.

If a rule includes Minimum, Preferred and Maximum values, the autorouter will use the Preferred value.

The most important rules are the Width and Clearance rules. These routing technology settings define how tightly the routing can be 'packed'. Selecting these is a balancing process - the wider the tracks and bigger the clearance, the easier it is to fabricate the board; versus the narrower the tracks and clearances, the easier it is to route the board. It is advisable to consult your fabricator to establish their 'price points' for routing widths and clearances, those values which if you go below will result in lower fabrication yields and higher priced PCBs. As well as satisfying the electrical requirements of the design, the routing technology should also be chosen to suit the component technology, to allow each pin to be routed to.

The third rule that is part of the routing technology is the Routing Via Style. It should also be selected to suit the track and clearances being used, while considering the fabrication costs of the chosen hole size and annular ring.

You should also avoid excessive or unnecessary rules - the more rules, the more processing time, the slower the routing. Rules can be disabled if not required for autorouting.

Routing Width

Ensure there is a Routing Width rule with a Query of All (a default rule), and that the Preferred setting is appropriate for the most common routing width you require. Make sure that this width, in combination with the appropriate clearance rule, allows all pads to be routed to. Configure additional routing width rules for nets that require wider or narrower routing.

If there are fine pitch components that have pins on nets with wider routing widths - for example, power nets - test route out from a power pin and also route out the pin on either side to ensure that it is physically possible to route these pins.

Clearance Constraint

Check for special clearance requirements, such as fine pitch components whose pads are closer than the standard board clearances. These can be catered for using a suitably scoped and prioritized design rule. Note that while you can define a rule to target a footprint, it will not target the routing that connects to that footprint. As just mentioned in the Routing Width section, test route to ensure that the component pins are routable.

Routing Via Style

Ensure there is a Routing Via Style rule with a Query of All and that the preferred setting is appropriate. Include higher priority rules for those nets that need a different via style than the default rule.

Altium NEXUS supports blind and buried vias, when these will be used is determined by the layer swaps allowed by the Via Types defined in the Layer Stack Manager (Design » Layer Stack Manager). Like interactive routing, when the autorouter switches between two layers it checks the current Via Type definitions - if these layers are defined as a blind or buried layer pair then the via that is placed will have these layers as its start and end layers. It is important to understand the restrictions to using blind/buried vias; they should only be used in consultation with your fabricator. As well as the restrictions imposed by the fabrication stackup technology, there are also reliability and testing accessibility considerations. Some designers consider it better to add more routing layers than to use blind/buried vias.

Routing Layers

Ensure there is a Routing Layers rule with a query of All. All enabled signal layers (defined in the layer stack) will be listed. Enable the layers upon which you wish to allow routing as required. Include higher priority rules for nets that you want to have routed on specific layers only.

Should you wish to exclude a particular net (or class of nets) from being routed by the autorouter, define a Routing Layer rule targeting that net or net class and, in the Constraints region for that rule, ensure that the Allow Routing option for each enabled signal layer is disabled. The priority for the rule must be higher than that of the default rule (the one with a query of All).

Layer Directions

Layer routing direction is specified in the Layer Directions dialog, which is accessed from the Situs Routing Strategies dialog. All enabled signal layers (defined in the layer stack) will be listed. Choose appropriate layer directions to suit the flow of the connection lines. Situs uses topological mapping to define routing paths, so it is not constrained to route horizontally and vertically. Typically it is best to have outer layers as horizontal and vertical. If, however, you have a multi-layer board with a large number of connections at a '2 O'clock' angle, then set one or more internal layers to have this as the preferred routing direction. The Layer Patterns pass in particular makes use of this information, and choosing the right direction can make a significant difference to routing performance in terms of both time and quality. Note that when you use angled layers you do not need to have a partner layer running at 90 degrees to this layer, since the router will typically route horizontally or vertically if it needs to avoid an obstacle on an angled layer.

Avoid using the Any direction - the layer that is chosen to route a connection on is based on how closely the connection is aligned with the layer direction, so this layer becomes the layer of last resort. The Any direction is typically only used on single-sided boards.

Routing Priority

Use the Routing Priority rules to set a higher priority on difficult nets, or those that you want to have the cleanest routing.

SMD Fanout Control

The query system includes keywords that specifically target the different surface mount component packages including IsLCC (Leadless Chip Carrier), IsSOIC (Small Outline IC), and IsBGA (Ball Grid Array). Default rules are automatically created for the most common packages and since fanout passes are run early in the autorouting process, there is little penalty in keeping rules that do not apply to any components. You should have at least one SMD fanout control design rule if there are surface mount components on the board - a suitable query for a single rule targeting all surface mount components would be IsSMTComponent. For information on how each query keyword identifies a component package, open the Query Helper, type in the required keyword and press F1 .

The fanout rules include settings that control if the pads are to be fanned in or out, or a mixture of both. To help become familiar with the behavior of the Fanout Control rule attributes, the Route » Fanout » Component command can be run on any surface mount component that has no nets assigned to it. As well as using this to check how well a component fans out with the current routing technology defined in the board, you can also use it to fan out a component that you want to keep in a library as a pre-fanned out footprint. Once it is fanned out in the PCB workspace, copy and paste the component and the fanout tracks and vias into a library.

Rule Priorities

The precedence, or priority, of rules is defined by the designer. The rule priority is used to determine which rule to apply when an object is covered by more than one rule. If the priority is not set correctly, you may find that a rule is not being applied at all.

For example, if the rule with a query of InNet('VCC') has a lower priority than the rule with a query of All, then the All rule will be applied to the VCC net. Use the Priorities button in the PCB Rules and Constraints Editor dialog to access the Edit Rule Priorities dialog, from where priorities can be refined as necessary. Note that priority is not important when two rule scopes do not overlap (do not target the same objects). For example, it makes no difference which of these two rule scopes has a higher priority - InNet('VCC') or InNet('GND').

The Golden Rule

The most important step is to perform a design rule check (DRC) prior to starting the autorouter. When using the Route » Auto Route » Setup, or Route » Auto Route » All commands, Situs conducts its own pre-routing analysis and presents the results as a report in the Situs Routing Strategies dialog.

Make sure that the Routing Setup Report is clean before starting the autorouter.

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 in the better preparation of the design for 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.

Check all errors, warnings and hints to understand what potential problems the autorouter will face.

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.

Tips on Running the Router

• The Autorouter commands are in the Route » Auto Route sub-menu.
• Both the Route » Auto Route » All and Route » Auto Route » Setup commands open the Situs Routing Strategies dialog, the difference is that when you choose All, the dialog includes a Route All button.
• Don't be afraid to experiment. If the results 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.
• As you experiment with the router - creating your own strategies to control the order of passes, changing the number of vias with the Via control, changing the routing layer directions, constraining the router to orthogonal routes only, and so on - keep notes of the combinations that you have tried. That way you will be able to identify and reuse which configurations work best with your designs.
• Run fanout passes on their own first and assess the quality. You may need to manually fanout any problem areas.

Summary of the Routing Passes and Routing Strategies

Currently defined routing strategies are listed in the lower region of the Situs Routing Strategies dialog. Click the Add button to access the Situs Strategy Editor dialog, from where you can specify the passes to be included in a new strategy. Alternatively, use the Duplicate button to duplicate an existing strategy, and then edit it as required.

Example of editing a duplicated strategy.

The following routing passes are available. The passes can be used in any order, as a guide examine an existing strategy to see the order of passes.

See Also