Create a routing desing rule for connection - Page 1
Forum section: electronics / general

author: Dartherick
author_rank: Newbie
timestamp: November 09, 2022, 01:13:11 pm
content: Hello Everyone,I would like to create a routing design rule (width) for a connection in my PCB in altium designer 22. Does anybody know how to do it?https://www.altium.com/documentation/altium-designer/pcb-connection?version=21Regards,

author: ajb
author_rank: Super Contributor
timestamp: November 09, 2022, 04:00:12 pm
content: There are many ways to do this depending on what exactly you want to do. Terms you should look for in the documentation are inboldbelow.From the PCB Editor, select Design > Rules to edit the existing rules or add new ones. If you want to set a minimum (and/or maximum) routing width, you can create a singlerouting width rule(or edit the one that's already there) that will apply to the entire PCB. As you'll see, there are many categories and types of rules (your PCB file may not have all types defined), and you'll want to become familiar with many of them to get the most out of Altium.If you want to apply a rule to a specific net, you can create a routing width rule that targets that specificnet name. If you want to apply a rule to a whole set of nets, you can define anet classto contain those nets, and create a rule targeting that net class. Net (and other) classes can be created and edited in theObject Class Explorer, but it's usually better to usedirective objects in the schematic to assign nets to their net class (you can also use directives to directly apply rules to the net from the schematic, although this is harder to maintain). If you want to apply a rule to a specific segment of a net, for example from one specific pin to another within the net, then you can define anxSignalin the PCB pane and create a rule targeting that xSignal or thexSignal Class(xSignals are generally meant for high speed routing, but you could use them for other things). You can do more complex targeting of rules by constructing aquerythat defines what objects the rule should affect. Altium's query language is clunky and inconsistent, so for complex applications you may want to use thePCB Filterpane to develop a query semi-interactively and then copy and paste it into the rule. Note that if an object is covered by more than one rule of a given type (for example, more than one routing width rule) you will need to use thePrioritiesbutton in the Rules Editor to ensure the rules are applied in the correct order.Note that most rules can be targeted at different objects using these or similar methods, although different things will make sense for different rules. Understanding the query system can make for very powerful rulesets, although there are some limitations and weird corner cases. Rules can be imported and exported, or saved as part of a PCB template file for future use so you don't have to go through all of this from scratch on every project.Design rules can get very complicated, especially with complex queries involved, and Altium is far from the most consistent or reliable piece of software in the world, so if you need more specific help with a challenging rule situation, please let us know what you're trying to do.