Hi Mattylad,
I noticed your question and dug up an article about this topic, please see below.
There are several approaches to defining rules from schematic. The most common way is to just define net classes and then define the specific rules for each class within the PCB document. This way the PCB designer can specify the exact rules for width, clearance, without having to go back to the schematic each time.
Place a Net Class directive and attach it to a net on the schematic, then modify it:
- The Name is seen on the schematic but isn't transferred so give it a name (or leave as Net Class).
- The parameter has a special name called ClassName. Change the value from Undefined to the name of the Class you want in PCB, e.g. Power.
- Click OK
Copy the directive and paste it on each other net you'd like to be included in the same net class.
(You can also attach a directive to a Blanket, if you'd like to include every net within a specific area of a schematic.)
Design > Update the PCB. The Class will be created and it will include each net you added in the schematic.
Over to the PCB!
----------------
Design rules can be setup and used in many ways, so I'm going to show you an example of usage that I've been teaching students for the past few years. Others may have different approaches that are perhaps a little simpler, but I show this method because it highlights the various features built in and shows the way they can be used:
Create a Width Rule
-------------------
In the PCB menu (Design > Rules) open the Design Rules dialog and create a new Width rule. Notice the new rule is named Width_1 and is set to Priority 1. This rule will be acted on first because it has the highest priority, so you can scope it to your new Class, then the other more general rules will be applied afterwards.
Rename the rule to something sensible like Width_Power (or whatever your Class is called).
Set "Where The Object Matches" to Net Class and choose Power from the list.
Set different widths for Min Width, Preferred Size and Max Width, i.e. the common sizes you're likely to use on the board.
(Repeat for Clearance rules)
Switch Sizes on the Fly
-----------------------
When interactively routing (i.e. in Altium Designer press PT to route a track), while the track is being placed you can press several shortcut keys to affect the track with and other actions. To see a list of them, press the ~ button (above TAB) while placing the track.
Design Rules can be setup to have a different track width for Minimum, Preferred, or Maximum. If you take the time to setup the rules properly then you can save a lot of time when routing by changing the width "source" during routing, to toggle between the three sizes you defined for Minimum, Preferred, or Maximum. The shortcut key for this is 3.
Watch the Status Bar at the bottom of the screen, which will cycle from Rule Minimum; Rule Preferred; Rule Maximum; User Choice when pressing the 3 key.
When you're routing you sometimes want to just type in a width. In this case, this time press the Tab key and type in a number and that will be the width. The track width will no longer follow the rules described above, but will specify the width source as "User Choice".
The next time you route, the source will be remembered, either User Choice, Minimum, Preferred, or Maximum.
One more subtlety: If you start routing from a net that is already partially routed, e.g. create a T intersection with another track, the width of the new piece of track will conform to the existing track if the source is set to User Choice at the time. Otherwise it will be whatever source you see on the status bar.
Pressing Shift + W while routing will let you choose from a list of sizes, similar to pressing the Tab key and typing a size.
Vias
----
While routing, if you change layer, a via is automatically inserted. The same technique can be used, see below.
Pressing Tab while placing a Via from the menu only changes it for that instance. During interactive routing if you change layers such as by pressing * key or Shift+Ctrl+Mouse wheel then the automatically inserted via can be controlled by pressing Tab to specify a User Choice. This is also restrained by the RoutingVias design rule. Further control can be gained by specifying minimum, preferred and maximum sizes and using the 4 shortcut while the new via is inserted (watch the Status Bar cycle from Rule Minimum; Rule Preferred; Rule Maximum; User Choice). Pressing Tab will reset the setting to User Choice.
Also when interactive routing and inserting a via, pressing Shift + V will choose from the list of favorite via sizes (defined in Preferences > PCB Editor > Interactive Routing).
Best regards,
James Harriman
Altium