Net Classes explanation

Software
1

is there any short clear explanation about this for example a video showing what its about and how to use it? long ago I used eagle and it was simple, can it be simple in kicad too?

2

Net classes are quite simple, but you do have to apply them properly.

First, open: PCB Editor / File / Board Setup / Design Rules / Net Classes

image
image1076×552 60.3 KB

In the top you see a matrix with dimensions (clearance, Track width, via sizes etc) and at the left most a list of names. So this screenshot has two net classes Default and Power.

Once you have a few named net classes, you can assign nets to these. (Usually in combination with labels used in the schematic.

Combined:

  1. Use labels to give names to nets.
  2. Set up the net classes and their dimensions.
  3. Use Schematic Editor / File / Schematic Setup / Project / Net Classes to make links between the (labeled) nets and the Net classes.
  4. Alternatively, you can use Schematic Editor / Place / Add Net Class Directive to directly assign net class names to nets on the schematic, but if you use a lot of these this becomes a bit messy.
  5. All nets that are not explicity put into a net class, are automatically part of the Default net class.

In KiCad V9 it’s apparently possible to assign multiple net classes to a net. I’m not exactly sure how this works (I’m still on V8). I assume that this only has an effect if certain sizes in the net classes themselves are not defined in all of the net classes. (This also implies some kind of priority).

3

thanks Paul, I did what you describe and as “power” I made the PCB track 1.5mm to test it but when routing the tracks for “power” it becomes same as “default”

I also run 8.0.9 and this net class setting is not working but when open the project in 9.x or 9.9.9 net class working the way you describe but I don’t want to upgrade projects to 9.x yet

4
  1. Are you sure you’ve added the correct nests to that netclass? You have to use the patterns in Schematic Editor / File / Schematic Setup / Project / Net Classes In the screenshot below “+*” means any net starting with a plus. In the center column you select the net class for your pattern, and then KiCad shows in the Nets matching box to the right the list of nets that match the pattern in the first column. In this case the “+24V” net has become a part of the Power net class.

image
image983×632 59.8 KB

  1. Additionally, you also have to keep track of the three menu items indicated below. Depending on their status, it’s possible netclass settings are ignored and another method for selecting the track width is used.
    image

  2. Also remember that changing netclass settings does not change existing tracks. It only applies to new track segments.

  3. Track segment properties can also be changed with: PCB Editor / Edit / Edit Track & Via Properties.

I am also still using KiCad V8. V9 is apparently a bit different again, but I have not used it yet. You can upload a small dummy / test project if you can’t figure it out, then I (or someone else) can have a quick look to see what setting you missed.

5

thanks again, guess what, after restarting kicad 8 net class settings works! (I don’t use pattern texts as I don’t understand it). net classes is a bit messed up/hard to understand in this app. btw, some years ago it was a YouTube channel Contextual Electronics who made easy to understand kicad videos. did they stop and or then did any other continue?