I could use some help with a Kicad v9. It’s getting beyond my basic knowledge, but I
hope to learn from it.
It seems much advice on the internet is outdated referring to old versions.
But I need step by step guidance on how to go about changing track widths.
In Schematic Setup I have set net classes to Power (0.508 mm) and default (0.3048 mm). Why those sizes I do not know, but why does it say wire thickness ?? then what is Bus thickness ??
I have set Net Class - Power to include VCC VDD and GNDREF, with nothing for default net class.
In the schematic it shows wires set to VCC and GNDREF, with all others left to be default.
These thicknesses are your preferences for your schematic drawing. To make your schematic easier to read, if you wish, you can have different line/bus/whatever widths and colors. These settings, as the title reads, are for the Schematic only. They have nothing to do with the PCB.
To set your track widths using net classes, you first update your PCB from your Schematic then open your PCB and go to File > Board Setup > Net Classes and fill in all the details much as you did for your wires etc. in your schematic.
ERC is not very smart. It can be useful for finding drawing mistakes, not design mistakes. One of its tests is that inputs must have outputs connected to each other. One reason being to help prevent different outputs being connected to each other because of a wiring mistake.
If you are happy with your drawing and don’t like the warnings, turn whatever warnings you don’t like off at Schematic Setup > Electrical Rules > Violation Severity.
Much more information for the use of Kicad can be found at https://docs.kicad.org/. This information source is kept up to date and is vastly superior to most of the other information on the internet.
You can also show these columns in the net class settings in the schematic editor by right-clicking on the column headers. That will show a list of all net class settings, and you can add the PCB ones to the displayed list.
Thanks, I’d forgotten that function.
Also, there is no need to update the PCB before going to the Net Classes in the Board setup, but the OP seemed a bit lost and I thought that may help.
Line Width and Line Style are in the schematic, and only a visual aid. Track Width and Clearance are for the tracks on the PCB, but setting up these in the net classes does not change anything on the PCB. The resulst are not visual immediately.
The three buttons marked below influence what properties are used for new tracks.
In the PCB Editor go to File > Design Rules > Predefined Sizes OR click on the triangle in the “Track: use netclass width” box (red arrow).
Use the + (magenta arrow) to add all the track widths you want for this project (yellow arrow)
Hover your mouse over the U shaped icon (green arrow) and take note of its purpose. This is worth remembering.
To route a track of a certain width click the “Track: use netclass width” box (red arrow), select the track width you require from your created list then route using the Route Track icon or hotkey X.
A quicker and more efficient way to select your track width is to use hotkeys to select your track width.
Open your hotkey list (Preferences > Hotkeys) and type “track” into the search line (cyan arrow).
Note the two hotkeys in the red rectangle. These hotkeys scroll the track widths in your list with the result showing in the “Track: use netclass width” box.
So, to route various width tracks, or change track widths as you route, on your PCB, after setup, all you need are the three hotkeys:
X, W & Shift + W.
Working with the Pre-defined sizes is indeed also an option to work with different track widths, but the netclasses would still be the logical first choice to learn. But both these methods work only while drawing new tracks. If you want to change track width after they have been drawn, you have to modify the tracks explicitly. There is no automated mechanism that changes track width after they have been laid.
I am using netclass approach to have bigger clearance for some nets as all net have the same voltage so clearance dependence on net seems logical.
I have never tried to use netclass approach to track width as track width depends on current and you don’t have the same current in all net tracks. Consider VCC. You have tracks supplying power (let say 1A) to several places at PCB, but you also have tracks to pull-up 47k resistors (0.0001A).
Using a few net classes and different widths for them is an easy and quick way to automatically use different track widths for “signals” and “power”.
Yes, true, but the vast majority of the tracks of the “power” net will benefit from more copper, while an occasional pullup resistor with a “too wide” track is harmless. And you can always overrule the netclass width. Netclass width is not asserted during DRC, and narrower tracks to (for example) pullup resistors do not cause DRC violations.
On a sidenote, I find it useful during fault finding on a PCB to have a wider track width for power. It helps with identifying the purpose of tracks without having to look up the pin numbers in the schematic each time.
