I’m new to KiCad and trying to understand the differences between KiCad and other tools I’ve used.
In other tools I’ve used I could define net properties like PCB copper trace width while in the schematic capture process. This information would then be conveyed to the PCB layout tool via the netlist file.
Does KiCad have a similar feature? I’m finding information about net classes in both the schematic editor and PCB editor, but they don’t seem to have the same attributes that can be defined/changed.
In the schematic editor the net class “wire thickness” only changes the appearance (thickness) as displayed on the screen.
How do I assign a copper trace width in the schematic editor?
True, but very short.
In KiCad the usage of net classes is divided over the schematic and PCB editor, and each programs has settings that are relevant for that part of the schematic / PCB design.
You can assign track widths to net classes in: PCB Editor / File / Board Setup / Design Rules / Net Classes.
OK, I now see the relationship between net class in the schematic editor and PCB editor.
Now for assigning a net class to a wire in the schematic editor. Are my only two options to use “Add a net label” or “Add a net class directive label”? If I use “Add a net label” the label shows up in my schematic even if I uncheck the Show and Show Name boxes. If I use “Add a net class directive label” I get the ball and stick attached to the wire and visible even if I uncheck the Show and Show Name boxes.
Can I hide the net label / Connection Name so they are not visible in my schematic?
In other words, I’d like to assign a wire a net class that has a PCB trace width associated with it (done in PCB editor), but not clutter the schematic view with net / connection names or the net class directive symbol.
Net labels and net class labels are different: only the second one puts nets in a class.
Nets should be labeled or have a net class directive attached in order to be added to a net class. You can’t hide net labels, but you can make them smaller if you want. However I recommend leaving them the default size and just spacing out your schematic more.
Net class directives are maybe the better way if you are assigning a net class to a small net (like, say the junction between 3 passive components) that you might not otherwise label. Net labels are the way to go if you are assigning net classes to a larger group of related signals (like, a data bus)
You can’t really do this. KiCad has a workflow where the schematic visually shows information about what nets or net classes wires are assigned to for the most part. It is standard practice to show connection names in KiCad schematics. If you are coming from a tool like EAGLE that supports a concept of “hidden connection names”, this is just a different paradigm that KiCad doesn’t use.
KiCad-Nightly (Going to be KiCad V8 soon) has a Schematic Editor / View / Show Directive Labels. You still have to place them, but you can easily hide them. You can even assign a hotkey to this toggle switch if you like. (It has none by default).
And there are also other tricks.
For example, you can make all nets of the “Default” netclass show as bright red, and then assign the “normal” green color to your own netclass. This way any net you missed an assignment for will show as red in your schematic. This gives visual feedback even if the directive labels are not visible.
all good replies from everyone.
Suggest if you must have, for example thick traces, create a NET CLASS in sch and assign these to those nets.
Then, create a rule in PCB for constraint( trace width ) matched against that NET CLASS.
You might need also a ZONE clearance constraint if its high voltage etc… So when you pour copper around those traces the clearances are automatically respected. PCB Rules are all about making your life easier.
When the one guy is both SCH and PCB it’s not so much of a problem , when PCB is a handover, this stuff has to be comprehensive.