KiCAD 7.0, Net Class for an Eagle Convert

[mprowe]

Hi,
As a long-time Eagle user, I’m finding it very difficult to use/understand Net Classes in KiCAD.
Having spent days trawling the web, all I have learnt is that Net Classes in Version 7 is very different to earlier versions. But as I have not used them either, that fact doesn’t move me very far forward.

What is the workflow needed to define a handful of nets to have 5mm wide tracks?

Regards, Martin

[mf_ibfeew]

in short (from memory, so could have forget some points):

• schematic editor → schematic setup–>project–>netclasses: define (“Add”-button) some netclasses (for instance: “netclass_5mm”). The parameters in this dialog are only for graphical distinction of the netclass in the schematic - so could be left on default
• than in schematic editor: as a start there are two options to assign netclasses (decide for one and try to stick with that workflow)
  • assign netclasses graphically: add a netclass-directive (right toolbar) to every net (only nets you want inside netclass_5mm)
  • or assign a label to every net, than RMB-click–>context-menu–>assign-netclass command. With this way the specific net is added to the (previoussly used) netclass dialog (you can look later)
• save schematic
• update board from schematic → now the netclass-assignment is transferred to the board
• borad setup–>design rules–>net classes: here you see the already defined netclassed, and now you can change the clearance, minimal_width and similar parameters for these netclass

In long: look at kicad-documentation: Schematic Editor | 7.0 | English | Documentation | KiCad

addition:
if you want something like the eagle-clearance-matrix: than you have to individually add special custom rules for every netclass1<–>netclass2 combination. These custom rules are added in board-setup–>Design rules–>custom rules. There is link to syntax-help in this dialog, with examples. More instructions for custom rules can also be found on the micad manual (documentation).

[mprowe]

Thank you, I think I’ve got that bit sorted now.
Sorry for the delay in acknowledging - been away.

I have now fallen into another problem! These wide (high current) tracks are backed up with filled zones. To join the track on the F.Cu with the polygon on the B.Cu, I would normally add two (or more) strings of vias.
It seems that these vias take on the width of the track they are connected too. Thus greatly enlarging the 5mm track! Can this be avoided?
I have tried setting a specific via size in the “board Setup | Pre-defined Size” but that has not worked.

Regards, M.

[mf_ibfeew]

It seems that these vias take on the width of the track they are connected too. Thus greatly enlarging the 5mm track! Can this be avoided?

I need a different explanantion (or better a picture or movie), I don’t understand this sentence.

I have tried setting a specific via size in the “board Setup | Pre-defined Size” but that has not worked.

This was already a good first step. in summary you have to:

• first set some useful via-sizes (along with useful track-width-values) in board Setup–>Pre-defined Sizes. My standard values in this dialog is (as example):
  • track-width 0.15mm-0.2mm-0.3mm-0.5mm-1.0mm-2.0mm
  • via: 0.6-0.2mm / 0.7-0.3mm / 0.8-0.4mm / 1.0-0.6mm / 1.2-0.8mm / 1.5-1.0mm / 3-2.0mm
• set the via-size / via-hole parameter for the netclass
• than before adding a new via: choose the right setting in the via-dropdown (below top toolbar)

[mprowe]

@mf_ibfeew

I need a different explanation (or better a picture or movie), I don’t understand this sentence.

Thank you very much for taking the time to help me with this. Greatly appreciated.
My skills are definitely not up to providing a video! Will the original project help?

The track (/IP_PT) is a mock-up. I have not been able to make this in KiCAD.
Tracks /IP+ and /IP- are the “work in progress”.

And here is the archive of my project:
ACS758LCB-050U_Ammeter.zip (65.1 KB)

Regards, M.