HQG or "High Quality Ground" or "Star Ground"

[Scott_Cox]

Hello

I create audio equipment that uses what is commonly referred to as a HQG or “star” ground to prevent ground loops from occurring in design and use. What I am looking at myself is that I use 3 different copper pours to facilitate grounding of separate circuits etc… Usually I use one for earth, one for the digital components and another for the analog side of things. Then, after meticulously designing each of these, I like to join them at one particular point. The problem that I have is that each of these needs to be labeled with a different net to keep them separate, then when doing this, it becomes impossible to join them on the board in practice. What i used to do using the older versions of KiCAD is design everything and get it to the final point before exporting, then I would disable the DRC and place a track over the grounds to connect them, then export the Gerbers. In the nightly versions of KiCAD, I havent found a solution for this feature that I would like. In this, I would like to get some opinions of potential solutions. What I would really like would be something like a special pad that would allow me to join multiple nets without complaining. Almost like a special part or something that is specifically designed as a “star” ground. I have a PCB mount AC connector with an ‘earth’ pin on it in which I would like to use for a purpose like this, however I don’t have even a hack for doing this. RIght now I have to use resistor footprints with a short in place to create this, however I would really like to not have to do this.

Any ideas?
Thanks
S

[John_Pateman]

Have you explored the ‘net ties’? These allow you to join nets at a specific point.

EDIT Here is an example;

[Scott_Cox]

thanks
what library is the symbol in?
I have to cherry pick symbols because I use all my own for the most part

THanks
S

[John_Pateman]

For KiCad 5.1.x (and, I believe the same applies for 5.99 -> future 6) you can find the Net Ties in the ‘Device’ library.

There area variety of associated footprints in the ‘NetTie’ footprint directory.

[Scott_Cox]

Ok,

So for a “tee” such as your own, the usage basically shows as three pads that you can connect together without a physical jumper? If one uses an smd solution, is it three stacked pads?

Thanks

[paulvdh]

Apparently you’re reacting to John’s posts without having looked at net ties in KiCad itself.
There is a schematics symbol library with a bunch of different Net-Ties as you can see in John’s screenshot, and for the footprints there are variants with both SMT and THT pads, and if that is not enough, you can easily use one as an example to make your own.

A Net-Tie footprint is a few pads with graphics copper. The pads provide the attachment points for the different nets, and the graphics copper connects them.

There is one extra thing for the net ties.
It has to have the “net tie” name in the Footprint name, Description, or Keywords section in the footprint properties (I don’t know which). This is a trigger for the DRC to not flag the graphics copper overlapping with pads as an error.

[Scott_Cox]

Thanks guys

Got it to work!
S

[eelik]

@paulvdh

It has to have the “net tie” name in the Footprint name, Description, or Keywords section in the footprint properties (I don’t know which).

bool IsNetTie() const
{
    return GetKeywords().StartsWith( wxT( "net tie" ) );
}