[kicad-users] Assign stitching vias to a net?

[[e-mail] [kicad-users]]

Is there a way to assign a via to a net? For example, when dropping "stitching vias" into a copper pour ("zone"), I need the via to take on the zone's net name. Currently I have been running a trace around the board, adding vias as I go. But I've found that this invites a nasty little error where removing one trace in that path causes all of the vias to revert to "unassigned". They cannot be "reassigned" to the original net, so I have to go around and delete them all, as well as the traces, and start over.
There should be a way to drop these stitching vias and keep them assigned to a net without having to route.
Is there a way?

[Pedro Martin [e-mail] [kicad-users]]

Hi Dan,

Not yet. It is under development.

There are some workarounds.
I route a track that will be overlapped by the zone after filling.

Other people make a component in the schematic lets say a 4 pin
component with all p4 pins connected to the same net. Then, they assign
to this component a 2x2 hole footprint.

With create array (Opengl canvas), place as many of those footprints as
needed.

Regards,
Pedro.

Post by dan-***@austin.rr.com [kicad-users]
Is there a way to assign a via to a net? For example, when dropping
"stitching vias" into a copper pour ("zone"), I need the via to take on
the zone's net name. Currently I have been running a trace around the
board, adding vias as I go. But I've found that this invites a nasty
little error where removing one trace in that path causes all of the
vias to revert to "unassigned". They cannot be "reassigned" to the
original net, so I have to go around and delete them all, as well as the
traces, and start over.
There should be a way to drop these stitching vias and keep them
assigned to a net without having to route.
Is there a way?

['[e-mail]' [e-mail] [kicad-users]]

I made a via "part" that I put on the board and when you click it,
choose the PAD in stead of the FOOTPRINT and you can add a netname like
GND. duplicate the footprint to place them where you want. set your grid
coarse enough to line them.

Post by dan-***@austin.rr.com [kicad-users]
Is there a way to assign a via to a net? For example, when dropping
"stitching vias" into a copper pour ("zone"), I need the via to take on
the zone's net name. Currently I have been running a trace around the
board, adding vias as I go. But I've found that this invites a nasty
little error where removing one trace in that path causes all of the
vias to revert to "unassigned". They cannot be "reassigned" to the
original net, so I have to go around and delete them all, as well as the
traces, and start over.
There should be a way to drop these stitching vias and keep them
assigned to a net without having to route.
Is there a way?

[[e-mail] [kicad-users]]

Thanks for everyone's replies. I like the via component. I just made one and it looks like it will work fine. The only problem I see is that it will have thermal reliefs, like any other pad. When you run a trace with vias it floods over them - for some reason. If they make a "stitching via" tool at some point, it would be nice for the "zone" settings to include "flood over vias".

['[e-mail]' [e-mail] [kicad-users]]

well, you can already. :-) in the pad properties in footprint editor,
click on the tab: "Local clearance and settings". set pad connection to
solid.

[x] Done

Post by dan-***@austin.rr.com [kicad-users]
Thanks for everyone's replies. I like the via component. I just made one
and it looks like it will work fine. The only problem I see is that it
will have thermal reliefs, like any other pad. When you run a trace with
vias it floods over them - for some reason. If they make a "stitching
via" tool at some point, it would be nice for the "zone" settings to
include "flood over vias".

[[e-mail] [kicad-users]]

Sweeeeeet!