EEVblog Electronics Community Forum
Electronics => PCB/EDA/CAD => KiCad => Topic started by: timsu on February 10, 2017, 09:07:47 pm
-
Hello,
how do you do via stitching in KiCad?
I don't need a huge amount of vias, just connect top and bottom plane together.
It seems there are two ways:
- Creating a footprint just containing a via
- drawing traces with vias all over the board
They both seem to make the board cluttered and don't seem to work with the remove unused track/footprints option on netlist import.
What is your workflow? What is the best way?
-
- Creating a footprint just containing a via
They both seem to make the board cluttered and don't seem to work with the remove unused track/footprints option on netlist import.
I use a separate single-pad footprint, usually tied to the GND net, that can be copied one-by-one or with the grid-copy tool. Together with GND filled zones it works ok.
I don't know if there's a solution to the remove-unused-footprints issue (i.e. since the stiching vias are not in the schematic/netlist you can't use remove-unused-footprints or your stiching vias will disappear).
see also:
https://forum.kicad.info/t/protip-nicer-via-stitching/1103
-
I use a separate single-pad footprint, usually tied to the GND net, that can be copied one-by-one or with the grid-copy tool. Together with GND filled zones it works ok.
I don't know if there's a solution to the remove-unused-footprints issue (i.e. since the stiching vias are not in the schematic/netlist you can't use remove-unused-footprints or your stiching vias will disappear).
see also:
https://forum.kicad.info/t/protip-nicer-via-stitching/1103
Doesn't that mean you won't be able to tent the vias unless you cover it in the footprint?
-
Doesn't that mean you won't be able to tent the vias unless you cover it in the footprint?
right. I think you could create a separate tented-via footprint and use that?
Some solution where the manually inserted via-footprint won't disappear during a netlist-update (that updates/adds/removes regular footprints) would be good.
-
https://www.youtube.com/watch?v=Hp5ngKtl7S4 (https://www.youtube.com/watch?v=Hp5ngKtl7S4)
ive tried this it works well enough for me , hope you find it helpful
regards Neil
-
Check out this great video to see the via stitching in Kicad. https://www.youtube.com/watch?v=Hp5ngKtl7S4 (https://www.youtube.com/watch?v=Hp5ngKtl7S4)
-
Here is a written description, for those who don't like to watch videos:
Open the footprint editor,
make a new footprint in a project-specific library or another library.
Call your footprint something like VIA-0.6mm.
Make the name and reference designator invisible.
Put in a circular pad, 0.3 hole size, 0.6mm overall size.
Specify all copper layers, un-check any other layers.
Change the pad connection to Solid in the Local Clearance and Settings tab.
Save the footprint into the library you chose.
Close the footprint editor.
Go back to Pcbnew.
Use the "Add footprints" button to drop in the via footprint wherever you want it on the board.
Select the Pad, not the entire footprint, and edit the properties.
In the Net Name: box, type GND or whatever your net is called.
Back at the PCB, Fill or Refill All Zones ("B" hotkey).
Now it becomes a stitching via.
Mouseover and Ctrl-D to duplicate it, or right-click and Create Array to make an array of them.
Adjust the parameters in the Create Array box as necessary to put your stitching vias where you want them.
-
This workaround is no longer required as version 5 has the option to add stitching vias directly (via tool in right toolbar).
-
I used this plugin for many time ago: https://github.com/jsreynaud/kicad-action-scripts
just put it in KiCad\share\kicad\scripting. Then open Pcbnew -> Tools -> External Plugins -> refresh and enjoy