Via Stitching - Best Practice - Page 1
Forum section: electronics / general

author: timsu
author_rank: Contributor
timestamp: February 10, 2017, 09:07:47 pm
content: 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 viadrawing traces with vias all over the boardThey 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?

author: awallin
author_rank: Frequent Contributor
timestamp: February 11, 2017, 04:35:39 pm
content: Quote from: timsu on February 10, 2017, 09:07:47 pmI 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

author: bentomo
author_rank: Contributor
timestamp: March 14, 2017, 05:06:03 pm
content: Quote from: awallin on February 11, 2017, 04:35:39 pmDoesn't that mean you won't be able to tent the vias unless you cover it in the footprint?

author: awallin
author_rank: Frequent Contributor
timestamp: March 15, 2017, 06:10:39 am
content: Quote from: bentomo on March 14, 2017, 05:06:03 pmright. 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.

author: neil t
author_rank: Regular Contributor
timestamp: March 15, 2017, 06:19:58 am
content: ive tried this it works well enough for me , hope you find it helpfulregards Neil

author: richardlawson1489
author_rank: Regular Contributor
timestamp: March 15, 2017, 09:51:13 am
content: Check out this great video to see the via stitching in Kicad.

author: Clear as mud
author_rank: Regular Contributor
timestamp: April 26, 2020, 06:15:17 pm
content: 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.

author: poeschlr
author_rank: Regular Contributor
timestamp: April 26, 2020, 09:28:08 pm
content: This workaround is no longer required as version 5 has the option to add stitching vias directly (via tool in right toolbar).

author: vunq.dx
author_rank: Newbie
timestamp: August 02, 2020, 03:12:28 pm
content: I used this plugin for many time ago:https://github.com/jsreynaud/kicad-action-scriptsjust put it in KiCad\share\kicad\scripting. Then open Pcbnew -> Tools -> External Plugins -> refresh and enjoy