Author Topic: Via Stitching - Best Practice  (Read 15165 times)

0 Members and 1 Guest are viewing this topic.

Offline timsuTopic starter

  • Contributor
  • Posts: 27
  • Country: de
Via Stitching - Best Practice
« 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?
 
The following users thanked this post: mmagin

Offline awallin

  • Frequent Contributor
  • **
  • Posts: 694
Re: Via Stitching - Best Practice
« Reply #1 on: February 11, 2017, 04:35:39 pm »
  • 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
« Last Edit: February 11, 2017, 07:30:06 pm by awallin »
 

Offline bentomo

  • Contributor
  • Posts: 37
Re: Via Stitching - Best Practice
« Reply #2 on: March 14, 2017, 05:06:03 pm »

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?
 

Offline awallin

  • Frequent Contributor
  • **
  • Posts: 694
Re: Via Stitching - Best Practice
« Reply #3 on: March 15, 2017, 06:10:39 am »
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.
 

Offline neil t

  • Regular Contributor
  • *
  • Posts: 77
  • Country: au
Re: Via Stitching - Best Practice
« Reply #4 on: March 15, 2017, 06:19:58 am »



ive tried this it works well enough for me , hope you find it helpful

regards Neil
 

Offline richardlawson1489

  • Regular Contributor
  • *
  • Posts: 124
  • Country: us
    • PCB Assembly
Re: Via Stitching - Best Practice
« Reply #5 on: March 15, 2017, 09:51:13 am »
Check out this great video to see the via stitching in Kicad.
 

Offline Clear as mud

  • Regular Contributor
  • *
  • Posts: 207
  • Country: us
    • Pax Electronics
Re: Via Stitching - Best Practice
« Reply #6 on: April 26, 2020, 06:15:17 pm »
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.
« Last Edit: April 26, 2020, 06:17:09 pm by Clear as mud »
 
The following users thanked this post: pierreraymondrondelle, I wanted a rude username

Offline poeschlr

  • Regular Contributor
  • *
  • Posts: 52
  • Country: at
  • Head of KiCad library; Writer of tutorials
Re: Via Stitching - Best Practice
« Reply #7 on: April 26, 2020, 09:28:08 pm »
This workaround is no longer required as version 5 has the option to add stitching vias directly (via tool in right toolbar).
 
The following users thanked this post: Clear as mud, Palmitoxico, SiliconWizard

Offline vunq.dx

  • Newbie
  • Posts: 1
  • Country: vn
Re: Via Stitching - Best Practice
« Reply #8 on: August 02, 2020, 03:12:28 pm »
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
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf