I’m designing an RF pcb and i need to add as much as possible a vias to connect the two ground planes.
I didn’t find a tools inside Kicad to make this happen automatically,
i tried to add a via then i fill the copper planes but unfortunately the via is kept away from the filled zone like this :
so the only trick that let this happen is to connect the via with a GND pad to be considered by the kicad as GND via :
after filling the zone
it works fine but just annoying to add the via like this way and its hard to keep the via alligned and keeping them at equal distance.
is there any other solution in KICAD to make this happen ?
We just discussed this over in this thread: Protip: nicer via stitching - #32 by ozindfw
I also made a video showing how to implement Chris’s nicer via stitching. It goes SO much faster
How do I get stitching vias to remain in the layout when using the “Update PCB from schematics” in the nightly builds?
Open the footprint properties of your via footprint and set the move and place option to lock footprint. (Press e while your mouse is above the footprint to open the properties window.)
If you have a lot of them already placed you can use a text editor to get this done faster. (Make a backup first because you might screw this up.)
You can use also @jsreynaud via stitching kicad plugin: https://github.com/jsreynaud/kicad-action-scripts
It doesn’t have an option to lock generated vias but it’s not really necessary because you can regenerate when needed pretty easy and fast.
I’m very satisfied with it and it’s really a great addition to KiCAD imho. Big thanks to @jsreynaud for providing this.
Hello ChrisGammell, (Or anyone who can help. Your video is great and it works well. Except! CTRL+D does not work on my version of Pcbnew (Version 4.0.7), and the only way I can duplicate is with the mouse and wade through the clicks to select duplicate. This is extremely slow to do for hundreds of holes. Is this a bug? I can select other components, but not this VIA-0.6 pad.
Cheers, Michael (in New Zealand)
Micheal, what OS are you using?
Are you in open gl canvas? The array tool only exists in open gl.
Switching canvas is done via the view menu. (F11 is the shortcut to switch to open gl)
I’m using daily builds and vias work well with copper zones. The zone must have the proper net, of course. Then when I put in a via it will usually get the right net from the track into which I’m putting it. For example, I have GND plane in back side and 5V track in front side. I add a via to the track and it works normally. But if I have a GND track and add a via there it will be connected directly and wholly to the back side GND zone without problems. Sometimes the net is wrong (if there are many/none possibilities nearby) but it can be changed from the via’s properties. Also two zones can be connected just by adding vias.
However, I haven’t even tried to get them automatically aligned, kept or arranged when connecting zones.
Rene_Poschl - Fantastic! I Love it, thank you so much. It works in open-gl well and this will save hours… I am impressed with KiCad. As a first time user with some complex boards, it is pretty easy to use.
I would like to see in ‘add tracks and vias’ mode the possibility to use the Move and Rotate keys, as it is a few extra clicks to get out and back. I realise a click starts a track, but after a M or R the first click could place, then another clisk start the track…
eelik Thanks for your comment…
Cheers guys from New Zealand, Michael (Wisdom Counselling .co.nz / Wise Enterprises)
Another little help please friends. I stitched up the board with vias, but made an error in not having the mask right. I edited the footprint, then tried to ‘Exchange Footprints’ in default (F9) mode, but it does not work - ie the pop up does not come up. It works with other components however. Ideas? M
For single pad footprints it can be a bit tricky to get the properties dialog of the footprint instead of the one for the pad.
Maybe try switching to the legacy canvas for that. (but it should work in open gl as well. when hovering above the pad press e. The clarification dialog should come up asking if you want the properties dialog for the pad or the footprint. You want the properties dialog for the footprint.)
It helps if you have graphics on some graphics layer. This makes selecting the footprint easier sometimes.
1º make Front Ground plane -> name it GND. (rignt click over plane edge,-> properties and name NET as GND)
2º make Back Ground plane.-> name it GND.
3º Fill both ground planes.
4º Make via over BOTH ground planes.
Via will automatically be named as GND, and will not be isolated from GND planes.
This only works in version 5. The original poster explicitly wrote that they are using version 4.
The original post dates back to 2015… That’s why it has been asked why old threads can be resurrected while new ones will be automatically closed after some time.