Hello Community,
does anyone know how to create a catwalk (a partly filled area around the PCB for EMC improvements)? I don’t know if catwalk is the correct name, in my company everyone is just talking about a catwalk. In the catwalk will be placed a lot of vias (like a Faraday cage). Often the housing is conducted with the catwalk.
I added also a picture to make it more clear:
Thanks
Timo
You should be fine with ground pours (Filled Zones) and if you want to expose copper on the edges (to attatch EMC tape for example) draw a couple of polygons on the F.Mask and B.Mask layer in a way to make the shape you want.
If you don’t want to have a ground plane on a specific layer, you can use rule areas and set it to keep out copper fills. Hope that helps.
Thanks for you fast reply. How can i make circular arks with the ground pours?
I’m assuming that you have your board shape on the Edge.Cuts layer already.
Just draw a rectangle to encompass the entire PCB, areas outside the board edge will be automatically discarded, and you will get a nice round arcs on the ground plane.
You may have a look at here
@T1992 This may help.
I could have made the inner shape to have smaller Radius corners but, wanted to keep the Video file small so, I selected the both shapes… You’ll get the idea, though…
Oh, I drew the inner shape on a User layer only to make selection of it quicker (and hide the Fcu layer)
ADDED: I should have demo’s added Via’s… Place the Via’s before Filling the Zone but, you’ll want them to be in contact with the zone… do it how you want it… Both ways’s are shown in screenshot
I call it an ESD ring – surrounds the board edge to tie connector shells and such and catches the sparky-sparky events and dumps them back to battery/power-supply ground via a net-tie.
Kicad has no bezier curves, and arcs are super primitive, so it is challenging on an non-rectangular board to do it with traces. See my attempt to hack it:
But @blackcoffee’s technique looks like a good way to go.
A couple of my boards have this perimeter GND, made as a zone. I block the solder mask and use ENIG finish to contact a screening can.
Except one of the cat tails will cause a DRC violation! 
How do you block the solder mask (F.Cu Zone) in order to get the copper exposed?
You draw graphic items on one of the solder mask layers.
But I would like to do the same thing that David says he does. By using a Zone not a graphic item. A track without solder mask could be fine as well. In few words here’s what I need for example.
Not clear on what you want but, if just wanting a Mask that exposes the Cu, see below…
And, moving it back to see it in the Exposed Copper…
It’s easy to understand. Basically I would like to create tracks, polygons, zones, with exposed copper (no solder mask) on Top/Bottom. I think it should be much easier. At least in Altium it is: https://www.youtube.com/watch?v=L0m_qoBcjHk
I don’t have much patience for video tutorials, but in that youtube link he just draws lines over the existing tracks. You can just as easily draw graphic lines on the mask layer over tracks in KiCad. I do not see any significant difference.
An addition I would like to see in KiCad though is to add a property to track segments to make a cutout in the solder mask too. This is a common feature for guard tracks, and when it is added as an extended property to tracks, it will move along with the tracks if they are pushed and shoved.
The difference is the exposed copper. I’ve traced a line (Draw Line) in KiCad but I’m not able to remove the solder mask
You draw a line on a copper layer (F.cu), not on the soldermask layer (F.Mask).
Select the desired layer first, then draw a line or other shapes.
@BlackCoffee: thanks for the instruction. It works but how can i create a filled layer in the middle of the pcb? We defined a “keep out copper fill” but i need in the inner layer a filled GND plane. For the keep out area i cannot define a priority. Any ideas?
Thank you very much!
Timo
Let’s assume I’m confused and you know what you want (because I don’t know what you want).
Best help I can give is based on a Hand-Sketch that clearly identifies everything and uses the correct words, meaning, if it’s a Filled Zone to be used as a Ground-Plane and you want on an Inner-Layer, then, draw it and label it. Don’t call it a ‘Keep_Out_Zone’ unless you want to 'Keep stuff out of it, such as Track/Pads,etc). You can have a Filled-Zone (Gnd-plane) that Keeps stuff out. But, it’s your design so, I don’t know what you want to keep out…
And, most likely, you want to connect something to it (such as GND). And, Layers are Multiples of ‘Two’ so, can’t have Top, Btm and only one Inner. And which inner layer? (You don’t Have to put anything on an Inner or outer layer but you can’t select to Have Only One inner layer).
See what I mean? You need to be specific about what you want to do ( and need to understand Kicad’s Layer and electronic design/etc…).
That said, screenshots below show CheckBox for Filled Rectangle, result on ‘One’ Inner-Layer and Via and Terminal…
