Hi! My first post here! I’m one of the “victims” of the videos Chris released some time ago. Got into KiCad and i guess i’ll stick with it, as it’s getting better and better in time. In my last board design i also wanted to use a few capsense buttons and encountered the problem of generating hatched zones. I used the free version of Diptrace to generate them. Apparently, despite the pin number limit in the free version you can still import a gerber layout and use an automatic pad detection, even if it has more than 300 pads. The board i was working on had over 500 of them.
Anyway, here is a photo tutorial on how i did this. Hope it will help some of you. I’m using windows, but as far as i know there is a Diptrace version for linux and os x, so it should work on these platform too.
-
I created a simple cap sense buttons project in KiCad:
-
Export the gerber files:
-
Import the top, bottom and board outline gerber layers into Diptrace:
-
Create the hatched zones (4 mil track width should be 7 actually, Cypress has a document about the capsense layout guidelines):
-
Once filled, move the zones away and delete the rest of the board (imported gerbers). Move the zones to one layer and export them as a gerber file:
-
Now, you could import the gerbers directly into KiCad, however, since there is no way of grouping objects, they will appear as separate tracks, not really handy if you plan to do some changes to the rest of the board or even to precisely position the zones on the board. Preferably the zones should appear as separate objects. The next steps are similar to the previously posted tutorial. Load the gerber file into the Gerbv viewer and export them as an SVG file:
-
Load the SVG file into Inkscape and export separately as 1200DPI PNG, changing the background to black and the stroke colour to white:
8.Use the KiCads bitmap converter to import the zones as a silkscreen objects and use any text editor to move the objects into the copper layers (leaving out the reference/value):
-
Zones imported into Kicad:
-
Position the zones, a good idea is to write down the x,y coordinates for each zone:
-
Since there are no pads in the component,it can’t be assigned to any net. I ended up adding a large rectangle smd pad at the border of the zone to connect it with the rest of the solid gnd plane:
This is just an example board i do for the purpose of the tutorial. Unfortunately, in my main design, much more complex one, i found out that the imported zones were causing KiCad to crash every time i refilled the native zones. I ended up moving hatched zones away from the board for any editing. When the rest of the board was finished, zones filled up, i moved hatches back where they belong using the previously written down coordinates.
Here is the end result:
Lots of steps to get these hatched patterns… I hope someday such a feature will be added to KiCad.
Btw, i’m using one the latest builds (past 5050).
Cheers!
Piotr