Hello,
In my PCB design there is copper fill connected to ground net.
I can define fill area and keep outs.
I am able to fill with solid copper area.
My question is:
How do I fill with a hatched pattern instead of solid copper pour?
Where can I find option for these?
Regards,
Vinay
Currently only solid copper pour is possible.
There is no automatic hatched fill. If you want something which looks like a hatched fill you will need to manually place cutouts in your fill outline.
Thanks madworm and cbernardo for the clarification.
Regards,
Vinay
Hello,
As I may need hatched fill for partial ground below capsense buttons on intended project.
I will wait till KiCad provides these feature.
Meanwhile found a bit tedious workout was posted at
https://groups.yahoo.com/neo/groups/kicad-users/conversations/topics/16733
where in user Gerd V. Egldy had suggested following
"Hi Andy,
Have a play with the bitmap2component utility (on the main kicad screen)
I finally solved my problem based on your idea, thanks.
Here is how I did it:
- create the pcb layout
- create a regular flood fill area where you later want the hatched one
- do the flood fill
- export the copper layer as svg
- open the pcb in inkscape
- select just the object defining the fill area
- export the selected object as bitmap, use a high resolution (I used 1200dpi)
- open gimp and create a black&white crosshatched pattern as you want it,
export it as gimp pattern, copy it to your gimp pattern directory, restart
gimp
- load the fill area bitmap in gimp and fill it with your pattern
- replace the background transparency with white
- set the color mode to grayscale
- invert the colors (so all traces are white, empty background black)
- save as bmp
- use bitmap2component and save as mod
- use this tool to scale to 0.25 (for 1200 dpi) and move to copper layer:
http://escalalibre.com/edwt/kicad_sizeConverter.php- open pcbnew, add the new .mod file
- remove the flood fill area
- place the hatched fill as module on your pcb
Here two more links that where helpful in this process:
http://gimp-tutorials.net/gimp-pattern
http://www.re-innovation.co.uk/web12/index.php/en/blog-75/230-adding-logo-to-kicad
Kind regards,
Gerd
"
That will work, but every time you make a modification to the wiring you have to remember to create the hatched fill zones again. Unfortunately a hatched zone is not high on the agenda either so there’s no telling when (if) it will be implemented. It’s not something which is trivial to implement either.
Thanks for the heads up.
Will convert filled to hatched zone at very end of PCB design / Project completion.
Will remain with KiCad and support it, till more and more advance features are implemented 
Regards
Vinay
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
Piotr
Thanks for posting nice illustrated step by step hatched pattern fill work around.
Vinay
Hi,
Thanks for all this great guidance. I used a combination of these methods to create top and bottom hatch planes for my project. Everything seems to look good except one thing I noticed. In the Properties sheet for my bottom hatch, under Board Side, Front is selected (although I set the layer to B.Cu using a text editor on the .mod file, and it does appear as a green object and hides when I hide the Bottom layer, as you would expect). Selecting Back on the Properties sheet inverts it, turns it Red making it part of the Front layer. So clearly I don’t want to do that, but should I be worried about this attribute being backwards? I did scan through the .mod file for the hatch, but see no clues there.
Thank you to Gerd V. Egldy (via @VinayDand) and @PzP for the diligent documentation on your methods. I don’t know how I overlooked this missing feature for so long. Now that I’ve had reason to apply hatched fills (yes, one of those picky CapSense sensors), this thread has been crucial.
That all said, I abandoned both the documented solutions! Trying to maintain control over edges and dimensions between vector export, rasterisation and re-vectorisation through 4 separate software tools just became too much. And the result is too difficult to tweak, due to the prolonged edit-preview cycle.
In the end I drew it by hand, all in KiCad. KiCad’s trace drawing behaviour is definitely not ideal for this, but actually helped surprisingly well. Being able to set a grid, copy and paste, still get track snapping, and work directly on the PCB allowed consistent, albeit arduous, progress.
See attached for the result. Like with painting, all the hard work is in the cutting in. Doing so with straight edges was probably the biggest limitation, but if you’re willing to have a bit of arbitrary aliasing in your “curves”, it’s fine. Zoom in to see the details.
So after this 5 year old thread has been dragged up, I started KiCad V5.99 and about a minute later I had:
“Default” of the zone was filled, but I got the above results by just edting the zone properties:
Wonderful news!
But AFAIK the latest version is 5.1.8. What is V5.99? Is that a nightly build of the master branch? I don’t even see a git tag for that version.
Yes. All nightly builds of what will become 6.0 call themselves 5.99 (and all leading to 7.0 will be 6.99, etc)
The development branch is currently at what is known as a “feature freeze”, meaning that (except for a couple well documented (for the developers, of whom I’m not a member) exceptions) there are no new features being developed for the targeted 6.0 release. So all (most) of the current development work on 6.0 is crushing bugs. The hope is that they will start releasing Release Candidates for 6.0 early next year.
It would be great to be able to set the fill hatch pattern right here in the properties so I can have solid grounds on all the board but hatched ground areas under the capsense buttons.
It could be handled like like style formats in a word processor. I can predefine and name my hatch styles somewhere and then select it’s name here in the fill property.
Only zones can be hatched. It’s of course complicated if you need a circle, but I doubt it’s really the case. A four corner polygon would be fine enough.
I know, it’s a feature idea/request 
You might ask your fabricator if he can crosshatch your copper pour. It might well be that he prefers to receive the simple solid fill and crosshatch on his CAM system rather than receive the large and complicated crosshatched Gerbers. Or he might not.
