Hello everyone, in the previous versions of pcbnew, in the “copper zone properties” there was a fill mode option (you could choose between segmented and polygon), but in version 5.1 of kicad that option is not. Was it removed or is it elsewhere?
Seems this does indeed no longer exist. Can i ask for the usecase you had for this? Maybe we can offer an alternative.
My local PCB manufacturer has problems with the segmented copper zones, so i have to change them to polygons to make it work.
I would have assumed that the segmented option is the one that got removed not the polygon one.
But i can see a way how this can be a problem. Loading an old design could leave you at a place where you can not change it to the polygon option. (I am currently in the process of testing this. You might be forced to use a text editor or the older version of kicad you originally used to create these files.)
In v5.1 the zones are always polygons.
Edit: all new zones
I played around with it. A zone that was in mode segmented stays in mode segmented when saving with v5.1.
Meaning use a text editor to remove this option from the file or redraw the zone in kicad as that will create it in mode polygon.
Bug reported: https://bugs.launchpad.net/kicad/+bug/1823087
Sorry, i wanted to say that my manufacturer has problems with “polygon fill” and I need to change it to “segmented fill”. Apparently, “polygon” was left by default and the option to change it by “segmented” was eliminated, but in this case, this option is so helpfull.
Ok i added this info to the bug report as well. I wonder why this was in the zone settings in the first place. After all the only place where it matters is on export so i would have expected it as part of the gerber export settings.
For now you might be stuck with either working with text editors to fix this up or go back to 5.0 (at least for exporting, You could install it in a virtual machine and use it only for this task)
Thank you very much for the answers and solutions. I think I’ll take the option to work on version 5.0 hehehe.
Hi Daniel,
This option, at least in V5.0.0, only controls the way zone is displayed on the screen. It has no effect on the filling algorithm, the zones are always filled as polygons. There are some traces of segment zone filling code in V4.0.7 although I never used it and I can’t say if it works. What is the exact problem with polygonal zones your manufacturer has?
Tom
The SEGZONE object (which output segments) has not been an option in KiCad for some number of years. See JP’s response here[1]. The upshot is that SEGZONEs never had proper connectivity or DRC. Nor did they maintain their outline after filling.
[1] https://lists.launchpad.net/kicad-developers/msg37686.html
1 Like
I would have assumed segzones as described by that mailing list entry are different to the setting “fill mode segmented”. I know that these where no longer used long before version 4 as we had a board here recently that had them. (We where unable to get it back up and running without removing that zone and creating a new one.)
Did the zone setting really do nothing?
For reference the zone settings in the file i uploaded to the bug:
(zone (net 2) (net_name GND) (layer F.Cu) (tstamp 0) (hatch edge 0.508)
(connect_pads (clearance 0.508))
(min_thickness 0.254)
(fill yes (mode segment) (arc_segments 16) (thermal_gap 0.508) (thermal_bridge_width 0.508))
Notice in the last line the (mode segment) setting. This is neither removed when using 5.1 nor is it possible to create a new one with these settings.
Update: according to the bug report it should be removed by refilling. I can not check this right now.
I thought that the filling mode had to do with the gerber files. My manufacturer asks that the ground planes be “grilled” (segmented). I think it must be because it’s an old machine (it’s a low cost and express service). The last time he could only manufacture the pcb when the fill mode option was changed from polygon to segmented.
@Daniel- I suspect that your manufacturer is requesting that you not have large, solid copper fills. Whether these are segments or polygons is not the issue. Older production processes could warp the board due to differences in cooling rates between the prepreg and copper. By creating copper zones that were partially filled by a grid, you reduce the warpage.
An option to create these zones has been added to the nightly builds but is not available in 5.1
1 Like
This
The fab is asking for a hatched fill.
This was not just about warping, it also affects etching rates and I remember long ago being told about the holes allowing steam to escape during wave soldering.
Just a general remark on the original topic:
It is not true that there was no difference between segmented fill and polygon fill on gerber export. Segmented fill really creates lines that overlap while polygon fill is a polygon (They use different gerber codes and kicads gerber viewer shows one of them as lines and one of them as a polygon if i set them to show in sketch mode.)
This means that files created with v5.1 will be different compared to the ones from version 4 after gerber export.
If now there is a manufacturer that really uses some very old toolchain then the user might run into trouble. This might be something that should be documented properly in the release notes of kicad 5.1
test_zone_fill.zip (203.6 KB)
The remark from the bug report that refilling the zones will remove the segmented fill option is also not true.
Meaning we still have the topic that it is impossible to convert a segmented fill area in a polygon area using version 5.1
V5.1 has however a different fill algorithm for segmented fill
gerber_v5.1.zip (2.5 KB)
1 Like
We’re chasing down the discrepancies between what Rene sees and what we see in the bug report. It is annoying to respond to the same post in two places, so this is a reference that anyone interested in the differences should read the bug report.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.