i messaged them, i’m waiting for their reply
im long time supporter of kicad, totally 4 production PCB im made using kicad, i would be happy if i answer the question from PCB manufacturer
Here’s one problematic pad on a copper layer. There’s something wrong with it. It has teardrops inside it. The teardrop plugin may be the culprit.
i uploaded earlier backup of this project without tear drops, in bottom of question detail
That one looks much better. Please yell at the teardrop plugin’s author 
Could you still ask your fab about problems with the one without teardrops?
I’m wondering why they’re saying they’re having trouble with every KiCad gerber and I don’t think that teardrop extension is that widespread.
i think teardrop is not problem, in their software it shows pad:0, traces 204 , they want it to be pad:1
6 month ago i submitted one of my project , in which same problem for SSOP4 footprint ( NOT official kicad footprint, i downloaded fronm here https://github.com/savenlid/kicad) , ON that project i didn’t use tear drop plugin… ill upload that gerber here soon, after that i only use official kicad and digikey footprints
EDIT:
same problem on previous project, on footprint U5,U6,U7,U8
GERBER BELOW
kicad info.zip (69.5 KB)
i move on that time , because i concluded that i used 2 year old footprint from internet on latest version of kicad v5
And it’s exactly those three pads which you have circled, not any other?
Perhaps we should just wait for a reply from the fab.
That aside, two more points:
- The footprints themselves can’t be the origin of the issue, there’s no way to define “painted pads” or something in the files, whether they’re from the official lib, Digikey or some random GitHub repo.
- Either way, all the lines the teardrop plugin generates are unnecessary at best, no matter if your fab is having other issues with KiCad gerbers or not.
- Edit: Also, the teardrop plugin doesn’t handle roundrects correctly, as seen in my or @eelik’s screenshots.
What is interesting is that exactly the pads marked as problematic have ComponentPad attribute, while other pads don’t.
EDIT: the problematic gerber file doesn’t have real X2 attributes. KiCad adds them as comments if X2 isn’t selected when plotting and gerbview can read those comments. But it’s still a mystery why only those three pads have those comments.
1 Like
yes exactly on circled one, checkout my previous project gerber on my reply
Could you update to the latest testing build (5.1.6+) and regenerate the gerbers and attach them here? There’s a remote possibility that this is a bug which may have been fixed, and if it hasn’t been fixed but is a bug in KiCad, this should be replicated with the latest version anyways.
okay im downloading, ill regenerate it using latest build
I don’t find anything else common between those problematic pads and any other difference with other pads than the shape and the attributes. The attribute metadata shouldn’t affect because it’s only in the gerber comments. What is left is the free polygon shape instead of other simple predefined gerber shapes: rectangle, oval, circle. All other pads seem to be one of these three shapes.
If the polygon is the problem, it’s what Frederik said:
As I read it, the “painted pads” is not some kind of setting in any PCB program, but a way to describe generic way of how some PCB programs handle generation of pads internally.
Is it clear yet where the problem is? Teardrops, Polygons in Pad, or possibly other?
I opened “kicad info.zip/uboard-B_Cu.gbr” in gerbview and then:
**GerbView / File / Export to Pcbnew".
In Pcbnew the rounded rectangles are a polygon and look like:
A bit strange that there is no clearance drawn around these polygons, but there is no real netlist with the back import.
Zooming in on a corner, shows each corner of the polygon is 16 line segments, the polygon has “68 points” (=4*16+4):
I do not see any problem with the file. If the polygons are the problem, then I see a few possible paths.
The most logical to me would be if your PCB manufacturer updates their software to support these kind of pads. ( I think “zones” / “copper pours” are the same kind of polygon in KiCad. Does your manufacturer have problems with those?). There are plenty of PCB manufacturers who do not have any problem with these pads.
You could modify your footprints to not use rounded or oval pads at all. Simplest is to use rectangular pads with no rounded corners. Other idea is to use several overlapping pads. The pad above can be made out of 2 overlapping rectangular pads and 4 circular pads in the corners.
The root cause of the problem is probably that “Gerber” files never were a “proper” standard. It started with a photoplotter and a proprietary format and over 30 to 40 years or so it evolved into what it is now. As far as I know KiCad files are conform to modern and standardized gerber versions.
2 Likes
I am not sure a user should ever make workarounds for outdated manufactuer software. If the manufacturers is not prepared to go with the times then it is time to let them go.
1 Like
so what requirement does PCB fabricator need to process kicad Gerber file? or simply how do i ask whether they support kicad Gerber format, like ,“do u support x format Gerber files ?”
1 Like
thank you for the information
They should be able to support polygonal pads with up to 5000 vertices, as described here https://www.ucamco.com/files/downloads/file_en/399/the-gerber-file-format-specification-revision-2020-09_en.pdf#page=55
There’s still the possibility that there’s actually something wrong with KiCad’s output. I assume you haven’t gotten a detailed reply yet?
PCB manufacturer message me now that , property is not Pad, it shows as polygonal fill in their cam software , no more information about their software
I think they have a point there.
Using a G36/G37 fill together with CompontentPad/SMDPad attributes is not how it’s supposed to be done.