Copper connection too narrow for generated zone fill

This DRC error is unexpected for the zone fill:

Test case: drc_error_for_zonefill_width.zip

KiCad Version

Application: KiCad PCB Editor x64 on x64

Version: (7.0.0), release build

Libraries:
	wxWidgets 3.2.1
	FreeType 2.12.1
	HarfBuzz 5.0.1
	FontConfig 2.14.1
	libcurl/7.83.1-DEV Schannel zlib/1.2.13

Platform: Windows 11 (build 22621), 64-bit edition, 64 bit, Little endian, wxMSW

Build Info:
	Date: Feb 12 2023 01:35:19
	wxWidgets: 3.2.1 (wchar_t,wx containers)
	Boost: 1.80.0
	OCC: 7.6.2
	Curl: 7.83.1-DEV
	ngspice: 39
	Compiler: Visual C++ 1934 without C++ ABI

Build settings:
	KICAD_SPICE=ON

added 7.0 priorityundecided statusnew labels

It looks like the contents of this project are for a different issue

assigned to @sethhillbrand

closed with commit a0f99ea8

added statusfix-committed label and removed statusnew label

changed milestone to %7.0.1

mentioned in commit 51b9d8e7

I think I might be seeing a similar issue. I'm seeing an DRC error "Copper connection too narrow" but I'm honestly not sure what it's talking about. (See arrow near Pin 1 in image.)

The issue only seems to occur with square pads in my case. Setting pin 1 to even a 1% rounded rectangle pad makes the DRC error go away.

Example project: Bug_Report_2023-03-05.zip

Possible steps to reproduce:

• Create project loading in the same footprint I'm using here
• Create a zone covering the entire footprint. Set clearance and min. width to 0.2mm. Set pad connections to Solid. Connect the zone to any pin, or no pin at all.
• Set project board setup constraints all to zero or very low values. Set Minimum Connection Width to 0.1mm
• Run DRC check

I'm running the testing build from today that I believe would already include the previously referenced fix commit, FYI.

Application: KiCad PCB Editor x64 on x64

Version: (7.0.0-163-g8f1237e629), release build

Libraries:
	wxWidgets 3.2.2
	FreeType 2.12.1
	HarfBuzz 5.0.1
	FontConfig 2.14.1
	libcurl/7.83.1-DEV Schannel zlib/1.2.13

Platform: Windows 10 (build 19043), 64-bit edition, 64 bit, Little endian, wxMSW

Build Info:
	Date: Mar  5 2023 04:13:37
	wxWidgets: 3.2.2 (wchar_t,wx containers)
	Boost: 1.80.0
	OCC: 7.6.2
	Curl: 7.83.1-DEV
	ngspice: 39
	Compiler: Visual C++ 1934 without C++ ABI

Build settings:
	KICAD_SPICE=ON

Huh. Doesn't happen anymore with master. Will see where the difference is

Turned out that master was using the revised zone fill so it didn't get all the tiny bits of segmented copper. Good test case for DRC, not so great for other things. This fixes the DRC check. Will follow with the zone fill cherry-pick

Yes, your build includes Seth's earlier fix....

reopened

added statusin-progress label and removed statusfix-committed label

closed with commit 7653a2bf

mentioned in commit 7ef5e079

added statusfix-committed label and removed statusin-progress label

It looks like the contents of this project are for a different issue

I downloaded the ZIP that I attached, opened the project, performed the DRC on it, zoomed in and I still get the screenshot below with that test case in 7.0.0 .

So IMHO the test case is valid. (I do see that you submitted a fix, so I hope that this applies to my test case as well).

I updated to 7.0.1 - unfortunately the issue persists in my design. I had to update the test case a tiny bit to demontrate this - I shifted a track by 0.2 mm to allow the zonefill to extend a bit further so that it become less wide.

This is the updated test case:

interconnect_drc_7.0.1.zip

KiCad Version

Application: KiCad PCB Editor x64 on x64

Version: 7.0.1, release build

Libraries:
	wxWidgets 3.2.2
	FreeType 2.12.1
	HarfBuzz 5.0.1
	FontConfig 2.14.1
	libcurl/7.83.1-DEV Schannel zlib/1.2.13

Platform: Windows 11 (build 22621), 64-bit edition, 64 bit, Little endian, wxMSW

Build Info:
	Date: Mar 11 2023 03:41:46
	wxWidgets: 3.2.2 (wchar_t,wx containers)
	Boost: 1.80.0
	OCC: 7.6.2
	Curl: 7.83.1-DEV
	ngspice: 39
	Compiler: Visual C++ 1934 without C++ ABI

Build settings:
	KICAD_SPICE=ON

reopened

I see the mentioned drc-error with current testing and nightly version. Using the last provided project: interconnect_drc_7.0.1.zip

testing: Version: 7.0.1-35-g819a9da5, release build, Win10

nightly: Version: 7.99.0-535-gad5d3d4e, release build, Win10

Oh, wow, we have got to do something about our zone fills. Check out what happens to this particular section:

Here, inflating the segmented circle leads to a kind of saw-tooth pattern that is now confusing our algorithm for identifying necks.

I see a solution for this issue in the DRC checker but I think we also need to smooth the output of our inflate routine to both reduce the point count and speed up our display/UI. Fewer triangles = faster responsiveness

changed milestone to %7.0.2

removed statusfix-committed label

added statusnew label

closed with commit 914b5a4d

added statusfix-committed label and removed statusnew label

mentioned in commit c1818104

I can confirm the problem persists. KiCad complains about the copper to be too narrow (0.18mm instead of the required 0.2mm):

I have KiCad 7.0.9, release build

EDIT: I just updated to 7.0.10, but the problem is still there.

Attach the project you are using that shows this issue

Hi @sethhillbrand , Thank you for your quick response. It's open source hardware that I'm working on. The KiCAD project is freely available here: https://github.com/Embeetle/tiny-scarab

Cheers, Kristof

Hi @sethhillbrand , I recently updated my layout and for some mysterious reason the problem disappeared. So if you would now clone my GitHub repo, you won't be able to reproduce the problem from the latest main branch.

Therefore, I've zipped the "old" project such that you can still reproduce the problem:

Just clone my GitHub repo (https://github.com/Embeetle/tiny-scarab ) and take that tiny-scarab-old.zip as your KiCAD project.

@kristofmulier please attach that zip to this issue - drag and drop it into the editor or use the paperclip icon. External links tend to rot and external repos tend to march forward, as we see here. We want the reproducing project archived in the issue tracker so we know we're looking at the same thing and so we can reference it in the future if needed.

Hi @gkeeth , Here is its:

tiny-scarab-old.zip

Hi, I'm having this issue too. What seems to be happening is that there is some kind of "overhang" on the tips of the fill. Like the radius of the "pen" that is used to draw the polygon is big enough to make the sides touch. Does that make sense?

Sorry I don't have better words to describe it. I hope the picture makes it obvious:

Thanks

Edit: Version info

Application: KiCad PCB Editor x86_64 on x86_64

Version: 7.0.10-1.fc39, release build

Libraries:
	wxWidgets 3.2.4
	FreeType 2.13.1
	HarfBuzz 8.2.1
	FontConfig 2.14.2
	libcurl/8.2.1 OpenSSL/3.1.1 zlib/1.2.13 libidn2/2.3.4 nghttp2/1.55.1

Platform: Fedora Linux 39 (Workstation Edition), 64 bit, Little endian, wxGTK, gnome-xorg, x11

Build Info:
	Date: Dec 28 2023 00:00:00
	wxWidgets: 3.2.4 (wchar_t,wx containers) GTK+ 3.24
	Boost: 1.81.0
	OCC: 7.6.3
	Curl: 8.2.1
	ngspice: 41
	Compiler: GCC 13.2.1 with C++ ABI 1018

Build settings:
	KICAD_SPICE=ON

Relevant discussion

@marcelomd Your case is exactly what we are checking for. That copper connect is too narrow. You need to adjust the design or the parameters to fix

Yeah, I tried a bunch of permutations, within reason, of the parameters and can't get it to make the errors disappear. Kinda frustrating because this is not pushing any limits. Just PTH on a 0.1" grid and 0.25mm clearance. Default footprints.

Best I can come up with now is to make all pads round.

Anyway, just adding to the discussion. Thanks!

I'm working in KiCAD 8.0.2 now (KiCAD 7 before), and the problem persists. This is my current version:

Application: KiCad PCB Editor x64 on x64

Version: 8.0.2, release build

Libraries:
	wxWidgets 3.2.4
	FreeType 2.12.1
	HarfBuzz 8.3.0
	FontConfig 2.14.2
	libcurl/8.5.0-DEV Schannel zlib/1.3

Platform: Windows 11 (build 26217), 64-bit edition, 64 bit, Little endian, wxMSW

Build Info:
	Date: Apr 27 2024 23:05:17
	wxWidgets: 3.2.4 (wchar_t,wx containers)
	Boost: 1.83.0
	OCC: 7.7.1
	Curl: 8.5.0-DEV
	ngspice: 42
	Compiler: Visual C++ 1936 without C++ ABI

Build settings:

@kristofmulier If you are referring to tiny-scarab, attach a screenshot. I've tested that board and the connection width errors look valid to me

Hi @sethhillbrand , To reproduce the issue, please try this project: tiny-scarab-copper-too-narrow.zip

I get the "copper too narrow" error here:

An auto-generated copper fill should never cause a DRC error, so this looks like a bug to me.

If you measure the distance between those two notches, you will find that it is less than the minimum width. The fill does currently generate connections that are too small when the knock outs are spaced just right. We have an open issue to prevent these sorts of small connections but at the moment, the DRC check is reporting correctly

Hi @sethhillbrand ,

the DRC check is reporting correctly

I agree that the DRC check is reporting correctly. However, the bug is in the copper filling algorithm. It fills copper in a way that causes DRC errors.

We have an open issue to prevent these sorts of small connections

That's great KiCAD developers are fixing this. Wonderful. Thank you so much.

Hi @sethhillbrand , Is there any news on this issue?

No.

You can change the minimum width of the zone fill to be smaller and you will not encounter this issue.

@kristofmulier There is now a some testing code to resolve this. You can add ZoneConnectionFiller=1 to your kicad_advanced file to test out the new code in a nightly build. If you do not already have a kicad_advanced file, you can create it in a text editor in %APPDATA%\kicad\8.99