Component offset in POS file

Hi, To be fair, I am not sure if it is some configuration I have, or something to do with the plugin…

Describe the bug Position data is offset for components selected through the JLCPCB component selector. ~7.6mm in -x direction

To Reproduce Steps to reproduce the behavior:

1. Go to PCBNEW
2. Click plugin button
3. Select JLCPCB Components
4. Generate assembly files
5. View POS file is incorrect (Within JLCPCB viewer) -> components are shifted 7.61118mm -x

Expected behavior POS file to be correct

KiCad Version

Application: KiCad (64-bit)

Version: (6.0.6), release build

Libraries:
	wxWidgets 3.1.6
	libcurl/7.82.0-DEV Schannel zlib/1.2.12

Platform: Windows 11 (build 22000), 64-bit edition, 64 bit, Little endian, wxMSW

Build Info:
	Date: Jun 26 2022 02:39:06
	wxWidgets: 3.1.6 (wchar_t,wx containers)
	Boost: 1.79.0
	OCC: 7.6.0
	Curl: 7.82.0-DEV
	ngspice: 37
	Compiler: Visual C++ 1929 without C++ ABI

Build settings:
	KICAD_USE_OCC=ON
	KICAD_SPICE=ON

[Bouni]

Thank you for your detailed research! I guess when we use the PR #199 and add popt.SetUseAuxOrigin(True) as well we cover most cases.

[Jan21493]

I was a bit impatient, so I modified the plugin a bit. I replaced a part in file fabrication.py:

    def generate_pos(self):
        """Generate placement file (POS)."""
        posname = f"POS-{self.filename.split('.')[0]}.csv"
        self.corrections = self.parent.library.get_all_correction_data()
        designSettings = self.board.GetDesignSettings()
        m_place_Offset = designSettings.GetAuxOrigin()
        self.logger.info(f"origin point for POS data is origin point for drill files (%d, %d) mm" % (ToMM(m_place_Offset.x),ToMM(m_place_Offset.y)))
        with open(
            os.path.join(self.assemblydir, posname), "w", newline="", encoding="utf-8"
        ) as csvfile:
            writer = csv.writer(csvfile, delimiter=",")
            writer.writerow(
                ["Designator", "Val", "Package", "Mid X", "Mid Y", "Rotation", "Layer"]
            )
            for part in self.parent.store.read_pos_parts():
                for fp in get_footprint_by_ref(self.board, part[0]):
                    if get_exclude_from_pos(fp):
                        continue
                    fp_pos  = fp.GetPosition()
                    fp_pos -= m_place_Offset
                    writer.writerow(
                        [
                            part[0],
                            part[1],
                            part[2],
                            ToMM(fp_pos.x),
                            ToMM(fp_pos.y) * -1,
                            self.fix_rotation(fp),
                            "top" if fp.GetLayer() == 0 else "bottom",
                        ]
                    )
        self.logger.info(f"Finished generating POS file")

It should be easy to find. It looks that this solves the problem for myself. I haven’t ordered a new pcb yet and I’ve only verified the top layer, so I’m not sure if this solves the problem completely.

I also found this: https://forum.kicad.info/t/coordinate-system-grid-and-origins-in-the-pcb-editor/24535 to explain the topic.