The workflow from Inkscape SVG to cut part is three stages: prep the drawing, generate G-code (CAM), then stream that G-code to the machine. The Genmitsu 4030 runs GRBL 1.1 on an Arduino-based controller, so any GRBL-compatible sender works — no vendor lock-in.

1. Prep the SVG in Inkscape. Set the document units to mm and make the drawing size match real-world dimensions (File → Document Properties). Convert any strokes or text to paths (Path → Object to Path, Path → Stroke to Path). Combine subpaths only if they're meant to be a single contour. It's worth simplifying (Path → Simplify) to reduce node count on curves, but not so aggressively that the shape drifts. Save as plain SVG.

2. Generate G-code. This is the CAM step, and it's where you specify tool diameter, cut depth, feeds/speeds, stepdown per pass, and whether the toolpath is inside/outside/on the line (offset direction matters — for cutting a shape out, you want an outside offset by the tool radius, plus tabs so the piece doesn't move mid-cut). Good Linux-native options:

• •FreeCAD Path workbench — heaviest but most capable. Import the SVG, extrude to a body if needed, then create a Job, Profile operation, and post-process with the grbl post. Best if you'll be doing this often.  

• •Kiri:Moto (grid.space/kiri) — runs in the browser, no install, has a CNC mode with good SVG import. Fast to learn.  

• •Inkscape gcodetools extension (Extensions → Gcodetools) — stays in Inkscape but the UX is dated and it's easy to get wrong offsets. Fine for engraving; less pleasant for profile cuts.  

• •Estlcam runs well under Wine if you want something closer to what the Genmitsu community typically uses.  

For a first cut in wood with a common 1/8" (3.175 mm) 2-flute endmill, reasonable starting numbers: feed 800–1000 mm/min, plunge 200–300 mm/min, stepdown 1–1.5 mm per pass, spindle at whatever fixed speed your 4030 spindle runs. Add 3–4 tabs (0.5–1 mm thick) around the perimeter.

3. Stream to the machine. The 4030 comes with Candle, which has a Linux build, but on Kubuntu you're likely happier with one of:

• •UGS (Universal G-code Sender) — Java, mature, apt-friendly-ish (grab the platform build from winder.github.io/ugs_website).  

• •gSender — Electron app from Sienci; polished UI, has a .deb and .AppImage.  

• •bCNC — Python/Tk, feature-dense (autoleveling, probing, etc.), install via pip.  

Any of them will connect to the controller as a serial device — usually /dev/ttyUSB0 at 115200. Add yourself to the dialout group so you don't need sudo: sudo usermod -aG dialout $USER (then log out/in).

Running the job. Secure the stock (double-sided tape, clamps, or a spoilboard with screws in waste areas). Home the machine if you have limit switches; otherwise jog to your work origin manually and zero X/Y/Z there. Z-zero is the fussy one — a piece of paper as a feeler gauge is the traditional method, a touch plate is better. Run with the spindle off first as an air pass over the material to confirm the toolpath fits, then run for real.

One thing worth doing early: cut a simple test rectangle (say 40×40 mm) and measure it. If it comes out 39.6 or 40.4, your steps/mm are off and you can tune them via $100/$101/$102 in GRBL before you waste stock on the real part.