Feeds, speeds and the G-code check

The CNC G-code export tutorial writes a program per sheet. Two helpers in the same CNC view answer the next questions: are the spindle speed and feed of my cutter sensible, and what will the machine really do with this program? Both run in your browser with the same engine as the kerfwise-feeds-speeds and kerfwise-gcode-inspector tools.

1. Open a project with sheets

Start from the L-shaped kitchen 3.6 × 3.0 m template and press 6 (or click CNC). Leave the material on White melamine chipboard 18 mm and the controller on GRBL.

2. Read the G-code check

Scroll below the operations and the tool library to G-code check. The inspector has read the program line by line, like a controller:

• Machining time 36 min 55 s, Cutting path 162.07 m, Rapid path 46.76 m, Z range −18.3 … 15 mm and Tool changes 3 for sheet 1 of 3.
• A green note says The inspector reads the same cutting path and time from the G-code as the program estimate above. That is the cross-check: the program estimate and an independent reading of the written G-code agree.
• Bounds (mm) shows all moves and the cutting moves. Compare the maximum X and Y with your machine's travel.
• Per tool lists cutting and rapid length, cutting time, arcs, lowest Z and the highest feed. GRBL programs change tools with an M0 pause and carry no tool numbers, so the table shows one row (no tool number).

Warnings appear in an orange box, for example an arc whose radius does not match or a sideways rapid below Z0. Notes, such as a G28 home move, are folded away under notes.

3. Add your machine's acceleration

Type 500 into Machine acceleration (mm/s², 0 = ignore). The card now shows Time with acceleration 41 min 49 s next to Time without acceleration 36 min 55 s. Every move now speeds up and slows down, and corners are taken at a GRBL-style cornering speed. The value is remembered in this browser for every project. Set it back to 0 to compare with the plain estimate.

4. Feeds & speeds for the end mill

In Tool library, the end mill row T1 has a Feeds… button. Click it to open Feeds & speeds for T1:

• Material is guessed from the sheet material (MDF / particle board for melamine chipboard).
• Flutes 2, Spindle speed (rpm) 18000 and Spindle maximum (rpm) 24000.
• With a full slot 6 mm deep the result is Spindle speed 18000 rpm, Feed rate 12352 mm/min, Chip load per tooth 0.343 mm and Spindle power 0.46 kW. The line under the numbers shows the chart range for Ø6 mm, 0.305–0.381 mm.

Now enter 2 in Width of cut (mm, empty = full slot) and choose Low end (safer, finer finish) under Start in the chart range at. The chip-thinning factor rises to 1.061 and the Feed rate becomes 11646 mm/min. Click Apply speed and feed to T1: the tool row now shows 11646 in Feed, and the G-code, the time and the check are recalculated. Ctrl+Z undoes the change.

5. Check any G-code file

Click Check a G-code file… in the CNC toolbar. Choose a file under G-code file or paste a program into G-code, then press Check. A 13-line test square with one R10 corner arc reads G-code: 13 lines in mm., about 9 s and 0.16 m of cutting path, with a top-view preview. Set Rapid rate (mm/min), Tool change (s) and Machine acceleration to your machine's values first. Nothing is uploaded.

Good to know

• Chart chip loads are starting values for sharp solid-carbide router bits on a rigid machine. Listen to the cut, look at the chips and adjust.
• Power is only estimated for materials with a built-in specific cutting energy (MDF and aluminium).
• The inspector skips macros, parameters and subprograms with a warning and measures the programmed path, not a G41/G42-compensated one.