1. Export one .nc file per tool

Select the Job and change these in the Property view (they’re also on the Output tab when you double-click the Job):

PropertyValue
OrderOutputByTool
SplitOutputtrue
PostProcessorOutputFile%D/%d_%S_T%T.nc

In the file name, %D is your file’s folder, %d is the document name, %S is a sequence number (0, 1, 2…) and %T is the tool number. Then run CAM → Post Process once and you get one file per tool.

2. Fix the operation order first

Profile is the first operation and cuts down to Z −42.76, which is the full stock thickness, with no tabs. Running it first cuts the part loose before any carving happens.

  • Move Profile to the end of the Operations list, so the order is Pocket3D → Pocket3D001 → Surface → Profile.
  • Add tabs to it (Dressup → Tag), or screw the blank down outside the cut line.

After reordering you get 4 files: T1 → T3 → T2 → T1 again for the cutout.

3. Changing the bit between files

Your Z zero is the top of the stock, and the roughing passes cut most of that surface away. For bits 2 and onward, zero Z on the spoilboard instead, since that never changes:

Before file 0:

  1. Measure the real board thickness T with calipers. Your FreeCAD stock is 42.76 mm, and the real board must match it.
  2. Set X/Y zero, and set Z zero on the stock top.
  3. Run file 0.

For each later file:

  1. Raise Z and stop the spindle. Leave X/Y alone and don’t re-zero them.
  2. Swap the bit.
  3. Put the touch plate (thickness P) on the spoilboard next to the part. Probe with G38.2 Z-50 F50, then send G10 L20 P1 Z{P − T}. For example, with a 42.76 mm board and a 20 mm plate: G10 L20 P1 Z-22.76. Without a probe, jog down onto paper on the spoilboard and send G10 L20 P1 Z-42.76.
  4. Raise Z, start the spindle, and run the next file.

GRBL saves G54 offsets in EEPROM, so the X/Y zero survives between files. If you’d rather keep one file, add --tool-change to the Job’s PostProcessorArgs to output real M6 lines. That only works if your sender handles M6 (CNCjs, bCNC and UGS have tool-change options).

Before you cut

  • Feed: everything comes out at F300 mm/min, which is why the Surface pass takes about 7 hours. The tool controllers are set to 5 mm/s. Your older jesus.nc had F18000, so check that the feed you run with is what you intend.
  • Spare tool controller: TC: Tapered Ball R0.5 (T15) still has feed and spindle at 0. It isn’t used now, but fix or delete it so it doesn’t get picked by mistake