Your first part

This walks through one part, from a DXF to G-code: a plate with holes, cut out with an outside profile. The same steps follow in the app and on the command line.

In the app

1. Import the drawing: File > Import DXF… (Ctrl+I).

   • If the DXF doesn’t say whether it’s in mm or inches, Chipload asks. It never guesses.
   • The report under the canvas lists what was imported, and anything skipped or repaired: duplicate lines, gaps it closed, splines turned into arcs.

2. Check the job settings: click Job settings in the Browser on the left. A new project starts with:

   • stock just covering the drawing, 10 mm thick;
   • work zero at the drawing’s origin, Z zero on the stock top;
   • the GRBL post, a safe height of 5 mm;
   • a 6 mm endmill at 18 000 rpm.

   With a tool library and machine profiles set up, your defaults come instead. Set the real stock thickness now: depths are measured from its top.

3. Select what to cut:

   • click the outline on the canvas;
   • Ctrl+click adds more;
   • right-click selects a whole layer;
   • or click a DXF or one of its layers in the Browser.

4. Add an operation: Profile, in the ribbon’s OPERATION group.

   • Side: Chipload picks outside for an outline and inside for holes, and asks when a selection mixes both.
   • End depth: for a cut-out, the stock thickness plus a little, e.g. 10.3 mm into a spoilboard. More than the allowed overcut (0.5 mm by default, under Job settings) is refused.
   • Step down: how deep each pass goes.
   • Tabs: they keep the part from coming loose on the last pass. Add them under Tabs.

5. Generate: F5, or leave View > Update toolpath automatically on.

   • The toolpath shows on the canvas: arrows give the cutting direction, rapids are dashed, and each operation’s number sits at its first plunge.
   • Problems show in red on the field they’re about.
   • Warnings appear in the report.

   

6. Look at it: 3D shows the toolpath at its real depths. View > Show stock shows the stock as cut, and the slider under the canvas plays the program back.

7. Export: File > Export G-code… (Ctrl+E).

   • You can only export once the checker has passed the program.
   • Next to the G-code comes a setup sheet (part-sheet.html) for the operator: stock, zero, tools in order, operations and times.

8. Save the project: Ctrl+S. A project (.chipload) keeps the drawing itself, so the DXF isn’t needed again unless it changes.

On the command line

chipload import plate.dxf -o plate.chipload        # add --units mm if the DXF doesn't say
chipload inspect plate.chipload                    # contours with their numbers and layers
chipload set plate.chipload stock.thickness=12 \
  'operations.0={"type": "profile", "name": "Outline", "part": 1,
    "select": {"layer": "CUT_OUTSIDE"}, "side": "outside", "direction": "climb", "tool": 1, "start_depth": 0,
    "end_depth": 12.3, "clearance": 0, "step_down": 3, "feed": 1500, "plunge_feed": 400,
    "ramp_angle": 0.0524,
    "tabs": {"count": 4, "width": 6, "height": 2, "flank_angle": 1.5707963267948966}}'
chipload plan plate.chipload                       # warnings, cycle time, chip load
chipload run plate.chipload -o plate.nc            # checked G-code and plate-sheet.html

• set adds the operation (see Scripting); part is the project’s one part, which a new project has as part 1.
• select picks the outline by its layer, as inspect lists it. To pick single shapes instead, use {"shapes": [ids]}: inspect --json gives each contour’s shape ids.
• Angles in project files are in radians: 0.0524 is the 3° spiral ramp every profile goes down at, and 1.5707963267948966 is 90°, a straight tab.
• The app makes the same project. Open plate.chipload in it to see and change the operation.

The checker

Before Chipload writes a program, an independent checker reads the G-code back and refuses it if it finds, among other things:

• a rapid move (G0) down into the stock, or sideways while the tool is below the safe height;
• a cut deeper than the stock bottom plus the allowed overcut;
• a move beyond the machine’s travel, when the travel is set;
• an arc whose ends don’t lie on its circle;
• a cutting move with no feed, or with the spindle off;
• other units than the machine’s, or relative coordinates;
• a tool change with the spindle running or below the safe height.

The checker is separate code that shares nothing with the part of Chipload that makes the toolpath, so a bug in one is likely caught by the other. chipload check part.nc --job part.chipload runs it on any G-code, also from other programs.

Before you cut

• Work zero: the setup sheet says where X0 Y0 and Z0 are. Set them on the machine exactly there.
• Clamps: look at the 3D view or the simulation for clamps in the toolpath. Chipload doesn’t know where your clamps are.
• Air cut: run the program once above the stock.
• What holds the part: in the last pass, tabs or an onion skin should keep it in place.