Machining operations
Common settings
The settings every operation shares: start and final depth, feeds and spindle speed, depth per pass, stepover, cut direction diagram, chip load and accessories.
Parameters are grouped by theme. A grayed-out field has no effect with the current settings (for example the ramp angle when the entry is a plunge). Defaults are cautious starting points; feeds and speeds come from the tool.
| Group | Parameters |
|---|---|
| Depths | Start depth (0: the surface); Final depth, as a value or as a percentage of stock (100% = the whole thickness). |
| Feeds and speeds | Feed rate (cutting), Plunge rate, Ramp feed rate, Spindle speed: taken from the chosen tool. |
| Passes | Depth per pass (the last pass may be shorter); Stepover as a % of the diameter or as a length (pockets, surfacing); Cut direction. |
| Strategy | What is specific to the type: side, pattern, stock to leave… |
| Entry | Entry type and Ramp angle: see Entering the material. |
| Tabs | Profile only: see Tabs. |
| Accessories | Vacuum and Coolant (mist M7 or flood M8), written only if the machine declares these accessories (see Machine settings). |
Cut direction
Climb (the default) usually gives a better surface; conventional is more forgiving of the backlash of light machines. Below the choice, a diagram shows it seen from above (clockwise spindle): the tool, its rotation, its feed and the side of the material that is kept.
Chip load
Below the spindle speed, the editor computes the chip thickness with the operation’s feeds: feed rate ÷ (spindle speed × number of flutes of the tool). Too thin, the bit rubs and heats up; too thick, it strains and may break: compare it with the one the manufacturer recommends (see also Feeds and speeds calculator). For a drill operation, it is the feed per revolution: plunge rate ÷ spindle speed.
Clearing pattern (pocket, rest pocket, dogbone slot, surfacing, reliefs): a thumbnail shows the path on a sample shape, concentric offsets or raster at the chosen angle with its outline pass. It follows the settings; check the real machining in the preview.
Depth
A final depth greater than the stock thickness cuts into the spoilboard; Dusty points it out. To cut through, go a few tenths of a millimeter deeper.
This manual is also built into Dusty: press F1, or open the Help menu, to read the topic for what you are doing. A mistake, a missing answer? Tell us
Try it in Dusty, for free.
Free CNC milling software: design, toolpaths and machine control. Mac, iPad, iPhone, Windows and Linux.