RockCAM is not a script that replays a fixed recipe. It analyses the part, decides what needs machining, and assembles a program from three things you control: the operation templates, the tool library, and the parameters.
It does this in a small local model that runs on your own computer. There is no internet connection and no cloud service involved, and nothing about your part leaves the machine.
What RockCAM decides, and what you decide #
RockCAM identifies the features from the geometry, then matches them to machining methods. From there it looks up three resources:
- The operation template for that method, and the parameters stored on it.
- The tool to use, chosen from the tool library.
- The speed and feed, taken from the parameter table by tool type, diameter and method.
The RockCAM settings dialog listing the tool library, the parameter table and the operation templates.
Only a few values come from outside the template. Everything else — the engage and retract settings, the coolant, the tolerances stored on the operation — stays exactly as your template defines it.
If a template is not found #
If RockCAM cannot match an operation template for a given method, it falls back to its own built-in template. It does not stop and it does not skip the operation.
That fallback is what makes the first run useful: you get a complete program without configuring anything, and you then replace the parts of it that do not match your shop.
Default machining strategy #
When a setting is left on its default, RockCAM follows a standard machining strategy. These defaults are choices, not rules — in most cases a different choice is just as valid, and the point of the settings is to let you change them.
Operation order #
For a general part, RockCAM works in this order:
- Face the top face.
- Rough the outer profile, or run 3D rest roughing if the part is complex.
- Rough the pockets.
- Rough the holes.
- Finish the pockets.
- Finish the holes.
- Chamfer.
- Tap.
Any stage can be switched off in the machining preferences, and RockCAM then leaves it out of the program.
Hole strategy #
Holes are sorted into four kinds, each with its own default machining method.
| Hole type | How it is recognised | Default method | Tool choice |
|---|---|---|---|
| Bore (counterbore) | Geometry | Spot, hole-mill rough, hole-mill finish | About half the hole diameter, a little larger |
| Countersink | Geometry | 3D or chamfer-tool rough, then surface finish | About half the hole diameter; a radius tool for finishing |
| Precision hole | By diameter, or by a marked colour | Spot, drill, hole-mill rough, then ream or spiral-finish | Reaming under 6 mm, hole milling above |
| Threaded hole | By diameter, or by a marked colour | Spot, drill, hole-mill rough, then tap or thread-mill | Tap or thread mill |
Holes that carry no tolerance and no thread are treated as plain holes: spot, then drill — and if the hole is larger than 10 mm, hole-mill roughing after the drill as well.
Precision and threaded holes are inferred from diameter, because a 3D model has no annotations. That inference can be wrong; you correct it in the tables described in Hole Making.
Pocket strategy #
Flat-bottomed pockets and walls are machined with either planar milling or floor-and-wall milling. RockCAM prefers planar milling where the geometry is easy to select, and floor-and-wall milling for more complex shapes.
The default sequence for a pocket is:
- Rough the whole pocket — either as a bulk cut or by following the contour.
- Rest-rough the walls, repeatedly if needed.
- Finish the floor.
- Finish the walls, sometimes together with the floor.
- Clean the wall corners, sometimes several passes.
For outer profiles and open pockets RockCAM roughs along the contour. If a pocket has a floor, it still prefers contour roughing, provided it can reach everything. Where the shape is not flat or has surfaces that must be swept, RockCAM switches to 3D roughing followed by rest roughing instead.