RockCAM chooses tools from a tool library and speeds and feeds from a parameter table. It never invents a tool, so the quality of the program is bounded by the quality of the library. This is the page nearly every shop has to change before the output matches reality.
The RockCAM settings page holding the tool library and the parameter table.
Tool library #
RockCAM supports two kinds of library: a standard Excel tool library, and the tools already defined in your operation template. You choose which one to use.
The setting that switches between the standard Excel library and tools from the template.
The standard Excel tool library #
Choose the standard library and RockCAM opens a file in an Excel-style editor. Edit it, save it, done.
The tool library open in the editor, with one row per tool.
The columns, from left to right:
| Column | Meaning |
|---|---|
| ID | Leave blank |
| Diameter | In millimetres |
| Corner radius | Tool tip corner radius |
| Tool length | Overall length |
| Flute length | Cutting length |
| Flutes | Number of flutes |
| Taper angle | Used by spot drills, chamfer tools and drills |
| pointLength | Leave blank |
| Description | The name shown for the tool in NX. This one matters — write it clearly |
| Type | One of the fixed types below |
| Tool number | The pocket number on the machine, shown in NX |
| Usage | What the tool is for — roughing, semi-finishing, finishing and so on |
The tool types:
- ChamferC — chamfer tool.
- Mill — general end mill, cutting with either the bottom or the side. A corner-radius mill is also this type.
- MillBall — ball nose.
- MillFace — face mill, facing only.
- Drill — drill.
- PDrill — flat-bottom drill.
- Spot — spot or centre drill.
- REAMER — reamer.
- TAP — tap.
- THREAD — thread mill.
The usage values apply mainly to milling tools:
- F — finishing.
- SF — semi-finishing.
- R — roughing.
- FE — floor finishing only.
- CK — plunge milling only.
Tool number and tool usage #
The tool number is the pocket it occupies on the machine. It also acts as a priority: RockCAM’s tool selection is involved, but a tool with a number is preferred. Give your routine tools a number — the 10 mm rougher, the 63 mm face mill — and they will come up in the programs.
Usage matters almost as much. A tool marked for roughing is used on roughing operations, which is how you keep roughing and finishing tools apart. Leave it blank and the tool is treated as suitable for both. Numbered and typed tools are preferred over untyped ones.
Using tools from the template #
Instead of the Excel library you can draw tools from the operation template. The names have to match, so this needs a bit of care.
The tool list in the operation template, in the machine view.
Select use tools from the template and a set of name fields appears. They must be filled in, or RockCAM will not find the tools. Each field is a pattern that matches the template tool names.
The name-pattern fields that match template tool names.
The pattern is written as prefix, , suffix. The matches anything.
Two patterns entered: one for roughing tools and one for semi-finishing tools.
Two examples: D matches every tool whose name begins with D, and D_ZD matches names that begin with D and end with _ZD. The wildcard can cover text as well as digits, so D*Rough would match D10Rough — but keep the prefix and suffix as specific as you can, or a pattern will pick up tools you did not intend.
Parameter table #
The parameter table holds speeds and feeds. RockCAM picks the tool first, then looks the speed and feed up by tool diameter, tool type and the method being used.
The speed and feed table, indexed by tool type and diameter.
Selection uses three things:
| Input | Where it comes from |
|---|---|
| Tool type | The type in the tool library |
| Diameter | The diameter in the tool library |
| Method | One of: side finish, side rough, side hole-milling, chamfer, bottom finish, bottom rough, bottom hole-milling, drill, surface finish |
The methods are what makes one tool behave differently on a wall and on a floor, and differently again when it is milling a hole rather than cutting a slot.