Machine tools — Services

Admin panel section: Services → Machine tooling.

Why this matters — the main thing. The client themselves maintains their tooling magazine of all types: saws, cutters, blind and through-hole drills. Then our service does 100% of the technologist's work: for each part in the order the postprocessor picks the cutter for the contour radius itself, calculates the number of depth passes, selects drills by diameter, and — more importantly — adapts operations to what your machine can actually do. A drilling that cannot be performed is replaced with a pocket (routing). A routing that lacks tooling is replaced with a groove. A groove that the machine cannot saw — by routing. Everything that can in principle be done on this machine will be adapted and assembled into a program. Everything that cannot be done at all is carefully cleaned up with a note in the order log. This way each of your machines gets 100% working programs: the technologist doesn't need to intervene, no «operation on operation» occurs at the machine. What competitors spend hours of technologist work on per order, our service does in seconds after confirmation. All exceptions (what was cleaned up, where and why) the user sees immediately — in the order's log file. See «CNC program generation system overview».

What it is

The catalog of tooling physically installed on your machines: saw blades, cutters, drills. This section and Machines are a unified pair: the machine describes «what it can do in principle», the tooling — «what exactly it cuts with». The postprocessor picks tools from this catalog automatically, based on the geometry of each part in the order.

Tooling categories

Saws and cutters (cutting and routing)

Kerf width (mm): The thickness of your specific saw's cut — measured by fact, not from datasheet. Used by the cutting optimizer: every gap between parts = saw width. Accuracy here affects the number of parts that fit in a sheet.
Max routing depth (mm): How deep the cutter can plunge into material. Must be ≥ thickness of the thickest panel you process. If the groove depth exceeds this value, the postprocessor automatically splits the operation into several passes.
Diameter (mm): For saw blades and cutters. The postprocessor picks the cutter of maximum diameter depending on the internal radii of the part contour. If the biggest cutter does not «fit» into corners, a second pass with a smaller cutter is added for finishing.
Cutting type: Full sheet (cutting) / along contour / curvilinear routing.
Cutter side (right / left): If the project is calculated for a right cutter and you have a left one — the postprocessor automatically reverses the toolpath.

Blind-hole drills (dowelling)

Drill holes not all the way through — for pins, confirmats, dowels.

Diameter (mm): The diameter your drill has. We assume no «typical» values — the postprocessor works with the toolset you entered in the magazine.
Max depth (mm): How deep your specific drill goes into the panel. The value is taken from its datasheet or measured by fact.
Directions (checkboxes): Face (F), left end (L), right (R), top (T), bottom (B), back (BB). Tick only those actually available — not «per datasheet», but by physical machine tooling. If you have one seat for an edge drill, the postprocessor accounts for that and excludes operations with two different diameters on the same side, distributing them or replacing with other methods.

Through-hole drills

Drilling all the way through — handles, pass-through fasteners. Same fields, usually fewer directions. Through holes from the face side the postprocessor may automatically move to the back side if the program is shorter or more convenient that way.

Control fields

Machine: Which machine it sits on. One machine has several cutters/drills.
Primary: Marks the primary (main) drill group on this machine — upper or lower. The program generation algorithm starts from this group and distributes operations from it to use the equipment optimally. If the primary group lacks the needed diameter or direction — the algorithm falls back to the auxiliary one.
Active: Disable during regrinding/replacement — the postprocessor will not use this tool in new programs.
Tool number: The tool number in the machine's tool magazine — a whole number only, no letter. When the NC program is exported, the prefix T is added to the number automatically: 1 → T1, 8 → T8. If the number is not set, the field stays empty — this is not an error.
Excluded from tool auto-selection, must be named explicitly: The flag removes the cutter from automatic selection: the platform stops picking it on its own when it looks for a tool by diameter, depth and radius. The cutter stays operational and is used whenever it is named explicitly — in a template or in the operation itself. If the flag leaves an operation with no suitable cutter at all, the operation is not performed and an error is raised: the platform will not fall back to the flagged cutter. The flag exists for cutters only, and it cannot be set on the main cutter — that one supplies the firm-wide default cutter diameter.

What the postprocessor automates for you

Behind a correctly described tooling magazine and machine parameters, dozens of technological nuances are resolved automatically — nuances that take a technologist hours:

Cutter selection by radii — the largest that fits into part corners; a smaller one for finishing straight corners; splitting into passes when depth is exceeded.
Operation substitution when tooling is missing — no required drill → automatic substitution by a pocket; vertical groove by saw → if the machine cannot, it is substituted by routing.
Toolpath reverse — for machines with the opposite cutter side.
Edge pre-cut — on machines with both cutters it is included in the program; on machines with only the right one — a separate pre-cut program is created.
Cutter entry/exit — with the given parameters the cutter does not exit the part boundary, lead-in points are placed on part sides (important for machines with auto-trim).
Six-sided processing — for machines supporting only five sides, the program is split into 2–3 parts or the part is rotated 90 / 180 / 270°.
Part orientation — the long side is automatically laid horizontally for optimal processing.
Minimizing the number of programs — layout variants are explored to yield the minimum possible number of files under all machine constraints.

Everything the system cleaned up itself (replaced one operation with another, discarded the impossible) and everything that didn't work automatically is written to the order log file: what was done, where (which part, which side, which coordinate) and why (no required drill diameter, max depth exceeded etc.). The user sees this log immediately: it's clear what to pay attention to, whether something needs fixing in the tooling magazine, or whether this is a normal adaptation to the current machine fleet. The program generation history is available in CRM.

What matters

Accurate sizes = accurate programs. Declared saw width 4 mm, actual 4.4 — every cut is 0.4 mm shorter than expected. On large cutting plans the centimeters of error accumulate. Measure «by fact», not «by datasheet».
Drilling directions require physical verification. The brochure says «6 directions», but physically there is a group for 3. Tick only what exists — otherwise the postprocessor will place an operation where there is no spindle.
After regrinding a cutter its diameter decreases — update the value, otherwise the CNC program calculates the toolpath by the old diameter and leaves gaps or overflows.
Blind and through-hole drills are separate entries, even if physically it's the same drill: for the blind one the exact depth matters, for the through one — it doesn't.
Before changing a material collection (thin 16 mm → thick 38 mm) check that the max cutter and drill depth allows processing this. Otherwise first «update tooling», then «accept orders».
Supported program formats: MPR (WoodWOP), BPP (BiesseWorks), XML-KDT (Kitchen Design Technology), SCX (Nanxing), CSV for Cutrite. From you — correctly describe the tooling, everything else the postprocessor assembles itself.

How the dowel drill is chosen

The postprocessor picks the end-face drill for a dowel from your tool store itself, starting from a nominal diameter:

The nominal is Ø5 mm. For the AGT firm the nominal is Ø5.5 mm, and it applies to all of its projects regardless of the part thickness.
If a drill of exactly that diameter exists, it is used.
If not, the nearest one within ±1 mm of the nominal is taken. When two drills are equally far away, the smaller diameter wins.
The drill must be a blind end-face one and must reach the required hole depth.
If there is no suitable drill in that range, no dowels are placed at all. Not out of stubbornness: such a hole physically cannot be drilled, so it must not go into the program.

So if the project was expected to have dowels and it has none, look into the store of blind drills first: is the needed diameter there, and does it reach deep enough?