Studio computes toolpaths itself. You describe the part as features: a pocket, a contour, holes, an engraving. Studio chooses the cutting data with the twin's physical models and writes the G-code. It then runs the program in the twin before you cut.
Everything runs on your computer. Making a program needs no internet connection.
The quickest way is to describe the part to the AI assistant, for example:
Make a program for a pocket 40 × 30 mm, 3 mm deep, in 6061-T6, with a 6 mm flat end mill. |
The assistant uses the program_generate tool. It says what it made, how long it takes, and what the twin found.
A job is what Studio keeps about the part:
bracket.nc;Each program Studio writes is kept as a version, with the job that made it, in the programs folder. Nothing is lost when you make it again: the older versions stay.
The assistant can open a job and change it, the one you made in the CAM workspace too, for example:
Show me the job of bracket.nc, then make its pocket 3 mm deep and remove the second drilling. |
It uses the job_get tool to read the job, with a line on each operation, and job_edit to change values, remove, add or move operations. The changed job is made again as the program's next version and checked in the twin as before. When a change cannot be made, nothing is changed and the assistant says why. After the twin's own tries (the closed loop that takes chatter away), the job it reads is the last version's, with what those tries changed.
| Operation | What it cuts | Tool |
|---|---|---|
| Face | The top of the blank, flat | End mill |
| An area to a depth: rectangle, circle, polygon or a shape | End mill | |
| Contour | Along an outline: outside, inside or on it | End mill |
| Slot | A slot of a width along a line | End mill |
| Drill | Holes at points, pecked when deep | Drill |
| Bore | Holes larger than the tool, round a helix | End mill |
| Ream | Drilled holes to size | Reamer |
| Thread | Internal threads | Thread mill |
| Groove | A ring groove in a bore's wall: a circlip, an O-ring, a light trap | T-slot cutter |
| Chamfer | An outline's edge | V-bit or chamfer mill |
| Engrave | Text or lines | V-bit or small end mill |
| V-carve | Text or shapes, the depth following the width | V-bit |
| Perlage | Overlapping spots on a face, the watchmakers' decoration | End mill as wide as a spot |
| 3D roughing, 3D finishing | A mesh | End mill or ball end mill |
In the CAM workspace the panel has forms for facing, pockets, contours and chamfers (a shape imported, or a rectangle, circle or polygon given in the panel), slots, drilling, boring, thread milling and engraving. A job with other operations - an AI client's, or an example's - opens all the same: those operations are kept as the job gives them, and generated and checked with the rest. Selected, the panel lists their settings by program_generate's names (lengths in mm); an AI client changes them, or the job's file.
A pocket is cleared in layers. Its strategy sets the path in each layer:
Islands in a pocket are left standing. Rest machining clears only what a larger tool before it left.
A contour cuts along an outline, a layer at a time, climb milling. Tabs can hold a part that the contour cuts out.
A slot is cut full width in layers, then out to its width. A slot wider than the tool can be cut trochoidal: small loops along its line, for less load on the tool.
A chamfer follows an outline's edge with a V-bit, to the width you give. Engraving follows lines or the strokes of text at one depth; text starts at its X, is centred on it or ends there (Alignment in the panel). V-carving cuts a shape with a V-bit: the depth follows the shape's width, so corners come out sharp.
A mesh (STL, 3MF or OBJ) is roughed in levels, then finished. The finishing strategies are parallel, waterline, steep and shallow, and pencil.
A tool is written as its kind, its diameter and what else it needs, for example:
| Spec | Tool |
|---|---|
flat 6 n3 L20 | Flat end mill, 6 mm, 3 flutes, 20 mm stickout |
ball 3 L12 | Ball end mill, 3 mm |
drill 3.4 118 L20 | Drill, 3.4 mm, 118° point |
v 6 90 L18 | V-bit, 6 mm, 90° |
reamer 6 H7 n6 L32 | Machine reamer, 6 mm, for H7 holes |
thread 5 60 | Thread mill, 5 mm, 60° profile |
flat 2 n2 s4 l6 L10 | Flat end mill, 2 mm, on a 4 mm shank that starts 6 mm above the tip |
thread 2 60 d1.4 n1 s4 l6 L9 | Thread mill, 2 mm head, 1.4 mm neck up to 6 mm, 4 mm shank above it |
Give the stickout (L) for every tool. Studio then checks that the holder does not reach the blank, and the Z clearance on the setup sheet can judge the tool.
A small end mill on a stepped shank, and an undercut cutter (thread mill, T-slot, dovetail, lollipop), gives its shank's diameter (s) and how high above the tip the shank starts (l). Studio does not cut deeper than l where the shank would rub the walls of the cut. The twin checks the shank, and the touch probe's body, against the workpiece and the fixture.
The tool table lists the tools by their numbers. A feature names the tool it uses, and Studio adds the tool changes (T2 M6).
Studio starts from the material's cutting data for the tool. Then it uses the twin's models:
With verification on, Studio runs the program in the twin. If the run shows chatter or a load too high, Studio changes the program, for example with shallower layers, and tries again. Each version it tries is kept. The answer says what was changed and why.
These are estimates from physical models. Watch and listen to the first cut on the real machine.
Write a size with its fit, for example "d": "Ø12 H7" for a hole or "fit": "g6" for a shaft. Studio cuts the size to the middle of the fit's zone, and finishes the wall in a pass of its own.
Common fits can be named: sliding (H7/g6), locating (H7/h6), transition (H7/k6), press (H7/p6).
A small, tight hole is better reamed than milled. Studio says so, and you can drill it, then ream it with a reamer of its class.
The twin estimates the cutter's runout, and Studio allows for it on the sizes that have a fit.
A part machined from two sides needs two setups. Each setup has its own features, and says how the part comes to it: turned over about X or Y, held another way, its work zero found again. Studio writes one program for each setup, and checks each one in the twin on what the setups before it left. How to add setups and turn the part over: see Jobs with several setups.
Several parts can be cut from one plate. Studio places them close together, keeps a margin, and adds tabs so that the parts stay in the plate until the end.
With inch units, sizes can be written as fractions: 1/4, 1 1/2, 3/16". Inch tools are in the tool library, for example a 1/4" flat end mill. See Language and units.
Before you cut, run the program in the twin. The twin cuts its own workpiece and reports collisions, gouges, chatter, the spindle's load and the time. See Simulation.
|
A setup sheet tells the operator how to set the job up: the blank, the fixture, the tools, the work zero and the Z clearance. See Setup sheets.