This is the manual of Studio 1.0.2, an earlier version. The manual of the latest version
Documentation 1.0.2 User manual
Making programs (CAM)
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.
What the CAM does
- Shapes are data. A feature's shape is a rectangle, a circle, a polygon, a path from an SVG or DXF file, text, or a mesh (STL, 3MF, OBJ) for 3D work.
- Toolpaths are computed. Studio offsets the shape, clears the area, and links the moves.
- The twin chooses the cutting data. Speed, feed and depth come from the material, then from the twin's models of the spindle's power, the cutting forces, chatter and the tool's deflection. They are estimates.
- The twin checks the program. Studio can run the program in the twin before you cut, and change what the run shows to be too much.
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: features, tools and material
A job is what Studio keeps about the part:
- its name, which is also the program's name, for example
bracket.nc; - the material, for example 6061-T6 (other standards' names, such as EN AW-6061, are understood);
- the tool in the spindle and the tool table;
- the features, in the order they are cut.
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.
Operations
| 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 |
| 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 |
| 3D roughing, 3D finishing | A mesh | End mill or ball end mill |
Facing, pockets and contours
A pocket is cleared in layers. Its strategy sets the path in each layer:
- rings (the default): rings from the middle out to the wall;
- zigzag: passes to and fro;
- adaptive: a path that keeps the tool's engagement even, for deep pockets in harder materials.
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.
Slots
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.
Holes: drilling, boring, reaming and threads
- Drilling uses the controller's drilling cycle. A hole deeper than three times the drill's diameter is pecked.
- Boring cuts a hole larger than the end mill round a helix. Up to twice the tool's diameter.
- Reaming brings a drilled hole to size with a reamer of the hole's fit. Drill the hole first.
- Thread milling cuts an internal thread with a thread mill, from the bottom up. Metric (M8), unified (1/4-20 UNC), pipe (G1/4) and tapered pipe threads (1/4 NPT, Rc1/4) are known by their names.
Chamfers, engraving and V-carving
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. V-carving cuts a shape with a V-bit: the depth follows the shape's width, so corners come out sharp.
3D roughing and finishing
A mesh (STL, 3MF or OBJ) is roughed in levels, then finished. The finishing strategies are parallel, waterline, steep and shallow, and pencil.
Tools and the tool table
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).
Cutting data from the twin
Studio starts from the material's cutting data for the tool. Then it uses the twin's models:
- the spindle's power: the cut uses at most about 80 % of it;
- chatter: the depth and speed stay where the twin's stability model expects a stable cut;
- the fixture: the cut's force stays well under what the fixture holds;
- the tool's deflection: finishing passes are kept light.
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.
Fits and tolerances
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.
Several setups
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.
Parts nested on a plate
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.
Inch dimensions and fractions
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.
Checking a program in the twin
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.
Caution
The twin checks the program against the set-up you gave it. Set the twin up as the real machine is: the same blank, fixture, tools and work zero.
The setup sheet
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.