CourseWiki/Machining/Milling

Milling Operations

Make a part on a simulated vertical mill: choose each tool, move it through the metal, and check what is left against the drawing. Facing, shoulders, pockets, slots, drilled, tapped and bored holes, countersinks and chamfers.

A vertical mill shapes a block with a turning tool moved in X, Y and Z

On a vertical mill the cutting tool turns in a spindle above the work. The work is clamped on the table, the table moves it front to back and side to side, and the tool comes down into it. Every shape the mill makes is the space the turning tool swept through.

X and Y: The two directions across the table. In this lesson X runs left to right as you face the machine and Y runs away from you, toward the back.
Z: Up and down, along the tool. Z+ is up, away from the work, so negative Z is below the finished top face. The raw top is at Z +1, so facing can remove metal at zero or positive Z while taking off that allowance.
Readout: The display that shows where the tool is, in X, Y and Z. A readout on a manual mill is often called a DRO, for digital readout. Here it shows the position of the tool’s tip.
Work zero: The point the readout counts from. In this lesson X 0, Y 0 is the front left corner of the block and Z 0 is the finished top face. Every dimension on the drawings is measured from those same edges and that same face.

The setup used in every job: a block 100 × 60, finished 20 thick, held by its front and back faces in a vise and resting on two parallels, bars of equal height that lift it off the floor of the vise. The raw block stands 1 mm proud of the finished top. Below Z −8 the vise jaws are in the way at the front and back, and a hole drilled through along those edges would run into a parallel.

On a real knee mill the table carries the work under a spindle that stays put in X and Y. In the simulator you move the tool instead. The readout tells the same story either way: where the tool’s tip is, measured from work zero.

Each kind of tool cuts a shape of its own, and some cannot cut sideways

The tools in the simulator, side on and at one scale, each with its tip on the same line. The darker part of each is the part that cuts.

Face mill: A wide body with cutting inserts round its rim. It is fed across the work to leave a broad flat face. The one in the simulator takes at most 4 mm in one pass. The inserts sit at the rim, not across the middle, so it is brought down beside the work and then fed in, never pushed straight down into the metal.
End mill: Cuts on its sides and its end. The end mills here are centre-cutting: their end teeth reach the middle, so they can be fed straight down into the metal and then moved across to cut pockets, slots, steps and walls. An inside corner they leave is rounded to the cutter’s own radius.
Spot and chamfer tool: A pointed tool with a 90° point. Fed down, it cuts a cone: the start of a hole, or a countersink round the mouth of one. Run along an edge, it bevels the edge, which is a chamfer.
Drill: Cuts only at its point, as it feeds down along its own axis. It leaves a round hole its own size, with a cone at the bottom from its point. It must never be pushed sideways in the metal.
Tap: Cuts a screw thread into the wall of a hole that is already there. It only goes straight in and straight back out.
Boring head: An adjustable single cutting point on an offset bar. Set to a diameter and fed down a hole, it opens the hole to that size. Its bar has no cutting edge at the centre, so it needs a hole to start in.

This is a teaching rack, not a list of what to buy or use. The sizes are illustrative. A real cutter’s length, number of teeth and depth of cut come from its own data and from the person responsible for the machine.

The tool’s centre runs one radius away from the wall it cuts

The readout shows where the centre of the tool is. The metal is cut by its edge. To leave a wall at a given place, put the centre one radius away from it, on the side being cut away.

Worked example. A shoulder’s wall belongs at X 75, with the metal to the right of it cut away. A Ø12 end mill has a 6 mm radius, so its centre runs along X 75 + 6 = X 81. Run it along X 75 instead and the wall ends up at X 69, 6 mm too far into the part. That metal cannot be put back.

Inside corners take the cutter’s radius. A round tool cannot reach into a sharp inside corner, so a pocket’s corners come out rounded to the radius of the cutter that made them. A drawing that allows R4 at most calls for a cutter no bigger than Ø8.
Outside corners stay sharp. Going round the outside of a corner, the tool swings about it and never cuts into it.
A slot is the width of the cutter that made it in one pass. A cutter moved in a straight line leaves a groove exactly its own width, with round ends of its own radius.

When a cutter cuts with its side, the metal is on one side of it or the other. With the cutter turning clockwise seen from above, metal on the cutter’s right as it moves is climb milling, and metal on its left is conventional milling. The simulator says which each side cut was. Climb and Conventional Milling explains the difference.

Holes: drilled to size, threaded by a tap, opened up by a boring head

A drill leaves a hole of its own diameter. A hole’s depth on a drawing is measured to where the hole stops being full size, not to the tip of the cone the drill point leaves below that.

A tapped hole starts as a smaller drilled hole

A tap cuts its thread into the wall of a hole, so the hole has to be drilled smaller than the thread first, to the tap drill size. For the common metric coarse threads that size is close to the thread’s outside diameter minus its pitch, the distance from one thread to the next:

Tap drill ≈ thread diameter − pitch. M6×1: 6 − 1 = Ø5.0. M8×1.25: 8 − 1.25 = Ø6.75, drilled Ø6.8.

Drilled too small, the tap has to cut too much metal and can break. Drilled too big, the thread is shallow. The simulator checks the hole against a simplified minor-diameter band and refuses a severely undersize pilot. This does not establish functional thread fit: pitch diameter, thread form and a real thread gauge are separate checks.

Drill deeper than the thread you need

The first few threads of a tap are ground away to a taper so that it can start in the hole. Those threads cut only part of a thread, so full thread stops short of the tap’s tip. In a hole with a bottom, the tap has to go deeper than the full thread you need, and the drilled hole deeper again, past the drill’s point. This simulated tap has a 4-pitch cutting chamfer; real taps vary. The job calls for full thread reaching Z −10 from the finished face. Its countersink removes the first part of the thread, so that is not 10 mm of surviving full-thread length.

Sizes no drill gives

Drills come in fixed sizes. A boring head is set to the size you need and fed down a hole already big enough for its bar, which makes it the tool for a hole of an exact, larger size.

Simulator: make the part on the drawing, then inspect it; Interactive

Simulator: make the part on the drawing, then inspect it

Job 1: Face the top, then cut a shoulder. Face the top flat at Z 0.00, then mill a shoulder 25 mm wide and 6 mm deep across the right-hand end.

Job 2: A pocket with tight corners, and two clearance holes. Face the top, mill a 40 × 24 pocket 6 deep whose inside corners are no rounder than R4, and drill two Ø6.6 holes right through.

Job 3: A slot and two tapped holes. Face the top, mill a slot 10 wide with full-round ends, and make two countersunk M6×1 holes whose full thread reaches Z −10 or deeper, measured from the finished face.

Job 4: A boss with a bored hole and chamfered edges. Face the top, mill away everything round a 50 × 30 boss so it stands 5 high, bore a Ø20.00 hole through it, and chamfer its top edges 1 × 45°.

Start by examining the finished Target, then choose a tool and cut Your work. In Compare, gold is metal still to remove and striped red-orange is metal cut past the drawing. The inspection measures the part that is left after every move. Nothing checks which tools you used or in what order: any way of making the right part passes.

How to drive it. Target shows the finished nominal part; Your work shows the block you are making. Compare marks what still needs work, using the drawing’s allowed limits. In Inspect / orbit, dragging and the arrow keys move only the camera. Home restores the view; the View list also offers top, front, below and 2D sections.

Choose a tool and its size, then choose Feed X, Feed Y or Feed Z to drag its tip along that machine axis. The path previews while you drag; releasing starts the feed. Place XY places the centre at the current Z. In these feed modes the arrow keys move the selected machine axis. To go to an exact place, type X, Y and Z under Move to and press Move; the tool goes up before it goes across, and across before it goes down. The handwheel buttons and the selected-axis keys move one step at a time. A move that would break a tool or hit the vise stops where it would happen, and says why. Undo takes back the last move: the one thing a real mill cannot do.

Things to try in the simulator; Checklist

Things to try in the simulator

In job 1, load the face mill, move it over the block and try to lower it straight onto the metal. Read why it stops.
Lower the face mill to Z 0.00 beside the block and drag it across. Watch the top view and the sections: the raw top is 1 mm above Z 0. Overlap a second pass until the top face check matches.
Cut the shoulder with the Ø12 end mill with its centre on X 75 instead of X 81. Read the inspection, then use Undo and cut it again in the right place.
In job 2, clear the pocket with the Ø12 end mill and read what the inspection says about its corners. Undo, and clear it with a smaller cutter.
Watch the gold as you cut: it is metal the drawing does not keep. Cut one pass a little too deep and see where the striped red-orange appears in the top view and the section.
In job 3, try to tap a hole you drilled with the Ø6.0 drill, then one you drilled with the Ø4.2. Then drill Ø5.0 only 10 mm deep and tap it as deep as it will go. How much full thread do you get?
In job 4, try the boring head before there is any hole. Then drill one first.
Make one part two different ways, for example job 4 with the face mill doing the area round the boss, and again with an end mill. Both pass.

What the simulator leaves out

The 3D target is a nominal guide sampled at 0.25 mm in X and Y. Its flat floors have the drawing’s depth; its small curved outlines are approximations. The cut surface is derived separately from the analytic tool paths. Neither picture is a dimensional gauge: inspection uses the drawing’s allowed limits, including smaller corners where the drawing says R4 max. Complex conical histories or very long cut histories switch to 2D sections to keep the controls responsive. The work is kept, and Undo or a fresh block can restore the 3D view.

The simulator is a model of where metal is and where tools can reach. It does not check speeds, feeds, forces or finish, and passing a job here says nothing about whether a real setup could take the same cuts. Feeds and Speeds is about those numbers.

Only straight down and straight across. The tool axis is always vertical and nothing is undercut, so every shape is a height above each point of the table.
Tools are exact and rigid. A hole is exactly the drill’s size, a cutter never bends or wears, and edges come out without burrs.
Threads are recorded, not drawn. The simulator keeps the size of the hole a thread was cut in and how deep its full thread runs, and checks that later cuts have not taken the metal it is in. It does not model the thread’s form or fit.
No chips, coolant or heat, and no limit on depth of cut except where a tool’s cutting edges run out.

How the inspection decides, and what its numbers are

The part is kept as a list of every cut: the space each tool swept through. The top of the metal at any point is the raw top lowered by every cut that reaches that point. The inspection measures walls, floors, holes and chamfers at sampled locations on that surface, with numbers rounded to a hundredth of a millimetre. A display grid plus probes derived from each cut and drawing boundary look for excess metal and gouges. Passing means the modeled checks pass; it does not certify every point of a real surface. Removed volume is an estimate from the 0.25 mm grid; very small cuts can change the analytic surface without a resolved grid volume. Walls and holes pass within ±0.10 mm, the bore within ±0.05 mm, and floors and faces within ±0.05 mm.

Tapped holes are accepted when their drilled diameter falls inside the minor-diameter limits for a 6H internal thread: 4.917 to 5.153 mm for M6×1, and 6.647 to 6.912 mm for M8×1.25. These are finished minor-diameter limits, used here as a teaching proxy for pilot quality; they are not universal tap-drill recommendations or a complete 6H inspection.

Sources: Gühring’s metric table, page 46, distinguishes nominal tap-drill sizes from finished minor limits. Haas’s M6×1 example specifies a 5 mm tap drill and a 2P–3P chamfer, illustrating why the model’s 4P is not universal. Vermont Gage explains the separate thread and cylindrical gauge checks.

Appears in

DET 330 DET Machining Fundamentals