7 Conventional Milling Methods: How Many Do You Know?
Most milling work still falls into seven basic setups. This guide walks through each one: what it cuts, which tool to load, what parameters to start with, and where the setup goes wrong. Read it before you quote a part or program a first article.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
- 7
Key takeaways
Face Milling: Squaring a Part and Setting a Datum
Face milling is the first operation on most blocks. A face mill or shell mill with a 45° lead angle sweeps across the top of the workpiece to produce a flat surface. That surface becomes your Z datum, so the flatness you get here propagates into every later operation.
For aluminum, run a 63 mm or 80 mm face mill at 800–1,200 m/min surface speed and 0.08–0.15 mm per tooth feed. For 4140 steel, drop to 150–250 m/min and 0.05–0.10 mm per tooth. Depth of cut of 0.5–2.0 mm per pass is normal on a rigid setup.
The classic mistake is taking a heavy cut on a part held only in a vise with 5 mm of grip. The part lifts, the insert chips, and the surface shows chatter marks. Support the part across its full width, or use a fixture plate with toe clamps.
Check flatness with a dial indicator before you move on. If the face is out by 0.03 mm, every hole you drill after that inherits the error.
Slot Milling and Step Milling: Two Cuts, Two Cutter Choices
Slot milling cuts a channel narrower than the cutter diameter in most cases, or exactly the cutter diameter when you plunge. A two-flute carbide end mill is the safe choice for slots because chip evacuation is the real constraint, not cutter strength.
For a 6 mm slot in 6061, a 5 mm two-flute end mill at 12,000 rpm and 0.05 mm per tooth feed works well. Take 0.5–1.0 mm axial depth per pass and use air blast or flood coolant. Never let chips recut; a packed slot snaps small tools.
Step milling cuts a shoulder or a ledge. Here a three or four-flute cutter gives a better wall finish because the extra flutes stiffen the core. Leave 0.2–0.3 mm on the wall and floor for a finishing pass.
One warning that matters: if your slot is exactly the cutter diameter, the tool rubs on both sides at once. That is the fastest way to burn an edge. Use a smaller cutter and a trochoidal path when the slot is deep.
Contour Milling and Pocket Milling: Controlling the Path
Contour milling follows a profile, inside or outside. It is how you cut curved edges, bosses, and the outline of a plate. Use a cutter with a small corner radius rather than a sharp corner; a 0.4–0.8 mm corner radius spreads the load and lasts much longer.
Lead in with a tangential arc, not a straight plunge. The arc lets the cutter enter the cut gradually, which avoids a witness mark on the finished wall. Keep radial engagement at 5–10% of cutter diameter for finishing passes on hardened or gummy material.
Pocket milling removes material inside a boundary. The two standard strategies are offset (following the pocket shape inward) and trochoidal (circular loops at a constant radial engagement). Trochoidal wins on deep pockets in steel because the chip load stays even.
For a 40 mm deep pocket in 4140, a 10 mm four-flute cutter at 2,500 rpm, 0.06 mm per tooth, and 0.3 mm radial step-down is a realistic starting point. If the floor shows a spiral pattern, your step-down is too aggressive or the tool is pulling out of the holder.
Rough the pocket to within 0.3 mm of the wall, then finish in one continuous pass. Stopping mid-wall leaves a visible step.
Thread Milling and Form Milling: When a Tap Will Not Do
Thread milling cuts a thread with a single or multi-point tool that orbits the hole. It costs more per hole than tapping, but it gives you a full thread in a blind hole with no chip packing, and one tool covers a range of diameters.
Run thread mills at 30–50% of the surface speed you would use for a tap in the same material. For an M8 × 1.25 thread in 316 stainless, a single-point mill at 1,500–2,000 rpm and 0.05 mm per tooth is reasonable. Use a helical entry, not a straight plunge.
Form milling uses a shaped cutter to produce a profile in one pass: a radius, a dovetail, a T-slot, or a gear tooth. The cutter shape is the limiting factor, so lead time for a custom form tool runs longer than for a standard end mill.
Use form milling when the profile repeats many times and the volume justifies the tool. For one or two parts, a standard ball or corner-radius cutter with a 3D toolpath is cheaper and faster to set up.
Step by Step: Choosing and Running a Milling Method
Work through this sequence from the drawing to the finished feature.
- 1Read the feature, not the drawingList every feature on the part as a shape: flat face, slot, shoulder, pocket, thread, profile. Each shape maps to one of the 7 conventional milling methods. Do this before you open CAM.
- 2Set the datum from the largest flat faceFace the part first. A face mill at 0.5–2.0 mm depth gives you a flat Z zero. Mark the datum on the setup sheet so the operator and the CMM agree.
- 3Pick the cutter by feature width and depthSlot width 6 mm: use a 5 mm two-flute cutter. Pocket 40 mm deep: use a 10 mm four-flute cutter with a corner radius. Never match cutter diameter exactly to a slot width.
- 4Set speeds from the material, not the machineAluminum 6061: 800–1,200 m/min. 4140 steel: 150–250 m/min. Titanium TC4: 40–70 m/min. Start at the low end and raise feed until the chip color and sound tell you to stop.
- 5Choose climb milling and check backlashClimb milling throws the chip behind the cutter and gives a better wall finish. Confirm the machine has backlash compensation on the axis you are using, or the cutter will rub on the return pass.
- 6Leave stock for a finishing passLeave 0.2–0.3 mm on walls and floors during roughing. A single continuous finishing pass removes it and produces Ra 0.8–1.6 μm on most materials.
- 7Measure the first part, then adjustCheck the critical dimension on the machine or on a CMM before releasing the run. If the wall is 0.04 mm over, offset the cutter radius and re-cut one test part.
- 8Log the parameters that workedRecord cutter, speed, feed, and depth for the job. The next run of the same part should start from that log, not from scratch.
Milling Method Selection Chart
Match the feature to the method, then to the cutter and a starting parameter.
| Method | Best for | Typical cutter | Starting point |
|---|---|---|---|
| Face milling | Flat top surfaces, datums | 63–80 mm face mill | 0.08–0.15 mm/tooth, Al |
| Slot milling | Channels, keyways | Two-flute end mill | 0.05 mm/tooth, 0.5–1.0 mm deep |
| Step milling | Shoulders, ledges | Three or four-flute end mill | 0.3 mm stock on wall |
| Contour milling | Profiles, bosses, outlines | Corner-radius end mill | Tangential arc lead-in |
| Pocket milling | Closed cavities | Four-flute, trochoidal path | 0.3 mm radial step-down |
| Thread milling | Blind holes, hard material | Single-point thread mill | 30–50% of tap speed |
| Form milling | Repeating profiles | Custom shaped cutter | One pass, tool shape sets limit |
Pick the method before you pick the machine
The seven conventional milling methods cover almost every prismatic feature. Match the method to the shape, set the datum from a faced surface, and leave stock for one finishing pass. That sequence holds ±0.005 mm without heroics.
Frequently Asked Questions
Which of the 7 conventional milling methods should I use for a flat plate with holes?
Face milling first to establish a flat datum, then drill or interpolate the holes. If the holes are large or need a tight tolerance, circle-mill them with a helical entry instead of drilling, because the interpolated path lets you correct the diameter with a cutter offset.
Slot milling is not the right choice for round holes. Use it only for straight channels and keyways.
Is climb milling always better than conventional milling?
On a machine with backlash compensation and a rigid setup, climb milling gives a better surface finish and longer tool life. It also pulls the part toward the cutter, which is safer when the workholding is solid.
Use conventional milling when the machine has significant backlash, when you are cutting a rough scale or casting skin, or when the part is held lightly. Conventional milling pushes the cutter away from the workpiece, which protects the edge on interrupted cuts.
How deep can I cut in one pass when pocket milling?
For a 10 mm four-flute cutter in 4140 steel, 0.3 mm radial step-down with 1.0–1.5 mm axial depth is a realistic starting point on a rigid setup. In 6061 aluminum you can go deeper, often 2–3 mm axial, because the material clears chips more easily.
The limit is usually chip evacuation and tool overhang, not the spindle. If you hear a high-pitched squeal, reduce depth before you reduce speed.
When is thread milling worth the extra cost over tapping?
Thread milling pays off in blind holes, in hard or gummy materials, and when one tool must cover several thread sizes. It also produces a full thread with no risk of a broken tap stuck in the part.
For high-volume through-holes in aluminum, tapping is still faster and cheaper. Choose thread milling when part value or material cost makes a broken tool expensive.
Do I need 5-axis machining to run these methods?
No. All 7 conventional milling methods run on a 3-axis machine. The part is repositioned between operations, or a rotary table is added for the fourth axis.
Five-axis machining helps when one setup must reach several faces, when the part is too heavy to move repeatedly, or when a contoured surface needs the tool held normal to the surface.
What tolerance can I hold with these methods?
On a rigid setup with a finishing pass, ±0.005 mm is achievable on critical dimensions. Surface finish typically lands at Ra 0.8–1.6 μm after finishing, and down to Ra 0.2–0.8 μm with a dedicated finishing pass and the right cutter.
The practical limit depends on the feature. A deep pocket wall is harder to hold than a short shoulder because tool deflection grows with depth.
Send us your part and we will pick the method
Upload a STEP file and get a quotation with free DFM analysis within 12 hours. No minimum order quantity, from one prototype to 10,000+ part runs.
12-hour quote±0.005 mm100% inspectionNDA on request
More machining notes
We publish setup notes, tooling trials and inspection data from the factory floor.
