Slotting, Plunging and Helical Interpolation: The Right Entry Strategy in Full Engagement

Full-slot milling is the most demanding engagement condition in milling: the tool removes material equal to its own diameter in a single pass, and there is no free surface for the chip to escape into. This article covers the limits of full-slot milling, the straight plunging, linear ramping and helical interpolation methods used to enter a closed pocket or slot, the permissible angle ranges, and the feed correction that is mandatory in helical interpolation.

1. The engagement condition in a full slot

In a full slot the radial engagement equals the tool diameter (ae = D). From the point where it enters the material to the point where it leaves, the cutting edge stays in contact along half the tool circumference, that is, through an engagement angle of 180°. Unlike the short contact arc typical of side milling, here the edge is under load for roughly half of each revolution.

This condition has four direct consequences:

• Chip evacuation is blocked. The only route out for the chip is the tool's own flute. Once the flute fills up, the chip is recut; a chip cut a second time on the edge is both abrasive and a source of adhesion.
• Heat accumulates. Because the contact time is longer, the cooling interval of the edge is shorter. Inside a closed slot it also becomes harder for the coolant to reach the cutting zone, which accelerates the wear mechanisms.
• Radial forces balance out, but are not stabilised. The two walls of the slot push the tool against each other. Although the forces theoretically cancel out, uneven wear of the edges and runout upset this balance; the result is dimensional deviation and chatter.
• The share of face cutting increases. At the bottom of the slot the end face of the tool also cuts. For this reason the feed in slotting has to be reduced relative to side milling.

Critical point: A full slot is less a cutting parameter problem than a chip evacuation problem. Even with correctly chosen parameters, the tool breaks if the flute volume is insufficient.

2. Keeping the flute count limited in slotting

By the relation vf = fz × Z × n, increasing the flute count directly increases the feed. However, at a fixed diameter the cross-sectional area of the chip flute shrinks as the flute count rises. In a full slot, where the flute is the chip's only way out, this narrowing means clogging outright.

The last row is a deliberate exception. On very small diameter tools the dominant cause of breakage is not clogging but deflection and core weakness; for this reason manufacturer publications recommend a high flute count and very small axial steps.

The same logic applies to axial depth. Whereas an axial depth of one to two times the diameter is considered normal in side milling, in a full slot the depth has to be divided into steps and the chips cleared between each step. Stepped progression allows the flute to empty out on every revolution.

3. Avoiding the full slot: the trochoidal approach

When the slot width is greater than the tool diameter, entering full engagement is not mandatory. In the trochoidal (slicing) strategy a smaller diameter tool opens the slot by following circular paths at narrow radial engagement and high axial depth. In practice the radial engagement is kept in the range of roughly 5–15% of the diameter; Sandvik Coromant states that the radial depth of cut in trochoidal milling should not exceed 20% of the diameter. The axial depth, on the other hand, can be taken up to twice the diameter.

When the radial engagement is reduced, chip thinning comes into play and the feed has to be increased accordingly; this correction is covered in detail in the chip thinning guide. The method as a whole is examined in the trochoidal milling guide.

4. Entering a closed volume: four methods

When a closed pocket, a blind slot or a hole is machined, the tool has to enter the material in the axial direction. The four basic methods used and their conditions are as follows.

Pre-drilling

Manufacturer publications present the safest practice as drilling a pilot hole to the pocket depth that is 5–10% larger than the end mill diameter. The end mill descends into this hole without force and passes into side milling. The method carries the cost of a tool change, but in return gives the most predictable result in terms of tool life.

Straight plunging

In straight plunging the entire cutting force is concentrated along the Z axis and the chip is trapped underneath the tool. Since the end face of an end mill is not designed like a drill, the cutting speed falls to zero towards the centre; at the centre there is crushing rather than cutting. For this reason straight plunging is only possible with centre cutting tools, and on a tool that does not cut to centre it leads directly to breakage.

Straight plunging does have an area of advantage of its own. When a deep pocket is machined with a long tool, the force acting axially rather than radially creates a stable load on the spindle and limits the tendency to chatter. For this reason plunging performed with dedicated plunge milling tools is regarded as a separate strategy for deep cavity roughing and long overhang set-ups. Straight plunging with a standard end mill, however, does not fall within this scope.

Linear ramping

In linear ramping the tool advances simultaneously along the Z axis and one of the X or Y axes. Cutting takes place in three separate zones at once: the periphery of the leading edge, the face of the leading edge and the face of the trailing edge. For this reason manufacturer publications recommend reducing the feed along the ramp to roughly 75% of the normal value and continuing at the reduced feed for a distance equal to the tool diameter after the ramp ends.

The permissible ramp angle depends on the tool and the material. The maximum value given in the catalogue is binding; the general ranges are as follows:

Linear ramping has to be kept to narrow slots; manufacturer publications recommend the method for slots narrower than 30 mm. In deep slots the ramp is repeated back and forth (stepped ramping), and the tool has to be lifted a certain distance before each change of direction.

Helical interpolation

In helical interpolation the tool follows a circular path in the X–Y plane while descending in Z at a defined pitch. The cutting forces are distributed over three axes, the radial engagement stays small, full climb milling becomes possible, and the chip is evacuated from the open side of the path. Manufacturer publications state that this method is the most favourable form of entry in terms of tool life.

Two geometric limits are taken into account. The first is that the helix diameter is kept above 110–120% of the tool diameter; when the ratio falls below this, the centre region approaches the full-slot condition. The second is that the largest hole diameter that can be produced with a single continuous helix is twice the tool diameter. At that diameter the engagement returns to the full-slot condition, and in blind holes a small boss can remain at the centre; the boss has to be cleared with a separate pass.

The axial step (pitch) cannot exceed the maximum axial depth defined for the tool, and the hole diameter is determined by the tool diameter together with the ramp angle.

5. The difference between centre feed and peripheral feed

This is the most frequently overlooked point in helical interpolation. The feed value given to the machine is the speed of the tool centre; the chip, however, is formed at the cutting edge on the periphery. When the tool follows a curved path these two speeds are not equal.

On an internal contour (when a hole or pocket is machined) the arc followed by the cutting edge is longer than the arc followed by the centre. If the centre feed is not corrected, the edge moves faster than expected and the actual feed per tooth rises noticeably above the target value. On an external contour (when the perimeter of an island or a pin is machined) the situation is reversed; the edge slows down, and although the tool appears to be cutting, it dulls by rubbing.

Once the peripheral feed has been calculated with the relation vfm = n × fz × zc, the centre feed is found as follows:

• Internal contour: vf = vfm × (Dm − Dcap) / Dm
• External contour: vf = vfm × (Dm + Dcap) / Dm

Here Dm is the machined diameter and Dcap is the effective cutting diameter of the tool at that depth.

Worked example. A hole 20 mm in diameter is to be produced by helical interpolation with an end mill 12 mm in diameter. The calculated peripheral feed is 1,200 mm/min.

vf = 1,200 × (20 − 12) / 20 = 480 mm/min

When the program is written with 1,200 mm/min, the cutting edge works at two and a half times the intended feed per tooth. Had the external contour of a 20 mm diameter pin been machined with the same tool, the correction would run in the opposite direction:

vf = 1,200 × (20 + 12) / 20 = 1,920 mm/min

The effective radial engagement and the corresponding entry angle can also be calculated. On an internal contour the relation ae,eff = (Dm² − Dw²) / (4 × (Dm − Dcap)) is used, where Dw is the hole diameter before machining. The corresponding angle is found with β = arccos(1 − 2 × ae,eff / Dcap).

For the basic cutting calculation and the definitions of the symbols, the cutting speed, spindle speed and feed calculation guide can be consulted.

Most modern CAM systems apply this correction automatically. In hand-written programs, in edits made at the machine and in cases where the feed rate is changed by the operator, however, the correction has to be verified.

6. Helical interpolation versus the drill in hole making

The two methods are not alternatives to one another; they solve different constraints.

Where machine power and rigidity are sufficient, the most efficient method in terms of metal removal in series production is the drill. Helical interpolation comes to the fore when the part carries many different diameters, when a large diameter hole is required on a low-power machine, when chip evacuation is critical in a material prone to adhesion, and when the hole diameter has to be held to a tight tolerance. When a corner radius tool is used, the load in the corner region is distributed and wear slows down; for this reason corner radius end mills are widely preferred for helical entry.

Sources

• ISO 8688-2:1989 — Tool life testing in milling — Part 2: End milling. iso.org
• Sandvik Coromant — Slicing and trochoidal milling (upper limit of radial engagement and axial depth range). sandvik.coromant.com
• Sandvik Coromant — Ramping: two axis linear and circular. sandvik.coromant.com
• Sandvik Coromant — Milling formulas and definitions (centre and periphery feed relations in circular interpolation). sandvik.coromant.com
• Sandvik Coromant — Plunge milling. sandvik.coromant.com
• Harvey Performance Company — Most common methods of tool entry and Ramping to success. harveyperformance.com
• Harvey Performance Company — Circular interpolation: machining circular tool paths. harveyperformance.com
• Kennametal — Helical milling interpolation calculator (ramp angle, axial step and centre/edge feed outputs). kennametal.com