Helical Milling: Process, Tool Selection, and Cost Trade-offs

Helical milling is a CNC machining method where the cutting tool follows a spiral path while it feeds along the tool axis. Instead of plunging straight down like a drill, the tool traces a circle in the X-Y plane and descends through the workpiece in the Z axis at the same time. This combined motion lets a single end mill create holes, pockets and bores across a wide range of diameters, without changing tools for every size, which improves the shop’s efficiency and keeps tool inventory down.

For engineers who design parts with non-standard hole sizes, or with tolerances that a standard drill cannot reliably hit on a given workpiece, helical milling solves a real production problem. It also matters to procurement managers comparing quotes, because a shop that runs helical milling well can often avoid extra tooling costs and shorten lead time on prototype or low volume runs.

This guide covers how helical milling works, how it compares with conventional drilling and thread milling, and how to select the right tool and calculate the correct cutting conditions. It also looks at where helical milling stops making financial sense, and the common problems that show up on the shop floor. The aim is a clear, practical reference for anyone specifying, quoting or programming this process.

What Is Helical Milling?

Helical milling is a CNC process that combines circular motion in the X-Y plane with continuous feed along the Z axis. The cutter moves like a spring winding down into the material, cutting a spiral path rather than a straight vertical line. Because the tool moves in three axes together, the resulting hole diameter can be larger than the cutter diameter itself, which is not possible with a straight drill.

Conventional drilling forces a fixed diameter tool straight down into the workpiece. The cutter diameter and the hole diameter are always the same number. Helical milling removes that constraint. One end mill, programmed with different tool-centre paths, can cut multiple hole sizes. This suits prototype work, low volume production, and parts where a non-standard hole diameter would otherwise need a custom drill.

The terms helical milling and helical interpolation are often used for the same thing. Helical interpolation is the more precise, programming level term. It describes the coordinated motion of circular interpolation, commanded through G02 or G03, combined with a linear Z move executed at the same time by the CNC control. Helical milling is the broader, shop floor name for the process that this interpolation produces.

How Does Helical Milling Work?

Circular Interpolation and Axial Feed Combined

The core of helical milling is two motions running at the same time. The first is circular interpolation, where the tool centre moves around a circle in the X-Y plane. The second is a steady feed along the Z axis, which is the axial direction of the cut. Combined, these two motions create a spiral motion, tracing a path down into the material rather than a flat circle or a straight line. This is sometimes called circular ramping, since the tool ramps down while tracing the circle. Linear ramping, by comparison, moves the tool down in a straight diagonal line rather than a circle, and suits slots more than round holes.

Each full turn of the spiral is called a pitch. A smaller pitch means the tool descends less per revolution, which keeps cutting forces lower but takes longer to reach full depth. A larger pitch increases the material removal rate per revolution and cuts faster, but puts more load on the tool. Balancing pitch against material removal is one of the first calculations in setting up a helical milling operation, covered in detail later in this guide.

Helical Interpolation and CNC Control Requirements

Helical milling requires a CNC control that can handle this coordination without hesitation between the circular and linear moves. Not every CNC control handles helical interpolation the same way. The control needs to coordinate three axes at once, keeping the circular motion and the linear Z feed synchronised throughout the cut. Most modern controls support this natively through standard G-code commands, but older or simpler controls may only support two-axis circular interpolation, with Z motion handled separately in small steps.

CAM software plays a large part here too. The software generates the toolpath, including feed rate corrections, lead-in moves and other cutting parameters, and the CNC control then executes it. A mismatch between what the CAM system calculates and what the control can interpolate smoothly is a common source of poor surface finish, discussed further in the problems and solutions section.

3-Axis vs Multi-Axis Machine Requirements

A standard 3-axis CNC machine is enough for most helical milling work. Since the process only needs coordinated X, Y and Z motion, it does not require a rotary axis or simultaneous 5-axis control. This keeps helical milling within the machine capability already available on most shop floors, without extra capital investment.

Multi-axis machines, including a vertical machining centre fitted with a rotary table, become useful for helical milling on angled or curved surfaces, where the hole axis does not line up with the machine’s own Z axis. Most vertical machining centre models on the shop floor already carry enough axes for this. In these cases, a 4-axis or 5-axis setup positions the part so the helical tool path still runs as straightforward three-axis interpolation relative to the tool. Without that repositioning, the geometry needs far more complex programming to reach the same result.

Helical Milling vs Conventional Drilling

Helical milling offers a different approach to the same basic problem that conventional drilling solves, making a hole. The way each one loads the tool, and the flexibility each one gives, are very different. The comparison below covers the practical differences that matter most when choosing between the two.

Hole Diameter and Tool Flexibility

A drill only produces a hole equal to its own diameter. If a design calls for multiple hole sizes, the shop needs a separate drill for each one. Helical milling uses one end mill to cut a range of diameters, simply by changing the programmed tool-centre path. This cuts down on tool inventory and tool changes, which matters more as the number of unique hole sizes on a part increases.

Cutting Force and Tool Life

Drilling pushes the full cutting edge into the material at once, concentrating axial thrust at the tool tip. Helical milling spreads the cut around the circumference of the path, so the tool engages the material more gradually. Lower axial load generally means less tool breakage and longer tool life, particularly in hard materials.

Cycle Time and Production Volume

Drilling is faster for high volume production of a single, fixed hole size. The tool goes straight in and straight out, with no interpolation overhead. Helical milling takes longer per hole because of the spiral toolpath, so it tends to suit lower volumes, prototypes, or parts where the flexibility in hole size outweighs the extra cycle time.

Helical Milling vs Thread Milling

Both helical milling and thread milling use a spiral toolpath and a cutting tool moving in three axes together. The difference lies in what the spiral is actually cutting into.

When to Choose Helical Milling for Holes

Helical milling is the right choice when the goal is a plain, round hole, bore or pocket. The toolpath traces a smooth circular path with no thread profile involved. It suits oversized holes, counterbores and internal contours where accuracy and surface finish matter more than a threaded feature.

When to Choose Thread Milling for Threads

Thread milling uses the same three-axis helical motion, but the cutter has a thread form profile ground into it. As the tool spirals into the hole, it cuts a complete thread in a single pass or a small number of passes. Thread milling is generally chosen over tapping for larger threads, harder materials, or blind holes where a broken tap would scrap the part.

Tool Selection for Helical Milling

End Mill Types Suited to Helical Milling

Solid carbide end mills are the standard choice for smaller helical milling operations, generally for holes under about 20 millimetres. They offer good rigidity and hold a sharp cutting edge well across a range of materials. For larger hole diameters, indexable end mills become more practical, since a solid carbide tool of that size is expensive and hard to regrind economically.

Flute count is one part of the tool geometry, and it affects chip evacuation as much as it affects surface finish. Tools with more flutes generally leave a better finish, but fewer flutes give more space for chips to clear, which matters more in deep holes where chip packing is a real risk.

Cutter Diameter and Tool-Centre Path

The cutter diameter cannot be chosen independently of the target hole diameter. A commonly used starting point is a cutter diameter of roughly 40 to 60 percent of the finished hole diameter. Too small a tool relative to the hole increases cycle time and reduces rigidity. Too large a tool leaves too little clearance for chip evacuation and lead-in movement.

The tool-centre path itself, the circle that the tool axis follows, is always smaller than the finished hole. This relationship is set out with the exact formula in the calculations section below.

Ramping Angle and Cutting Edge Load Limits

As the tool enters the material along the helical path, cutting edge load builds gradually rather than all at once. Every end mill has a maximum ramping angle stated by the manufacturer, based on the load the cutting edges can take without excessive wear, tool damage or breakage. A steeper ramping angle means the tool descends faster per revolution, which increases the load on each cutting edge as it engages the material. A high feed rate makes this worse, so ramping angle and feed need to be balanced together.

Exceeding the tool’s rated ramping angle can easily lead to premature tool failure in helical milling. Checking the manufacturer’s specification, and the published ramp angles for the tool line, before programming the tool path avoids this, and is a cheap step compared with the cost of a broken tool mid cycle.

Tool Overhang and Rigidity

Helical milling puts continuous side load on the tool as it traces the circular path. A long tool overhang, where the tool extends far out of the holder, flexes under that load and produces an out-of-round hole in the workpiece. Keeping the overhang as short as the job allows supports high accuracy and longer tool life.

Toolholder choice matters here too. A shrink-fit or hydraulic holder grips the tool more evenly than a standard collet, reducing runout and supporting the high precision that helical milling depends on under the side loads it generates.

Helical Milling Calculations and Cutting Conditions

Tool-Centre Path Diameter and Calculated Values

The tool-centre path diameter is the circle that the centre of the tool follows as it cuts. It is calculated by subtracting the cutter diameter from the target hole diameter.

Dc = Dh – Dt

Dh is the finished hole diameter and Dt is the cutter diameter. This calculated value is the starting point for every other calculation in helical milling, including the ramping angle and the feed rate correction.

Ramping Angle Formula

The ramping angle is the angle of the spiral relative to a flat circle. It depends on the pitch, the Z axis depth the tool descends in one full revolution, and the tool-centre path diameter calculated above.

tan(α) = Pz ÷ (π × Dc)

Pz is the pitch per revolution and Dc is the tool-centre path diameter. A smaller pitch gives a shallower ramping angle and a gentler engagement on the cutting edges, reducing the chance of tool breakage. Manufacturers publish ramp angles for each tool line, so checking the chart before programming avoids exceeding the limit.

Helical Pitch, Feed Rate, and Number of Revolutions

Once the ramping angle is set within the tool’s rated limit, the number of revolutions needed to reach full depth follows directly from the pitch.

Number of revolutions = total hole depth ÷ pitch per revolution

Feed rate also needs correcting for helical milling. The tool centre travels a smaller circle than the cutting edge at the outer diameter of the hole. If the feed rate is programmed at the tool centre without correction, the actual cutting speed at the edge ends up higher than intended. Spindle speed stays constant through the cut, so the feed correction is what keeps chip load consistent as the radius changes. The correction factor is the ratio of the tool-centre path diameter to the finished hole diameter.

Commanded centre feed = target cutting-edge feed × (Dc ÷ Dh)

Worked Calculation Example

The following example shows how the calculations and cutting parameters above translate into real numbers for a typical hole. Take a finished hole diameter of 25 millimetres, cut with an end mill of 12 millimetres in cutter diameter. The tool-centre path diameter is 25 minus 12, which gives 13 millimetres. With a pitch of 1.5 millimetres per revolution, the ramping angle works out to just over 2 degrees, comfortably within the rated limit of most standard end mills.

For a hole depth of 18 millimetres, the tool needs 12 full revolutions to reach full depth. If the target cutting-edge feed is 300 millimetres per minute, the commanded feed at the tool centre should be corrected to around 156 millimetres per minute, using the ratio of 13 to 25. Programming the uncorrected 300 millimetres per minute directly at the tool centre would push the actual cutting speed at the edge well above the intended value, risking excessive tool wear.

Benefits of Helical Milling

Lower Cutting Forces and Longer Tool Life

Because the tool engages the material gradually around a circular path rather than plunging straight in, the peak cutting force stays lower than with drilling. Lower peak force means less stress on the tool, the spindle and the workpiece, which extends tool life and reduces the risk of chipping or breakage in hard materials.

Better Hole Quality and Surface Finish

The smooth, continuous motion of helical milling reduces the chatter and vibration that often show up with straight plunging. This produces rounder holes with better dimensional accuracy and a better surface finish, often without a separate finishing pass, which saves a step in the process.

One Cutter, Multiple Hole Diameters

A single end mill can cut a range of hole diameters just by changing the programmed tool-centre path. This cuts down on tool inventory and tool changes, which matters most on parts with multiple hole sizes or in low volume work, where buying a dedicated drill for every size is not economical.

Applications of Helical Milling

Helical milling applications span several industries, wherever a shop needs one tool to cover a range of hole sizes or wants to keep cutting force low on a delicate part. Aerospace manufacturing, medical device work and mould making are the three sectors where it shows up most often.

Aerospace Manufacturing and Medical Device Parts

Aerospace manufacturing relies on helical milling for holes in thin walled brackets and structural components, where lower cutting force reduces the risk of distortion. In aerospace circles, this technique is sometimes called orbital drilling, reflecting the orbiting motion of the cutter around the hole, and orbital drilling is widely used on composite materials as well as metals. Medical device manufacturing benefits for similar reasons, particularly where tight tolerances, high precision and a clean surface finish are needed on small features.

Mould and Die Cavities

Mould and die makers rely on helical milling for mould making tasks such as opening circular pockets and cavities without needing a separate plunge or pilot hole, along with profiling operations on complex cavity walls. The process handles hardened tool steels, among the more difficult to cut materials in the shop, while keeping cutting forces manageable.

Thread Milling and Energy Sector Components

Helical milling is closely related to thread milling, used across the energy sector for large diameter threaded connections in valves, pipe fittings and downhole components. The same spiral toolpath principle applies, with a thread form cutter replacing the plain end mill.

When Helical Milling Is Not Worth the Cost

Batch Size and Cycle Time Trade-off

Helical milling takes longer per hole than straight drilling, because the tool has to trace a spiral path rather than simply plunge and retract. On a high volume job with a standard hole size, that extra cycle time adds up fast across thousands of parts. For batches large enough to justify a dedicated drill, drilling usually wins on cost per part, even after accounting for tool purchase.

The break-even point depends on the specific hole size, the material properties and the machine available, but as a general rule, helical milling earns its keep on low to medium volumes, prototypes and parts with several different hole diameters. Once a single hole size repeats across a large enough run, it is worth checking whether a standard drill would cut total cost per part.

Hole Depth and Tool Reach Limits

Deep holes push helical milling toward its practical limit, and depth is often the limiting factor rather than diameter. As depth increases, chip evacuation becomes harder, tool overhang increases, and the risk of deflection and out-of-round holes grows with it. Past a certain depth to diameter ratio, the extra care needed to keep the process stable can outweigh the flexibility benefit that helical milling offers.

In these cases, a combination approach often works better. Drilling a pilot hole first reduces the depth the spiral toolpath has to cover, then helical milling finishes the final diameter and surface finish. This keeps the process within a stable range instead of pushing one method to its limit.

When Drilling or Boring Wins on Cost

For a single, standard hole diameter with generous tolerance, plain drilling is almost always cheaper and faster. For a large hole that needs high accuracy in diameter and roundness, in a part that already needs boring for other features, boring can hold tighter tolerances than helical milling, without the programming overhead of a helical toolpath.

The decision comes down to matching the process to the job. Helical milling earns its cost when flexibility, tool reduction or gentler cutting forces matter more than raw cycle time. When none of those factors apply, a simpler process usually wins.

Common Problems and Solutions

Hole Diameter and Roundness Errors

An out-of-round hole usually points to tool deflection, an incorrect tool-centre path calculation, or a ramping angle that is too steep for the tool and material combination. Checking the tool-centre path calculation first is the quickest way to rule out a programming error before looking at the machine or tool itself.

If the calculation is correct and the roundness error persists, reducing the ramping angle and increasing the number of passes usually resolves it, at the cost of extra machining time.

Tool Deflection and Runout

Tool deflection under the side load of helical milling shows up as a tapered or barrel shaped hole rather than a straight cylinder. Shortening the tool overhang, switching to a more rigid toolholder, or reducing the depth of cut per pass all help bring deflection back under control.

Runout in the spindle or toolholder has a similar effect but is easier to miss, since it looks like normal wear at first. Checking runout with a dial indicator before a critical job catches this before it turns into a scrapped part.

Chip Evacuation and Tool Wear

Chips have limited space to escape inside a hole, more so as the hole gets deeper. Poor chip evacuation leads to chip recutting, where chips get caught between the cutting edges and the wall, accelerating tool wear and leaving poor surface quality on the hole wall. In softer materials such as aluminium, built up edge can form on the cutting edges if chips are not cleared quickly, adding further tool wear and degrading surface quality. High helix tools help move chips up and out of the cut more effectively than a standard flute design.

Heat generated during the cut also builds up faster when chips are not cleared, accelerating wear on the cutting edges. Coolant delivery through the spindle, or an air blast where coolant is not practical, clears chips from the cutting zone directly rather than relying on the flutes alone. This matters most in hard materials and deeper holes, where chip evacuation problems compound quickly.

Helical Milling FAQs

Q: Can helical milling create a hole larger than the cutter diameter?

A: Yes. This is one of the main reasons the process exists. Because the tool moves along a circular tool-centre path rather than plunging straight down, the finished hole diameter is always larger than the tool diameter, by the amount of the tool-centre path diameter added to the tool diameter itself.

Q: Does helical milling require a multi-axis CNC machine?

A: No. A standard 3-axis machine handles most helical milling work, since the process only needs coordinated X, Y and Z motion. Multi-axis machines are only needed when the hole axis is angled relative to the machine’s own Z axis.

Q: What materials can be machined with helical milling?

A: Helical milling works across a wide range of materials, from aluminium and mild steel through to titanium and hardened tool steel. Different materials call for different settings, and harder materials generally need a shallower ramping angle and a slower feed rate to keep cutting edge load within the tool’s rated limits.

Q: Is helical milling suitable for small batch production?

A: Yes, and this is one of its strongest use cases. Because one end mill can cut a range of hole diameters, small batch and prototype work avoids the cost of stocking a dedicated drill for every hole size on a part.

Q: What is the difference between helical milling and helical interpolation?

A: Helical interpolation is the specific CNC programming term for the coordinated circular and linear motion that produces the spiral path. Helical milling is the broader name for the machining process that results from that interpolation. In practice, the two terms are often used interchangeably.

Conclusion

Helical milling earns its place in a machine shop by solving a problem that drilling cannot. It produces a range of hole diameters from a single tool, with lower cutting force and a better surface finish along the way. It suits prototypes, low to medium volumes and parts with several different hole sizes.

It is not the right choice for every job. High volume runs of a single standard hole size, or holes deep enough to strain tool reach and chip evacuation, often cost less with straight drilling or boring instead. Getting the tool selection and the calculations right, covered earlier in this guide, is what separates a stable helical milling process from one that chews through tools and produces out-of-round holes.