Please select your country! -English (US) -EN Settings


Please select your country!


{{"ifind_go-back" | translate}}



Milling holes and cavities/pockets

Milling holes and cavities/pockets
  1. Two-axis ramping linear
  2. Circular ramping
  3. Widening a hole​
  4. Circular external milling or ramping
  5. Plunge milling
  6. Peck milling
  7. Slicing methods
  8. Closed pockets or angles​​

Hole milling: creating openings

  • Creating openings in a solid workpiece
  • Widening a hole or a cavity
  • Opening up / widening a cavity or pocket

Creating openings in a solid workpiece

Linear ramping
Peck milling
Opening a slot

When milling a hole, linear ramping (2 axes simultaneously) is always preferred to peck milling.

Peck milling is an alternative hole milling method, but it often produces long chips and generates undesirable cutting forces on the cutter.​

Opening a hole or a cavity
Circular ramping
Ramping a cavity

Drilling is the traditional and fastest method for producing a hole, but chip breaking can be a challenge in some materials. It also lacks the flexibility to produce varying diameters and non-round shapes.

Circular ramping (3 axes simultaneously) is a less productive method than drilling a hole, but can be a good alternative in cases of:

  • Large diameter holes when machine power is limited
  • Smaller series production. A rule of thumb for diameters larger than 25 mm: milling is cost-efficient up to a series of approx. 500 holes
  • When a range of hole sizes are to be machined
  • Limited tool magazine space to store many drill sizes
  • Production of blind holes, when a flat bottom is required
  • Non-rigid, thin walled components
  • Interrupted cuts
  • Materials that are difficult to drill due to chip breaking and chip evacuation
  • No cutting fluid is available
  • When milling cavities/pockets (“non-round holes”)

Choice of method – example

Opening up a cavity/pocket

Drilling and circular milling
Drilling and plunge milling
Circular ramping


+ High material removal for non-round holes

+ First choice in aerospace frame titanium structural parts


– Requires a stable machine

– Chip evacuation – horizontal machine

– Careful programming required


+ Problem solver in long overhang applications

+ Simple programming suitable for older/multi-spindle machines


– Low material removal


+ Fewer tools (no drill needed)

+ Flexible (produces a wide range of sizes)

+ No cutting fluid required = good for open machines

+ Suitable for all machine concepts and configurations


– Less productive for large cavities

The basic choice for pockets
Problem solver
Long overhangs
The basic choice for 3D cavities

Widening a hole or a cavity

Circular ramping
Circular milling
Widening a hole

Boring is normally the fastest method, for the same reasons as drilling, but hole milling is sometimes a good alternative. Two alternate milling methods can be used: circular ramping (3-axis) or circular milling (2-axis). Circular ramping is preferred when the hole is deeper than ap max or in vibration-sensitive applications. In addition, the roundness/concentricity of the hole becomes better when ramping, especially with long overhangs. Roundness will be improved if the workpiece is rotated instead of moving the milling cutter in a circular path in both circular ramping and milling operations.

Widening a cavity

Internal shoulder milling and plunge milling require a starting hole and should be compared to ramping a cavity directly into a solid block.

  • Ramping (3-axis) is advantageous because it only requires one tool and can produce 3D shapes, making it suitable for profile milling. If applied with high feed techniques (light and fast), the cutting forces will be directed in a favorable manner that minimizes vibration problems
  • Plunge milling often solves problems with long overhangs and/or deep cavities
  • Internal shoulder milling requires more programming than plunge milling, but it is faster
Internal shoulder milling
Plunge milling
Rest (remaining stock) milling

When the roughing of a cavity is completed, stock often remains, especially in corners. Plunge milling with a smaller cutter is one method for coming closer to the finished shape. Slicing (light and fast) is another technique often used in corner milling. Trochoidal milling is one type of slicing technique that is also used for milling slots, pockets etc.​

Plunging in corners
Slicing technique – light and fast
​Slicing in corners

How to open up / widen a cavity or pocket


There are two clear strategies:

1. Circular ramping (3-axis) – small ap

Use a cutter with a small entering angle. A round insert cutter is another alternative.

This “light and fast” technique provides an excellent metal removal rate and is the First choice for less stable machines (according to ISO 40) and when the cavity has a profiled shape, i.e. die and mold.

Note: Avoid machining all the way against a 90° shoulder, because the effect of a low approach angle will be lost, i.e. the depth of cut increases dramatically.

Cutting parameters:

  • Maximum cutter diameter = 1.5 x component corner radius
  • Circular ramp to depth – counterclockwise
  • Roll into the next cut
  • Radial cut – max. ae = 70% DC
  • Axial cut for round insert cutter 25% iC
  • Tool path radius in the corner = DC
  • Reduce corner feed
2. Circular milling (2-axis) – large ap

Drill a hole, then change to a shoulder end mill or a long edge cutter. A typical application area is found in aerospace framing – titanium machining.

Application hints

Ensure good chip evacuation to prevent re-cutting of chips / chip jamming:

  • A horizontal spindle (ISO 50) is preferred
  • High pressure coolant or compressed air with through tool coolant
  • DC should be no greater than 75% of hole dia. Use a large axial cut – maximum ae = 2 x DC

The drilled hole should be entered in a circular path:

  • Control radial engagement, maximum ae = 30% of DC

Control radial engagement to minimize vibration in corners and to maximize productivity:

  • Use the largest radius possible in the corners, spiral morph programming
  • Use the largest DC possible and complete rest milling separately at no greater than 1.5 x the corner radius

Small corner radius

Spiral morph programming
We use cookies to enhance the experience on our website. More about cookies.