Widening a hole or a cavity
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
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.
2. Circular milling (2-axis) – large ap
- 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
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