HSC milling, in other words, milling at high speed, offers great potential in CNC machining since it promises shorter throughput times, increased productivity and yet high quality. In this article we focus in more detail on HSC milling and clarify the following issues:
One of the greatest problems during HSC milling is the occurrence of vibrations. How do they happen? Since every system (shaft, holder) which is able to vibrate has a natural frequency, it continues to oscillate when stimulated (knock, deflection) until it stops due to damping loss (tuning fork) or a momentarily equally large negative frequency. If however external stimulation occurs at regular intervals and this stimulator frequency is also within approximately the same frequency range of the natural vibration of the system, then both these frequencies overlap. This is then called a case of resonance → The system starts to bounce (vibrate).
What are the consequences of vibrations during milling?
* Tool diameter in mm
The dissipation of temperature with the chip is a primary problem when HSC machining. The above diagram describes the temperature behaviour of individual materials.
With our test, the wear escalates at a cutting speed of approx. 600 m / min. According to this series of tests, the upper limit for ball-nosed end mills where Z=2 and Z=4 is a cutting speed of 580 m / min.
The choice of cutting width when HSC milling contributes significantly to a longer tool life. When HSC milling it is evident that it is better to work with a smaller width of cut, than wanting to achieve as high a removal rate as possible similar to rough milling. This is not achieved by the width of cut but by the maximum cutting speed that can be reached.
An amortisation comparison shows that in spite of the higher purchase costs of a milling machine with a high-frequency spindle, machining is considerably cheaper as it is more cost-effective.
Small businesses in particular, which are geared up for the flexible production of medium-sized workpieces, can benefit greatly from HSC machining. With an average time saving of 50%, this also leads to a production cost saving of approx. 25%–27%.
The term HSC milling or drilling must be defined according to the material. It is clear that the HSC range for aluminium must be in a different cutting speed range than for steels or special materials, for example. The limitation of the cutting speed in this case must be compared with conventional milling.
It should be noted that when the cutting speed increases, the cutting forces decrease significantly at first and then increase significantly again.
It is also worth noting that for extremely high cutting speeds of approx. 130,000 m / min, the wear increases disproportionally. If however you stay within the cutting speed range up to approx. 5000 m / min, the flank wear increases significantly at first, depending on the material, and then remains constant for a while.
Of similar interest, when the cutting speed increases, the passive force (reaction force to the milling cutter force) can be reduced up to 70%. This is especially the case with extremely thin-walled profiles and to achieve a near-grinding surface.
With aluminium machining it appears that the specific chip volume shows a maximum at cutting speeds of 3100 to 4700 m / min. The chip volume, which is approx. 35% greater, also produced a surface with an average surface finish of 1 μm. Optimum values however are significantly alloy-dependent.
When machining aluminium, a spiral tool with large chip chambers is needed. A 2-flute cutter with approx. 45° spiral pitch is advantageous here. The tool should have a rake angle of 15°–20° and a side clearance angle of 10°–12°. If a machine with less spindle power, small feeds or deep slots is used, then a single-edged spiral tool is preferable. Where the average cutting speed is approx. 2000 m / min, a tool life of 500 m is easily achievable.
When machining copper and copper alloys, the same tools should be used as when machining aluminium. The feed rate values per tooth are between 0.02 and 0.4 mm depending on the alloy composition.
Pure copper should only be milled with a precision-ground tool cutting edge to prevent the built-up edge formation.
Climb milling in this case is preferable to conventional milling. The use of ceramic tools here is however advantageous since up to ten times higher cutting speeds can be used.
When machining fibre-reinforced plastics, HSC machining is ideal since when the cutting speed increases, the cutting forces decrease significantly and the high feed rate values counteract the edge zone lamination. By removing the cutting energy with the chip, the basic material is subjected to minimum thermal stress.
CFK and GFK materials
Where possible, machining should be conventional milling and against the fibres and not parallel to the fibre. Satisfactory to good results however are only provided by polycrystalline diamond tools. The optimum machining range is approx. vc = 4500 m / min and vf to 30 m / min. The tool should have a rake angle of approx. 5° and a side clearance angle of 10°.
Since force transmitting fibres have to be cut through, sharp tool cutting edges and a geometry similar to that for light metal machining are preferable. The best results are provided by tools which can be classified in ISO group K. The optimum machining range is a cutting speed of 2000 m / min to 3000 m / min and a feed rate of
10 m / min to 15 m / min.
When high-speed milling steel, a tool life of
20–25 m can be achieved at a cutting speed of 750 m / min. Cutting speed ranges of 500 m / min to 1500 m / min can certainly be reached with solid carbide milling cutters of ISO class P. Especially for die production and toolmaking, where complicated forms are usually produced with a spherical cutting edge geometry during the traverse milling process, HSC milling has proven successful.
Here, high feed rates and cutting speeds ensure that huge time and surface quality improvements are made. It has been shown that where the rake angle is constant (0°) with an increasing side clearance angle and a feed increase, the tool life is improved.
The optimum side clearance angle has levelled off at approx. 12°–20°. For stability reasons, straight fluted tools which are pilot or centre cutting, have proven to be ideal in tool and die production. The aim should be to achieve feeds of 0.3 to 0.7 mm, climb milling and
dry cutting, whereby the cutting speed should be between 500 m / min and 1500 m / min.
Machining cast iron is possible using solid carbide tools where the rake angle should be 0° to 6° and its side clearance angle 12°. The tools must be coated. It is important to make sure that the formation of comb cracks and transverse cracks on the coating due to the gentle entry and exit action into or out of the material, is kept to a minimum.
With cutting speeds of 1000 m / min, the chip volume can for example be increased tenfold for GG 25. The tool life is around 20 m per cutting edge and the surface resembles grinding quality. The tool life can be increased if the feed is relatively high, i.e. feed per tooth approx. 0.3 to 0.4 mm.
When machining graphite, it is not only the low cutting forces which are advantageous, but also the powdery chip material. The chip material should be removed fully and as quickly as possible from the machining process, since the tool life is essentially dependent on the evacuation of the chip powder. In order to counteract the emery effect, our graphite milling cutters are diamond-coated.
This ultra-hard coating counteracts the abrasive wear optimally, which in turn leads to a longer tool life. In order to improve the chip removal, machining should involve climb milling.
|Conventional milling (green)|
|Tool||Solid carbide, 2 teeth Ø 3.0 mm|
|Task||Slot 3 mm x 700 mm x 6 mm|
|Number of cuts||3||3|
per tooth (mm)
|Tool life (m)||25||37|
|Main time (s)||25.8||421.8|