The main application areas for High Speed Machinig include:

      •Milling of cavities. It is possible to apply HSM-technology (High Speed Machining) in qualified, high-alloy tool steels up to 60-63 HRc. When milling cavities in such hard materials, it is crucial to select adequate cutting and holding tools for each specific operation; roughing, semi-finishing and finishing. To have success, it is also important to use optimized tool paths, cutting data and cutting strategies.

      •Die casting dies. This is an area where HSM can be utilized in a productive way as most die casting dies are made of demanding tool steels and have a moderate or small size.

      •Forging dies. Most forging dies are suitable for HSM because of the shallow geometry that many have. Short tools always results in higher productivity due to less bending (better stability). Maintenance of forging dies (sinking of the geometry) is a demanding operation as the surface is hard and often also has cracks.

      •Injection molds and blow molds are also suitable for HSM, especially because of their (most often) small size, which makes it economical to perform all operations (from roughing to finishing) in one set up. Many of these molds have relatively deep cavities, which calls for a good planning of approach, retract and overall tool paths. Often long and slender shanks/extensions in combination with light cutting tools are used.

      •Milling of electrodes in graphite and copper is an excellent area for HSM. Graphite can be machined in a productive way with TiCN-, or diamond coated solid carbide endmills. The trend is that the manufacturing of electrodes and employment of EDM is steadily decreasing while material removal with HSM is increasing.
      •Modeling and prototyping of dies and molds is one of the earliest areas for HSM using easy to machine materials, such as non-ferrous, aluminum, kirkzite, etc. The cutting speeds are often as high as 1500-5000 m/min and the feeds are consequently also high.

      HSM is also often used in direct production of the following:

      •Small batch components.

      •Prototypes and pre-series in Al, Ti, Cu for the aerospace industry.

      •Electric/Electronic industry.

      •Medical industry.

      •Defense industry.

      •Aircraft components, especially frame sections but also engine parts.

      •Automotive components, GCI and Al.

      •Cutting and holding tools (through hardened cutter bodies).

Targets for HSM of dies and molds

      One of the main targets with HSM is to cut production costs via higher productivity, mainly in finishing operations and often in hardened tool steel.

      Another target is to increase the overall competitiveness through shorter lead and deli times. The main factors, which enable this, are:

      •Production of dies or molds in (a few or) a single set-up.

      •Improvement of the geometrical accuracy of the die or mold via machining, which in turn will decrease the manual labor and try-out time.

      •Increase of the machine tool and workshop utilization via process planning with the help of a CAM-system and workshop oriented programming.

Advantages with HSM

      Cutting tool and work piece temperature are kept low, which gives a prolonged tool life in many cases. In HSM applications, on the other hand, the cuts are shallow and the engagement time for the cutting edge is extremely short. It can be said that the feed is faster than the time for heat propagation.

      Low cutting force gives a small and consistent tool deflection. This, in combination with a constant stock for each operation and tool, is one of the prerequisites for a highly productive and safe process.

      As the depths of cut are typically shallow in HSM, the radial forces on the tool and spindle are low. This saves spindle bearings, guide-ways and ball screws. HSM and axial milling is also a good combination as the impact on the spindle bearings is small and the method also allows longer tools with less risk for vibrations.

      Productive cutting process in small sized components. Roughing, semi-finishing and finishing is economical to perform when the total material removal is relatively low.

      Productivity in general finishing and possibility to achieve extremely good surface finish. Often as low as Ra ~ 0,2 microns.

      Machining of thin walls is possible. The contact time, between edge and work piece, must be extremely short to avoid vibrations and deflection of the wall. The micro geometry of the cutter must be positive and the edges sharp.

      Geometrical accuracy of dies and molds gives easier and quicker assembly. No human being, no matter how skilled, can compete with a CAM/CNC-produced surface texture and geometry. If some more hours are spent on machining, the time consuming manual polishing work can be cut down dramatically, often with as much as 60-100 percent.

      Reduction of production processes as hardening, electrode milling and EDM can be minimized, which gives lower investment costs and simplifies the logistics. Less floor space is also needed with fewer EDM-equipment. HSM can give a dimensional tolerance of 0,02 mm, while the tolerance with EDM is 0,1-0,2 mm.

      The durability, tool life, of the hardened die or mold can sometimes be increased when EDM is replaced with machining. EDM can, if incorrectly performed, generate a thin, re-hardened layer directly under the melted top layer. The re-hardened layer can be up to ~20 microns thick and have a hardness of up to 1000 Hv. As this layer is considerably harder than the matrix it must be removed. This is often a time consuming and difficult polishing work. EDM can also induce vertical fatigue cracks in the melted and resolidified top layer. These cracks can, during unfavorable conditions, even lead to a total breakage of a tool section.

      Design changes can be made fast via CAD/CAM. Especially in cases where there is no need of producing new electrodes.

Disadvantages with HSM

      The higher acceleration and deceleration rates, spindle start and stop give a relatively faster wear of guide ways, ball screws and spindle bearings, which often leads to higher maintenance costs. Specific process knowledge, programming equipment and interface for fast data transfer needed. It can be difficult to find and recruit advanced staff.

      Considerable length of trial and error period.

  Emergency stop is practically unnecessary. Human mistakes, hard-, or software errors give big consequences.

  Good work and process planning necessary - “feed the hungry machine.”

Cutting fluid in milling

      Modern cemented carbides, especially coated carbides, do not normally require cutting fluid during machining. GC grades perform better as regards to tool life and reliability when used in a dry milling environment. This is even more valid for cermets, ceramics, cubic boron nitride and diamond.

      Today’s high cutting speeds results in a hot cutting zone. The cutting action takes place with the formation of a flow zone, between the tool and the workpiece, with temperatures of around 1000 degrees C or more. Any cutting fluid that comes in the vicinity of the engaged cutting edges will instantaneously be converted to steam and have virtually no cooling effect at all.

      The effect of cutting fluid in milling is only emphasizing the temperature variations that take place with the inserts going in and out of cut.

      In dry machining, variations do take place but within the scope of what the grade has been developed for (maximum utilization). Adding cutting fluid will increase variations by cooling the cutting edge while being out of cut. These variations or thermal shocks lead to cyclic stresses and thermal cracking. This of course will result in a premature ending of the tool life. The hotter the machining zone is, the more unsuitable it is to use cutting fluid. Modern carbide grades, cermets, ceramics and CBN are designed to withstand constant, high cutting speeds and temperatures.

      When using coated milling grades the thickness of the coating layer plays an important role. A comparison can be made to the difference in pouring boiling water simultaneously into a thick-wall and a thin-wall glass to see which cracks, and that of inserts with thin and thick coatings, with the application of cutting fluid in milling.

      A thin wall or a thin coating lead to less thermal tensions and stress, therefore, the glass with thick walls will crack due to the large temperature variations between the hot inside and the cold outside. The same theory goes for an insert with a thick coating. Tool life differences of up to 40 percent and in some specific cases even more, are not unusual, to the advantage of dry milling.

      If machining in sticky materials, such as low carbon steel and stainless steel, has to take place at speeds where built-up edges are formed, certain precautions need to be taken. The temperature in the cutting zone should be either above or below the unsuitable area where built-up edge appears.

      Achieving the flow-zone at higher temperatures eliminates the problem. No, or small built-up edge is formed. In the low cutting speed area where the temperature in the cutting zone is lower, cutting fluid may be applied with less harmful results for the tool life.

      There are a few exceptions when the use of cutting fluid could be defended.

      •Machining of heat resistant alloys is generally done with low cutting speeds. In some operations it is of importance to use coolant for lubrication and to cool down the component, specifically in deep slotting operations.

      •Finishing of stainless steel and aluminum to prevent smearing of small particles into the surface texture. In this case the coolant has a lubricating effect and to some extent it also helps evacuating the tiny particles.

      •Machining of thin walled components to prevent geometrical distortion. When machining in cast iron and nodular cast iron the coolant collects the material dust. (The dust can also be collected with equipment for vacuum cleaning).

      •Flush pallets, components and machine parts free from swarf. (Can also be done with traditional methods or be eliminated via design changes).

      •Prevent components and vital machine parts from corrosion.

      If milling has to be performed wet, coolant should be applied copiously and a cemented carbide grade should be used which is recommended for use in wet as well as in dry conditions. It can either be a modern grade with a tough substrate having multi-layer coatings. Or a somewhat harder, micro-grain carbide with a thin PVD coated TiN layer.
      Essential savings can be made via dry machining:

      •Increases in productivity as per above.

      •Production costs lowered. The cost of coolant and the disposal of it represent 15-20 percent of the total production cost. This could be compared to that of cutting tools, amounting to 4-6 percent of the production cost.

      •Environmental and health aspects. A cleaner and healthier workshop with bacteria formation and bad smells eliminated.

      •No need of maintenance of the coolant tanks and system. It is usually necessary to make regular stoppages to clean out machines and coolant equipment.

      •Normally a better chip forming takes place in dry machining.

 

Cutting fluid in HSMtc "Cutting fluid in HSM"

      In conventional machining, when there is much time for heat propagation, it can sometimes be necessary to use coolant to prevent excessive heat from being conducted into; the work piece, cutting and holding tool and eventually into the machine spindle. The effects on the application may be that the tool and the work piece will extend somewhat and tolerances can be in danger. This problem can be solved in different ways. As mentioned earlier, it is much more favorable for the die or mold accuracy to split roughing and finishing into separate machine tools. The heat conducted into the work piece or the spindle in finishing can be neglected. Another solution is to use a cutting material that does not conduct heat, such as cermet. In this case the main portion of the heat goes out with the chips, even in conventional machining.

      It may sound trivial, but one of the main factors for success in HSM applications is the total evacuation of chips from the cutting zone. Avoiding re-cutting of chips when working in hardened steel is absolutely essential for a predictable tool life of the cutting edges and for a good process security.

            The best way to ensure a perfect chip evacuation is to use compressed air. It should be well directed to the cutting zone. Absolutely best is if the machine tool has an option for air through the spindle. The second best is to have oil mist under high pressure directed to the cutting zone, preferably through the spindle. Third comes coolant with high pressure (approximately 70 bar or more) and good flow, preferably also through the spindle.