Milling is the most flexible and available method of machining that allows the production of almost any shape. Milling is used to separate the layer of material from the processed part with the use of a tool, usually the cutter. In this technology, the part is fixed, while the cutter rotates to allow cutting.
The high flexibility of the process means that a wide range of elements for various industries can be produced on CNC milling machines. The most typical elements produced by this method are mainly parts of machinery and equipment, in particular: bodies, covers, blocks, distributors and various housings.
Our CNC milling centers allow the processing of a wide range of materials used in the industry. We can machine difficult materials, e.g. aircraft alloys or materials with increased hardness. However, due to the specialization and high market demand, the core portfolio includes the milling of carbon, low-alloy, alloy and stainless steel grades. A substantial part of our offer is also the milling of non-ferrous metals, such as aluminum, brass and bronze.
CNC milling is a very extensive field of technical knowledge. Due to its flexibility, milling shows enormous potential in the production of various components. Apart from the traditional applications, milling is often an alternative to other methods, for example CNC. The basis for designing efficient and productive processes on milling machines it to know the technology and programming rules. Frequently, the same tasks can be made by using several or even more than ten methods. It does not mean that every method is good. The milling configuration must be well-thought out. Problems that should be considered include the occurrence of deep pockets, thin walls, an intermittent process or inclusions in the material. The surfaces of the part can be hard to machine due to casting skin or scale on forgings. The selection of the milling method depends largely on the available machine, its type, size and power. Horizontal milling centers and 5-axis centers with smooth control in all axes offer different options.
Our specialists are proficient in the field of CNC milling with modern, high-performance machining centers. Therefore, they are able to plan the process in such a way that the customers’ parts are processed in the most productive manner, consistently attaining an extremely high quality of products.
This type of milling uses the face and side edges of the cutting tool to process two surfaces simultaneously. The process can be performed with not only traditional heads, but also with router bits, cutters with a long edge called turbo helical cutters and face and side cutters. The wide variety of options require the accurate selection of tools to achieve the optimum effect of processing, with one of the basic requirements being the true 90 degree angle between the machined surfaces. The best solution in shoulder milling is to use the so-called climb milling, in which the tool moves in the direction of rotation. Thus, chip thickness decreases from the beginning of the pass, gradually reaching zero at the end. This prevents the generation of high stresses in the moment when the blade leaves the part, which is beneficial for part life. If possible, programming should include cutter entrance on an arc, which means that chip thickness is reduced to zero at the exit point, thus extending the feed and tool life. Additionally, wherever possible, milling should be performed so as the cutting forces are directed towards the support points of the chuck, particularly on machines with lower rigidity. Another way to achieve stable cutting on less rigid machines is to use a cutter with a coarse pitch. Mounting the cutter hard and fast is also crucial, especially for the process results in heavy machining.
A specific operation in this category is external milling, i.e. edge machining. It requires careful planning due to the fact that there are usually problems with the cutter being pushed away and obtaining good surface quality. In this case, it should be noted that cutters with replaceable inserts will always show higher radial runout and a lower precision of the blade than sintered carbide cutters. This is why, if the product side edge requires a high quality, round tools should be selected, particularly those with a high angle of the helix and fine pitch. This ensures a sufficiently large number of blades engaged simultaneously in cutting, which produces a stable process and optimum effects.
Face milling is the most common milling operation, often referred to as surface milling. It can be performed using a wide range of different tools. Cutters with a 45O entering angle are normally used, but round insert cutters, square shoulder cutters and side and face mills are also used. When starting to plan the machining process, a number of factors must be considered; from machine stability, size and type of spindle to available power. If possible, use cutters with diameters that are larger than the processed surface width by 20 – 50 %. The alignment of the cutter in an eccentric position in relation to the axis of a processed item to allow the reduction of chip thickness at the exit from the cut, is also important. In order to achieve a smooth entrance to cut, the path should be programmed along an arc entrance or the feed should be reduced. Whenever possible, avoid frequently putting the tool in and out of the material as it can cause adverse stress on the cutting edge and lead to vibrations. It is better to program the path so that the cutter is kept in constant contact with the material, instead of several parallel passes. During a change in the direction of machining a pass on a radius can be used to keep the cutter in movement with constant contact. Down milling is the first choice here for the planned machining strategy.
An additional alternative for face milling operations is to use cutters with a small entering angle and milling with a fast feed. It is a special method of processing, in which the special design of the tool allows a reduction in the chip thickness. This enables the use of a very fast feed, reaching up to 4 mm per blade. Despite the fact that tool geometry requires a reduced depth of cutting to below 2 mm, the high level of the feed makes it a very productive milling method. Another characteristic feature of this processing method is the very good distribution of cutting forces. Due to the low entering angle of blades, the cutting force vector points are mainly directed towards the spindle, which makes it a very stable method that allows a higher overhang than with standard tools.
It is also worth mentioning that wiper insets can be used in finishing face milling. These are special inserts with a larger edge width in order to improve surface quality. They are used in combination with standard inserts so that one or more wiper inserts are positioned in the head, next to the milling inserts, protruding below the latter by approx. 0.05 mm. This means that all uneven areas on surfaces which have been left by other blades are removed.
Profiling is a group of operations typical for CNC machining, which are not possible on traditional machines. This category covers multi-axis milling, convex and concave shapes in two and three dimensions. The advanced programming of tool paths is required to achieve the optimum results of processing. Basically, the process can be divided into at least three operation types: roughing, semi-finishing and finishing. Super-finishing, often performed using high-speed machining techniques, is sometimes required, known as HSM. In order to achieve high accuracy and productivity, the performance of rouging and finishing on separate machines, with the use of dedicated cutting tools for each operation, is highly recommended. Finishing should be performed on 4- or 5-axis machines with the use of advanced programming techniques.
Due to the fact that profile milling is used in the production of many different products, starting from various molds and dies to the components of power-generating turbines or aircraft engine turbines, knowledge concerning this milling category is very extensive. Our company is not specialized in this type of machining, so we will focus only on the main points. In rough milling, it is important to choose machining methods that can leave an allowance for further operations. Shoulder mills or extra-long cutters leave an uneven allowance, which should be removed later. This results in variations in the cutting force and tool deformation in subsequent stages of machining, which impacts on the geometrical accuracy of the final shape. Using cutters with round inserts for high feed rates will guarantee smooth transitions between subsequent passes, thus, a more even allowance for subsequent finishing tools. After the rough starting of the profile, profiling proper can be continued. We offer two basic strategies for machining: contour milling and copy milling. The latter is the easiest method from the path programming point of view and involves the reproduction of the shape with multiple uniform passes of the tool guided across the contour. However, this method is not recommended due to the non-optimum use of machine capabilities and the high number of entrances and exits of the cut. Contour milling is more favorable as it guides the tool along the profile edge, gradually entering the Z axis as the material is removed. This is a more productive method, as cutting is performed on a larger diameter, which allows a reduction in machining time. Additionally, the tool constantly remains in the material, which extends tool life. Contour milling also results in fewer quick changes of the working load and direction. This is particularly important when milling at a high speed and feed rate, as well as the milling of hardened materials, as the process in such cases is particularly prone to vibrations.
Most milling applications require the production of various types of grooves, slots or reliefs. Grooves can be shallow or deep, closed or open, short or long, wide or narrow, straight or curved. Depending on the individual task, the proper method and tool should be selected. Side and face cutters are dedicated to grooving or cutting off. They are effective in the production of long, deep open grooves, while ensuring stability and productivity, and can also be combined in groups to increase the amount of removed material in a single pass. The benefits of this type of cutters are decidedly the stable milling of narrow and deep grooves, therefore, this should be the first type chosen in such applications. However, there are many applications where side and face cutters cannot be used. These include curved, closed, key grooves or grooves that are hard to access with the side and face cutter due to its dimensions. In such cases, side and face milling should be performed with router bits. An advantage of this method is its versatility. Here, there are three basic grooving strategies to choose from. Traditional milling which guides the cutter tool along the axis of symmetry of the groove. This is the simplest method to program offering good results in stable conditions. However, high radial forces are generated which makes the process prone to vibration. Trochoidal milling can be defined as circular milling within the groove width that includes simultaneous forward movements. This method requires advance programming, though it exhibits many benefits. The main strong point is the generation of lower radial forces, which makes the process more stable than classical milling. Another benefit is lower heat during cutting, which is also important when producing narrow and deep grooves. Chip control is also improved. The last available method is plunging. This strategy is dedicated to situations, where tool overhang is so large that processing the part in stable conditions without vibration would be impossible with any other method. It includes removing the material from the groove in multiple subsequent passes with the cutter face instead of cutter circumference. This means that most of the cutting forces are directed towards the tool axis, which significantly improves the process stability. However, it should be noted that it is a less efficient method than other ones and it should only be used in situations justified technologically.
The milling of threads is possible in the full scope of applications both for internal and external threads, right and left threads, with any pitch. The main tools used in threading still include taps and threading dies. These are shaping tools with multiple cutters, having the same geometry as a given thread with its diameter and pitch. During the operation, the cutters cut the material in a continuous way, reproducing their shape in the machined element. Their popularity results from the availability, easy use and relatively low price. A disadvantage is low durability, low machining efficiency and the fact that they are prone to damage due to poor chip control. A more advanced method of internal threading is forming. The process is performed with forming taps, whose construction is similar to that of threading taps. The difference is that forming taps do not have cutting blades but only tips and lubrication channels that can form the thread without generating chips. This is associated with the improved stability of the process and higher possible parameters, thus, higher productivity. Another method of thread production is milling. Here, we have a line of tools which are more or less versatile and allow almost every type of thread to be cut. Milling is not as efficient as forming, but it offers better control of the process and completes the process in situations where forming taps cannot be used.
Apart from the basic methods of CNC milling, specific production tasks often require special methods in order to improve or speed up machining. The first category of such operations is cutting holes in a solid material. In this case, the simplest method is drilling, of course. It is the fastest and most efficient operation for holes, though not always ideal. Alternative methods must be used when, for example, the hole diameter is not circular. There are more similar situations: in the case of hard-to-drill materials due to difficult chip breaking, in the case of intermittent cutting, when holes with a flat bottom are required, when machine power is not sufficient to drive the drill (larger diameters) or for holes in thin-walled materials prone to damage. In such cases we have a whole range of methods available, such as linear two-axis ramping, peck milling, helical ramping, circular ramping, linear ramping, etc. In general, these are strategies that combine tool movement in the Z axis together with the radial movements in X and Y axes. This allows the efficient removal of the material from various types of holes, pockets and cavities, where traditional drilling would not work well. Other special strategies include plunging and trochoidal milling. Both methods reduce radial cutting forces, which improves process stability. They are discussed in detail in the chapter related to groove milling. Frequent operations also include chamfering, V grooving, deburring after previous operations or chamfering for welds. Depending on the type of machine and specific operation, these tasks can be performed with different methods, nevertheless dedicated chamfering tools are usually used. These tools have blades at the required angle and often allow single-pass chamfering.