Machining holes in the sleeve and disc class parts plays an important role. When we pay attention to the general technological processes of these parts, in the case of classic technological processes, the general technological process of the sleeve class parts with hole-based is used. Selected problems of hole machining are presented below. Information about roughing holes is given in the article under the same title: Roughing holes. In the article Structural drawing and technology. How to read discussed the basics of reading a technical drawing from a technologist’s point of view. Figure 1 shows an example of the sleeve design. The selection of production equipments, including machine tools, manufacturing techniques and specific machining methods depends on the usage and quality requirements (accuracy of geometric dimensions and surface roughness and hardness of the surface layer). From a technological point of view, hole machining methods (drilling, drilling, reaming, boring, grinding, EDM) are characterized by significantly better quality effects than machining of cylindrical outer surfaces. This article addresses issues related to drilling and reaming.
In figure 1 we can see that the Ø40H8 hole is the basis for the radial runout tolerance of the outer surface of Ø50h6. The hole should be machined in accuracy class 8 and the outer surface in 6.
There are holes in almost every construction of machine parts and devices regardless of the class of parts. We distinguish the following criteria for the division of hole types. Most of them are usually classified simultaneously into several types.
- Qualitative criterion (accuracy of geometric dimensions and surface roughness): inaccurate, accurate and very accurate holes. Holes for fastening screws do not require high accuracy and are made in the workshop accuracy class (IT14-15).
- Criterion for machining in solid material or pre-made holes in the blank (figure 2). Pre-made holes in castings or forgings are characterized by an uneven surface with high roughness, which contributes to faster wear of the twist drills. It is recommended that this type of hole be machined with bits with cutting inserts at first or bored.
- Criterion for through holes and blind holes. Machining through holes is simpler than blind holes. For the latter, it is necessary to ensure efficient chip evacuation. It is necessary to use drills with internal coolant supply channels. External coolant supply with holes over 30mm deep does not work at all in terms of lowering the temperature in the cutting zone.
- Hole length criterion: normal and long holes.
- Diameter criterion: very small and very large holes.
Hole machining is usually associated primarily with drilling. This type of machining is treated primarily as roughing. This is also demonstrated by the achievable accuracy (IT11-12 accuracy classes) and surface roughness (Ra20-Ra5). Achievable quality parameters for this and other machining methods are presented in the article entitled Quality in manufacturing techniques. However, it should be remembered that this type of compilation was developed many years ago.
Today, hole machining is carried out using drills (solid carbide, with replaceable plates or with soldered carbide plates – figure 3). Different tools offer varying machining accuracy. Monolithic tools usually provide better accuracy and less roughness of the machined hole surface.
Modern drill bits such as CoroDrill from SANDVIK Coromant (figures 3 and 4) allow you to perform a single drilling operation without having to drill a guide hole (drilling and reboring).
Another example of a drill with replaceable inserts is CoroDrill 880 from SANDVIK Coromant for general drilling (figure 4) are dedicated to machining medium and large diameter holes with medium tolerance, including blind holes requiring a flat bottom. The correct configuration of CoroDrill 880 using a specific cutting insert allows boring.
CoroDrill families of interchangeable inserts are designed for machining a wide range of materials and ensure accuracy in IT12-13 class and surface roughness in the range of Ra1 to Ra5. It results from the fact that these are folding tools using cutting inserts.
Sandvik Coromant offers a wide range of drills with interchangeable inserts (CoroDrill 880, 881, Coromant U, T-Max® U for packets and trepanning) which allows economical machining when the reduction of machining costs has been considered crucial.
CoroDrill Delta-C solid carbide monolithic drills allow hole machining with accuracy in IT5-10 class. CoroDrill Delta-C drills should work at lower cutting speeds but with a higher feed rate than CoroDrill drills.
Spot drilling is used when machining a hole in the full material of the workpiece. The spot drilling cut involves making a recess in the axis of the planned hole. When performing this procedure on a lathe, spot drilling is usually performed in the workpiece axis. Modern CNC numerically controlled machine tools with high rigidity, providing specific positioning accuracy allow you to opt out of spot drilling.
In addition, the drill bit for spot drill should have a cone angle in the range of 90 ° ÷ 100º, which improves the drill position when entering the material. The advantage of using spot drilling is that you can opt out of the turning operation of the face of the part.
In the classical approach, in order to obtain an accurate hole (accuracy class IT6 ÷ 8) an operation consisting of a minimum of 4 operations should be performed: spot drilling, drilling, roughing and finishing boring. For holes with diameters up to Ø8, as a rule, a drill and a finishing reamer are used. In turn, for holes with diameters ranging from Ø16 to Ø50 in IT11 and IT 12 grades with deviations in the range of 0.11 to 0.25, instead of rough boring, shaping boring is performed. This results in improved hole alignment. If a low roughness is required, it is recommended to use a pre-finishing reamer. These types of tools are made to order, i.e. their economic use is limited to serial production. Commercially available tools and technological equipment should be used in piece and low-volume production.
In many cases, this type of technological operation configuration is still used. Modern tools, both monolithic and with replaceable cutting inserts, as well as machine tool constructions with high rigidity significantly affect the ability to process accurate holes. Thanks to this, the number of necessary treatments to achieve the required quality indicators is reduced.
The machining accuracy is influenced not only by the tool design but also by the machining parameters:
Cutting speed vc [m / min] is crucial for tool life. As the cutting speed increases, the temperature and tool flank wear rate increases. In the case of soft materials, whose machining is usually characterized by a ribbon chip, a higher cutting speed contributes to more favorable chip formation.
Feed rate fn [mm / rev] affects surface finish, hole tolerance and straightness. The feed value also affects chip shaping. High working feed rate during drilling means reduced main time, but also less wear for every meter of processed hole, but at the same time the likelihood of KSO (catastrophic blunting of the blade) increases by breaking the insert or drill (Figure 4).
Figure 5 shows an HSS tool steel drill used to drill holes in structural steel. Incorrect machining parameters, including too high feed, have led to the drill breaking in several places.
Chips and coolant
Chip evacuation plays an important role and must be ensured. Chip blocking and slow removal of chips affect hole quality and tool life. Correct chip formation primarily involves removing them without complications. According to , a good way to verify the correctness of chip removal is by hearing. A steady sound means that the chip removal process is taking place correctly. Intermittent sound means that the chips are blocked in the tool’s chip grooves.
Figure 6 shows the SANDVIK CoroDrill® 460 solid carbide drill tool and the effect of incorrectly selected machining parameters that led to scratching the surface of the machined hole in its initial part (halfway through the length of the through hole). Improper coolant supply from outside may have contributed to this. Chip removal was considered correct, although the surface of the machined hole suggests problems with proper chip evacuation during machining. The workpiece was a PA6 aluminum cube. This type of material has difficulties removing chips.
Damage to the surface of the holes (Figure 6) may indicate a lack of stability during the initial machining phase. The condition of correct hole performance is:
- the use of a tool holder with minimal radial runout;
- proper tool mounting in the holder;
- properly (firmly) fixture the workpiece;
- ensuring drill guidance.
Boring works very well in piece, small-lot and serial production when making fine holes. In series production, broaching is still used as a finish in justified cases. If the hole design does not contain grooves, reaming is the first choice over broaching. For broaching, it is necessary to design and manufacture the broach.
Boring is finishing by multi-edge tools. An example of a modern reamer with replaceable cutting inserts is a tool from SANDVIK CoroReamer 830 (fig. 7). As you can see in figure 7, the Cororeamer 830 reamer is a modular tool with an exchangeable head. Replacement of the head in this reamer can be carried out on the machine tool without having to remove this tool. The exchangeable head is fixed in the mandrel with a conical surface, which ensures the required repeatability of concentricity with beating up to 3 μm. In the head grooves, we see channels feeding the coolant directly to the cutting zone (lowering the temperature in the cutting zone and removing chips).
The SANDVIK CoroReamer 830 shown in figure 7 allows holes with H7 tolerance. The basic purpose of this reamer is machining steel and cast iron. The limitation of this tool is the ability to process only through holes. The SANDVIK Coromant range also includes monolithic reamers (figure 8). CoroReamer 435 and 835, which also ensure hole accuracy with IT7. Reamers with straight grooves are designed for machining blind holes, and with helical grooves for through holes.
Returning to the sleeve design in figure 1 let’s determine how we can make holes in this sleeve. We are dealing with through holes made in accuracy class 8 (H8). The holes were made initially in the casting or forging, depending on the material used. We should remember that in the case of bushes in the first operation of the technological process, we can make the hole ready, unless there are justified contraindications (high surface smoothness, keyways, transverse holes). We have several options to choose from. The first of these is machining the hole almost to the size of Ø40H8 using boring and making a technological groove. In the next treatment, the hole is finished by boring (a separate article is being prepared). The second option due to the diameter is the use of pre-machining a drill with interchangeable cutting inserts, and then performing the cut or reaming or boring operations.
The final selection of machining methods depends on their current availability, and the goal is to achieve the required quality parameters (accuracy of geometric dimensions and surface roughness). The required surface roughness may require finishing boring or grinding. For the sleeve analyzed, fine boring should provide the required surface roughness Ra0.63.
- Feld M., Podstawy projektowania procesów technologicznych typowych części maszyn, WNT 2000
- SANDVIK Coromant, Machining guide, SANDVIK 2010
- Company information materials Systemy i Technologie Mechaniczne Sp. z o.o.