Oil & gas materials require machining expertise

Aside from challenging features, the other unifying factor relating to the machining of oil and gas industry parts is tough workpiece materials. From heat resistant super alloys and titanium used for stationary gas turbines, through to super duplex alloys for piping components, cutting tool expertise is at the forefront of machining success.

 

 

Staying power

Nickel-based heat resistant super alloys (HRSAs) are deployed widely in landbased, industrial gas turbines for power generation applications. Here, turning operations dominate in parts such as discs, rings, and shafts, while milling is the primary machining process on components such as housings and blades.

 

The first point of note for machine shops processing HRSA materials is that coolant should be applied in all operations (excluding milling with ceramics). High pressure coolant (HPC) up to 80 bar will show positive results in terms of tool life and consistency, while dedicated HPC tools with fixed nozzles will also deliver benefits thanks to parallel laminar jets of coolant with high velocity directed accurately between the insert and chip. When turning, operators should use at least 20 l/min of coolant and a basic pressure of 70 bar. However, for milling and drilling, use at least 50 l/min to accommodate the extra nozzles on milling cutters and larger drill diameters.

 

Turning point

The turning of nickel-based HRSAs for stationary gas turbine applications can typically be deconstructed into three distinct machining stages. First stage machining (FSM) sees depths of cut taken of up to 10 mm. Here, forged components often have rough, uneven skin or scale, and this is best removed using carbide grades or ceramics (Sialon or whiskered ceramic) at high feed rates, large depths of cut and low speeds.

 

Intermediate stage machining (ISM) involves typical depths of cut of 0.5 to 5 mm. The material at this stage is mainly in the final hard/aged condition having undergone some form of heat treatment after FSM. The ISM process normally involves profiling operations at moderate tolerances, where productivity is important, but insert security equally vital. Again, ceramic inserts work well. As a rule of thumb when turning with ceramics, the entering angle should be optimised at around 45°, while maximum chip thickness should be between 0.08 and 0.15 mm.

 

Last stage machining (LSM) represents the least amount of material removal (0.2 to 1 mm depth of cut), but imposes the highest demands on surface quality. Cemented carbides are preferred to ensure a minimal deformation zone and correct residual stresses in the workpiece surface. Speed should not exceed 60 m/min for critical parts.

 

Through the mill

When milling super alloys, there are certain process requirements which must be observed. For instance, cutter accuracy in both radial and axial directions is essential to maintain constant tooth load and smooth operation, and to prevent the premature failure of individual cutter teeth. Cutting edges must also be sharp with optimised edge-rounding to avoid chip adherence at the point where the edge exits the cut. Furthermore, the number of cutting teeth actually in cut during the milling cycle must be as high as possible. This will give good productivity provided there is sufficient stability.

 

When milling, common practice is to employ a fairly low cutting speed in combination with a moderately high feed per tooth. This will help produce a chip thickness not less than 0.1 mm, which in turn prevents work-hardening of the material. The cutting edge geometry should always be positive. In addition, down milling (climb milling) is advisable to obtain the smallest chip thickness where the edge exits the cut. When machining in a single pass, an indexable insert cutter diameter 20 to 30 percent larger than the workpiece width is recommended. The milling cutter should always be positioned off-centre, producing the thinnest chip on exit.

 

Surface speed, together with material hardness, is the most important factor in determining tool life when milling HSRAs. Cutting temperatures for these alloys are typically 750 to 1020ºC – sufficiently high that oxidation and work hardening become contributory factors in tool wear. An increase in cutting speed of just 5 m/min can potentially reduce tool life and total material removed by approximately 30 percent. Other factors worthy of careful consideration in almost all milling operations on HRSAs include feed per tooth, entering angle, and grade selection.

 

Dynamic ceramics

Ceramic inserts have a much higher resistance to heat compared with carbide, making them an excellent option for machining HRSA where high cutting temperatures are present. Ceramic milling typically runs at 20 to 30 times the speed of carbide.

 

On the flip side, ceramics can have a negative effect on surface integrity and topography, and are therefore not used when machining close to the finished component shape. Due to the lack of toughness of ceramic material, round inserts are used to suppress the high notching tendency. In terms of cutting speed, this should be balanced to create enough heat in the cutting zone to plasticize the chip, but not so high as to unbalance the ceramic. Performed dry, the main application for ceramic milling is the machining of oil drilling equipment due to the high metal removal rates over carbide inserts.

 

Blades edged with benefits

The milling of gas turbine blades is a special case. Here, roughing the blade rhombus and aerofoil from blanks (to achieve the basic blade form) is often core focus as it represents the bulk of machining. Many blades are made from martensitic stainless steel but also from Duplex stainless steel, HRSAs and titanium. This operation has seen a number of different solutions through the years but round insert milling cutters and ball-nose end mills have become the mainstay through their ability to generate profiles with a secure and strong cutting edge, and also their cutter-to-part clearance.

 

When a milling cutter is used for rhombus roughing, a large amount of cutter engagement with the part is an important success factor, with 60 to 80 percent being the target. This can only be achieved by applying the most suitable cutter diameter in combination with the most advantageous tool path. Also, the best balance between feed, depth of cut, insert size, geometry, grade, insert pitch, and cutting forces should be established to help maximise performance, security, and results.

 

Ace in the hole

Moving to hole-making, the drilling content on certain stationary gas turbine components can be as high as 15-25 percent, particularly on housings and shafts. With this in mind, an efficient process is vital. In through-holes of 12-60 mm diameter, in stable conditions, indexable insert drills can be deployed for the first roughing operation on either turning or machining centres. For gas turbine parts with larger through-holes (60-110 mm diameter, up to 4xD deep), trepanning on a lathe is preferred as it saves expensive core material in readiness for other components. This method also reduces the power required and production time. For deeper holes the bar is trepanned from both sides.

 

Of course, many oil and gas shafts have very deep holes, sometimes in excess of 10xD. Here, indexable deep-hole drills are used which require a bushing or pre-machined hole to start. After drilling, either damped boring bars or special boring heads with support pads are used to finish the bore. Traditionally this operation has required special deep-hole drilling/boring machines; however, these are now being transferred to mill-turn or multi-task machines.