Heat resistant super alloys (HRSA) can be divided into three material groups; nickel-based, iron-based and cobalt-based alloys. Titanium can be pure or with alpha and beta structures. The machinability of both HRSA and titanium is poor, especially in aged conditions, which impose particular demands on the cutting tools.
In the aerospace industry, machining is divided into three stages: First Stage Machining (FSM), Intermediate Stage Machining (ISM) and Last Stage Machining (LSM). In LSM, surface integrity is of upmost importance, but this limits cutting data. It emphasizes the importance of sharp edges to prevent the formation of so-called white layers, with different hardnesses and residual stresses.
For more detailed information, see the application guide ”Heat resistant super alloys” order No. C-2920:24 or ”Titanium machining” order No. C-2920:22.
Insert shape and entering angle
A common wear criterion in both titanium and HRSA is notch wear. By choosing a small entering angle or round inserts, feed and tool life can be increased considerably.
The unique Xcel insert combines the accessibility of a 93° angle to the tool holder with the productivity of a 45° entering angle at the cutting edge, at cutting depths up to 2.5 mm. It is suitable for semi-roughing operations.
Avoiding notch wear when machining HRSA-materials
Notch wear can never be eliminated, but it can be minimized through good planning and by following some general rules:
- Use round inserts.
- Use the smallest possible entering angle.
- Use the correct relationship between the insert diameter and depth of cut (see figure).
- Roll over action is possible in programming, which can eliminate the need for pre-chamfering and it also minimizes notch wear. There will be one contact point, where the insert hits the hard scale/surface at the corner of the component, and one contact point at the depth of cut line.
- Ramping is ideally suited for CNC lathes. It ensures, that any damage is spread out along the cutting edge. It is the best solution with varying depths of cut. Multiple passes with varying depths of cut can also be a good alternative. When using ramping or multiple passes, the depth of cut should never be less than 0.25 mm; otherwise there is risk of
Depth of cut
In order to minimize notch wear, the best results are obtained by using a depth of cut that is a maximum of 15% of the diameter of a round insert, or 15% of the nose radius of a non-round insert.
Larger depths of cut can be used, but never greater than 25% of the insert diameter.
If these types of large depths of cut are being used, the workpiece must be free of forging scale/hard skin.
Recommended when using ceramics.
- Pre-chamfering minimizes the risk of burrs when the insert exits the cut. It also has a positive effect on the insert when it enters.
- To avoid notch wear when chamfering, use a direction feed of 90° to the chamfer that is being produced.
Coolant should always be applied when turning HRSA or titanium alloys regardless of whether carbide or ceramic inserts are used. The coolant volume should be high and well directed.
High pressure coolant (with coolant pressures up to 80 bars) is now common in modern machines and, together with the CoroTurn HP coolant supply technology, cutting speed can be increased by up to 20%, tool life by up to 50% and, last but not least, chip breaking can be considerably improved.
Jet-break technology, using ultra high pressure coolant (with coolant pressures from 80 to 1000 bars) can be applied when using vertical turning lathes (VTL).
Please contact your Sandvik Coromant representative for more information.
Titanium – Ti6Al4V (30 HRc)
CoroTurn® 107 conventional
CoroTurn® 107 with HP-technology
Similar improvements can also be achieved in HRSA materials.
Carbide insert grades
Carbide grades should be selected according to the table below, depending on the operation (finishing, medium, roughing), and the machining conditions (good, average, difficult).
Ceramics are not recommended for titanium.
Geometry and grade recommendations for titanium
HRSA, Roughing (First Stage Machining, FSM)
Machining is done in the annealed condition (approx. 26 HRc).
In materials with forged or cast skin, use single-sided inserts with geometries -HM or -SR in grades GC2025 or GC2015. The entering angle should be small (not larger than 75°) and the depth of cut should be large enough to reach under the hard skin in order to minimize the notch wear.
If a larger entering angle is necessary, PVD-coated grades like GC1105 and GC1115 are better choices. Grade H13A is the first choice for best bulk toughness.
CC670 (whisker reinforced) can be used, but both feed fn and cutting depth ap must be reduced, cutting speed, vc, on the other hand, can be much higher. Use a small entering angle or round inserts for best tool life.
HRSA, Medium (Intermediate stage machining, ISM)
Machining is performed in the aged condition, 35-46 HRc.
The first choice is GC1105. For operations requiring greater toughness, use GC1115.
Use grade S05F, combined with round inserts or small entering angles, for best productivity.
The advantages in using ceramics in Medium or ISM operations are obvious. The depth of cut in aged materials is lower than that required in the roughing (FSM) operations. Sialon ceramics have excellent notch wear resistance and can be used at much higher cutting speeds, vc, (150-280 m/min), in comparision with carbide grades. The feed, fn, can also be kept at a high level (0.15-0.35 mm/r). It is, however, of paramount importance to have a stable set-up and a correctly applied coolant supply (volume is more important than pressure). The first choice for maximum productivity is CC6060; for more
unstable conditions, select CC6065.
Ceramic grades application areas
Cutting parameters – ceramics
The speed should be balanced to create enough heat in the cutting zone to plasticize the chip, but not so high as to unbalance the
The feed, fn, should be selected to provide a chip thickness, hex, which is high enough so as not to work-harden the material, but not so high as to cause edge frittering.
Higher feeds and depths of cut require a reduction in the cutting speed, vc.
These boundaries will change depending upon the component material hardness and grain size.
Start cutting data recommendations (RNGN 12, RCGX 12) – Inconel 718 (38 to 46 HRc)
Finishing (Last Stage Machining, LSM)
Machining in the aged condition, 35-46 HRc. Due to the high demands for low
residual stress, ceramic inserts are not recommended, and cutting speed should be kept below 80 m/min. Other factors influencing the residual stress are:
- Flank wear – maximum 0.2 mm
- Chip thickness – maximum 0.1 mm
- Sharp edges, ground inserts to be preferred.
For finishing of HRSA
GC1105 (PVD-coated) has the best notch wear resistance, and is the first choice when:
- Feed is below 0.1 mm/r
- Turning thin-walled or slender components
- The entering angle must be 75° or more
- Long tool overhangs cannot be avoided.
S05F (CVD-coated) provides better tool life than GC1105, it a small entering angle or a round insert can be used.
Geometry and grade recommendations for HRSA
Predicting tool life − spiral cutting length, SCL
Because inserts have a relatively short tool life when turning HRSA and titanium materials, one insert can often only machine one pass before it is indexed. The spiral cutting length, SCL, calculation is a method used to predict the tool life of an insert edge to avoid unwanted insert changes in the middle of a cut.
- Each SCL graph is unique and is only applicable for that particular insert, geometry, grade, depth of cut and material.
- In finishing, it is especially important to avoid an insert change in the middle of a pass. Therefore, we offer a range of cutting speeds to allow for different lengths of cut.
- For roughing, we have identified the optimum cutting data for each insert style and the corresponding spiral cutting length, SCL.
The objective is to identify the correct cutting speed, vc, that will manage a full pass without an insert change.
1) Select insert style to suit the component.
2) Use optimized ap and fn for that insert.
ap=0.25 mm, fn=0.15 mm
3) Calculate SCL.
Dm1 = 600 mm, lm = 150 mm
4) Select cutting speed, vc, from the SCL / vc -diagram
CNGP 120408 1105
SCL = 1885 m = >vc = 50 m/min
So, with vc = 50 m/min, one edge will manage a spiral cutting length of 1885 m corresponding to a turned component length, lm, of 150 mm.
The diagram is valid for Inconel 718 (46 HRc), and for other nickel alloys with the same hardness – Udimet 720, Waspalloy.
The objective is to predict when the insert needs to be indexed/changed.
1) Select insert style to suit the component.
2) Use optimized vc, ap and fn for that insert.
CNMX 1204A1-SM S05F
vc = 50 m/min, fn = 0.35 mm/r, ap = 2.7 mm
3) Note SCL capability (tool life) for that insert.
SCL = 450 m
4) Calculate SCL.
Dm1 = 600 mm, lm = 150 mm
5) Calculate the number of insert edges required.
807/450 = 2 edges
For more information, order the Application guide for Heat Resistant Super Alloys, C-2920:24.