HRSA and titanium turning

​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 utmost 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” or “Titanium machining”.
Contact your Sandvik Coromant representative for a copy or visit www.sandvik.coromant.com/us.

A common wear criterion in both titanium and HRSA is notch wear. By choosing a large lead angle or round inserts, feed and tool life can be increased considerably.

The unique Xcel insert combines the accessibility of a -3° angle to the tool holder with the productivity of a 45° lead angle at the cutting edge, at cutting depths up to .098 inch (2.5 mm). It is suitable for semi-roughing operations.​​​

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 largest possible lead 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 .010 inch (0.25 mm); otherwise there is risk of chipping.

Depth of cut​

Pre-chamfering

• 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 1160 psi) 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 1160 to 14500 psi) can be applied when using vertical turning lathes (VTL).

Please contact your Sandvik Coromant representative for more information.

​CoroTurn^® 107 conventional

​CoroTurn^® 107 with HP-technology

​Carbide insert grades

Geometry and grade recommendations for titanium

​Machining is done in the annealed condition (approx. 26 HRc).

Carbide inserts:

In materials with forged or cast skin, use single-sided inserts with geometries -HM or -SR in grades GC2025 or GC2015. The lead angle should be small (not larger than 15°) 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 lead angle is necessary, PVD-coated grades like GC1105 and GC1115 are better choices. Grade H13A is the first choice for best bulk toughness.

Ceramic inserts:

CC670 (whisker reinforced) can be used, but both feed f_n and cutting depth a_p must be reduced; cutting speed, v_c, on the other hand, can be much higher. Use a small lead angle or round inserts for best tool life.

​Machining is performed in the aged condition, 35-46 HRc.

Carbide inserts:

The first choice is GC1105. For operations requiring greater toughness, use GC1115.

Use grade S05F, combined with round inserts or large lead angles, for best productivity.

Ceramic inserts:

The advantages of 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, 492-918 ft/min (150-280 m/min), in comparision with carbide grades. The feed, fn, can also be kept at a high level .006-.014 inch/rev (0.15-0.35 mm/r). It is, however, of paramount importance to have a stable setup 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 ceramic.

The feed, f_n, should be selected to provide a chip thickness, h_ex, 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, v_c.

These boundaries will change depending upon the component material hardness and grain size.

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 262 ft/min (80 m/min.) Other factors influencing the residual stress are:

• Flank wear – maximum .008 inch (0.2 mm)
• Chip thickness – maximum .004 inch (0.1 mm)
• Sharp edges, ground inserts to be preferred.

Carbide inserts:​

GC1105 (PVD-coated) has the best notch wear resistance, and is the first choice when:

• Feed is below .004 inch/rev (0.1 mm/r)
• Turning thin-walled or slender components
• The lead angle must be 15° or more
• Long tool overhangs cannot be avoided.
  

S05F (CVD-coated) provides better tool life than GC1105, if a small lead angle or a round insert can be used.

​Note:

• 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.

Finishing

​4) Select cutting speed, v_c, from the SCL / v_c -diagram

Example:

CNGP 432 1105

SCL = 6184 ft = >v_c = 164 ft/min

So, with v_c = 164 ft/min, one edge will manage a spiral cutting length of 6280 ft corresponding to a turned component length, l_m, of 5.906.

​Roughing

The objective is to predict when the insert needs to be indexed/changed.

1) Select insert style to suit the component.

2) Use optimized v_c, a_p and f_n for that insert.

Example:

CNMX 43A1-SM S05F
v_c = 164 ft/min, f_n = .014 inch/rev, a_p = .106 inch

3) Note SCL capability (tool life) for that insert.

Example:

SCL = 1476 ft

4) Calculate SCL.

Example:

D_m1 = 24 inch, l_m = 6 inch

​5) Calculate the number of insert edges required.

Example:

2691/1476 = 2 edges