John MitchellClick image to enlargeby John Mitchell

Selecting proper lead angles can extend tool life

Selecting the correct speed and feed to run your parts is essential to optimize your output. However, it's not enough. Consider the lead angle of a turning tool. A 90° lead angle will result in an average chip thickness equal to the programmed feed rate. So a 0.008 in. (0.20 mm) feed per revolution will result in an average chip thickness of 0.008 in. (0.20 mm). Conversely, a 45° lead cutter with a 0.008 in. (0.20 mm) programmed feed rate per revolution will result in an average chip thickness of 0.005 in. (0.13 mm).

To the informed machinist, this can work to your advantage. Using a 45° lead cutter, the machinist should program his tool to feed at 0.011 in. (0.28 mm) per revolution to produce an average chip thickness of 0.008 in. (0.20 mm) while reducing the cycle time. Since the tool is in cut less time, it will extend the tool life. On the other hand, if the average chip thickness is too light, it can result in the tool "rubbing" and often "work hardening" the part and will reduce tool life dramatically.

Selecting the proper lead angle can extend your tool life. Think about the entry angle of the tool as it is introduced to the part. The most common turning insert on the market is a CNMG (an 80° included angle at the cutting tip) which has a -5° lead angle. The minus lead angle means you enter the cut with the weakest point on the insert, the nose radius. On the other hand, using a 45° lead to produce a gradual entry into the cut will lead in at the strongest point on the insert. Of course the part being produced must lend itsself to a lead angle or another operation may be required. That is, if the part being machined has a 90° shoulder, a second operation may be required or you may have to revert to the CNMG option.

Cutting forces act tangentially to the lead angle. If you use a 45° lead tool, the cutting forces will act downwardly into the part at 45°. In the case of a 90° lead, the cutting forces will act parallel to the centre line of the part. This puts little pressure on the part and instead, directs the pressure back into the chuck. A 45° lead tool will put pressure into the part and, in the case of a thin wall or small diameter part, may deflect or deform the part.

A good option is to use the obtuse corner (100° corner) of a CNMG. This will produce a 40° lead angle and allow the user to get eight corners from a CNMG rather than the traditional four corners. This is a good option for interrupted cutting.

These same principles apply to milling. A 90° milling cutter will produce an average chip thickness equal to the programmed chip per tooth. A 45° lead cutter will produce an average chip thickness of only 70 per cent of the programmed chip thickness. This allows for higher feed rates and longer tool life. However, in the case of a thin wall part being milled, the cutter may push the part down as it passes. Once the cutter has passed, "oil canning" occurs, which means the part bounces back to its original form, but in doing so, the part may end up out of spec or create a poor surface finish.

This is the basic principle behind high feed milling. Due to the lead angle, a typical high feed milling cutter will produce an average chip thickness of less than 20 per cent of the programmed chip per tooth, allowing for extremely high feed rates. The cutting force is directed down into the part and directly up into the spindle, which causes little deflection and reduces perpendicular cutting forces on the spindle, extending machine tool life. A common mistake when using high feed milling is running the cutter too slow. This can result in rubbing and can reduce tool life. A better option is to run the tool at the recommended elevated feeds taking small depths of cut and increasing each time until you achieve desired results. Take a trial cut with the recommended speed and feed, (0.060 in./1.52 mm chip per tooth), take a small depth of cut at 0.010 in. (0.25 mm) and monitor the horsepower on the machine's monitor. If everything is ok, take incremental depths of cuts at 0.020 in. (0. 508 mm), 0.030 in. (0.762 mm), then 0.040 in. (1.016 mm), etc. up to the point the horsepower is running in an optimum range.

The same idea applies to round insert (or button cutters) milling cutters, although with a round insert, the lead angle is dependent on the depth of cut. A light depth of cut produces extreme chip thinning and you can achieve high feed rates. However, when the button cutter reaches a wall, the lead angle changes quickly from a small lead angle of 10° to a 90° one, which can cause catastrophic failure. By comparison, the high feed cutter has clearances built into its design to accommodate this operation. SMT

John Mitchell is general manager for Tungaloy in Canada.

Emuge industry first: general purpose tap

Calling it an industry first, Emuge's MultiTap is a high performance tap designed for threading a range of materials including carbon steel, steel alloys, stainless steel, aluminum, cast iron, copper, brass and bronze.

Iscar: High speed face milling cutters

Iscar Tool's latest innovations includes new adjustable-pocket face mills in the Alutang family, designed to carry primarily PCD or PCBN tipped inserts for use on cast iron, hardened steel, aluminum or any other non-metallic materials.

Kennametal: Tapping into the wind turbine market

New high performance taps for large diameter tapping from Kennametal feature a wear-resistant powder metal substrate and proprietary top layers and coatings, designed wind turbine component machining of hubs, rings and gearbox housings.

Threading Options

by Mary Scianna

Whatever your machining process, external or internal threading is likely a part of your manufacturing process.

Cutting Tool Tips: When to Use Coolants

Coolant can be an effective way to cool a cutting tool, help expel the chip and prevent built up edge.

Stay In Touch

twitter facebook linkedIn