Technical Tips - Turning
(1) (2) (3) (4) (5) (6) (7) (8) (9/10)
ANSI Inch C N M G 4 3 2 __ LF
ISO Metric C N M G 12 04 08 __ LF
- First station indicates shape of insert and together with 2nd station determines number of useable cut edges.
- Second station indicates relief angle or rake angle of the insert.
- The third station provides a working gage for repeatability. It sets tolerance to the I.C. (inscribed circle) and creates a gage tolerance for the I.C. to the over-the-nose radius along with the thickness of the insert.
- Fourth station indicates insert type. Indicates with or without hole, shape and size of hole, chipbreaker form, and single- or double-sided insert.
- Fifth station indicates I.C. size of the insert.
a. For under ¼-inch inserts, I.C. is measured in 1/32-inch increments.
b. For ¼-inch and greater inserts, I.C. is measured in 1/8-inch increments.
Note: Use larger I.C. inserts for heavier or interrupted cutting conditions, and
smaller I.C. inserts for finishing operations. - Sixth station designates insert thickness.
a. For under ¼-inch inserts, thickness is measured in 1/32-inch increments.
b. For ¼-inch and greater inserts, thickness is measured in 1/16-inch increments. - Seventh station designates nose radius of the insert.
Note that the nose radius size of the insert, along with federate inches per revolution (ipr), have the greatest impact on the attainable surface finish of the cut. - Optional designates R for right-handed or L for left-handed insert.
- Designates edge preparation: sharp edge, radius hone, T-Land
- Designates edge preparation: sharp edge, radius hone, T-Land
1. Utilize Lead Angles
Lead angles provide three primary functions:
1) Control the direction of radial cutting forces
2) Provide effective chip thinning
3) Protect weakest part of the cutting edge
Note: In finishing operations with a shallow depth of cut, the nose radius of the insert acts as an extension of the lead angle.
2. CVD Coatings Over Carbide Inserts (Chemical Vapor Deposition):
- The most common coatings consist of TiC, TiCN, TiN and Al2O3.
- Materials are multi layered and contain thermal cracking on surface.
- Coating cannot be used on sharp cutting tools.
CVD-coated cutting edges require a larger edge preparation. This larger edge preparation requires an increased feed (ipt) to obtain satisfactory tool performance. CVD process produces significant heat shield and increased speed capability.
3. PVD Coatings Over Carbide Inserts (Physical Vapor Deposition):
PVD adds lubricity and seals porosity and keeps material from penetrating the tool surface. PVD coatings have finer grain size than CVD coatings and can be coated over sharp edges.
Primarily used as a top coat of TiN or TiAlN. It is used to coat over CVD coatings to seal surface. Also used on finish turning applications.
4. Cermet Ceramic and Metal Combination
Grades come in coated or uncoated.
Advantages: High flank wear, good crater resistance, high chemical stability and hot hardness (resistance to heat).
- Good in stainless steels, steels, and ductile irons.
- Used at high speeds for finish turning, precision turning with low chipload, and light DOC.
5. Alumina Ceramics consist of nearly 100% Alumina (Al2 O3)
Good for machining steel and cast irons
- White ceramic tool has best wear resistance but is not too strong.
- Dark gray is stronger but has less speed capability
Advantages:
- Low thermal conductivity
- Good hot hardness
- Chemically inert with steel
- Higher speeds & Feeds
Disadvantages:
- Poor transverse rupture strength
- Low toughness
- Expensive processing
- Unreliable tool failure
6. Ceramic Composite Materials (Al2 O3 + TiC)
- Addition of TiC or TaC increases toughness
- Addition of Zircronium Oxide (ZrO2) increases fracture toughness by 25%, making it possible to machine nickel-based alloys
7. Silicon Whisker-Reinforced Alumina (SiC) 25%
- Fracture toughness and resistance to crack close to carbide grades.
- Proven successful for machining nickel-based alloys.
8. Sialon Ceramics (Si3 N4 and AlN + Alumina + alloying agent)
The combination creates better bend strength, high hardness and low coefficient of thermal expansion, to create good thermal shock resistance.
Sialon grades use negative rake angles with heavy hones or T-Lands.
Successfully applied for roughing cuts, rough surfaces, and interrupted cuts. Also successfully machine steel and cast irons.
9. Polycrystalline Cubic Boron Nitride (PCBN)
- Extremely hard, and second in hardness only to diamond.
- PCBN is used in hard steels and cast irons with hardness greater than 45RC. It can be used for finish turning cast iron and high-temp alloys.
- Applied using negative rake heavy hones or T-lands.
- Has excellent abrasive resistance and long predictable tool life.
- Parts can be machined without grinding.
- It can be used on interrupted cuts.
10. Polycrystalline Diamond (PCD)
- Provides significant productivity and tool life advantages. They are generally limited to machining nonferrous and nonmetallic materials such as aluminum, copper, magnesium and various nonmetals.
- Grade exhibits good abrasion resistance and high strength.
- Not recommended for nickel alloys because diamond and ferrous metals turn to graphite at high temperatures.
Achieve Double Productivity with the Same Surface Finish or a Better Workpiece Finish
Milling inserts have used wiper technology to improve surface finishes for years. By applying a facet (flat) or a wiper to the insert, improvements to the milled part surface are achieved.
This same technology is being applied to turning applications. As a result, in many applications a subsequent grinding operation can be eliminated.
Download the PDF file attached for the complete Technical Tip on this subject. The PDF contains many images that cannot display in this smaller view window.
The 80° diamond insert has a 100° corner that is widely under-utilized. The insert utilization can increase from 50% to 100% using this corner.
The 100° corners have the same cutting capabilities as the 80° corners for straight turning, facing, and profiling.
Toolholders are available for the utilization of the 100° corner. Consider using toolholders MCHNN164C, MCKNR164C, and MCRNR164C.
Technical Tip #137 - Using 100-Degree Corner of 80-Degree Diamond Insert
Applying the correct chipbreaker for the application will help you get the most out of your insert performance.
When choosing the right chipbreaker, first determine two things: the material being machined and the depth of cut.
For example, steels primarily use a negative chipbreaker. Stainless and non-ferrous materials use a positive chipbreaker.
There is range on the depth of cut for chipbreakers.
For example, a finish chipbreaker should not be used for roughing. The roughing cut is a larger depth of cut, and the finish chipbreaker has a weaker edge. The correct chipbreaker will give more performance life to the insert.
Center height should always be checked after installing a new tool.
The tolerances of the tool shank and pocket, along with the tolerances of the insert, could affect the overall center height.
It is possible for the tool to become above center, or in some cases, below center. Most machines do not take this into consideration.
The machine is manufactured to a specific height and tolerance, which in turn might affect your center height. The improper center height will cause the tool to perform incorrectly.
This why it is important to check the center height after a new tool is installed.
Technical Tip #139 - Stacking Tolerances Affect Center Height
Using the correct number of passes will prevent premature insert failure.
When more passes than recommended are used, tool life will decrease.
If too few passes are used, the insert could chip and suffer failure.
The pitch of thread dictates the numbers of passes (see chart on attached pdf). Using the correct number of passes will provide better tool life and good thread quality.
Download the pdf file to view the entire technical tip document.
Technical Tip #140 - Using Correct Number of Passes in Threading
Cut-Off Inserts:
Cut-off inserts are designed in neutral and right-hand or left-hand cut.
- Neutral inserts -- (cutting edge parallel with work piece) are used primarily in solid material and produce a center “stub“ on both the workpiece and the part when using solid material stock. Neutral inserts also reduce side deflection.
- Right-hand cut or lead inserts leave a center “stub“ or bur on the chuck side of the workpiece and produce a clean part.
- Left-hand cut or lead inserts leave a center “stub“ or bur on the part and produce a clean workpiece nearest the chuck side.
Guidelines:
Right- or left-handed inserts are most often used in cut-off operations for tubing.
The use of handed inserts may decrease tool life and increase side deflection.
Note that when using handed inserts in inverted holders, the above mentioned will be reversed.
Programming:
Modern CNC controls enable the programmer to easily adjust infeed angles, the number of passes, and depth-of-cut for each pass.
Threading inserts perform best at an infeed angle of 29 1,2-degrees, although 15-degrees to 30-degrees is acceptable.
Also, it is important to maintain a minimum of .005” depth of cut per pass. In most applications, use of CNC canned cycles produces only marginally successful results. Custom-written programs are better and thus are recommended.
Last Pass:
Some CNC controls require the last pass to be at a 0-degree infeed angle. The chip will not break on the last pass at a 0-degree infeed angle.
On most carbon and alloy steels, the last pass can remain at .005” depth of cut and produce an acceptable finish. For some materials, a .001” to .003” (spring) pass may be used to improve surface finish, however, chipbreaking action may be compromised.
A common problem in boring applications is that the boring bar is extended further than recommended, or the diameter-to-length ratio is exceeded for that particular bar.
Boring bars are made of different materials, and they all have different diameter-to-length ratios. Where one boring bar will work, another may not.
The most common materials for boring bars and their diameter-to-length ratios are:
Bar Materials Diameter-to-Length Ratio
· Steel 4:1
· Heavy Metal 4:1 to 6:1
· Steel Devibrator 6:1
· Tungsten Carbide 6:1
· Carbide Devibrator 8:1
· Standard Tunable 6:1 to 10:1
· Special Carbide Devibrator over 10:1
· Special Tunable 10:1 to …
When choosing a boring bar, look at the diameter and length of the hole to be bored. Then choose the proper boring bar based on the diameter-to-length ratio that will work best for the application.
Carbide inserts are designed in many different shapes to work their best in a variety of materials, based on their insert strength.
To see the basic insert shapes from strongest to weakest and learn more, download the pdf file
0° Radial Angle: Cuts on both sides of the thread form, which puts all the cutting edge in the cut and protects the edge from chipping. The disadvantage is the tool develops a channel cut that may be difficult to handle. Tip chipping occurs when cutting high tensile materials.
10° Modified Flank Angle: Cuts using both sides of the thread form, but more on the leading edge than the trailing edge. The tool is protected from chipping similar to the 0° infeed angle. A channel-type chip can develop, but uneven chip thickness helps remove the chip in a way similar to the flank infeed below.
10° Flank Angle: Cuts with the leading edge of the threading tool, which gives the chip a definite flow out of the thread form area. This flow reduces the burr problem on the trailing edge of the tool. To avoid bad surface finish, chipping, or excessive flank wear due to rubbing of the trail edge, the infeed angle should be 3° to 5° smaller than the angle of the thread. This is a type of modified flank thread. The disadvantage is the trailing edge of the insert may drag or rub, and tends to chip. Torn threads or poor surface finish can result when cutting soft, gummy materials like low carbon steels, aluminum, and stainless steels.
Alternating Flank Angle: The alternating infeed increases tool life because both cutting edges are used equally. Please note that some machine tools may require special programming techniques to achieve this method of infeed. The main disadvantage is this type of infeed is difficult to cut on conventional machinery.
To reduce burrs:
- Use left-handed or right-handed inserts at slower feed rates.
- Pre-chamfer the workpiece, both externally and internally.
- Holder should be on center or .005” to .015” above centerline.
- If using a neutral insert, use the most narrow width possible.
To reduce chatter in cut-off applications, follow these guidelines:
- Minimize blade and holder overhang.
- Minimize chucking overhang.
- Adjust speed up or down.
- Adjust feed rate up or down.
Technical Tip #156 - Chatter Reduction in Cut-Off Applications
Selecting a full profile threading insert versus a partial profile insert depends on the end user’s needs.
The full profile insert is the preferred choice if the same thread pitch is made repeatedly.
A partial profile insert enables flexibility with standard and non-standard thread pitches within a range.
The full profile achieves high thread concentricity due to the insert cutting the major and minor diameters concurrently. Also, deburring is not needed with a full profile insert, which reduces machining costs.
Technical Tip #158 - Full vs Partial Profile Threading Inserts
Romicron boring systems can produce finish bores with tolerances of a few microns (1 micron = 0,001 mm) in diameter. Because many factors can influence finish-boring tolerances, Kennametal suggests plus or minus 2 microns on the diameter. Typically, Romicron can achieve bore-to-bore variations of just a few tenths of a micron under ideal machining conditions.
To achieve optimum results in high-accuracy boring, follow these requirements:
- Good, solid clamping of the workpiece.
- Thin-walled workpieces are prone to distortion under boring, clamping, and vibration. Evaluate the workpiece to determine if proper clamping is needed.
- Long bores, where the length of bore exceeds 2.5 times diameter, require special care. In some cases, special shanks and shank shapes, and heavy metal shank materials will be required.
- Using extensions for extended-length boring results in overhangs. Properly evaluate and analyze of these cutting conditions.
- Good machining practices must be followed when using diameter extenders.
- Machinability of exotic materials should be examined to determine the best machining methods.
- Machining of interrupted cuts can alter bore accuracy and configuration.
- Coolant supply must be used to prevent thermal distortion.
- Ultra-high accuracy boring requires planning prior to starting the operation. As a general rule, try to plan for ultra-high accuracy boring last in the sequence of operations.
Technical Tips #164 - High-Accuracy Boring with Romicron System
AccordianPage
HOW TO BUY
Contact Kennametal US Representative 800.446.7738
Contact Kennametal UK Representative +44/1384 408060
