Thread milling becomes more mainstream

Tool cutting diameter (DC) should be approximately two-thirds of the major diameter (Do). ISCAR

The catalyst for thread milling entering the mainstream in thread production can often be traced back to four factors: a need to produce threads in hard materials, a need for tight tolerances, creating different threads with a single tool, and the need to create expensive parts that can’t be ruined by a broken tap.

Canadian Metalworking (CM) asked tooling experts Marlon Blandon, thread milling product manager at EMUGE-FRANKEN USA, and Yuri Sorkin, product manager - thread turning, thread milling, and taps at ISCAR, for their advice. Here’s what they had to say.

Blandon: Selecting the proper tool for internal threads starts by knowing the material you are cutting. This knowledge will help determine if you want to use a tap or a thread mill to make the internal threads.

With a tap, you must select the proper geometry for the material substrate to cut, rake angle of the cutting face, flute angle, and chamfer style. The proper flute style for proper chip evacuation, depending on the hole shape (through or blind), and threading depths is an important attribute to be aware of.

Material hardness and tensile strength are also important to know when thread milling is the thread cutting method of choice. However, it is not as important for selecting the best cutting geometry as it is for helping you determine the best programming approach, where the value of each radial engagement or number of cut passes you should use in a particular application factor in.

Sorkin: Tool cutting diameter (DC) should be approximately two-thirds of the major diameter (Do). A tool that has too large of a tool diameter causes distortion and incorrect thread profile.

Blandon: The hole shape should always be as round and straight as possible. This ensures you have an even-loaded torque for the threading process. Threading a non-cylindrical hole will result in a badly gauged thread or premature catastrophic failure of the tap, resulting in unnecessary repair or scrapping the whole part altogether.

Sorkin: Cylindricity and minor asymmetries in the hole are not as critical for thread milling. It’s best to produce a thread profile by using a mill thread cutter and 3-axis interpolation.

Blandon: For this type of hole shape, I recommend using a thread milling process instead of a continuous cut process, such as tapping. The continuous cut process has the tendency to jam up chips in interrupted hole shapes similar to threading pass crossed holes.

This is where an interrupted cutting process such as thread milling, where you can control the chips and evacuate them with coolant or air, becomes an excellent option for asymmetrical hole threads.

Multiple sizes and types of thread mills are available for your material and hole size. EMUGE-FRANKEN USA

Sorkin: This is a very important issue. Lowering your cutting forces at a thinner wall is necessary to prevent hole distortion when using a single-tooth cutter. However, you can machine parts with thin walls better by using a multirow tool.

Blandon: Thin walls are a problem for threading, regardless of the threading method employed. The best you can do is use a cutting method (versus forming). Be sure to use enough lubrication with a cut tap to avoid distorting the hole shape with torque. When using a thread mill, having good stability from the workpiece clamping to the toolholder is critical because everything must be as rigid as possible. This will avoid creating a lot of vibration which will lead to harmonics causing premature wear and breakage of the carbide thread mill cutting edge.

Blandon: With an interrupted thread cutting method [thread milling], you produce a comma-shaped chip, which can be easily evacuated with coolant or air. The same thread milling tool, being a single-plane cutter or a full milling section cutter with straight flutes or spiral flutes, can be used for either through or blind holes regardless if you are threading a through hole all the way through the part shape or only partially, or if it is a blind hole requiring full bottoming threads.

Sorkin: This is related only to the design of the tool. Some tools have a central coolant hole and excellent chip evacuation, which prevents recutting in blind holes.

It’s preferable to use indexable tools that can work in blind and through holes, which have internal coolant holes that direct coolant to the cutting edges along the flutes.

Blandon: The answer is heavily linked to the workpiece material, the thread sizes, the volume of parts, and the equipment available (a spindle connection of 40 taper, 50 taper, or HSK). In general, the holders available to hold the thread milling cutter and the desired cycle time per hole have a big influence on the preference of choosing a single row or multirow.

Sorkin: With indexable tooling, you can create many different thread profiles using the same tool. Also, easy insert indexing increases productivity.

However, they are not suitable for small threads.

Solid-carbide thread mills reduce cutting forces and have more flutes in relation to cutting diameters, making chip evacuation easy. They come at a high cost, especially at large diameters, and are typically limited to around 0.75 in.

Sorkin: Horsepower is somewhat important for thread milling but not the sole deciding factor. It influences the material removal rate and the size and depth of the threads you can achieve.

When thread milling, horsepower is not as critical as compared to tapping. A machine with a small spindle is all that is needed. ISCAR

Blandon: When thread milling, horsepower is not as critical [as compared to tapping]. You can use a small spindle CNC machine with a BT 30 connection and achieve and produce larger thread diameters using thread milling cutters with ease.

When tapping, the spindle size and horsepower required will vary depending on the thread size and the material you are cutting. Tapping is a continuous, form-fitting threading method, so horsepower and torque factor in much more significantly than with the interrupted thread cutting method, such as thread milling, which removes small amounts of material until the thread pitch and profile are formed.

Blandon: To use a thread mill, which is an interrupted thread cutting process (not a form-fitting one), you must create a program that tells the machine the toolpath to follow using 3-axis movement that will recreate the continuous thread pitch for the fastening effect on the part.

You cannot tilt the machine to achieve the thread lead. Instead, we use something called profile correction. The cutting tooth on a thread mill is ground smaller than the pitch you will produce on the part. This is done to allow the space to move the tool in this pocket using X/Y/Z axis movement and making the desired pitch value continuously.

Sorkin: The machine must be able to move the cutting tool along all three axes (X, Y, and Z) simultaneously. This is crucial for creating the helical path of the thread.

Using this method, you can achieve excellent and controlled thread surface finish and be repeatable.

Blandon: Yes. Because you are moving in three axes simultaneously and thread milling cutters are smaller than the hole you are threading, rigidity is paramount.

If a customer can only hold the tools using ER-type collets, we recommend using single-plane cutters and full milling section cutters with a skip tooth design to minimize the side load and radial pressure when moving around the circumferential path. ER-type collet holders do not provide the required holding power to achieve these movements without generating a lot of deflection, which will negatively affect the gauging of the thread. A holder that grabs most of the shank or clamping zone of the tool is the best choice for 3-axis simultaneous movement, such as an end mill holder with side lock screws or precision chucks with a Weldon flat. Hydraulic chucks, and even shrink-fit holders are better for thread milling than ER collet types.

Sorkin: The toolholder should be rigid enough to minimize deflection during cutting. This is especially important for small-diameter threads or hard materials. The toolholder also should have minimal run-out (eccentricity) to ensure accurate thread profile and prevent premature tool wear.

Choosing a toolholder that allows for proper coolant delivery to the cutting zone for optimal chip evacuation and tool life is also a good idea.

When thread milling the toolholder should be rigid enough to minimize deflection during cutting. ISCAR

Blandon: Left-hand threads are used more for security to avoid unintentional loosening and are fastened in a counter-clockwise fashion. Left-hand treads are the reverse of right-hand threads, which point the other way and tighten clockwise.

Blandon: I can say each milling direction has its pros and cons. Simply, climb milling tends to require a lot more stability, but it delivers the best tool life.

Conventional milling is a very stable cutting direction but, in some cases, doesn’t deliver the best tool life. The best situation is when you can employ only the benefits from each milling direction in one thread milling cutter. This is the case for the EMUGE LH helix cutters, requiring a LH spindle rotation but entering from the outside or the top of the hole in a corkscrew motion or conventional milling (best stability). This right-hand move plus the LH spindle rotation [G code] M04 equals a climb milling effect, which is the best chip shape for optimal tool life.

Sorkin: Conventional milling produces a thin-to-thick chip. It is best for machining cast iron or hardened materials (because the cut begins under the surface of the material). It can also be used when machining with a long overhang.

Climb milling produces a thick-to-thin chip. It creates a better surface finish, requires less power, lengthens tool life, and enables better chip evacuation.

Blandon: When thread milling, rolling into the cut guarantees a soft entry, allowing the cutting edge to penetrate the material gradually with ease rather than in a straight move into the wall of the hole with no room to ramp up into the cut.

Sorkin: If you do this, you will produce superior thread profile, reduce the cutting forces, increase tool life, and reduced chatter.

Blandon: I recommend both, but it depends on the workpiece material and hardness, the machine setup, holder type available for the cutting tool, and the thread size and depths.

Sorkin: When deciding between single and multiple passes for your thread milling application, you need to consider the thread size and complexity, material, machine capabilities, and production requirements.

A single pass is faster and has less tool wear. Milling with multiple radial passes is best for hard-to-cut materials, produces a better surface finish, reduces cutting forces, and reduces tool deflection.

Sorkin: The helix angle in thread milling refers to the angle between the cutting edge of the thread mill and a line perpendicular to the axis of rotation. It's a crucial factor influencing the cutting process and feed rate selection.

A higher helix angle (closer to 45 degrees) allows for better chip formation and evacuation. It also distributes the cutting force more evenly along the cutting edge for better tool life.

With a higher helix angle, you can typically use a slightly higher feed rate compared to a lower helix angle.

Generally, a range of 30 to 45 degrees is common for thread milling.

Blandon: Lubrication is not as critical for thread mills as it is with a tapping method. When thread milling, we just need to have an agent capable of evacuating the chips and cooling the cutting edges. Wet or dry, it doesn’t matter, as long as the short chips are evacuated.

Sorkin: For me, it’s wet for better chip evacuation and better surface quality.

EMUGE-FRANKEN USA, www.emuge.com

ISCAR, www.iscar.ca