Thread milling, simplified

Author Susan Woods
September 01, 2012 - 11:15am

While thread milling is a well-established process, some machine shops are still afraid to try it, fearing it is too complicated. “Thread milling is not a big mystery, but some shops are hesitant to do it,” said Joe Mazzenga, sales manager for J.M. Sales - USA, Troy, Mich., which offers solid-carbide and indexable-insert thread mills. “In reality, we can set up a customer to successfully thread mill fairly easily—as long as they have the right tooling.”

Thread milling requires a machining center capable of helical interpolation, which requires three axes of simultaneous movement. Two axes perform circular interpolation while the third moves perpendicular to the circular plane. Most CNC machines built in the last 10 to 15 years have this capability.

The same KOMET JEL thread mill cutting two different diameter holes—an M10×1.5 (left) and an M18×1.5. Courtesy of KOMET.

Courtesy of KOMET

The same KOMET JEL thread mill cutting two different diameter holes—an M10×1.5 (left) and an M18×1.5. 

“Rarely do I run across someone who can’t do it,” noted Jim Hartford, vice president of Advent Tool & Manufacturing Inc., Antioch, Ill. Advent manufactures single- and multiple-flute inserted thread mills and solid-carbide thread mills.

The inserted type with multiple flutes is typically for thread milling holes ¾ " in diameter or larger because there has to be enough room for the tool body and inserts. Smaller inserted thread mills are available but they usually have only one or two flutes.

“In a lot of cases, when you get into holes ¾ " and smaller you can still get a 4- or 6-flute solid cutter in there to do the job,” Hartford said. “With the inserted cutter, you could only get possibly one insert in there so your cycle times would be slow. For example, in 316 stainless steel, a single-flute thread mill would take 40 to 45 seconds to thread a hole. With a 4-flute, solid-carbide thread mill, it would take 6 to 8 seconds.”

Comparing solid-carbide and inserted thread mills at larger diameters, solid carbide is generally better for high production because it enables faster cycle times. 

“While both solid-carbide and inserted thread mills are suited for larger diameter holes, it can be advantageous to use smaller solid-carbide tools as they can typically run at higher feed rates,” said Wolfgang Ruff, vice president of engineering for KOMET of America Inc., Schaumburg, Ill. “For instance, if you have an M80×1.5 thread, you can run a 50mm-dia. inserted thread mill, which would have five cutting edges. You can also choose a 20mm-dia. solid-carbide thread mill, which will also have five cutting edges, but will run at more than twice the feed rate, effectively cutting the production time for each hole by half. This makes a huge difference for large production runs.”

Inserted thread mills can be good for smaller job shops with small production runs. One tool body can use multiple replaceable inserts with different thread forms, so it is more versatile and less expensive overall.

“They operate the same, but there is the cost difference,” Hartford said. “The tool body would cost about $300 to $450, but the inserts are only about $30 when replacement is needed. With the solid-carbide thread mill, the entire tool needs to be replaced at a $200 to $300 price tag. Also, it is easier for an operator to change an insert than to change an entire tool and requalify it.”

KOMET’s Ruff pointed out that inserts must be precisely positioned in the pockets. “If they are not, there is a mismatch from one insert to another and you cannot produce the proper thread.” KOMET offers solid-carbide thread mills as standard tools and inserted ones as specials. 

Solid-carbide and inserted thread mills come in helical- and straight-flute designs. Helical flutes reduce cutting pressure by distributing the cutting pressure along the flute.

“We use the helical almost exclusively,” Mazzenga said. “With a helical-flute cutter, you get a much smoother, quieter cut because the engagement of the teeth is spread over a greater range. On a straight-flute cutter, all the teeth on a given flute engage at the same time. This creates a greater amount of radial pressure, causing chatter and deflection.”

Nevertheless, straight flutes have a geometry suited for hard materials from 55 to 64 HRC. “The rake angle on a straight flute is constant,” Mazzenga noted.

Multiple vs. Single Form

Most thread mills, solid carbide or inserted, are multitooth tools. The teeth are arranged parallel, rather than helically like a tap. Multitooth thread mills cut the full depth of the thread in a single rotation around the hole.

Most thread mills, solid carbide or inserted, are multitooth tools.

Courtesy of J.M. Sales

J.M. Sales offers its Quattro indexable-insert thread mill (left), GFT thread mill with three rings of teeth for small diameters and 3 diameters deep (second from left), BGFS-W drill/thread mill for steels and titanium (second from right) and BGFS-H drill/thread mill for hardened steels (right).

One multitooth thread mill can cut threads of the same pitch in a range of diameters. This is because the diameter is determined by the CNC toolpath instead of the tool (as with a tap). “With a fixed pitch, the multiform tool can cut any 20-pitch thread, whether it is ¼-20, ¾-20 or 2"-20, as long as it can fit in the hole,” said Stephan Francescone, production manager for Harvey Tool Co. LLC, Rowley, Mass., which makes single- and multiple-form solid-carbide thread mills.

“The multiform thread mill is fast because all those peaks and valleys are cutting at the same time to create the thread,” said Jeff Davis, vice president of engineering for Harvey Tool. “The downside is that you’re locked into the pitch because of those peaks and valleys. Anytime you see more than one triangular thread form on a tool, you have a fixed-pitch situation.” Each thread pitch requires a different tool.

In addition to being able to cut any diameter, the advantage of a single-form thread mill is it can cut any thread pitch or a range of thread pitches. However, a single-form thread mill can only cut one thread in a single pass and must move around the hole as many times as there are numbers of threads.

“Even though they have to buy a thread mill for each pitch, larger production shops lean toward a multiform so they have a nice array of tools,” Davis said. “The single-form tools lend themselves more to smaller job shops that want a more flexible tool.”

The AlTiN-coated thread mills are suited for threading difficult-to-cut materials, ferrous materials, steels and aerospace materials. Photo credit: Harvey Tool

Courtesy of Harvey Tool

Harvey Tool’s AlTiN-coated thread mills are suited for threading difficult-to-cut materials, ferrous materials, steels and aerospace materials. They are also available with TiB2 coating for aluminum workpieces.

"KOMET’s single-form thread mill, typically for deep threads, has replaceable carbide heads.  Courtesy of KOMET. "

Courtesy of KOMET

KOMET’s single-form thread mill, typically for deep threads, has replaceable carbide heads.

J.M. Sales - USA’s Mazzenga said his company doesn’t subscribe to the belief that thread mills can be used for any diameter as long as the pitch is the same. “It is somewhat correct, but we don’t define it that loosely,” he said. “Our thread mills are designed to cut the thread on the minor diameter as well as the flank and the crest. Most of our thread mills are manufactured for a specific pitch and diameter.

“We define that thread mill more completely than just 60° included threads (standard thread forms are 60° included),” he continued. “In reality, if you try to make your thread mill as large as possible for a specific thread and don’t compensate that form in the tool itself, you will produce threads that border the thread tolerance boundaries. It is quite possible to make an adjustment on the machine for pitch diameter and then have an oversize minor diameter. We correct the thread form of the tool to allow for this.”

KOMET offers both types of thread mills: those with the so-called “corrected profile” (M16 and under) and those without the corrected profile. When using the latter for larger diameter holes, it is crucial to follow the “23 concept” where the diameter of the thread mill has to be no larger than 23 of the hole to maintain the correct pitch for the threads.

In the Deep

In general, a thread mill is limited to going about 3 diameters deep because the cutting forces are not balanced.

“You really don’t want to take a thread mill any deeper than three times diameter, particularly with a course pitch,” Mazzenga said. “Anything deeper, and there is a tremendous amount of radial pressure being applied, which causes deflection. The chances of being successful in one shot are greatly reduced. If you have to go deeper, you should take a pass at the top of the thread, maybe go half way down and take a pass, then drop down deeper and take another pass. And, with CNC, your threads will link up.”

However, some manufacturers question the need for deep threaded holes. “When you get to 2.5 diameters deep, you have reached maximum strength for the thread. There is no benefit to designing a deeper thread,” Ruff said. “There is no need to overengineer the parts and make them more costly to produce.”

"J.M. Sales’ GFM thread mill cuts a thread much larger than the tool itself.  Courtesy of J.M. Sales. "

Courtesy of J.M. Sales

J.M. Sales’ GFM thread mill cuts a thread much larger than the tool itself.

Know the Program

Because the thread mill is circular interpolated, the actual feed rate at the cutting edge will be different from what is programmed at the center of the tool. “A thread mill is always traveling in a circle, so the centerline of the tool is going to be traveling at a different speed than the OD of the tool,” Harvey Tool’s Francescone said. “So you need to compensate for that in your feed rate. In the case of an internal thread, you scale your linear feed rate down, and in the case of an external thread, scale it up.”

Many thread milling programs start by going perpendicular into the hole wall, which causes vibration in the tool and tool marks on the thread, according to KOMET’s Ruff. Once the tool starts vibrating, it will not stop for the duration of the operation. To eliminate these prolems, he recommends starting the process by gradually approaching the hole wall with a circular motion, then going to the full cutting depth. KOMET offers a program for this that can be downloaded from its Web site. Apple and Android apps are also available.

Thread Milling Advantages

There are a variety of reasons thread milling is used instead of other threadmaking operations, specifically tapping.

As previously stated, a thread mill can address a range of hole diameters. The diameter of a tap is fixed.

For large diameters, thread mills can be more economical. Large taps can be expensive. 

"Through-coolant thread mills help flush chips out of blind-holes. Harvey Tool offer standard through-coolant thread mills as small as 10-32 and as large as ½-13. Courtesy of Harvey Tool. "

Courtesy of Harvey Tool

Through-coolant thread mills help flush chips out of blind-holes. Harvey Tool offer standard through-coolant thread mills as small as 10-32 and as large as ½-13. 

Advent’s Hartford gave this example. “Say you need to cut a 6"-12 thread and then a 5"-10 thread. Using an inserted thread mill, all you need to do is change inserts from the 12 pitch to the 10 pitch at $30 per insert. A tap of this size would probably cost $2,500, and you would need to buy two.”

Thread mills can produce internal and external threads. Taps cannot be applied for external threads. 

If a thread mill breaks during operation, the pieces can be removed from the hole and a new tool makes the thread. Because a tap produces a great deal of contact along the cut, creating a lot of force, taps can break and become stuck in the hole, possibly causing scrap.

"The JEL Micro is for threading materials with a hardness from 45 to 60 HRC. Courtesy of KOMET.  "

Courtesy of KOMET

KOMET’s JEL Micro is for threading materials with a hardness from 45 to 60 HRC. The M1×1.5 thread mill has a diameter smaller than 0.75mm.

With only a change in programming, one thread mill can produce a left- or right-hand thread. A tap can only do what is ground into the tool, so the user needs one tool for left-hand threads and another for right-hand threads.

Thread mills can produce a full thread close to the bottom of a blind-hole. When the hole is blind, a tap can only reach so far because it has a tapered point. “Your thread form will be within half a pitch from the bottom of the hole,” Advent’s Hartford said. “That is as close as you can get.”

A thread mill imparts a finer surface finish than a tap.

Thread mills produce a thread in one or more passes. “With thread milling, you can probably do it in one pass if it is a softer material, like aluminum,” Harvey Tool’s Davis said. “But in a hard material, you could take more passes without breaking the tool. Tapping uses the whole thread form and it jumps to final size in one pass.” 

KOMET’s combination Thriller drill/thread mill performs three operations on an automotive part: drilling, thread milling and spotfacing. The cutting edges are PCD coated.

Courtesy of KOMET

KOMET’s combination Thriller drill/thread mill performs three operations on an automotive part: drilling, thread milling and spotfacing. The cutting edges are PCD coated.

Thread mills can start at the top of the hole and go to the bottom or vice versa. Taps must start at the top and go to the bottom. “Very often, people like starting at the bottom and working toward the top because, hopefully, gravity will pull the chips down and they won’t get recut,” Davis said.

And finally, thread mills, unlike taps, can combine various operations into a single tool. For instance, manufacturers offer tools that can drill a hole, chamfer it, and then mill the thread in one step. CTE


Advent Tool & Manufacturing Inc.
(800) 847-3234

Harvey Tool Co. LLC
(800) 645-5609

J.M. Sales - USA
(248) 879-5984

KOMET of America Inc.
(847) 923-8400

Related Glossary Terms

  • blind-hole


    Hole or cavity cut in a solid shape that does not connect with other holes or exit through the workpiece.

  • chatter


    Condition of vibration involving the machine, workpiece and cutting tool. Once this condition arises, it is often self-sustaining until the problem is corrected. Chatter can be identified when lines or grooves appear at regular intervals in the workpiece. These lines or grooves are caused by the teeth of the cutter as they vibrate in and out of the workpiece and their spacing depends on the frequency of vibration.

  • computer numerical control ( CNC)

    computer numerical control ( CNC)

    Microprocessor-based controller dedicated to a machine tool that permits the creation or modification of parts. Programmed numerical control activates the machine’s servos and spindle drives and controls the various machining operations. See DNC, direct numerical control; NC, numerical control.

  • feed


    Rate of change of position of the tool as a whole, relative to the workpiece while cutting.

  • flutes


    Grooves and spaces in the body of a tool that permit chip removal from, and cutting-fluid application to, the point of cut.

  • gang cutting ( milling)

    gang cutting ( milling)

    Machining with several cutters mounted on a single arbor, generally for simultaneous cutting.

  • hardness


    Hardness is a measure of the resistance of a material to surface indentation or abrasion. There is no absolute scale for hardness. In order to express hardness quantitatively, each type of test has its own scale, which defines hardness. Indentation hardness obtained through static methods is measured by Brinell, Rockwell, Vickers and Knoop tests. Hardness without indentation is measured by a dynamic method, known as the Scleroscope test.

  • interpolation


    Process of generating a sufficient number of positioning commands for the servomotors driving the machine tool so the path of the tool closely approximates the ideal path. See CNC, computer numerical control; NC, numerical control.

  • machining center

    machining center

    CNC machine tool capable of drilling, reaming, tapping, milling and boring. Normally comes with an automatic toolchanger. See automatic toolchanger.

  • milling


    Machining operation in which metal or other material is removed by applying power to a rotating cutter. In vertical milling, the cutting tool is mounted vertically on the spindle. In horizontal milling, the cutting tool is mounted horizontally, either directly on the spindle or on an arbor. Horizontal milling is further broken down into conventional milling, where the cutter rotates opposite the direction of feed, or “up” into the workpiece; and climb milling, where the cutter rotates in the direction of feed, or “down” into the workpiece. Milling operations include plane or surface milling, endmilling, facemilling, angle milling, form milling and profiling.

  • milling machine ( mill)

    milling machine ( mill)

    Runs endmills and arbor-mounted milling cutters. Features include a head with a spindle that drives the cutters; a column, knee and table that provide motion in the three Cartesian axes; and a base that supports the components and houses the cutting-fluid pump and reservoir. The work is mounted on the table and fed into the rotating cutter or endmill to accomplish the milling steps; vertical milling machines also feed endmills into the work by means of a spindle-mounted quill. Models range from small manual machines to big bed-type and duplex mills. All take one of three basic forms: vertical, horizontal or convertible horizontal/vertical. Vertical machines may be knee-type (the table is mounted on a knee that can be elevated) or bed-type (the table is securely supported and only moves horizontally). In general, horizontal machines are bigger and more powerful, while vertical machines are lighter but more versatile and easier to set up and operate.

  • outer diameter ( OD)

    outer diameter ( OD)

    Dimension that defines the exterior diameter of a cylindrical or round part. See ID, inner diameter.

  • parallel


    Strip or block of precision-ground stock used to elevate a workpiece, while keeping it parallel to the worktable, to prevent cutter/table contact.

  • pitch


    1. On a saw blade, the number of teeth per inch. 2. In threading, the number of threads per inch.

  • polycrystalline diamond ( PCD)

    polycrystalline diamond ( PCD)

    Cutting tool material consisting of natural or synthetic diamond crystals bonded together under high pressure at elevated temperatures. PCD is available as a tip brazed to a carbide insert carrier. Used for machining nonferrous alloys and nonmetallic materials at high cutting speeds.

  • rake


    Angle of inclination between the face of the cutting tool and the workpiece. If the face of the tool lies in a plane through the axis of the workpiece, the tool is said to have a neutral, or zero, rake. If the inclination of the tool face makes the cutting edge more acute than when the rake angle is zero, the rake is positive. If the inclination of the tool face makes the cutting edge less acute or more blunt than when the rake angle is zero, the rake is negative.

  • spotfacing


    Similar to counterboring except that, in spotfacing, material around the original hole is cut. Application example: the recessed area into which a washer fits. See counterboring; countersinking.

  • tap


    Cylindrical tool that cuts internal threads and has flutes to remove chips and carry tapping fluid to the point of cut. Normally used on a drill press or tapping machine but also may be operated manually. See tapping.

  • tapping


    Machining operation in which a tap, with teeth on its periphery, cuts internal threads in a predrilled hole having a smaller diameter than the tap diameter. Threads are formed by a combined rotary and axial-relative motion between tap and workpiece. See tap.

  • threading


    Process of both external (e.g., thread milling) and internal (e.g., tapping, thread milling) cutting, turning and rolling of threads into particular material. Standardized specifications are available to determine the desired results of the threading process. Numerous thread-series designations are written for specific applications. Threading often is performed on a lathe. Specifications such as thread height are critical in determining the strength of the threads. The material used is taken into consideration in determining the expected results of any particular application for that threaded piece. In external threading, a calculated depth is required as well as a particular angle to the cut. To perform internal threading, the exact diameter to bore the hole is critical before threading. The threads are distinguished from one another by the amount of tolerance and/or allowance that is specified. See turning.

  • tolerance


    Minimum and maximum amount a workpiece dimension is allowed to vary from a set standard and still be acceptable.

  • toolpath( cutter path)

    toolpath( cutter path)

    2-D or 3-D path generated by program code or a CAM system and followed by tool when machining a part.

  • web


    On a rotating tool, the portion of the tool body that joins the lands. Web is thicker at the shank end, relative to the point end, providing maximum torsional strength.


Susan Woods served as a Contributing Editor for Cutting Tool Engineering magazine.