Courtesy of JBO-USA
A GFM thread mill from JBO-USA threads a large-diameter component.
With the right tools, thread milling large bore diameters doesn’t have to be daunting.
When a hole requires threads, part manufacturers basically can perform conventional tapping, cold-form tapping or thread milling. When it’s a large hole, meaning 1 " to 1½ " in diameter and larger or a taper pipe, thread milling is preferred. Partly, that’s because the total cost for applying taps for larger threadmaking applications can be higher than thread milling. For example, larger taps can cost $150 or more, according to Joe Mazzenga, owner of JBO-USA, Troy, Mich. He added that although a thread mill costs more initially—$250 to $350 apiece—it’s able to achieve higher productivity, making the thread mill more economical.
He added that a multiple-flute thread mill that creates all the threads in one pass is the quickest method for 1½ "-dia. and larger holes. “A solid-carbide or a multiple-insert thread mill would be your most economical way,” Mazzenga said.
In addition, tap costs can increase if a special tap is needed. “You might have larger diameters that don’t fall within the standard tap specification,” said Jeff Major, director of sales and marketing for Vargus USA, Janesville, Wis.
In addition to cost, there are several other advantages of thread milling large bore diameters compared to tapping them. This article examines those benefits and also explores coolant application, selection of the proper thread mill and toolholder for the job, issues related to a hole’s depth-to-diameter ratio and software to assist the thread milling process.
This video from Allied Machine & Engineering Corp. offers a brief threadmilling demonstration courtesy of Allied Machine & Engineering Corp.
Tapping vs. Thread Milling
Tapping is a common way to produce an internal thread, but that doesn’t necessarily make it the best method. “Taps become less of an advantage even in small diameters,” said Duane Drape, national sales manager for HORN USA Inc., Franklin, Tenn.
Because a thread mill cuts a thread using helical interpolation on a CNC machine with three simultaneous axes, the tool is smaller than the diameter of the hole being threaded. Therefore, if a thread mill does happen to break when threading, it doesn’t get stuck in the part and can be easily removed. “It definitely reduces rework costs,” said Rob Brown, product manager for Allied Machine & Engineering Corp., Dover, Ohio. “With a broken tap, you would have to burn the tap out and, a lot of the time, you have a significant amount of rework or you scrap the part.”
Not engaging all sides of a hole like a tap allows freer machining when thread milling. This reduces machine tool horsepower requirements while boosting productivity.
“It’s a freer-cutting tool, so you can run at a higher surface footage, resulting in shorter cycle times,” Major said.
Another thread milling advantage is that a standard tool can produce a nonstandard pitch diameter before operations like heat treating or plating to achieve the required thread specifications. This is performed by knowing how the workpiece material is going to respond when treated, such as shrinking or expanding a specific amount, and compensating for that movement when cutting the threads, Brown explained. “With a tap, it would require a special with a nonstandard pitch diameter,” he said.
As a result of its advantages when the application is appropriate, thread milling has become more prevalent. “People prefer thread milling because of the reduction in cycle times and increase in tool life. It also provides a cleaner, stronger thread than what you would get with tapping,” Major said.
Those advantages are only enhanced when thread milling large holes. In those applications, for example, there’s more room for chip evacuation and for flood coolant to effectively access the tool/workpiece interface, Drape noted, adding that through-coolant tools are more important for smaller applications. “Thread milling large parts is relatively easy and has been accepted for years now,” he said. “Versus tapping, you don’t have to convince people very much. That battle has been won.”
Courtesy of Vargus
An end user initially applied taps to manufacture an internal thread for a 59.6 "×11 "×65 " wind turbine body, but average tap life was 250 threads and the surface finish was poor. In addition, tools often broke inside the workpiece material. After switching to MiTM25 thread mills from Vargus, tool life reportedly increased to 1,500 threads per cutting edge with a fine surface finish, and machining time was reduced by 25 percent.
Flood coolant can be effective in most thread milling applications, according to Brown, because there’s only a single point of contact between the tool and workpiece and chips are not being trapped. Allied offers through-coolant indexable thread mills, but flood coolant is applied for solid tools, Brown noted.
In contrast, all of JBO’s standard thread mills are through-coolant and direct coolant out the front of the tool. For through-hole applications, the toolmaker plugs the front end and EDMs radial coolant holes. “It’s not a major shift to run a made-for-application tool,” Mazzenga said.
In addition, Vargus offers its MiTM (multiflute thread mill) and TMSD (thread mill for deep holes) tools for thread milling larger bore diameters with 1,000-psi, through-coolant capability, Major noted. He added that MiTM products have straight rather than helical flute geometry to thread more aggressively.
Minimum-quantity lubrication is less common when thread milling, but can be effective depending on the application, such as when threading aluminum with a solid-carbide tool. In addition to the application, Drape noted that use of MQL depends on geographic location. “In Europe, they are amazed we get to use coolant everywhere,” he said.
Courtesy of JBO-USA
A JBO-USA thread mill is applied for producing a large taper pipe thread.
The vast majority of large bores are thread milled with indexable- or replaceable-insert tools because, similar to other operations, the cost of a large, solid-carbide tool becomes prohibitive. Brown noted that the largest standard, solid thread mill Allied Machine offers is a 1 "-8 tool.
The choice often depends on the application. “If the customer wants flexibility and the ability to use one tool for a number of pitches, then I’d say go with a replaceable-blade tool,” said JBO’s Mazzenga. “If it’s a dedicated production operation, then it’s more than likely a solid-carbide tool is going to win out.”
For indexable- or replaceable-insert tools at the smaller end of the large spectrum, Drape noted that the options are a single-flute, multiple-pitch insert or a multiple-flute, single-pitch insert.
Drape added that as the bore diameter to be thread milled increases, space permits applying multiple-insert indexable tools. Those can either have a single pitch or multiple pitches. A user can feed a single-pitch tool substantially faster than a multiple-pitch one because there’s less contact area between the tool and workpiece. However, a multiple-pitch tool has less distance to travel because it’s cutting multiple threads simultaneously, he explained. “If the total length of your component is 12 threads, you take one circular pass and that’s it,” Drape said. “Whereas a single-pitch tool has to travel around the component 12 times but it’s traveling faster.”
When applying a multiple-pitch tool, at some point the level of coarseness and depth of pitch have too much contact with the workpiece surface and the cutting pressure overwhelms the tool and machine, Drape noted.
The type of toolholder is also an important consideration when thread milling large holes. Similar to any milling operation, minimizing runout increases tool life and part quality, and Drape recommends milling chucks or hydraulic toolholders.
Mazzenga concurred that milling chucks, with their combination of vibration dampening and high gripping power, are ideal for thread milling, which generates a significant amount of side pressure on the tool. Shrink-fit toolholders are subject to “penciling” when thread milling, he added, where a high level of vibration maneuvers the tool out of the holder.
In one application “that should have been a slam dunk,” Mazzenga recalled that an engine manufacturer wanted to mill a 36mm thread in cast iron. The manufacturer used shrink-fit holders exclusively, but experienced problems when thread milling. Mazzenga first tried adjusting the speeds and feeds, but to no avail. “So we went to a milling chuck and it settled down immediately,” he said. “That’s happened on more than one occasion.”
Mazzenga also doesn’t recommend hydraulic holders because they don’t have the strength and grip to handle thread milling’s high radial forces.
Not So Deep
Large-diameter bores are not necessarily deep, according to Drape, but because of the fixturing often required to hold large and heavy workpieces, a thread mill could have a long reach. “If your depth-to-diameter ratio is too great,” he said, “you may need to take multiple passes.”
In some cases, coarse-pitch thread milling requires a roughing and a finishing pass, and deep-hole threads require taking a pass at one depth into the hole and then another pass at a deeper depth, Mazzenga noted.
“One of our newest tools has only three rows of threads,” Mazzenga said. “We then take multiple passes all the way down the thread. Separate roughing and finishing tools are not needed and cycle times can still be acceptable with multiple passes.”
Nonetheless, too much side pressure when thread milling can negatively impact thread quality. “To compensate for that, generally you take a lighter feed, requiring more passes,” said Allied Machine’s Brown. “Sometimes, a standard tap is quicker.”
For example, machining 6 diameters deep might be beyond a thread mill’s capability. “Based on the deflection problems you’d have with a thread mill that long, thread milling probably isn’t the right way to do it,” Brown said.
When thread milling is suitable, software is readily available to aid the process. Brown noted that Allied Machine’s Web site has a program where an end user enters application information, such as the type of thread mill, workpiece material and thread specifications. The program generates NC code that can be dropped into the part program as a subroutine.
And Allied Machine’s program is not unique among toolmakers. “We provide customers with CNC programs for their specific applications,” said JBO’s Mazzenga.
In addition, Vargus offers technical software for identifying the proper thread mill based on the required thread form and workpiece material. The software provides a selection of different tool options while calculating machining parameters and estimated cycle time and generating the CNC program to complete the thread, Major noted.
“Thread milling is quite easy,” Mazzenga added. “Just becoming comfortable with the idea of thread milling is the only obstacle to overcome.” CTE
About the Author: Alan Richter is editor of CTE, having joined the publication in 2000. Contact him at (847) 714-0175 or firstname.lastname@example.org.
Allied Machine & Engineering Corp.
HORN USA Inc.
Related Glossary Terms
Workholding device that affixes to a mill, lathe or drill-press spindle. It holds a tool or workpiece by one end, allowing it to be rotated. May also be fitted to the machine table to hold a workpiece. Two or more adjustable jaws actually hold the tool or part. May be actuated manually, pneumatically, hydraulically or electrically. See collet.
- 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.
Fluid that reduces temperature buildup at the tool/workpiece interface during machining. Normally takes the form of a liquid such as soluble or chemical mixtures (semisynthetic, synthetic) but can be pressurized air or other gas. Because of water’s ability to absorb great quantities of heat, it is widely used as a coolant and vehicle for various cutting compounds, with the water-to-compound ratio varying with the machining task. See cutting fluid; semisynthetic cutting fluid; soluble-oil cutting fluid; synthetic cutting fluid.
- depth-to-diameter ratio
Ratio of the depth of a hole compared to the diameter of the tool used to make the hole.
Rate of change of position of the tool as a whole, relative to the workpiece while cutting.
- gang cutting ( milling)
gang cutting ( milling)
Machining with several cutters mounted on a single arbor, generally for simultaneous cutting.
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 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.
- minimum-quantity lubrication
Use of cutting fluids of only a minute amount—typically at a flow rate of 50 to 500 ml/hr.—which is about three to four orders of magnitude lower than the amount commonly used in flood cooling. The concept addresses the issues of environmental intrusiveness and occupational hazards associated with the airborne cutting fluid particles on factory shop floors. The minimization of cutting fluid also saves lubricant costs and the cleaning cycle time for workpieces, tooling and machines. Sometimes referred to as “near-dry lubrication” or “microlubrication.”
- numerical control ( NC)
numerical control ( NC)
Any controlled equipment that allows an operator to program its movement by entering a series of coded numbers and symbols. See CNC, computer numerical control; DNC, direct numerical control.
1. On a saw blade, the number of teeth per inch. 2. In threading, the number of threads per inch.
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.
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.
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.
Hole or cavity cut in a solid shape that connects with other holes or extends all the way through the workpiece.
Secures a cutting tool during a machining operation. Basic types include block, cartridge, chuck, collet, fixed, modular, quick-change and rotating.
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.