About Thread Milling
Thread Milling is a method for producing a thread by a milling operation. The most common way to produce a thread is still by tapping and turning but today we see more and more milling and this is because CNC milling machines with three simultaneous axes are very popular. These can now be found in every small workshop.
To perform a Thread Milling operation, a helical interpolation movement is required. Helical interpolation is a CNC function producing tool movement along a helical path. This helical motion combines circular movement in one plane (x,y coordinate) with a simultaneous linear motion in a plane perpendicular to the first (z coordinate)
Vargus Indexable Thread Milling system
Vargus thread milling tools are based on indexable multitooth inserts. The cutter rotates around itself at high speed and at the same time moves along the helical path. All the teeth are machined simultaneously so every tooth creates one pitch. At the end of the operation all pitches are combined into one complete thread and that by one pass only. This result is achieved with Vardex high accuracy inserts and use of a CNC milling machine.
Advantages of thread milling:
• Enables machining of large work pieces which cannot be easily mounted on a lathe
• Non-rotatable and non-symmetrical parts easily machined
• Complete operation in one clamping
• Threading of large diameters requires less power than threading by taps
• No upper limits to bore diameter
• Chips are short
• Blind holes without a thread relief groove can be machined
• Thread relief groove unnecessary
• One holder used for both internal and external threads
• One tool used for both right hand and left hand thread
• Tooling inventory can be reduced to a minimum as small range of tooling covers a wide range of thread profiles
• Interchangeable inserts
• Suitable for machining of hard materials
• Threads have a high surface finish
• Allows for correction of tool diameter and length
• Interrupted cuts easily machined
• One tool for a wide range of materials
• A better thread quality in soft materials where taps normally tear the material
• Short machining time due to high cutting speed and rapid feed rates
• Small cutting forces allow machining of parts with thin walls
Climb and conventional thread milling
There are two methods for the milling operation - climb milling and conventional milling. For many years it was common practice to mill against the direction of the feed due to the absence of backlash eliminating devices and the use of high speed steel cutters. This method is called conventional milling. In conventional milling, friction and rubbing occur as the insert enters into the cut, resulting in chip welding and heat dissipation into the insert and workpiece.
Climb milling, the second method, is now generally recommended. The insert enters the work piece
material with some chip load and proceeds to produce a chip that thins as it progresses towards
the finish. This reduces the heat by dissipating it into the chip.
Based on the above, Vargus recommends using the climb operation which will give you:
• reduced load from the cutting corner
• better tool life
• better surface finish
How does the thread milling cutter enter and exit the workpiece.... Tangential arc approach, the best method.
With this method, the tool enters and exits the workpiece smoothly. No marks are left on the workpiece and there is no vibration, even with harder materials. Although it requires slightly more complex programming than the radial approach (see below), this is the method recommended for machining the highest quality threads.
1-2: rapid approach
2-3: tool entry along tangential arc, with simultaneous feed along z-axis
3-4: helical movement during one full orbit (360
4-5: tool exit along tangential arc, with continuing feed along z-axis
5-6: rapid return
This is the simplest method.
There are two characteristics worth noting about the radial approach:
• a small vertical mark may be left at the entry (and exit) point. This is of no significance
to the thread itself.
• when using this method with very hard materials, the tool may have a tendency to vibrate as it approaches the full cutting depth.
Note: Radial feed during entry to the full profile depth should only be 1/3 of the subsequent
1-2: radial entry
2-3: helical movement during one full orbit (360
3-4: radial exit
Thread Milling Methods
Coarse pitch threads
Coarse pitch threads are a combination of small thread dia and relatively large pitches. The thread milling operation is based on three-axes simultaneous movement so the profile shape on the
workpiece is not a copy of the insert profile. In other words the profile is generated and not copied which is contrary to the thread turning operation.
This fact causes a profile distortion, especially when machining coarse pitch internal threads.
The profile distortion depends on four main parameters:
• Thread dia.
• Tool cut. dia.
• Thread pitch
• Profile angle
For internal threads, as a general rule, when the ratio between cutting tool dia. (D2) and
the thread dia. (minor dia.) is below 70% the profile distortion is neglected.
Above this ratio, however, the standard inserts will not give the correct profile. We have developed tools which correct the profile distortion and by that give a solution for the coarse pitch threads.
The inserts are identified in the catalogue by the no. 028/... and the toolholders by the number 124/... In our new catalog, tables can be found which indicate exactly which tools
to use for every standard thread.
Fine pitch threads
Fine pitch threads are threads with small pitches. It is dificult to produce multitooth inserts for small pitches because of the small radius between the teeth. Vargus developed inserts where every second tooth was dropped to enlarge the radius between the teeth.
• All the fine pitch inserts are partial profile type (as a result of the enlarged radius).
• Two orbits are required to complete the thread because we dropped every second tooth.
How to find the correct toolholder?
In general, Vargus recommends using the largest possible toolholder with the shortest overhang and with max. possible cutting edges. The inserts selection will be determined according to the toolholder size and the thread type. For that, and in order to avoid profile distortion, we have three methods:
Largest tool table method (see the Cutwel catalogue)
These new and friendly tables located at the begining of our catalogue are your guide and indicate the correct tool to use for every standard thread - coarse pitch and non-coarse pitch threads.
The recommended toolholder is the largest (largest cutting dia.) for a given thread
application, smaller or equal dia. can also be used.
E.g.: For M25XI.5 (no need for bore dia. calculation) the largest offered tool is TMC 20-3
which means that every tool that has a smaller cutting dia. e.g. TMC 16-3 can also give a suitable solution.
TM Genius software
This perfect software developed by Vardex engineers gives you the right tools (all suitable tools)
for each application and also automatically the CNC program.
Click the link below to view the program and access it through the thread milling pages on our website.
To download a full PDF of this guide, click the link below
We accept the following payment methods:
For latest news and updates, please follow us:
© Cutwel, All Rights Reserved. Terms & Conditions
Cutwel Ltd is registered in England and Wales No. 3202912. VAT No. 297217178