(with acknowledgment to Mike Kanagowski, General Manager, VNE Corp, Wi, a sister company of Vargus who contributed some of the material)
Introduction
If we are honest with ourselves, manufacturing engineers looking for increased productivity, spend a lot of time looking for optimizing tool set ups, choosing correct cutting tool grades for a given workpiece and finding the maximum feed and speed conditions in turning and milling applications. They do not necessarily spend the same of time in optimizing threading operations since there is still an aura of "black box" attitudes concerning this operation.
Threading technology today has advanced in parallel with turning and milling improvements as far as tool grades and coatings, however advance in the design of inserts for threading chip control and the rapid strides in thread milling technology, give the manufacturing engineers a much wider choice for optimizing productivity.
Thread Turning
There are over 40 types of internationally accepted thread standards, some rarely used others much more popular. In addition, many countries have established variations on the international standards for their specific manufacturing requirements.
Primarily the threads are used in four categories:-
Fasting: nuts and bolts
Containing: lids of jars, gas caps, etc
Connecting: fittings and pipe couplings
Actuating: lead screws to transfer power and motion.
The ISO and UN standards are widely used in all industries, the other popular standards have more specific applications: -
BSW Gas and water fittings
NPT- Pipe fittings
BSPT- Gas and water fittings
ACME- Moving parts
Metric buttress- Moving parts in machine tool construction
Trapeze- Moving parts
Round - Tube fittings for food and chemical industries
UNJ & MJ- Aircraft industries
API- Oil industry
A little over half of the thread forms are based on what we will call the 60º Vee geometry and only differ in such factors as the size of the tolerances and root and crest radii.
Threading versus Turning
Threading operations are much more demanding than straight forward turning operations. Cutting forces are in general higher in threading and the cutting nose radius of the insert smaller and thus weaker.
Comparing the feed rate for turning and threading, we see that in threading, the feed rate must correspond exactly to the pitch of the thread. In the case of an 8 TPI thread, the tool must travel at a feed rate of 0.125 inch/revolution. The nose radius of the threading insert is typically 0.015 ". In the case of turning, the normal feed rate is 0.012 inch/ revolution with a standard radius of 0.032 ". From this example we see that threading feed rates are typically 10 times greater than turning. Correspondingly, the cutting forces at the tip of the threading insert can be anywhere from 100 to 1000 times greater than those for straight turning operations. Thus the nose radius of a threading insert plays a vital role in threading and its dimension is strictly limited by the allowable radius at the root of the thread form as defined in the relevant standard. Unlike turning where the material can be sheared, if, in the case of threading, material is "pushed" then thread distortion will be occur.
Further, since the thread is formed by carrying out a number of passes over the length of the thread, the leadscrew of the cross slide is working excessively hard, stopping and starting, moving forwards and backwards and this factor alone results in a limitation in optimization potential.
Partial Profile versus Full Profile Inserts
Partial profile inserts, sometimes referred to as "non topping" inserts cut the thread groove without topping or cresting the thread. These inserts allow production of a wide range of threads, however the nose radius of the insert ( the most vulnerable part of the insert) must be small enough to produce the smallest pitch. The depth of thread is also affected by the small nose radius. For example for a 8 TPI thread, a partial profile insert requires a thread depth of 0.108" while the same thread with a full profile insert will be no deeper than the specified 0.81". Thus a stronger thread is produced with a full profile insert and further, up to four less passes in producing the thread.
Multi Tooth Inserts
Multi tooth inserts are designed with a number of teeth so that each one cuts deeper into the thread groove than the previous tooth. Thus the number of passes required to produce a thread can be reduced by up to 80%. The tool life of these inserts is considerably longer than single point inserts since the final tooth is only machining a half or a third of the metal removal of a given thread.
These inserts obviously can give a big push to improve productivity, however, due to the higher cutting forces they are not recommended for thin walled parts as chatter can result. The design of the workpiece should have a sufficient amount of thread relief or run out to allow all the teeth to exit the cut.
Infeed Per Pass
The depth of cut or infeed per pass is critical in threading because each successive pass engages a larger portion of the cutting edge than the preceding pass. If a constant infeed per pass is defined, forces and metal removal rates increase dramatically on each pass.
Producing a 60º thread form using a constant 0.010" infeed per pass will result in the second pass removing three times the amount of metal as the first pass. For each succeeding pass the amount of metal removed grows exponentially. Thus the pressure on the nose radius increases accordingly. The depth of cut should reduced on each pass in order to achieve more realistic cutting forces.
Infeed Methods
a) Radial - not recommended for general use
Whilst, controversially, this method is probably the most common method of producing threads, it is the least recommended. Since the tool is fed radially (perpendicularly to the workpiece centerline) metal is removed from both sides of the thread flanks, giving a V shaped chip. This form of chip is difficult to break this chip flow can be a problem. Further, since both sides of the insert nose are subject to high heat and pressure, tool life will generally be shorter than other infeed methods.
b) Flank Infeed - generally not recommended
In this method of infeed, the chip formed is similar to that produced in conventional turning and is easier to form and guide away from the cutting edge, providing better heat dissipation. With this infeed however, the direction of infeed is parallel to one of the thread flanks (30º ) and the trailing edge of the insert does not cut only rubs along the flank causing burnishing of the thread resulting in poor surface finish and maybe,chatter.
c) Modified Flank Infeed - highly recommended
This method is similar to the flank infeed except that the infeed angle is somewhat less than the 30º. This gives the advantages of the flank infeed method while eliminating the problems of the training edge of the insert. A 29½º infeed angle will normally produce the best results but in practice an infeed angle of between 25º and 29½º are generally acceptable.
d) Alternating Flank Infeed - not recommended
This method utilizes both flanks of the insert to form the thread and gives longer tool life since both sides of the insert nose are used. In reality, this method can result in chip flow problems, which can affect surface finish and tool life. This method is usually used for very large pitches and such forms as ACME, TRAPEZE etc.
Clearance Angle Compensation
The ability to precisely tilt the insert in the direction of cut by changing the helix angle is probably one of the most powerful features of the laydown system.
This feature gives a higher quality thread because the insert will not rub against the flank of then thread form and also give a longer tool life since the cutting forces are evenly distributed over the full length of the cutting edge.
In the diagram above, the cutting edge of the insert on the left is parallel to the centerline of the workpiece. Note that the clearance angles under the leading edge and the trailing edge of the insert are not equal. In the case of many thread forms, particularly coarser pitches, this inequality can cause the flank to rub against the side of then insert.
With the laydown anvil system, (a helix angle chart appears in most catalogs allowing ease of choice of the correct shim to be used for the application under consideration) the proper anvil will tilt the cutting edge of the insert (in the direction of feed) in a plane perpendicular to the helix angle of the thread. The clearance angles beneath the insert's leading and trailing edges will be equivalent. This ensures that the insert will rub on the thread flanks and edge wear will develop uniformly.
Thread Tolerances
Most manufacturers specify the thread tolerance for which their inserts will be suitable and it is important for the manufacturing engineers to take note of this.
Although inserts can be produced which are suitable for other tolerance defined threads, it usually necessary to contact a manufacturer to have these tools manufactured by special order.
Miniaturization
The success of the laydown system has resulted in manufacturers looking for similar applications in smaller and smaller bore diameters.
The laydown system typically will allow threads to be formed in bores down to ½" diameter. For smaller diameters down to approximately 0.3" diameter, interchangeable inserts with 2 or 3 edges are available
Mini threading laydown inserts offer many advantages over traditional machining of small bores. The quality of the thread formed is usually higher, the insert design allows chips to flow out of the bore with little damage to the thread and being indexable the tooling investment for machining a considerably lower.
This tooling is usually available in a range of carbides and coatings giving the manufacturing engineer the flexibility to chose an optimum set of conditions.
The carbide used in these applications permit machining at lower surface speeds than is normally associated with threading. This is more the result of machine tool limitations than the capability of the tooling.
For bores even smaller than 0.3" the micro range of tooling offers a complete package of machining in addition to threading. This includes turning, copying, chamfering and both radial and axial grooving.
Those Special Needs
In spite of the large range of tooling available for seemingly unending applications, there is always that "special" problem for which standard tooling does not provide the answer.
In one of these cases, a manufacturer had a problem producing tens of thousands of brass fittings using a Schutte 6 spindle machine. There were two threads to be formed on the component and the previous method of manufacture produced each thread one at a time. Thus a more efficient method was required and the company turned to its tooling supplier.
The supplier came up with an innovative solution - using two thread milling inserts on a special holder enabling the machining of both threads at the same time. The inserts were used in the style of multi tooth thread turning inserts. The customer successfully threaded over 70,000 components without changing the inserts!! As well as saving inventory costs over the previous method, a considerable productivity saving was also achieved.
This is just one example of thousands of special applications that are solved year on year. If
Your application is not solved with standard tooling, don't hesitate to contact your tooling supplier, you will be surprised at his innovative solutions!!
Thread Milling
The principle of the screw was invented in the third century BC by Archimedes. Industrial production of screw threads began after 1850 utilizing lathe technology. Over a hundred years later in the late 20th century, threading production by milling was developed.
Without screws the Industrial Revolution would not have taken place. Without thread milling technology, efficient means of production would have been just a dream.
The advent of 3-axis CNC milling machines with helical interpolation opened the door to thread milling technology. Helical interpolation is the simultaneous movement of the tool in the chuck in the "X", "Y" and in the "Z" axis perpendicular the "X" and "Y" plane.
Thread milling is a system based on indexable multi tooth inserts. The cutter rotates on its own axis and at the same time moves along a helical path. The inserts are precision ground so that each tooth is within the specification of the thread form required and forms one pitch of the thread. At the end of a single revolution each tooth has completed the forming of one pitch which combine together to give the thread over the length of the insert.
Advantages
There are numerous practical advantages of this technique of forming threads, each giving cost savings and higher output levels.
- enables machining of large workpieces not mountable on a lathe
- non symmetrical parts easily machined
- all operations can be completed in a single clamping set up
- threading of large diameter threads require considerably less power than taps
- no upper limit to diameters, external or internal
- short chips for easy control
- blind holes do not require a thread relief groove
- a single toolholder can be used for both internal and external threads
- one insert can be used for both right hand and left hand threads
- major reduction in tool inventory costs as a small range of tooling covers a wide range of applications
- interchangeable inserts
- suitable for machining hard materials
- high quality surface finish
- the CNC program can be correct for diameter and length during production
-interrupted cuts machined without any special conditions
- one insert is suitable for a wide range of workpiece material
- short machining time due to high speeds and rapid feed rates
- low cutting forces allowing machining of components with thin walls
With such an outstanding list of advantages, it is quite clear why this technology is growing at such a rapid rate.
Infeed Methods
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
Radial Approach
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 circular feed !
1-2: radial entry
2-3: helical movement during one full orbit (360°)
3-4: radial exit
Coarse Pitch Threading
Coarse pitch threads are defined as a result of the combination of a small thread diameter and relatively large pitches. Since contrary to thread turning, the thread milling operation does not produce an exact copy of the profile of the insert. This fact can cause profile distortion particularly when machining internal threads.
The distortion can be caused as a result of one or more of the following parameters; thread diameter, tool diameter, pitch and profile angle. It is always necessary to refer to the manufacturers recommendations in this regard.
CNC Program Generator
In order to avoid programming errors, manufacturers provide software to make the job easier. Whilst one can learn the techniques, it is rather like the now defunct slide rule which was overtaken by the pocket calculators.
Summary.
The information in this article merely touches the surface of two of the more popular threading techniques. Coating technology, chip breaker designs, sintered inserts and sintered chip breakers all provide the opportunity for better production rates.
The development of threading tooling will continue in the foreseeable future
By: Stuart Palmer, Marketing Consultant
