Thread turning application tips
A common problem in thread turning is that chips coil around robots, chucks, tools and components. The chips can also get caught in conveyors, causing damage and loss of productive machining time. Successful chip control is the key for good component quality when thread turning. Follow our thread turning application tips for good chip control and long tool life.
OptiThreading™
Use the OptiThreading™ method for the best possible chip control. This method enables tool oscillation movements giving interrupted cuts on all passes except the last one. It provides the highest process control and component quality.
Modified flank infeed
For conventional thread turning applications, use modified flank infeed for the best chip control. The modified flank infeed allows threading to be treated more like a normal turning operation. It provides a controlled process, producing fewer chip problems, and hence, offering a predictable tool life and higher thread quality.
Opposite flank infeed
With opposite flank infeed, the insert can cut using the back flank (opposite flanking) meaning that the chip can be steered in the correct direction. This is important for internal thread turning operations, especially when machining in bottom holes. Use this method for continuous, trouble-free machining, without unplanned stoppages.
| Standard modified flank infeed | Feed direction | Opposite flank infeed |
 | ||
| Chip direction | Chip direction |
Cutting fluid and coolant
Cutting fluid and tools with precision coolant are recommended for optimized chip control and chip evacuation. Precision coolant has the following advantages when thread turning:
- Controlled temperature at the cutting edge
- Good chip evacuation
- Improved chip control
When external coolant is applied, it is often just a small amount of coolant that gets into the thread and therefore very little of the coolant will have effect.
With internal coolant, the coolant jet accesses the cutting edge even in deep threads. The coolant effectively decreases the temperature, which:
- Allows for higher cutting data or a tougher grade to be used
- Improves chip control and surface finish
A lower temperature can decrease insert wear from e.g. flank wear and plastic deformation, and thereby extend tool life. Too low temperature will however shorten tool life, since decreasing the temperature too much in sticky materials, e.g. stainless steel, will lead to built-up edge (BUE).
Diameter check
Make sure the workpiece diameter is according to specifications before thread turning.
- With a too large diameter in case of external threading or two small in case of internal threading, the first cut will be very large and can cause insert breakage.
- With a too small diameter in case of external threading or too large in case of internal threading, a wrong thread diameter may be generated.
A: Too large turned diameter for external thread case
B: Correct external thread diameter
C: First pass generated by the threading cycle
Tool life
A careful observation of the insert after the threading operation will allow you to achieve optimum results regarding tool life, cutting speed and thread quality.
The two main machining parameters, that each has an effect on tool life, are infeed and speed. Increasing either of these parameters will decrease cutting time per component, but also increase the temperature. A too high temperature will decrease tool life.
To find optimal tool life, it is more beneficial to first optimize the infeed/chip thickness. When increasing the infeed/chip thickness, the temperature increase is less than when increasing the cutting speed. On the other hand, a too big chip thickness can overload the insert.
Use coolant to reduce the temperature. Precision under coolant has the biggest effect.
Impact on temperature when increasing cutting speed and infeed
| Infeed, ap |
|
|
| Cutting speed,vc |
|
|
Chip thickness
When machining work-hardening materials, avoid small depth of cuts and hence cutting in the work-hardened skin.
If the radial cut is 0.2 mm (0.008 inch), the chip thickness on the flanks will be:
- 0.05 mm (0.002 inch) with a 30° profile
- 0.1 mm (0.004 inch) with a 60° profile
Insert nose radius and tool life
The nose radius is the smallest point on the insert and the most liable to break under the extreme pressure of a thread turning operation.
Nose radii differ considerably for different insert types and consideration should be made to the cutting speed and number of passes in order to optimize performance and machining security.
NPT and NPTF thread profile inserts have the smallest nose radii within the standard range. For optimized performance, increase the number of passes and reduce cutting speed.
The internal insert has a significantly smaller nose radius than the external insert.
Pre-machining with a turning tool
Both productivity and tool life can be improved by pre-machining the thread using a turning tool with a 55° or 60° insert before the finishing pass is made with a threading tool.
When machining threads with small-radius roots and crests, similar pre-machining can also be applied by rough threading using an insert with the same angle, but larger nose radius. Allowance is then left for the remaining finishing passes to be machined with the thread turning insert.
Deburring
Deburring start of thread
If burrs appears, they tend to form at the start of the thread before the insert creates the full profile. These burrs can cause problems and should be removed, especially in the hydraulics and food processing industry where tolerance and quality demands are high.
Burrs are most common to appear in difficult stainless steels and duplex materials.
Thread deburring is achieved with standard turning tools. It is important to consider the correct positioning of the deburring insert, in relation to the thread, pitch and thread cycle.
How to deburr a thread
- Use a standard thread cycle with the recommended infeed data. The tool should exit the thread at a 45° angle
- Use the same thread program, with the same cutting speed and a parting and grooving insert at half the number of passes. Program the deburring length before the 45° exit to 1 x pitch, and measure the zero-point according to the setting instructions below
Setting instructions
- Set the zero point of the threading insert
- Measure the zero point on the parting and grooving insert
- Offset the parting and grooving insert with distance
Deburring of thread diameter
When turning a thread with a V-profile insert, a burr is often created on the thread crest. For a high quality thread, this burr needs to be removed.
Multi-start thread
Threads with two or more parallel thread grooves require two or more starts. The lead of this type of thread will then be twice that of a single-start screw.
The lead increases relative to the pitch by a multiple equal to the number of starts:
- Single-start thread - lead and pitch are equal
- Double-start thread - lead is twice the pitch
- Triple-start thread - lead is three times the pitch etc.
To produce a multi-start thread, make a single thread groove with a number of passes, followed by the second thread groove with a number of passes, then the third thread groove with a number of passes.
It is important to select the right shim. Use the lead value to calculate the correct inclination angle (helix angle), and select shim correspondingly. See section: How to choose thread turning insert and shim.
Adjustment of external tool holder
With the pitch twice as big, three times as big and so on, there is a drastic change in the lead angle which in extreme cases is not covered by the range of shims. For these extreme cases, the external tool holder can be milled/grinded in the direction of the lead angle.
- Do not grind on the shims. This will affect the stability of the complete system
- Calculate the lead angle φ (helix angle) and order a special holder
- If a large pitch is applied on a small diameter, the lead angle will be large
Thread turning
Thread turning is a demanding operation, where good chip control, consistent tool... chevron_right
How to achieve good component quality in turning
To achieve quality turned components, chip control is one of the most important factors... chevron_right
How to choose infeed method
OptiThreading What is OptiThreading? OptiThreading is a method with tool oscillation... chevron_right
How to choose thread turning insert and shim
When choosing the most suitable thread turning insert for your application you need... chevron_right
