{{ name }}
Article no. {{ combinedCodeWithHighlight }}
Article code:
EAN / GTIN:
Manufacturer number:
Cat. No.:
Thread turning – precise threads to optimally hold components in place
Without threads, the world around us would fall apart. Whether it’s powertrains in cars, the heating systems in our homes, brakes on bicycles, or ball screw drives in machine tools: threads can be found everywhere and keep screwed components securely in place.
But how are threads actually made? Different methods are used in the metalworking industry: alongside thread tapping, there are other tried-and-tested methods such as thread turning, thread rolling and thread milling. This article takes a detailed look at thread turning. With this method, a thread is produced by a cutting tool which moves up to a rotating workpiece and removes material from it in a spiral.
The approach taken by thread turning is similar to other production methods on a lathe: a cutting tool with a defined shape is moved up to the rotating workpiece and produces the characteristic spiral shape. It is important here that all parameters are precisely coordinated with one another. H2 Thread turning
Thread turning in practice – from selecting the right tool to reworking
Thread turning is certainly one of the more challenging production methods that can be performed on a lathe. This is because the quality of the thread contour depends decisively on choosing the right tool and setting the right turning parameters, such as inclination angle, cutting depth and feed rate. Even minor deviations can mean the thread no longer conforms to standards and jams later on when in use or does not hold the components as required. Additionally, thread turning is subject to very high requirements as it is usually the last work step when machining a part.
The following step-by-step instructions for thread turning explain how to produce the perfect thread on a lathe:
Step 1: Choose, clamp and align the tool
When it comes to thread turning, the tool comprises a clamping toolholder, a shim and a thread turning insert or indexable insert. The clamping toolholder secures the tool in the holder of the lathe. When choosing the clamping toolholder, ensure that it is suitable for the size of shank and insert. Also consider that there are turning toolholders for both left-hand and right-hand threads.
Towards the chuck:
- Right-hand thread with right-hand threading insert and right-hand toolholder
- Left-hand thread with left-hand threading insert and left-hand toolholder
Towards the lathe centre:
- Right-hand thread with left-hand threading insert and left-hand toolholder
- Left-hand thread with right-hand threading insert and right-hand toolholder
The choice of indexable insert depends on what the thread should look like later on. The profile of the insert matches the shape of the thread. For example, an indexable insert with an angle of 60 degrees is suitable for the classic metric 60-degree thread.
Moreover, there are different profile types to consider for the indexable inserts: full profile, partial profile and semi-profile. The difference between them is explained in the box below. After choosing the correct tool, the next step is to precisely align the tool at a right angle to the workpiece to ensure the thread is as symmetrical as possible.
Take care when clamping the workpiece
Full, partial or semi-profile?
When choosing which type of profile to use, you can use the following distinctions as a guide:
- Turning inserts with a full profile produce a standards-compliant thread that complies exactly with the required internal and external diameter. However, this type of insert does not allow for any variations in the profile or pitch – a separate profile insert is required for each type of thread and each size.
- In practice, turning inserts with a partial profile are a bit more flexible. This profile can be used to produce different pitches. When producing an external thread, for example, it is important that the external diameter is not also machined, which would mean the thread does not conform to standards.
- Turning inserts with a semi-profile are suitable for special cases, such as for very large pitches and trapezoidal-shaped thread contours.
Step 2: Choose the infeed method, attach the shim and set the parameters
As previously mentioned, thread turning is definitely one of the more challenging production methods due to the many different parameters involved, which all affect the result. As a result, by carefully and properly setting the tool, workpiece and process parameters, you’re already halfway to the finish line.
1. Type of infeed
Firstly, the type of infeed is important. It is important to understand that thread turning requires different passes with the tool in order to achieve the desired result. The infeed describes where (on the X-axis) the machining operation starts in each pass. In the most straightforward case – the radial infeed – the infeed is performed without an offset, i.e. always in the same place. This type of infeed is primarily suited to small pitches (<1.0 mm) and is usually the best choice for manual thread turning applications. Alternatively, there is also the flank infeed, which is mainly used on CNC lathes and for larger pitches.
Radial infeed
The radial infeed is recommended for:
- pitches smaller than 1.0 mm or with fewer than 24 TPI
- hard machining, since it generates the least rubbing at the cutter
- work-hardened materials (particularly suitable for austenitic stainless steels)
- short-chipping materials (best type of infeed)
Flank infeed
The method is recommended for:
- pitches greater than 1.0 mm or with more than 24 TPI
- trapezoidal threads
- as a remedy for the tendency to vibrate, since the main chip is generated in the feed direction
- good chip flow control
Since this infeed is parallel to the thread flank, this commonly used machining technique can lead to problems such as increased rubbing at the flank not facing the feed (where the insert is not cutting). A further disadvantage is the difficulty of individual block programming, meaning that a thread cutting cycle is a precondition for this machining technique.
Modified flank infeed:
This type of infeed differs from the flank infeed described above in that the infeed is not performed parallel to the flank. The infeed angle is reduced by about 1-5° compared to the flank angle of the thread. The consequence of this is that this infeed technique has all the advantages of the flank infeed described above, without the disadvantage of increased rubbing. This modification means there is always a certain oversize on the flank not facing the infeed. As a result, the profile insert now cuts cleanly, without rubbing.
Alternate infeeds
The machining is shared by each of the two flanks. Using the alternate infeed technique, the start-point for the pass is offset alternately in the plus and minus direction in the Z-axis. This technique permits long tool lives, thanks to the even distribution of wear along the cutting edge. Here too, however, there is the disadvantage of the difficulty of individual block programming, meaning that a thread cutting cycle is a precondition for this machining technique.
The method is recommended for:- very large pitches
- very sharp thread profiles
- long-chipping materials
2. Number of passes
To turn a perfect thread, you need to make multiple passes with the tool. The exact number depends on the material properties as well as the thread pitch and a few other parameters. Corresponding tables show the number of passes depending on the relevant parameters. Typically there are five passes for small pitches and up to 20 passes for very large pitches.
Thread pitch
[mm]0.50 0.75 1.00 1.25 1.50 1.75 2.00 2.50 3.00 3.50 4.00 4.50 5.00 TPI 48 32 24 20 16 14 12 10 8 7 6 5.5 5 Passes Standard geometry 4-6 4-7 4-8 5-9 6-10 7-12 7-12 8-14 9-16 10-18 11-18 11-19 12-20 Sintered chip breaker CB 3-4 3-4 3-5 4-6 5-6 6-8 8-10 9-12 10-14 3. Choose the shim
To ensure that the finished thread has exactly the right pitch, a shim is placed underneath the indexable insert. Its inclination angle ensures the correct thread pitch. To determine the inclination angle required for the shim, you can use the rule of thumb below or consult a graphic. Tip: most tools are supplied with standard shims for an inclination angle of 1.5 degrees and can therefore optimally cover most applications.
The use of an incorrect shim and the resulting incorrect inclination angle is the most frequent cause of problems in thread turning. The correct inclination angle generates the necessary flank clearance angle for the profile insert. If these angles are unequal or too small, this leads to increased rubbing and frictional heat, which in turn increases the wear and in extreme cases leads to vibration.
Formula for the inclination angle of the shim:
a = (20 P) / D
where a = inclination angle [°], P = thread pitch, D = diameter [mm]
4. Set the rotational speed and feed rate
Now it’s time to set the machine parameters. Select the spindle’s rotational speed depending on the material and thread pitch. Tip: a slightly lower rotational speed will protect the cutting edges of the indexable insert. The selected feed rate must also match the desired thread pitch (mm per revolution).
Step 3: The first cut
Once you have configured all the settings, carefully move the tool to the starting point of the thread and then set the depth of the first cut. The material you are working on plays a decisive role here. Whereas the cutting depth for stainless steel should be relatively small and amounts to 0.2 to 0.4 mm (depending on the pitch), you are allowed to cut much deeper in aluminium and can easily select 0.5 to 0.8 mm here. If you now start the lathe, you will feed in the tool to the desired depth of the first cut.Step 4: Feed in the tool again
The thread profile now becomes a little more visible with every infeed operation. After each one, correct the infeed depth so that a small amount of material is always removed. Carry out as many passes as are required to achieve the final dimension. Tip: during the last cut, only use a low infeed (finishing cut) to achieve a smooth surface.Step 5: Reworking and quality check
Once you have achieved the final dimension, you can chamfer the edge of the thread slightly. This not only removes dangerous sharp edges, but also makes it easier to screw in the thread later on. As the final step, you can use a thread gauge to check that the pitch and profile meet the specifications. Then check the thread for contamination and remove burrs if necessary. You’ll then have your finished thread.