{{ name }}
Article no. {{ combinedCodeWithHighlight }}
Article code:
EAN / GTIN:
Manufacturer number:
Cat. No.:
From longitudinal turning to facing – the basic turning methods at a glance
Turning is essentially the process of machining a rotating workpiece using a tool such that it ends up having the desired shape and size. Very different methods are used to achieve this depending on which properties you want to achieve. However, the first production step on the journey to the perfect turned part is almost always longitudinal turning and facing. Both turning methods enable us to produce the turned part in the desired dimensions as regards its diameter and length. Further machining steps, such as precision turning, groove turning, knurling, smooth rolling or thread turning, are not performed until after this has been done.
The initial workpiece, usually a cylindrical component, is first set to the desired dimensions by feeding in the tool. The first step is to feed in the tool to a flat end face, whereby the tool moves perpendicular to the axis of rotation (facing). Longitudinal turning is then used to change the diameter of the component. In this case, the tool moves parallel to the workpiece’s axis of rotation. In most cases the desired outer diameter is produced here (external turning), but when working on pipes or bore holes it may also be the internal diameter that is machined (internal turning). Afterwards, you then have the option of parting off the workpiece, or re-clamping it and facing it to the desired overall length on the end face that has not yet been machined.
The turning methods described here – longitudinal turning and facing – are the first and most important step in ensuring that the components work as required later on. Typical turned parts made of metal include bolts, axles, shafts and flanges, which take on important, safety-related functions in mechanical assemblies. This article provides brief step-by-step instructions to explain the main principles underpinning the three turning methods. We also provide some important practical tips and rules of thumb for lathes.
Longitudinal turning made easy – practical tips and tricks
As we mentioned above, longitudinal turning is about machining the workpiece diameter. These step-by-step instructions will put you on the road to success. But remember: no-one is born a master – and this applies equally to turning.
Take care when clamping the workpiece
The blanks for the turning work are typically supplied as “bar material” or pre-sawn blanks. When using bar material, the workpiece is clamped using a chuck or collet; finished components can then be parted off and the bar moved up. It is essential to ensure that the bar is always properly secured and does not protrude too far from the machine. When machining pre-sawn blanks, each workpiece is individually clamped in a three- or four-jaw chuck, meaning it generally does not protrude as far from the machine as bar material.
1. Prepare the workpiece
Securely clamp the workpiece in the lathe and check its concentricity. This is important to ensure the tool removes material evenly from all sides. Tip: if necessary, use a revolving lathe centre to provide additional support for longer workpieces.
2. Choose and attach the correct tool
External turning requires a clamping toolholder, whereas internal turning uses a special boring bar. There is a huge selection of tools to choose from – when making your selection, focus primarily on what the turning work is intended to achieve. We first need to distinguish between finishing and roughing here.
What is the difference between finishing and roughing?
‘Finishing’ and ‘roughing’ differ in terms of what the turning work is intended to achieve:
- Roughing focuses on removing a large amount of material in a short space of time. It combines a high infeed with a high feed rate and low cutting speed. The reason for this is the quadratic relationship between heat build-up and cutting speed: doubling the cutting speed causes a fourfold increase in heat build-up. As a result, by combining a high feed rate with a low cutting speed, roughing maximises the material removal rate while limiting heat build-up. Roughing works best with a “negative” indexable insert. The large wedge angle makes the cutting edge particularly sturdy, allowing for high infeeds and feed rates. . The negative indexable insert can be used on both sides, reducing the costs per cutting edge.
- Finishing focuses on achieving the highest possible dimensional accuracy and surface quality. It involves a low infeed with a small feed rate and high
Make sure that the tool is made of the right material. Carbide tools are suitable for machining almost all metals and can be identified by the letter “C” on the data sheet for the insert. If you are working on particularly hard materials, we recommend tools with special coatings or ones made of very hard cutting materials such as ceramic or CBN. Choose an appropriate insert for your project (cutting depth, feed rate, rotational speed). Attach the insert to a suitable clamping toolholder using a Torx screwdriver and secure this to the toolholder on the lathe.
Digression: the main cutting materials at a glance
- Carbide (C) is the most-used cutting material and can be used almost universally. It is generally made of tungsten carbide and cobalt as the binder and can be used for steel and steel alloys, cast iron, non-ferrous metals and stainless steel.
- Cermets combine ceramic and metal (usually titanium carbide and titanium nitride). Thanks to this combination, they are particularly hard and wear-resistant. This material is suitable for finishing work on low-alloy steels with high feed rates and rotational speeds.
- High-speed steel (HSS) is a relatively tough cutting material and is suitable for applications requiring tensile strength and resistance to impact loads, for example unalloyed and low-alloy steels as well as cast iron and aluminium alloys.
- Ceramic cutting materials are often made of aluminium oxide or silicon nitride and are characterised by extreme hardness and high-temperature hardness. They are suitable for materials such as high-strength steels and superalloys.
- Diamond (MCD) and polycrystalline diamond (PCD) are extremely hard and abrasion-resistant. They are ideal for non-ferrous metals such as aluminium or copper and are used when the surface quality is subject to very high requirements.
- Boron nitride (CBN) is particularly heat-resistant and abrasion-resistant, making it suitable for machining hardened steels, cast iron and high-strength alloys at high temperatures.
3. External turning: step-by-step procedure
During external turning, you machine the outer face of the workpiece. Proceed as follows: Start the machine. The workpiece begins to rotate on its own axis. Adjust the rotational speed to suit the material and diameter of the workpiece. Please note that the larger the workpiece diameter, the lower the rotational speed. A formula for calculating the rotational speed is provided below.
Rotational speed for external turning: rule of thumb
- A common formula for calculating the rotational speed is: n = (1000 * vc) / (pi * d)
- n = rotational speed (in rpm)
- vc = cutting speed (in m/min)
- d = workpiece diameter (in mm)
The cutting speed is primarily determined by the material, but also by other factors such as the workpiece geometry, the cutting material being used and the use of coolant. For a workpiece with a diameter of 50 mm, the rotational speed for steel would be approx. 955 rpm, but for aluminium it would be 1,910 rpm.
On machines with a constant rotational speed but not a constant cutting speed, make sure to use the average diameter for the calculation. If the starting diameter is 50 mm and the final diameter is 30 mm, the average diameter would be 40 mm and this is what should be used to calculate the rotational speed.
- Position the tool: move the tool with the insert near the workpiece. The tool should be positioned level with the centre of the workpiece to ensure optimum machining.
- Determine the cutting depth and feed rate: determine the cutting depth and feed rate based on the material and the surface properties you would like to achieve. Rule of thumb: for normal steel machining tasks, the cutting depth is typically between 0.5 and 3 mm and the feed rate is between 0.1 and 0.3 mm/rev. The minimum value for the infeed is the corner radius of the indexable insert.
- Machine the workpiece: guide the tool longitudinally along the workpiece. Work in several passes if you need to remove a lot of material. Whereas CNC machining enables more material to be removed in each pass thanks to its high precision and repetition accuracy, conventional turning often requires several passes with the tool, whereby the user can flexibly adjust the infeed and feed rate depending on the interim results obtained.
4. Internal turning: special requirements
Internal turning differs from external turning in that the inner face of the workpiece is machined. The steps are similar to the ones for external turning, but there are a few special aspects to consider:
- Choice of tool: use a boring bar designed specifically for internal turning. They generally have better access, e.g. an exceptionally slim shank to fit in the bore hole. The holder is usually also smaller. Make sure that the shank is sturdy enough to minimise vibrations.
- Cutting depth and feed rate: given the limited space available inside the workpiece, you should work with smaller cutting depths and a lower feed rate to ensure the tool does not jam.
Rule of thumb: for internal turning, the cutting depth should be a maximum of 2 mm.
Special factors for facing
Unlike longitudinal turning, facing machines the end face of the turned part. That means that the tool moves perpendicular to the workpiece’s axis of rotation. Tip: if the component is also being turned internally, facing should always be performed after the internal turning. Otherwise there is a risk that the facing surface becomes damaged by the drilling. Performing the steps this way round also extends the tool life as the cutting speed reduces as you move towards the centre.
The process for preparing the workpiece is the same for facing as for longitudinal turning. However, when choosing the tool you must ensure that it is suitable for facing and the application in question.
It is always essential to understand how the corner radius and setting angle affect things. A large corner radius makes the insert sturdier, which can extend the tool life when performing tasks such as rough machining. A small corner radius is more suitable for precision machining but can reduce the tool life. When performing facing, please note that the cutting speed reduces as you move towards the centre of the workpiece. As a result, we recommend choosing a tougher grade of cutting material.
With respect to the setting angle, consider how it affects the distribution of forces: by reducing the setting angle you can direct the forces more in the axial direction (in the direction of the chuck) and thus stabilise the component.
Another handy tip is that, during facing, workpieces tend to form burrs on the outer edge. Make sure to deburr the workpiece after it has been machined.