There are no technical requirements for this chapter; however, just in case you have tools and inserts floating around the room, you may want to collect them in order to observe them as you read.

Turning, long story short, it is a very old machining technique discovered thousands of years ago. While understanding Egyptian pottery may sound interesting to some, it is definitely out of the scope of this book, so we are going to jump right into the action!

Turning is a mechanical process where a cylindrical part is put on fast rotation, and then approached by a cutting tool that progressively removes material from it. The machine that lets us shape our part with this technique is called a lathe.

If you ask a professional CNC user, they will tell you that a lathe is a rather complex machine that consists of many components such as the saddle, the tailstock, the headstock, and so on. Don’t worry about all these intimidating words—we will approach turning in the simplest way possible. In the following screenshot, we can find a lathe stripped up to the bones:

Figure 1.1: Lathe main actors

Ultimately, there are only four actors involved in turning:

1. Chuck: A fast-spinning clamping device; it holds the stock to be machined
2. Cutting tool: A special hard-metal blade that removes material from the stock
3. Machined stock: Our part before machining is completed
4. Chip: The removed particles and filament (waste material)

If you have ever approached a working lathe, I’m sure you noticed that the material shape about to be machined—the stock—spins very fast, while the cutting tool moves quite slowly, with a lot of chips being generated and projected all over the surrounding environment.

Even if the chip is valueless, it doesn’t mean that we can pretend it doesn’t exist; if we did, it would very easily render our part and our tool valueless. Controlling chip formation is very important (not only for turning) because it has the bad habit of becoming an entangled mess (a little bit like pasta) and damages everything it comes into contact with.

There are several types of lathes on the market; some are really big and some are very complex, but at the end of the day, all of them are pretty similar to one another.

Now that we understand the main components of the lathe, we can dive just a little bit into the theory behind such an incredible machine!

Cylindrical coordinate system

In order to understand coordinates, we need to remember that we live in a 3D world. In our world, in order to specify the location of an object with exact precision, we must provide a set of three numbers (coordinates) that measure the distance from a point in space—the origin—in a given direction.

In our daily lives, we often use Cartesian coordinates; here, we have a few examples:

• When working in an Excel file or when playing Battleship, in order to locate a cell, we need to know the row number and column number (2D Cartesian coordinates)
• If we want to give the dimensions of an object, we must provide the length, the width, and the height (3D Cartesian coordinates)

However, as mentioned, all the examples previously listed are Cartesian coordinates, where coordinates are expressed as a length along axes oriented at 90° from each other.

Orienting all the axes at 90° is generally the best approach for parts with a cubic shape, however, when it comes to lathes, a different coordinate system may be better. This is because all parts machined with a lathe have an axial symmetry, meaning that basically every part looks more or less like a cylinder. Therefore, we can use cylindrical coordinates instead.

With cylindrical coordinates, we do not express a point position with three distances; we express a position with an angle and two distances. We can see this in the following screenshot:

Figure 1.2: Cylindrical coordinates’ components

Let’s specify what the labels mean:

1. The red arrow is the axial direction (longitudinal), which is the rotation axis.
2. The yellow arrow is the rotation angle ().
3. The green arrow is the radial direction. Note that the arrow is not static; you can pretend it is a hand of a clock, where all the ticks on the dial would be a possible radial direction. There are infinite green arrows around the rotation axis, each rotated by an angle () from 0° to 360°!

With these three numbers, we already can specify with extreme precision every single point inside and outside our stock. However, it will be useful to introduce another direction.

4. The blue arrow is the tangential direction. It may not be so simple to understand the tangential direction, but we can just say that it is a vector that starts from the tip of a radial vector with a direction perpendicular both to the radial vector and to the axial vector.

Now that we know a bit more about cylindrical coordinates, we can start using this knowledge to differentiate between turning operations!

Different types of turning operations

To discuss the different types of turning operations, we will look at the two main families of machining:

• External machining
• Internal machining

Let’s take a look at these in more detail.

External machining

These operations are the most common operations performed while turning. In this type of process, the material is removed from “outside-in” along the radial direction. This basically means that the average radial coordinate of our tool will keep reducing during the operation.

In the following screenshot, we have a typical external machining operation depicted:

Figure 1.3: External machining example

Just by glancing at the figure, we should understand that the tool starts on the outside of our part where the radial coordinate is at the maximum, while machining it will progressively reduce it when moving toward the center (where the radial coordinate is 0).

Since, as we will discover, there are many different types of machining strategies, it is a bit difficult to find a strict definition for external machining; however, everything will be clearer when compared to the next machining approach.

Internal machining

These operations are different from the previous case since the material is removed “inside-out.” So, the average radial coordinate for our tool is growing during the operation:

Figure 1.4: Internal machining example

As you can see from the previous screenshot, the tool is moving inside our stock, and the cut chip may find itself stuck in the cavity since there is material all around the tool. As you can also see, the tool is still quite visible, but there are cases where we may completely lose the line of sight after a certain depth, and this is not good for beginners.

As a matter of fact, when we first approach turning, it is always a good idea to look constantly at our part while being machined since we can check the surface finish, prevent unforeseen collisions with parts of the stock or parts of the lathe, and monitor chip evacuation. For all these reasons, internal machining may be a bit trickier than external machining.

Note

As a rule of thumb, if the forming chip is somehow free to flow and falls on the ground, we are in external machining; if it can be stuck inside, we are in internal machining.

It is now time to explore something a bit more technical but really important to understand: working parameters!

It is now time to talk about the parameters involved in our turning operations. First of all, what is a parameter? In short, a parameter is a value or a setting that we can change.

Of course, some parameters are easier to change than others. For example, changing the axial movement speed for our tool is very simple, while on the other hand, changing the maximum cutting power may require a bigger and more powerful lathe.

Also, as we will shortly discover, some values are somehow connected to others; changing one parameter may change one or more others, so we have to optimize parameters according to our lathe specs and to the part we want to machine.

Let’s find out what the main parameters are that we have to work with.

Turning speed

The turning speed is a measure of how fast the chuck is spinning; it may be measured in radians per time unit () or in revolutions per time unit ().

As shown in the screenshot, the bent vector represents the part spinning along the longitudinal axis:

Figure 1.5: Turning-speed visualization

One revolution of our chuck corresponds to an angle () of 360° or (depending on whether it’s measured in degrees or radians). But, since is measured in revolution per time unit, we need to divide the angle by the same time unit, so that from the angle, we get angular speed ().

In short, we just need to remember this formula:

Old lathes had turning speeds that were only adjustable by manually changing the belt and pulleys, or changing the gears. Today, there are lathes that can control the rotation speed with inverters and encoders. So, depending on your lathe, the turning speed may or may not be a parameter that's easy to change.

Note

Please be careful when dealing with time units: sometimes the time unit may be seconds and sometimes minutes. As you can imagine, one revolution per minute is very different from one revolution per second, so when using any formula, please always be sure of its units!

Cutting speed

The cutting speed () is the relative speed between our cutting tool and the surface it is cutting. There is only one important thing to notice, which is that the cutting speed is highly dependent on the radial position of our tool: the bigger the diameter means the higher the cutting speed (at a constant rotation speed).

As you can see in the screenshot, we have a common rotation speed for the two tools (since the chuck rotation is always the same); however, as you may have noticed from the different arrow lengths, the tool that is machining a bigger diameter has a much higher cutting speed (vertical vector) than the tool machining a smaller diameter:

Figure 1.6: Cutting-speed visualization

Note

A vector can be defined by a magnitude and a direction. Magnitude is represented by the arrow length, while the direction is represented by the direction of the pointed tip.

Cutting speed is typically measured in meters per minute (m/min), and there is a very simple formula for calculating it:

Here, is the diameter in millimeters (mm) and is revolutions per minute (RPM).

For example, let’s imagine we have a chuck rotating at 500 RPM, and we are performing a longitudinal operation at a constant radial distance of 50 mm (basically, we are machining a stock with a diameter of 100 mm). What is the cutting speed seen by our tool? It's very simple:

Now that we have seen the cutting-speed formula, it should be now clear that when machining a shape with different radial coordinates assumed by our tool, the cutting speed will be subject to changes. Since the working diameter is not a parameter we can change (it is related to the part shape we want to machine), in order to change the cutting speed, we can only adjust the chuck RPM. That’s why most of the time, you will see bigger parts spinning slower and smaller parts spinning faster! Once the tool is almost at the rotation axis, the cutting speed will always drop to zero, independently of how fast the chuck is rotating.

Cutting depth

The cutting depth () is a parameter that gives us a measure of how much we impose an interpenetration between our tool and our part; it is measured in mm. Basically, it is related to how much of our cutting edge is engaged with the stock:

Figure 1.7: Cutting-depth visualization

As we can see, there are two tools machining the same diameter. The one on the left, however, is engaging the stock at a very small cutting depth, and therefore it removes only a thin layer of material. The tool on the right is cutting at a much bigger cutting depth and therefore it is removing a much thicker layer, and most of the cutting edge is engaged.

Please note that cutting depth is not always measured in the radial direction; sometimes, it can be measured in the axial direction. It mainly depends on the type of machining process we use (we will explain this in the Exploring main machining strategies section later in the chapter).

Higher cutting depth means more material removed and therefore faster machining, but requires more cutting power and leads to higher stress on our tool and our part. For this reason, please consider that higher cutting depths may partially bend our stock (especially if it is long and supported on one side only). Bending may lead to weird shapes with a rough finish.

Cutting feed

The cutting feed () is a parameter that measures how much our tool is advancing along the cutting direction at every revolution of our chuck, and therefore it is measured in mm per revolution (mm/rev)

Similar to cutting depth, higher feeds lead to higher machining speed at the cost of higher tool wear and higher power being required. The part finish is highly connected with feed values; as a rule of thumb, a lower feed value means higher surface quality.

In the following screenshot, we have two tools machining the same stock at the same cutting depth:

Figure 1.8: Feed visualization

However, in the first example, there is a much smaller feed step than in the second, so though they have the same turning speed, the tool on the bottom will reach the end of the stock much quicker, at the cost of higher surface roughness.

Be careful, as certain operations must be performed at a constant feed, such as threading. Threads have a constant pitch per rotation; therefore, we must set the feed to be equal to the thread pitch in such a scenario.

Note

Threading is the process of making a thread. It may be related to a male thread (such as a screw) or a female thread (such as a nut).

Adjusting the feed will also affect the chip. We can assume that a lower feed will produce a very long and entangled chip, while a higher feed will produce small particles. This is illustrated in the following screenshot:

Figure 1.9: Chip formation related to feed

We should always try to hit a sweet spot in chip thickness, width, and length. The ideal chip shape is the one in the middle of the screenshot.

Note

Chip formation is a very interesting world of its own. I don’t really want to distract you from the main topic; however, if you want to learn more about chip formation and different chip types, I suggest you take a look at this interesting link: https://www.bdeinc.com/blog/types-of-chips-formed-during-cnc-milling/.

Cutting power

The cutting power is the mechanical power required to machine our part at a given set of parameters. It is measured in kilowatts (kW).

Before setting all our parameters, we must always check whether our lathe is powerful enough to handle the machining we want to perform. This is the simple formula to remember:

Here, is the cutting power measured in kW; is the cutting speed measured in m/min; is the cutting depth measured in mm; is the feed step measured in mm/rev; and, finally, is the specific cutting force measured in MegaPascal (MPa).

As you may have noticed, there is a new value called that we haven’t seen yet. is a parameter related to material strength, tool shape, feed ratio, and cutting depth. This is a difficult parameter to evaluate, and I don’t want to bother you with complex calculations… but luckily, I don’t have to. We can simply refer to tables where equations are already sorted out by experts. Please note that this is a rough approximation of the real value, so you may want to take it with a grain of salt and have a bit of a safety margin on cutting power!

Here, we can find an example of the most common iron alloys:

Figure 1.10: Kc approximation for steel and iron

Using such a table is quite simple: we simply select the row according to the material we are about to machine, then we select the column with a feed similar to the one we plan to use, and the result approximates the real value.

Note

If you are intrigued by this parameter, you can find all the formulas for a precise evaluation of here: http://www.mitsubishicarbide.net/contents/mhg/enuk/html/product/technical_information/information/formula4.html.

As you can see, there is a very useful formula where we can insert our cutting parameters to get our value. If you are hungry for more formulas, there is a very good explanation about here: https://www.machiningdoctor.com/glossary/specific-cutting-force-kc-kc1/#k1c-and-mc-chart-for-material-group.

With that last equation, it is now easy to understand that all parameters are connected and that we must change them accordingly to meet the maximum cutting power available for our lathe.

You may be wondering whether it is a must to target maximum power. No, it is not, but from the production point of view, not using our machine at its full potential will cost us more money per hour. However, a typical scenario where we will not use maximum cutting power is when we are machining a fragile material that we may damage with our chuck closed at maximum force to sustain chuck torque.

Now that we have covered the main parameters, we should better understand our lathe. Next, let’s jump into something juicier: turning operations and strategies!

When we plan how to machine our part out of the stock, we have to think like a chess master. What I mean by this is that we have several pieces we can play with, but in order to win the game, we have to use every component in the best possible way it can be used. Therefore, we need to plan which piece to play first and with which type of move: do we move the bishop or the queen? Do we move by one square at a time or full speed ahead?

In the following sections, we are going to discover the main moves we can play with when it comes to turning.

Longitudinal operations

Longitudinal machining is a simple and common operation strategy, suitable for rough machining with high power and strong tools. Let’s check a basic example in the following screenshot:

Figure 1.11: Longitudinal machining approach

The typical approach for longitudinal operations is to move the tool on the front of our stock (at a safe distance), set the cutting depth in the radial direction, and then move the tool forward. As we can see in the screenshot, while cutting, our tool is moving along the axial direction only, so we have a constant cutting speed per cutting pass. Once at the desired distance, the tool will disengage our stock radially and then repeat the process until the right diameter is machined.

Since this is longitudinal machining, the main cutting direction is on the longitudinal axis at a given radial distance; therefore, after a chuck rotation, our tool will be moved by one feed step along the longitudinal direction.

As a recap, in this type of machining, the cutting feed is along the axial direction, while the cutting depth is fixed and constant and is measured along the radial direction. As we are about to discover, there are other machining strategies where what we just said doesn’t apply.

Facing operations

Facing is used when we need to clean the front face of our stock:

Figure 1.12: Facing machining approach

As shown here, while cutting, our tool is moving in the radial direction only; therefore, the cutting power will keep changing unless we adjust the feed or rotation speed accordingly.

The standard approach for facing operations is to move the tool at a safe distance in the radial direction, set the cutting depth in the axial direction, and then approach the stock radially. Once at the desired position, the tool will disengage our stock axially and then repeat the process until the right length is machined.

Since in facing, we are basically cleaning a slice of our stock, we are operating at a fixed axial coordinate and our tool is moving radially. So, after a chuck rotation, our tool will be moved forward by one feed step along the radial direction.

As a recap, when facing, the cutting feed is along the radial direction while the cutting depth is along the axial direction (this is different than longitudinal operations!).

Plunging operations

Plunging is similar to facing since the tool is moving in the radial direction only; however, because plunging is used for grooving or cutting, the tool is much slimmer. That’s because circlips grooves can be very thin, and our tool needs to fit inside them. Another reason is that when cutting our part, it is not a good idea to perform a large cut because that would require a lot of material removed without a real need.

As already mentioned for facing, since radial coordinates are always changing, so does the cutting power, unless controlled by feed changes or RPM.

As shown in the following screenshot, the typical approach for plunging is to position our tool at a safe radial position, set the desired axial coordinate, and then approach the part radially:

Figure 1.13: Plunging machining approach

So, to recap this strategy, plunging is similar to facing since it has feed along the radial direction too, but the main difference is that we cannot set the cutting depth since the tool cutting edge is always engaged entirely; therefore, the cutting depth is always at the maximum possible value!

Profiling operations

Profiling is one of the most complex operations since the tool moves constantly radially and axially. Let’s check the following screenshot for an idea of how profiling works:

Figure 1.14: Profiling machining approach

As shown in the screenshot, the motion path of our tool can be very complex; therefore, this type of operation is the most flexible and is well suited for finishing our part. However, due to the fact that the cutting direction is not constant, there is always the risk of impact between the tool and our stock. As you may have noticed in the screenshot, after “climbing the first hill,” our tool will likely collide with the stock since the required path is too steep for the tool to pass.

To reduce the possibility of errors, an impact simulation is always a good idea in CAM, but for complex machining operations such as profiling, you must always check the results. Especially when a beginner is approaching turning for the first time, 99% of the time they will discover that the back of the tool or the shank will collide where the profile gets too steep or too narrow.

If we want to analyze what happens to our cutting parameters when profiling, we have to remember that the profile is not constant along the radial direction nor along the longitudinal direction; it keeps changing. So, unless our chuck is able to control rotation according to the tool’s radial position, the cutting speed will not be constant.

Having said that, we also need to remember that feed is measured along the cutting direction, so it will keep changing along the profile; the same can also be said for cutting depth.

Finally, we are at the end of yet another section. There is only one last major topic to cover: tool geometry.