From drawing to cutting data

Every machining operation can be described by a small set of numbers. How fast the cutting edge passes the material. How far the tool advances each revolution or each tooth. How deep and how wide it cuts. From those few values follow the spindle speed, the feed rate, the metal removal rate, the power, the time and, eventually, the cost.

People who machine every day often know good values by feel. That knowledge is valuable, but it is hard to transfer, hard to check and easy to stretch beyond the conditions where it was learned. Calculation gives a common language between the machinist, the programmer, the estimator and the customer. It also catches the expensive mistakes: the feed entered per minute instead of per revolution, the spindle that cannot reach the speed the program assumes, or the quote that forgets the time spent between cuts.

This chapter introduces the basic quantities, the sources of cutting data and the fictional part that runs through the book.

The basic quantities

The table lists the quantities used throughout the book, with the symbols commonly used by tool suppliers.

Most of the arithmetic in machining links these quantities with simple geometry. Cutting speed relates to spindle speed through the circumference of the work or tool. Feed rate is feed per revolution, or per tooth, times the number of teeth and revolutions per minute. Removal rate is cross-sectional area of the cut times feed rate. Power is removal rate times the energy needed to remove each unit of volume. Each relationship is derived in a later chapter.

Read the drawing for the numbers that drive the job

Before any cutting data is chosen, the drawing decides which operations, passes and tools the job needs. A few features usually drive most of the planning:

• Tight tolerances. The Ø40 H7 bore of the flange allows a band of 0.025 mm above 40.000 mm, from 40.000 to 40.025 mm. A drilled hole cannot hold that, so the bore needs a drilling operation to remove most of the material, a roughing bore and a light finishing bore, each with its own cutting data and time.
• Surface finish. A required roughness on a sealing face or bore sets the feed and nose radius of the finishing pass, as Chapter 3 shows, and may call for a separate finishing tool.
• Material and condition. The material specification, and whether the bar is supplied as rolled, normalised or hardened, sets the cutting speed range and the tool grade.
• Threads and small holes. The M8 tapped holes need a tap drill of the right size, a tapping cycle and a machine able to tap at the planned speed.

Reading the drawing this way produces a list of features with their governing requirements. That list, not the overall shape of the part, is what the estimate and the program are built from. A part that looks simple may hide one feature that needs three passes and an in-process check.

Quantity matters as well. The customer’s request for prices at 30, 120 and 500 flanges means the plan must work at all three. A feature that is acceptable to finish with a slow, careful pass on 30 parts may justify a dedicated tool or a different sequence at 500, and set-up time, which Chapter 10 separates from per-part time, weighs very differently across those quantities. Noting the quantity range beside the feature list at the start keeps those trade-offs visible.

Where cutting data comes from

No formula tells you the right cutting speed for a material. Cutting speed and feed are empirical: they come from testing. There are three common sources:

• Tool supplier data. Catalogues, online tools and application engineers give starting values for each tool, grade and material group, usually for a stated tool life and reasonably stable conditions. They are the best starting point for modern tooling.
• Handbooks. General reference works give speed and feed tables for broad material and tool groups. They are useful for older or generic tools and for sense-checking, but cannot reflect every modern grade and geometry.
• Your own records. Values proven on your machines, with your fixtures, coolant and materials, are the most relevant data of all, provided they are recorded with the conditions under which they were achieved.

A starting value is not a final value. Real machines differ in rigidity, power and spindle condition. Workholding may allow vibration. Material from one supplier may machine differently from another. The calculations in this book show what a set of cutting data implies for time, power and deflection, so that adjustments can be made deliberately.

Material condition changes the numbers

Two bars both described as medium-carbon steel can behave very differently under the tool. Hardness has the largest effect: harder material needs a lower cutting speed for the same tool life and produces higher cutting forces. Free-machining grades, which contain additions that help chips break, allow higher speeds and better finishes than standard grades of similar strength. Bar that has been cold drawn may machine differently from hot-rolled bar, and material from a new supplier may differ from the last batch even under the same designation.

Tool suppliers group materials by machinability, and their data applies to a stated group and hardness range. Recording the material designation, condition and, where available, measured hardness with every set of cutting data is what makes the data reusable. When a familiar job suddenly wears tools faster, a change in material condition is one of the first things to check.

Units and conversions

Most mistakes in cutting data are unit mistakes. Three precautions prevent most of them:

1. Keep feed per revolution and feed rate separate. Lathes are usually programmed in millimetres per revolution and machining centres in millimetres per minute. A turning feed of 0.25 mm/rev entered as 0.25 mm/min would barely move the tool; the reverse would crash it.
2. Use diameter, not radius, in speed formulas. Turning programs often work in diameter on the X axis. Cutting speed depends on circumference, πD.
3. Convert imperial data carefully. Older handbooks and some suppliers use surface feet per minute and inches per revolution. Multiply surface feet per minute by 0.3048 for metres per minute, and inches by 25.4 for millimetres.

Writing the units next to every number in a calculation, and checking that they cancel properly, is the simplest and most effective error check. The READOS chapter on SI units and calculation checking covers the habit in more detail.

The Harbourline pump flange

Harbourline Precision is a fictional small job shop with two CNC lathes, a vertical machining centre, a bandsaw and a small inspection room. A customer has asked for a quote on 120 pump flanges, with possible repeat orders, and wants to know how the price would change for 30 or 500.

The flange, part PF-100, is made from medium-carbon steel bar, similar to AISI 1045, 110 mm in diameter. Its main features are:

Harbourline’s estimator plans the work in three machining operations after sawing blanks 34 mm long:

• Operation 10, lathe, first side: face, drill and bore Ø40, rough and finish turn the Ø100 outside diameter.
• Operation 20, lathe, second side: face to length, rough and finish the Ø60 spigot and the back face of the flange.
• Operation 30, machining centre: drill the six bolt holes, drill and tap the two M8 holes, face mill the flat.

Later chapters calculate speeds, feeds, power and tool life for each operation. Chapter 10 builds the full cycle time and Chapter 11 the quotation.

Let the datums decide the operation order

Harbourline’s sequence is not arbitrary. Operation 10 bores the Ø40 hole and turns the Ø100 diameter in one setting, so the two are concentric to the accuracy of that setting. Operation 20 then grips on the finished outside diameter, or locates in the bore, to machine the second side, keeping the spigot concentric with what was already made. Operation 30 drills the bolt holes, locating from the bore and the face, so the hole pattern is positioned relative to the features that matter in assembly.

Each operation uses features produced by the previous one as its references. The same logic appears in fixture design: a surface that will locate the next operation must be finished first and accurately. Changing the order, for example drilling the bolt holes before the bore is finished, would leave the pattern positioned from a rough surface and make the relationship between holes and bore depend on two separate settings.

Record the conditions with the numbers

A cutting data record is only useful if someone can tell when it applies. A practical data sheet for each tool and material combination records:

The last line is the one most often missing. A record that says what was run but not how long the tool lasted, or whether the finish was acceptable, cannot tell the next user whether to start from those values or avoid them. Dating each record also shows when it may no longer reflect current tools or materials.

What the numbers cannot tell you

Calculation is a guide, not a guarantee. It cannot see a worn spindle bearing, a blunt edge on a fresh insert, an inconsistent bar from a new mill or a clamp that lets the part chatter. Machine tools also have limits that formulas do not respect on their own: maximum spindle speed, available torque at low speed, axis feed limits, the maximum swing and the safe operating envelope of chucks and fixtures. Chuck manufacturers, for example, specify maximum speeds and gripping forces that must not be exceeded regardless of what a cutting speed calculation suggests.

Safe work comes first. Guarding, interlocks, correct workholding, chip control and safe procedures for loading, measuring and changing tools are not optional and are not affected by any calculation in this book. Safe Work Australia’s code of practice on managing the risks of plant, listed in the references, is a good starting point for the wider obligations.

Common mistakes

• Treating catalogue data as exact. It is a starting point for stated conditions.
• Mixing feed per revolution and feed per minute.
• Calculating with radius instead of diameter.
• Ignoring machine limits on speed, power and torque.
• Estimating only cutting time. Chapter 10 shows that non-cutting time is often larger.

Questions to ask

• Where did this cutting data come from, and for what tool, grade, material and tool life?
• Which machine will run the job, and what are its speed, power and torque limits?
• Are all feeds and speeds in consistent units?
• What has been proven on our own machines for similar work?

Exercise: build a data sheet

Choose one tool you use often. Record the supplier’s starting values for cutting speed and feed for your most common material, the conditions they assume and the values you actually run. Note any difference and the reason for it. A small library of such sheets is one of the most useful assets a workshop can build.

The next chapter turns cutting speed into spindle speed and shows what happens on a lathe as the tool approaches the centre of a face.