Transcript: Manufacturing Processes

The full text of the narration of all 25 chapters. It was generated automatically from the on-screen captions, so small errors are possible. Back to the video course

0. Introduction: the map

a long way, from a block of raw material to a final shape with precise dimensions. the milling machine, grinding, and sometimes wire EDM or a laser. depth: how it works, what it can deliver, and what makes it expensive. of processes exist, and how to choose between them.

There are three main ways to give a part its shape. material changes shape, but almost nothing is removed. You can add material, layer by layer. That's additive manufacturing. Or you can remove material from a larger block until the shape you want is left. That's machining.

This series covers all three. We'll start with how the raw material is made: casting, forging and extrusion. From there we'll move on to machining, sheet metal work, and the non-conventional processes. And at the end, we'll get to additive manufacturing.

Material removal itself has several families. In machining, a tool with a sharp edge and a defined geometry shears a chip from the material. In abrasive machining, thousands of small, hard grains each scrape off a tiny chip. without a cutting edge: with an electric spark, a beam of light, a jet of water, or a plasma arc.

Every machining operation has two motions. The primary motion creates the cutting speed. The feed motion advances the tool into fresh material. On a lathe, the part rotates and the tool moves along it.

On a milling machine, the tool rotates, and the part or the tool moves along the axes. Three parameters will follow us throughout the series. cutting edge passes over the material, in meters per minute. Feed is how far the tool advances per revolution, or per tooth.

Depth of cut, ap, is how much material is removed in a single pass. The chip itself tells you a lot: its color, shape and length show whether the parameters are right. A grinding wheel is made of very hard grains, held together by a bond. Each grain removes very little material. So grinding is relatively slow, but very accurate.

Grinding also suits hardened material, which an ordinary tool struggles to cut. Honing and lapping are the next step, for even higher finish and accuracy. In EDM, electric sparks melt away tiny particles of the material. The tool never touches the part, so the hardness of the material hardly matters.

The one condition is that the material conducts electricity. A laser melts the material with a focused beam of light. A waterjet carrying abrasive grains cuts almost any material, with no heat-affected zone. Plasma cuts conductive metals fast, but with lower accuracy.

Choosing a process starts with five questions. What is the shape? A round part usually starts on a lathe, and a prismatic part on a milling machine. What is the material, and how hard is it? What accuracy and finish are required?

Turning and milling typically reach IT7 to IT9, with a surface roughness Ra of 0.8 to 3.2 microns. Grinding reaches IT5 to IT6, and a roughness Ra of 0.2 to 0.8 microns. Honing and lapping go below that. What is the quantity? A single part and a batch of thousands won't be made the same way.

In large batches, it often pays to forge or cast close to the final shape, and save on machining. And what is the total cost, not just the machine time? Take a steel pin that must be hardened, with a precise diameter. We turn it while the material is still soft, and leave a small machining allowance.

Then it goes through heat treatment. And finally, we grind it to its final size. That's how most parts go through a chain of processes, not just one. In every chapter, we'll also ask what makes the process expensive.

operations like heat treatment or moving between machines. And one important rule: the tighter the tolerance, the longer and more expensive the process. This is the series map: 25 chapters in six groups. In the next chapter, we'll start at the beginning: casting.

1. Casting

Casting is one of the oldest ways to make metal parts, and it is still one of the most common. An engine block, a pump housing, a valve body and a turbine blade all start life as castings. cavity shaped like the part, and wait for it to solidify. But to get a sound part, a lot of details have to be controlled.

Every casting has a mold, and inside it a cavity in the shape of the part. The cavity is formed with a pattern, a replica of the part, made of wood, plastic or metal. Internal cavities, like a hole or a channel, are formed with a core placed inside the mold. The mold is usually made in two halves, and the plane between them is called the parting line.

The metal enters through a gating system: a sprue, runners, and gates into the cavity. There is also a riser: a reservoir of liquid metal that keeps feeding the part while it solidifies. Metal shrinks in three stages. As the liquid cools, as it turns solid, and as the solid keeps cooling down to room temperature.

one: if there's nowhere to draw extra metal from, a cavity forms inside the part. keeps flowing from it into the part until the very end. dimensions, so the pattern is made larger than the part. About 1% for gray cast iron, about 1.3% for aluminum, and about 2% for steel.

A part meant for casting is designed differently from a part machined from solid. Walls need a draft angle, usually one to three degrees, so the pattern can be pulled out. thick section solidifies last, and that's where cavities tend to form. sharp corner concentrates stress and can crack during cooling.

machining allowance is left: a few millimeters of material above the final size. The most common method is sand casting. pattern, the pattern is pulled out, and the metal is poured. After solidification the mold is broken, and every casting needs a new mold.

from a few kilograms to tens of tons, and almost any metal. The drawback: a rough surface, around Ra 12.5 to 25 microns, and low accuracy. So almost every functional surface on a sand casting is machined. In investment casting, also called lost-wax casting, the pattern is made of wax.

It is coated with several layers of ceramic and heated: the wax melts out, leaving a ceramic shell. Metal is poured into it, and the shell is broken off after solidification. There's no parting line and no need for draft, so very complex shapes and fine details are possible. The surface is much smoother, around Ra 1.6 to 3.2 microns, and the accuracy is high.

This is how turbine blades, medical implants, and parts in steels, superalloys and titanium are made. The price: a long process, a lot of labor, and a high cost per part. When quantities are large, it pays to invest ina steel die that serves thousands of castings. In permanent mold casting, the metal flows into the die by gravity.

In die casting, the metal is injected into the die at high pressure and high speed. This gives thin walls, precise dimensions, and a very short cycle per part. The method mainly suits metals with a low melting point: aluminum, zinc and magnesium. But the die is very expensive, and only pays off in large quantities.

And because of the fast injection, air gets trapped in the metal. welded or heat treated: the trapped gas expands and forms blisters. Castings have a few typical defects. Gas porosity: small bubbles of gas trapped in the metal.

Shrinkage cavities: voids in the places that solidified last without feeding. Misrun: the metal solidified before filling the whole cavity, usually in thin walls. Hot tears: cracks that form when the metal shrinks and the mold restrains it. the tool opens a void that was hidden below the surface.

Critical parts are inspected by X-ray. So what does this mean for whoever machines castings? The outer layer is hard and abrasive: sand grains and an oxide skin wear down the cutting edge. So the first pass has to be deep enough to get below the skin.

so the points on the casting used for that setup are defined in advance. After the first pass, work continues from machined surfaces. What makes a casting expensive? steel die. Its cost is spread over the number of parts.

Cores: every core is more work and another risk of a defect. after machining has cost both the casting and the machining. gating system, cleaning, and grinding off excess metal. Inspections, like X-ray, and heat treatment when required.

And the machining allowance: every millimeter left on the casting is machine time. So how do you choose? For a few parts, it is often cheaper to machine from solid, or to sand cast. sand casting, or investment casting when accuracy is needed.

For thousands of aluminum parts or more: die casting. flow that follows the shape of the part, and it may contain tiny voids. So it's usually weaker and less fatigue resistant than a forged part of the same material. From here we'll move on to the next chapter: forging.

2. Forging

a compressor blade: all parts that must carry high loads and fatigue for years. Most of them start as forgings. the solid state, by the force of a hammer or a press. And the result is a stronger part than the same part made by casting or machined from solid.

Metal is made of grains, tiny crystals. When it is shaped by force, the grains are stretched along the direction the material flows. This creates grain flow, like the grain in wood. In a forged part, the grain follows the shape of the part, and wraps around corners and shoulders.

In a part machined from solid, the cut crosses the grain exactly in those areas. from casting the raw material, and the structure becomes finer and more uniform. The result: higher strength, fatigue resistance and impact resistance. Most forging is done hot.

the grains rebuild themselves while it is being shaped. degrees, and for aluminum about 400 to 500 degrees. The drawback: scale forms on the surface, a hard oxide layer, and the dimensions are less precise. In cold forging, the shaping is done at room temperature.

precise dimensions and a clean surface, and the material work-hardens as it is shaped. This is how screws and rivets are made, for example, in huge quantities. There's also warm forging, which combines some of the advantages of both. In open-die forging, the material is squeezed between simple dies, usually flat ones.

The material isn't enclosed on all sides, and the operator turns and moves it between blows. This is how material is drawn out, upset and thickened, to make large shafts, rings and discs. The tooling is cheap, and parts weighing tens of tons and more can be forged. But the accuracy is low, and a large machining allowance is left.

In closed-die forging, each part has a pair of steel dies, with a cavity shaped like the part. A hot billet is placed between the dies, and they close on it, forcing the material to fill the cavity. To make sure the cavity fills completely, a little more material is used than needed. The excess is squeezed out between the dies, forming a thin rim around the part called flash.

The flash cools quickly, gets hard, and restricts further outward flow. That way it pushes the material to fill the corners. At the end, the flash is trimmed off in a separate press. goes through several stations, from rough shaping to the final shape.

The dies are expensive, so the method pays off in batches. The force comes from a hammer or a press. A hammer strikes fast, many short blows, and the material flows mainly near the surface. A press squeezes slowly and continuously, and the shaping penetrates deeper into the part.

A part for forging is also designed differently. angles to release the part, usually 5 to 7 degrees on the outer walls. Generous radii at the corners, so the material flows without getting stuck and forming a lap. And no ribs that are too tall and thin, which are hard to fill.

And a machining allowance on every precise surface, which also covers the scale layer. Forging has its typical defects too. A lap: the material folds over on itself and forms a hidden crack, usually near a sharp corner. Underfill: there wasn't enough material or heat, and the corners didn't fill.

relative to each other, and the two halves of the part don't line up. And cracks, when material is forged too cold. Critical forgings are inspected with ultrasound, to find internal defects. So what does this mean for whoever machines forgings?

As with castings, the scale is hard and abrasive, so the first pass has to get below it. Walls with draft aren't parallel, so they're hard to hold in an ordinary vise. where the first setup is located, so it is checked before starting. A forged part also has internal stresses: removing a lot from one side can distort it.

symmetrically, leaving a finishing pass for the end. What makes forging expensive? The dies: tool steel, precision machining, and they wear and need repair and replacement. Heating: energy, furnaces and time.

heated and trimmed, and never ended up in the part. Trimming the flash, removing the scale, and heat treatment. Inspections like ultrasound. And the machining allowance, again: every millimeter is machine time.

So when should you forge? When the part carries high loads, fatigue or impact, and when its failure is dangerous. material and machining time compared with machining from solid. But complex internal shapes, cavities and thin walls are hard to forge, and there casting wins.

And for a single part, it's usually simpler to machine from solid, or from an open-die forging. In the next chapter we'll meet another way to shape metal by force: extrusion.

3. Extrusion

Rails, tubes, window frames, and heat sinks with dozens of fins. They all have one thing in common: a constant cross-section along their whole length. Most of them are made by extrusion. the material comes out through an opening, and takes the shape of the opening.

A cylindrical billet of metal is heated and loaded into a container. die, which has an opening in the shape of the cross-section. The metal flows through the opening, and comes out the other side as a long profile. billet and that of the profile is called the extrusion ratio.

and a single billet produces a profile tens of meters long. This way you get shapes that are very hard to make any other way, in almost unlimited length. There are two main ways to extrude. In direct extrusion, the ram pushes the billet, and it slides along the container wall.

force is highest at the start, when the billet is longest. relative to the container, and the die is pushed into it. There's no friction with the wall, so less force is needed, but the equipment is more complex. Most extrusion is done hot.

degrees, and it is the most common material for extrusion. higher temperatures and forces, and special lubrication. In cold extrusion, at room temperature, a small slug is squeezed in a fast blow. This is how aerosol cans, tubes and battery casings are made, for example.

How do you extrude a tube, or a profile with closed cavities? A special die is used, with a mandrel held in place by thin bridges. The metal splits around the bridges, and rejoins in the chamber around the mandrel before it exits. Where the streams rejoin, weld lines form along the profile.

but in critical parts these lines are taken into account. extruded around a central mandrel, giving a tube with no weld lines. The profile comes out hot, and is cooled in air or water. Then it is stretched slightly, to straighten it and relieve stresses.

It is cut to length, and many aluminum alloys are age hardened, which raises their strength. extruded to the end: it is cut off and sent for recycling. A profile for extrusion is also designed by rules. section flows faster than a thin one, and the profile bows.

Rounded corners, so the material flows easily and the die doesn't crack. And no deep, narrow channels: the part of the die that forms them is thin and long, and can break. A symmetric, smaller profile is easier to extrude, and gets a tighter tolerance. Extrusion has its typical defects too.

Die lines: fine streaks along the profile, from wear or dirt on the die. Surface cracks, when extruding too fast or too hot. Blisters, from air or gas trapped between the billet and the container. And twist and bow, when the flow isn't balanced.

So what does this mean for whoever machines profiles? A profile isn't perfectly straight and flat: it has bow and twist, within the tolerance of the standard. rather than relying on raw surfaces for precise dimensions. clamping forces, so they are supported and not clamped too hard.

final, usually only short operations are left: cutting to length, drilling and local milling. What makes extrusion expensive? even a custom profile pays off in medium quantities. But there is a minimum quantity: whole billets are extruded, giving tens of meters at a time.

Scrap: the billet butt, and the ends cut off after stretching. A complex profile, with cavities and thin walls, is extruded more slowly, and its die wears faster. And extra operations: age hardening, anodizing or painting, and machining. So when should you extrude?

When the part is long, and has a constant cross- section. When you can buy a profile close to the final shape, and save a lot of machining from solid. And when the material suits it, mainly aluminum. That completes the ways of making the raw material and the initial shape.

In the next chapter we'll start machining, with the most common process: turning.

4. Turning

Shafts, pins, bushings and screws: almost every round part goes through a lathe. Turning is the most common machining process. along the part or toward its center, removing a layer of material. operations, the tools, and what determines accuracy and cost.

On the left is the headstock, with the main spindle that rotates the part. A chuck with three jaws that grip the part is mounted on the spindle. moves in two axes: along the part, and perpendicular to it. On machines, the length axis is usually called Z, and the diameter axis X.

On the other side is the tailstock, with a center that supports the end of a long part. In chapter 0 we met three parameters: cutting speed, feed and depth of cut. In turning, the cutting speed depends on the spindle speed and on the diameter of the part. travels a longer distance each revolution, so its cutting speed is higher.

cutting speed of 200 meters per minute, you need about 1,270 rpm. When facing toward the center, the diameter gets smaller, and the cutting speed drops. speed: the machine raises the spindle speed as the diameter gets smaller, up to a preset limit. revolution, and depth of cut is how much is removed from the radius in a single pass.

Removing one millimeter from the radius makes the diameter two millimeters smaller. A lathe can do many operations. Longitudinal turning reduces the diameter along the part. Facing squares off the end of the part.

Grooving creates a groove, and parting cuts the part off the bar. Drilling and boring create precise bores in the center of the part. And threading creates a thread, when the feed per revolution equals the pitch exactly. You can also turn tapers, radii and profiles, with both axes moving together.

Most tools today are a holder with an indexable insert, made of carbide or another hard material. angle is stronger, and one with a sharp angle reaches tight spots. For example, an 80-degree rhombic insert suits roughing, and a 35-degree insert suits profiling. The nose has a radius: a large radius and a low feed give a smoother surface.

But a radius that is too large increases the radial forces, and can cause chatter. And the insert has a chip breaker: a shape that bends the chip and breaks it into short pieces. Turning accuracy starts with workholding. A three-jaw chuck centers the part by itself, but not perfectly.

bored to the exact diameter of the part, on the machine itself. For small parts and bar stock, a collet is used, which grips all around and is very accurate. A long, slender part deflects under the cutting force. the chuck exceeds 3 times the diameter, the end is supported with a center.

And a very long part gets a steady rest, which supports it in the middle. The chip tells you what is happening in the cut. tool, scratch the surface, and are dangerous to the operator. Short chips, shaped like a spiral or a C, are a sign of correct parameters.

depth of cut, or choose an insert with a different chip breaker. On a CNC lathe, a program controls the axes, and the turret changes tools by itself. A turning center also has live tools: drills and milling cutters that rotate in the turret itself. This way the part can be drilled and milled without taking it off the machine.

spindle to spindle, and its other side is machined too, without another setup. guide bushing, so the cut is always close to the support. This is how small, long, precise parts are made. Ordinary turning typically gives an accuracy of IT7 to IT9, and a roughness Ra of 0.8 to 3.2 microns.

parameters, better accuracy and roughness can be reached. A big advantage of turning: everything turned in the same setup rotates around the same axis. So diameters that must share an axis, like bearing seats, are turned in one setup. Turning has its typical problems too.

on a slender part or with a holder that sticks out too far. Built-up edge: soft material sticks to the insert, and the surface becomes rough. The common fix: raise the cutting speed. barrel-shaped, because where it bends away the insert cuts less.

batch, so it is measured and corrected in the program. What makes turning expensive? Setup time: jaws, tools, the program, and a first part for inspection. Cycle time: how much material has to be removed, and how fast the material allows you to cut.

Stainless steel, titanium and superalloys are turned much more slowly than ordinary steel. measurements, and sometimes grinding afterward. same setup, and on an ordinary lathe they need another machine. Turning suits every round part, from a small pin to a shaft meters long.

And when the part has flats, pockets and non- round shapes, it moves on to the next machine. In the next chapter: milling.

5. Milling

Flat surfaces, pockets, slots and free-form shapes: most parts that aren't round are milled. Milling is the opposite of turning: the tool rotates, and the part or the tool moves along the axes. A milling cutter has several teeth, and each tooth cuts a small chip every revolution. tools, the parameters, and what makes a milled part expensive.

On a vertical milling machine, the spindle stands upright, and the tool cuts from above. The table moves in two axes, X and Y, and the spindle moves up and down, in the Z axis. swaps a tool in seconds, and everything is controlled by a program. There are also horizontal mills, where the spindle lies flat; they suit large parts and clear chips well.

part can be reached, and we'll expand on that in chapter 21. The most common tool is the end mill: it cuts both on its side and at its tip. For large surfaces, a face mill with indexable inserts is used. For curved surfaces and molds, a ball end mill with a round tip is used.

Milling tools are usually made of solid carbide or high-speed steel, or carry indexable inserts. materials, and a tool with few teeth leaves room for chips, and suits aluminum and roughing. and spindle speed, but the diameter is the tool's, not the part's. For example, a 10 mm tool at a cutting speed of 150 meters per minute needs about 4,800 rpm.

tool advances while one tooth passes through the material. The table feed rate is the feed per tooth, times the number of teeth, times the spindle speed. In our example, with 4 teeth and 0.05 mm per tooth, that's about 960 mm per minute. along the tool, and width of cut, how much of the tool diameter is engaged in the material.

There are two ways the tool can meet the material. In conventional milling, the tooth enters thin and exits thick. At first it slides and rubs, which heats it and wears it. In climb milling, the tooth enters thick and exits thin.

Wear is lower and the surface is better, so on CNC machines this is usually the choice. On old machines with backlash in the screw, climb milling can pull the table. Milling can do many operations. Face milling flattens a large surface.

Shoulder milling creates a wall and a floor at a right angle. In a slot or a pocket, the tool plunges into the material and clears a closed shape. Contour milling follows the outline of the part. And a machining center also drills, taps, and machines curved surfaces.

Most parts are held in a vise, or in a fixture dedicated to the part. measured from, and every additional setup can add error. important surfaces as possible are machined in the same setup. And every setup you save also saves setup time.

Milling has its typical problems too. A long, slender tool deflects: the wall comes out out of square, and the tool may break. than 3 to 4 times its diameter, reduce the depth of cut and the feed. Chatter leaves marks on the surface, mainly on thin walls.

In deep pockets, chips that aren't cleared get recut, and can break the tool. And every edge of a cut leaves a burr, which has to be removed. The tool is round, so an internal corner in a pocket will always have a radius. If the drawing calls for a sharp internal corner, another process is needed, like EDM.

tool radius, so the tool passes through the corner without stopping. A deep, narrow pocket needs a long, thin tool, which is slow and risky for the tool. And every additional side to machine is another setup, and more time. What makes milling expensive?

The number of setups: every setup means setup time, a vise or a fixture, and inspection. Programming: a complex part takes programming time and verification of the toolpath. Cycle time: how much material is removed, and what the part is made of. Small tools in deep pockets, and thin walls, force you to work slowly.

And tight tolerances, deburring, and measurement. Turning and milling are the two core processes of machining. Turning for round parts, and milling for everything else: flats, pockets, slots and shapes. And a single part often needs both.

In the next chapter: drilling.

6. Drilling

Almost every part has holes: for screws, for pins, for fluid passages, or for assembling other parts. Drilling is the most common operation in machining, and usually the first one on every hole. But a drill alone gives limited accuracy, so a whole family of tools surrounds it. The common drill is the twist drill, with two cutting lips at the tip.

The helical flutes carry the chips out of the hole, and let coolant in. high-speed steel drill, and usually 130 to 140 ona carbide drill. At the center of the tip is a section that doesn't cut well, so a long drill tends to wander as it starts. To start the hole exactly on target, it is spot drilled first, with a short, rigid drill.

drill diameter and the spindle speed, and the feed is in millimeters per revolution. almost zero, and there the material is pushed more than it is cut. So the thrust force in drilling is high. The deeper the hole, the harder it is to clear the chips.

diameter, peck drilling is used: go in, retract to clear chips, and go back. much greater depths, and very deep holes use gun drills. A drill makes a hole fast, but not very accurately. nominal diameter, and its surface is relatively rough.

The position and straightness of the hole also depend on a good start and a rigid drill. a precise hole, like a pin or bearing seat, another tool follows. And this is the drilling family. a precise diameter, usually to an H7 tolerance, and a smooth surface.

But a reamer follows the existing hole, and doesn't correct its position. bored with a boring head, which also corrects position and straightness. A counterbore creates a flat seat for a screw head, so the head doesn't stick out. a conical head, and is also used to deburr the edge of the hole.

We'll cover threading a hole in the next chapter. A through hole goes from side to side, and a blind hole stops inside the material. At the bottom of a blind hole a cone is left, at the angle of the drill tip. If a flat bottom is needed, a special tool is required, and that adds cost.

And in a blind hole, the chips have to come out through the same opening the drill went in. Drilling has its typical problems too. Wandering at the start of the hole, mainly when the drill enters an inclined or curved surface. Chips packing in the flutes break drills, especially small ones.

A burr at the exit of a through hole, which has to be removed. And a worn drill cuts poorly, heats up, and gives an oversize or out-of-round hole. Holes are worth designing properly too. Use standard diameters, which have an off-the- shelf drill.

Give the drill a surface perpendicular to it, at the entry and at the exit. Avoid, where possible, very deep holes with a small diameter. need it, because every precision hole adds an operation. What makes drilling expensive?

every diameter is another tool and another tool change. Deep holes, which need pecking or special tools. Precision holes, which need reaming or boring after drilling. Hard materials, and small drills that break.

And deburring, especially where holes meet inside the part. Drilling creates the hole, and its family gives it accuracy and shape. diameter, boring for a precise position, and the counterbore for the screw head. In the next chapter: threading.

7. Threading

Almost every mechanical product is held together with screws. Threading creates a thread: a helical groove, internal in a hole or external on a shaft. the ways to make it, and what's important to know when designing a threaded part. A thread is a groove that winds around an axis, like a helix.

threads, and on an ordinary thread it is also the distance the screw advances in one turn. The most common thread is the metric thread, with a 60-degree angle between the flanks. For example, M10 is a 10 mm thread, with a coarse pitch of 1.5 mm. There are also fine threads, with a smaller pitch, for example M10 with a pitch of 1.25 mm.

that seal, and trapezoidal threads for motion, like a machine's lead screw. tolerance classes. The common ones: 6H for the nut, and 6g for the bolt. An internal thread in a hole is usually made with a tap. First a hole of the right diameter is drilled, and the tap cuts the threads into the walls of the hole.

about the thread diameter minus the pitch: for M10, drill 8.5 mm. A tap with spiral flutes pulls the chips up, and suits blind holes. A spiral point tap pushes the chips forward, and suits through holes. displaces the material into the shape of the thread.

it needs a slightly larger hole, and a ductile material. It's hard to remove, sometimes only by EDM, and sometimes the part is scrapped. Another way is thread milling. a circular, helical path, advancing one pitch per revolution.

One tool suits many diameters with the same pitch, and the chips are small. And if the tool breaks, it's smaller than the hole and easy to remove. So it's a good choice for expensive parts, hard materials and large diameters. An external thread can be turned or rolled.

makes several passes, going a little deeper each time. The machine synchronizes the feed with the rotation, so every pass lands exactly in the groove. with the thread form press on the bar, and the material flows into the shape of the threads. The thread is stronger, because the grain isn't cut, and the process is very fast.

This is how most standard screws are made. Threads are worth designing properly too. diameter is enough, and in aluminum about twice the diameter. Beyond that, the extra threads carry almost no load, and only add time and risk.

In a blind hole, drill deeper than the thread, to leave room for the tap's tip and for chips. On an external thread that runs up to a shoulder, design a thread relief groove, so the tool can exit. thread, so the screw enters easily and the first thread doesn't get damaged. closed many times, a thread insert is installed to reinforce the thread.

Threads are inspected with go and no-go gauges. side must enter all the way, and the no-go side shouldn't enter more than a few turns. For an external thread a ring gauge is used, on the same principle. Threading has its typical problems too.

A broken tap, mainly in small blind holes, and in hard or sticky materials. inspection, because of a worn tap or a wrong hole diameter. Torn threads, when the chips don't clear or there isn't enough lubrication. And a burr at the start of the thread, which stops the screw from entering.

What makes threading expensive? The number of threads and different sizes: every size is another drill and another tap. Small threads in deep blind holes, which need careful work. Hard materials, like titanium and stainless steel, and the risk of a broken tap in an expensive part.

Tight tolerance classes, special threads, and thread inserts. And gauge inspection of every thread. For an internal thread: a tap, and in expensive or hard parts, thread milling. For an external thread: turning, and in large quantities, rolling.

In the next chapter: grinding.

8. Grinding

When the tolerance is very tight, the surface must be smooth, or the material is hardened, you grind. In grinding, thousands of small, hard grains each scrape off a tiny chip. So grinding is relatively slow, but very accurate. A grinding wheel is made of three things: grains, a bond, and pores.

for most steels, silicon carbide for cast iron and non-ferrous metals. For very hard steels, CBN is used, and for carbide and ceramics, diamond. The bond holds the grains, and the pores leave room for chips and coolant. Coarse grains remove a lot of material, and fine grains give a smoother surface.

And there's a rule that seems backward: for a hard material, choose a soft wheel. out, and a new sharp grain is exposed. That way the wheel sharpens itself. on a magnetic table, and moves back and forth under the wheel. In cylindrical grinding the part rotates between centers, and the wheel grinds the diameter.

In internal grinding, a small wheel goes into a bore and grinds it from the inside. between two wheels and on a work rest blade, with no centers and no clamping. This is how pins are ground fast, in large quantities. The wheel spins very fast, usually at a surface speed of 30 to 35 meters per second.

But each pass removes very little, usually a few hundredths of a millimeter. At the end comes spark-out: a few passes with no feed, until the sparks almost disappear. Coolant is vital: almost all the energy in grinding turns into heat. Grinding usually reaches an accuracy of IT5 to IT6, and a roughness Ra of 0.2 to 0.8 microns.

It also gives good geometric form: roundness, flatness and straightness. And it suits hardened materials, after heat treatment, when an ordinary cutting tool struggles. Over time the wheel goes dull and gets loaded, and its shape changes. So it is dressed: a diamond tool removes a thin layer and exposes sharp grains.

The wheel is also balanced, because imbalance causes vibration and marks on the part. marked on the wheel. A wheel that bursts is very dangerous. Grinding has its typical problems too. hardness of the surface, and sometimes creates tiny cracks. It isn't always visible to the eye.

Chatter marks, from an unbalanced wheel or a poorly supported part. A loaded wheel, mainly in soft materials, which rubs instead of cutting. And a tapered or out-of-round part, when the machine or the support isn't aligned. Grind only the surfaces that really need it.

tenths of a millimeter, because each pass removes very little. At a shoulder corner, the wheel has a radius, so design a relief groove or a suitable radius. And harden the part before grinding, because heat treatment after grinding can distort it. What makes grinding expensive?

Slow material removal: every unnecessary tenth of a millimeter means more passes. Setup time, dressing and balancing. Dedicated machines, and a skilled operator. Precise inspection, and sometimes a check for grinding burn.

the end, after the part has already been through all the other processes. Grinding is the stage where a part gets its final accuracy and finish. It's relatively slow and expensive, so it is used only where it's needed. In the next chapter: broaching.

9. Broaching

A keyway in the bore of a gear, splines inside a bushing, or a hexagonal hole. These shapes are very hard to make by turning or milling. Broaching makes them in a single pass. The tool is called a broach: a long bar with many teeth in a row.

Each tooth is slightly higher than the one before it, usually by a few hundredths of a millimeter. each tooth removes another thin layer, and the last tooth leaves the final shape. the semi-finishing teeth, and at the end finishing teeth of equal size, which size the shape. At the front of the tool is a pilot, which enters the pre-drilled hole and aligns the tool.

Between the teeth is a chip gullet, and the chip stays in it until the tooth leaves the part. So the length of cut is limited: in a part that's too long, the gullet fills up. pilot hole, and turns it into the required shape: a keyway, splines, a square or a hexagon. In external broaching, the tool passes over the surface of the part, creating flats and profiles.

This is how, for example, the slots in turbine discs that hold the blade roots are made. In job shops, a keyway is often cut with a manual broach kit and a simple press. And there's also rotary broaching, done on a lathe or a mill, which suits hexagons in blind holes. It's a single pass, so the cycle time is very short, often seconds.

The accuracy is good, usually IT7 to IT8, and the surface is good. And every part comes out like the one before, because the shape is in the tool. The tool is expensive, and suits only one shape and one size. So broaching pays off mainly in volume, except for standard keyway broaches.

In ordinary internal broaching, the hole must be a through hole. And the cutting forces are high, so the part must be strong, and its walls not too thin. Broaching has design rules too. A through hole is preferred, with a reasonable length of cut relative to the tool.

The pilot hole must have the right diameter and tolerance, because the tool starts from it. And if the slot must stop inside the part, a relief groove is needed, or another process. Broaching has its typical problems too. A broken tool, mainly when the gullets fill up or the material is too hard.

A keyway that's shifted or not parallel to the axis, when the part isn't aligned well. Chatter marks on the surface. And a burr where the tool exits. What makes broaching expensive?

The tool: long, with many teeth, and made specially for the shape. Resharpening the tool, and maintaining it. A dedicated machine for high forces. And in small quantities, wire EDM or a slotting machine is sometimes cheaper.

Broaching produces precise internal and external shapes in a single pass. The tool is expensive, but in large volumes the cost per part is very low. In the next chapter: gears.

10. Gears

Gears transmit motion and torque between shafts, in gearboxes, engines and machines. To run quietly and last, the tooth form has to be very precise. That's why gears are made on special machines with special tools. when two teeth roll on each other, the speed ratio stays constant.

The size of the tooth is set by the module. number of teeth: a gear with module 2 and 30 teeth has a pitch diameter of 60 mm. The standard pressure angle is 20 degrees. quietly, bevel gears for shafts at an angle, and worm gears for a large speed reduction.

The common method is hobbing. cutting teeth, and it rotates in sync with the gear, so the teeth are formed by a generating process. Hobbing is fast and precise, and suits most external gears, with spur or helical teeth. In gear shaping, a gear-shaped cutter moves up and down and rotates together with the part.

It can also cut internal gears, and teeth near a shoulder, where a hob has no room. separately with a form cutter, but the accuracy is lower. And internal splines are often made by broaching, as we Saw in the previous chapter. Most gears are hardened, to resist wear and load.

surface takes up carbon and is hardened, while the core stays tough. precision gears the teeth are ground after hardening. Gears are inspected for profile, pitch and runout, on a dedicated measuring machine. In the shop, a span measurement across several teeth, or a measurement over pins, is often used.

The accuracy grade is set by a standard, and the tighter it is, the more expensive the gear. Gears have their typical problems too. Noise and vibration, when the tooth profile or the pitch isn't accurate. Pitting: small pits on the tooth surface, from contact fatigue.

Wear, when the hardening or the lubrication isn't enough. And heat-treat distortion, which changes the geometry. It's best to choose a standard module, which has ready-made tools. below about 17 teeth the tool undercuts the tooth root and weakens it.

Leave room for the tool to run out near a shoulder, or choose gear shaping. And don't demand a higher accuracy grade than you really need. What makes gears expensive? Dedicated machines, and tools that suit a specific module.

Heat treatment, and tooth grinding after it. Inspection on a dedicated measuring machine. sometimes better to buy a standard gear and machine it. Gears need special tools and machines, heat treatment and precise inspection.

That completes the machining group. In the next chapter we'll start sheet metal work: sheet metal fabrication.

11. Sheet metal fabrication

brackets, trays and chassis: they all start as a flat sheet. Fabrication turns flat sheet into parts: cutting, punching, bending, joining and finishing. next chapters we'll expand on some of the processes. Sheet metal is thin relative to its size, usually up to about 6 mm thick.

Above that, we usually talk about plate. In sheet metal work almost no material is removed: the flat shape is cut out, and bent. So it's fast and cheap, and the part's thickness is the same everywhere. The common materials: mild and galvanized steel, stainless steel and aluminum.

when bent to a small radius, so you choose an alloy that bends well, or a larger radius. This is what the typical workflow looks like. The part is designed, and the flat pattern is calculated: the flat shape, before bending. The flat pattern is cut and punched out of a sheet.

It's bent, joined, and finally finished, for example painted or coated. When sheet metal is bent, the inside of the bend is compressed, and the outside is stretched. In the middle there's a layer whose length doesn't change: the neutral axis. During bending, this axis shifts toward the inside.

Its position is described by the K factor, usually between 0.3 and 0.5. So the flat pattern is shorter than the sum of the part's outside dimensions. factor depends on the material, thickness and tooling, so a first part is checked. The flat pattern can be cut in several ways.

A shear cuts straight lines, fast and cheap. A turret punch holds dozens of tools, and punches holes and shapes quickly. It can also form small features, like ventilation louvers. good accuracy, so it suits prototypes and many kinds of parts.

Laser, waterjet and plasma get their own chapters, and punching comes next. Most bends are made on a press brake. A punch presses the sheet into a V-shaped die, and the depth it reaches sets the angle. After bending, the sheet springs back slightly.

So it's bent a little past the required angle. Every material and thickness has a minimum bend radius, and below it the outside cracks. rolling direction of the sheet, because the risk of cracking is lower. We'll expand on bending in chapter 13.

When cylinders and cones are needed, the sheet is rolled between rolls, and that's chapter 14. and stamped in a die, in a single blow or over several stations. We'll expand on that in chapter 15. Sheet metal parts are joined in several ways.

Spot welding joins two sheets at points, with electric current, fast and with no added material. TIG, gives a strong, sealed joint, but heats and distorts the sheet, and often needs grinding. Rivets, including blind rivets installed from one side, join without heat. are pressed into a hole in the sheet, giving a strong thread even in thin sheet.

Sheet metal fabrication has design rules too. A hole too close to a bend line gets distorted. A rule of thumb: keep the hole at least 2.5 times the thickness, plus the bend radius, from the bend. small relief cut is made, so the sheet doesn't tear at the corner.

A flange that's too short isn't held well by the die, and doesn't bend correctly. And it's best to use the same radius on every bend, to work with a single tool. And don't expect machining tolerances: every bend adds deviation. At the end, the edges are deburred, and the part is finished to suit the material and use.

galvanized. Aluminum is anodized, and stainless steel is passivated or polished. Note: paint and coatings add thickness, which matters in holes and in assembly. What makes sheet metal fabrication expensive? The bends: every bend is an operation, and every tool change on the press brake is setup time.

Welding and grinding: a lot of manual work, and sometimes straightening after distortion. Tooling: stamping needs an expensive die, while a laser needs no tooling at all. Material utilization: how many parts fit on one sheet, and how much goes to scrap. And finishing, installing press-in hardware, and tight tolerances.

So how do you choose? For prototypes and small batches: laser and a press brake, with no special tooling. For medium batches: a turret punch, and bending. For large quantities: die stamping, which produces a part with every stroke.

And when the part is thick, massive or very precise, machining is the better choice. In the next chapter: punching.

12. Punching

An electrical cabinet panel has dozens of holes, cutouts and louvers. goes through the sheet and back out in a fraction of a second. In this chapter we'll see how it works, what it delivers, and what makes it expensive. Punching has two parts: a punch on top, and a die below.

clearance, usually 5 to 10 percent of the sheet thickness per side. The punch comes down, presses the sheet, and shears it. burnished band forms, and below it a rough fracture zone. And on the exit side, below the sheet, a burr forms.

Too little clearance wears the tool, and too much clearance makes the burr bigger. When the piece that falls out is scrap, and the hole is what remains, that's piercing. When the piece that falls out is the part itself, that's blanking. The principle is the same; the difference is what you keep.

A turret punch press holds dozens of tools of different shapes and sizes. machine selects a tool and punches thousands of hits per hour. with small, closely spaced hits along the line: that's nibbling. stiffening ribs, extruded collars for tapping, and countersinks.

On some machines the tools rotate, so the same tool can punch at several angles. hole, the sheet thickness and the strength of the material. For example, a 20 mm hole in 2 mm steel needs about 4.5 tons. So in thick sheet or in stainless steel, the force rises fast.

Punching is very fast on holes and shapes that repeat. The accuracy is good, usually around a tenth of a millimeter. And the same machine can also form, which a laser can't do. Punching has design rules too.

than the sheet thickness, and in stainless steel a larger diameter is needed. A hole too close to an edge or to another hole can distort or tear the sheet. It's best to use standard sizes and shapes, which have ready-made tools. And remember that the burr is on one side, and mark on the drawing which side it's allowed on.

Punching has its typical problems too. A large burr, from a worn tool or the wrong clearance. Sheet distortion, when there are many closely spaced holes. Slug pulling: the cut-out piece comes back up with the punch and falls onto the sheet.

And a broken tool, mainly with small holes in thick sheet. What makes punching expensive? Tooling: a standard tool is cheap, but a special shape needs a special tool. Setup time and tool changes.

Nibbling large shapes, which takes many hits. And deburring, and forms that need dedicated tools. So when punching, and when laser? Punching suits many identical holes, batches, and parts that need forming.

Laser suits complex shapes and prototypes, with no tooling. And there are combination machines that punch and laser cut in the same setup. In the next chapter: bending.

13. Bending

Almost every sheet metal part has bends. a flat sheet bends by hand, but after one bend it's already much stiffer. how to reach an accurate angle, and what makes bending expensive. A press brake has a punch on top, and a V-shaped die below.

pushes the sheet into the V, without pressing it all the way to the bottom. The angle is set by how deep the punch goes, so the same die can produce many angles. the bottom of the die. The angle is more accurate, but much more force is needed. moves automatically and sets where the bend line will be.

A rule of thumb: the V opening is about 8 times the sheet thickness. In air bending, the inside radius is set mainly by the V opening, not by the punch. The thicker the sheet, the faster the force rises, and the wider the V, the lower the force. So for thick sheet a wide V is chosen, and the result is a larger radius.

After the punch goes up, the sheet springs back slightly. In aluminum and stainless steel the springback is larger than in mild steel. correct this, and some measure the angle during the bend. The flange must be long enough to rest on both shoulders of the V.

The wider the V, the longer the minimum flange. early bend can collide with the punch or the machine on the next bend. For boxes and deep channels, a gooseneck punch is used, which leaves room for the flange. panel benders, which bend all the sides automatically.

As we saw in chapter 11, the flat pattern is shorter than the sum of the outside dimensions. The CAD software calculates it using the K factor, and a first part is checked and corrected. Bending has its typical problems too. small, or when the bend line runs parallel to the rolling direction.

machine deflects in the middle. This is corrected by crowning. Die marks on the surface. On visible parts, protective film or a special die is used. And a hole close to the bend line, which distorts. A bend angle usually reaches an accuracy of half a degree to one degree.

A dimension between two bends is less accurate than a laser-cut dimension. bends stacks up, so it's best to measure from the same side, and not demand machining accuracy. What makes bending expensive? The number of bends: every bend is another operation.

Tool changes, and a complex bend sequence. Tall flanges and deep boxes, which need special tools. Tight tolerances, and inspections. And large panels, which need two operators.

Bending turns a flat sheet into a stiff part, at the required angle and shape. flanges and a feasible sequence, avoids most of the problems. In the next chapter: plate rolling.

14. Plate rolling

Tanks, large pipes, rings and cones usually start as a flat plate. In plate rolling, the plate passes between rolls, and curves gradually until it closes into a cylinder. A three-roll machine has one top roll and two bottom rolls. the top roll is lowered slightly, and the diameter gets smaller.

On a four-roll machine, an extra roll grips the plate, and the work is faster and more accurate. On a three-roll machine, the ends of the plate stay flat, because they don't pass between all the rolls. So the ends are pre-bent, on a press brake or ona four-roll machine. Without that, after welding there's a flat strip along the seam, and the cylinder isn't round.

a rectangle, and the rolls are tilted relative to each other. It takes more experience, and sometimes a special machine. Here too the plate springs back, so it is rolled gradually and checked. The diameter is checked with a template, or by measuring the circumference.

Finally, the seam is welded along the cylinder. rolled again after welding, to restore the roundness. The minimum diameter depends on the top roll diameter and the plate thickness. Thick, wide plates need a very large, powerful machine.

And hard materials spring back more, and make an accurate diameter harder to reach. Plate rolling has its typical problems too. Flat ends, when they aren't pre-bent. A barrel or hourglass shape, when the rolls deflect in the middle.

Ovality, when the diameter isn't uniform around the circumference. And ends that don't meet exactly at the seam. What makes plate rolling expensive? The thickness and width of the plate, which determine the machine needed.

Pre-bending the ends, and the number of passes. Welding the seam, and re-rolling after it. And roundness and diameter checks. Plate rolling turns a flat plate into a cylinder or a cone, in several gradual passes.

Pre-bending the ends and re-rolling after welding are the key to good roundness. In the next chapter: stamping.

15. Stamping

Car doors, beverage cans, sinks, brackets and electrical contacts. on the sheet, and in a second a finished part comes out. Stamping is the cheapest way to make a sheet metal part, but only in large quantities. dies, deep drawing and embossing, and understand when it pays off.

A mechanical press drives the tool with a flywheel. It's very fast, and suits mass production. over the whole stroke, so it's good for deep drawing. the air, and slow exactly when the tool meets the sheet. Press size is measured in tons, by the maximum force it applies.

The die is the heart of the process. It has a punch on top and a die below, with guide pins that align them precisely. A stripper plate holds the sheet and strips it off the punch after every stroke. expensive, and takes weeks, sometimes months, to build and try out.

A simple die performs one operation per stroke. In a progressive die, a strip of sheet moves through several stations inside the same die. piercing, bending, forming, and finally cutting off the part. station, and pilot holes make sure the strip advances precisely.

So every stroke of the press produces a finished part. each part is cut off at the start, and arms move it between the stations. Deep drawing turns a flat blank into a cup, a box, or the body of a container. material from the flange flows inward to form the walls.

To keep the flange from wrinkling, a blank holder presses on it during the draw. Too little pressure causes wrinkles, and too much tears the sheet near the punch radius. diameter can be about twice the cup diameter, no more. A taller cup needs several draws, one after another.

And beverage cans add ironing: passing through narrow rings that thin the wall and make it longer. Embossing presses a shape into the sheet without cutting it. It creates raised and recessed features: stiffening ribs, markings, a logo. A single rib along a flat panel greatly increases its stiffness, while adding almost no weight.

inside a closed die, giving sharp details and a precise thickness, like on coins. Not every sheet suits stamping: for deep forming, a soft, ductile sheet made for forming is chosen. Stainless steel and aluminum are harder to form, and tend to stick to the die. So oil or a lubricant is used, which reduces friction and prevents scratches.

And here too the sheet springs back, and this is corrected in the die design. Stamping has design rules too. Generous radii at every corner, and at every transition between wall and bottom. corners are better than a deep box with sharp corners.

Holes far enough from formed areas, or they'll distort. And it's best to design the part so all operations are done from the same direction. Stamping is highly repeatable: after a thousand parts, the part still matches the first. Stamping has its typical problems too.

Wrinkles in the flange, when the blank holder pressure is too low. Tearing in the wall or the bottom, when the draw is too deep or the radius too small. Earing on the rim of a drawn cup, because the sheet isn't the same in every direction. Scratches and galling, when lubrication is missing.

And burrs and dimensional changes, as the die wears. What makes stamping expensive? First of all, the die: design, manufacturing and tryout, before the first part comes out. A press big enough for the required force.

Die changes and setup time. And die maintenance, because it wears over time. low, so in quantities of thousands and up, stamping almost always wins. For prototypes and small quantities, laser cutting and a press brake are better.

Stamping turns sheet into a finished part in a second, using a die designed for a single part. The die is expensive, but in large quantities no method is cheaper. That completes the sheet metal group. In the next chapter we'll start the non-conventional processes, with wire EDM.

16. EDM wire

Stamping punches and dies, extrusion dies, hardened gears, and nearly sharp inside corners. All of these can be cut with a thin wire, without the tool touching the part and without cutting forces. This is wire EDM: electrical discharge machining. spark removes metal, what the process delivers, and what makes it expensive.

The wire is one electrode, and the part is the other. Between them there's a tiny gap, filled with deionized water, which doesn't conduct electricity. The machine sends a voltage pulse, and a spark jumps between the wire and the part. The spark melts and vaporizes a microscopic amount of metal, and the water flushes it away.

second, and that's how the wire advances and cuts. The wire is also eroded by the sparks, so it's fed continuously from a spool, and used only once. The wire is usually brass, with a common diameter of a quarter of a millimeter. The only condition: the material must conduct electricity.

Steels, hardened tool steel, carbide, titanium, Inconel, copper and graphite are all suitable. Hardness doesn't matter at all: hardened material cuts almost like soft material. But ceramics and plastics, which don't conduct, can't be cut this way. The table moves in two axes, and the wire runs between an upper guide and a lower guide.

lower one, the wire tilts, so you can cut a taper, or a different shape at the top and bottom. To cut a closed internal shape, a small start hole is drilled first, and the wire is threaded through it. so they can move from shape to shape without an operator. Usually there's one rough cut, followed by several skim cuts.

remove a thin layer and improve accuracy and surface finish. With several skim cuts, an accuracy of a few microns is reached. The kerf the wire leaves is slightly wider than the wire itself, because of the spark gap. So an inside corner will always have a small radius, about half the kerf width.

Speed is measured in area: length x height, in mm? per minute. Tall parts cut slower. surface that melted and resolidified: the recast layer. This layer is hard and brittle, and can contain micro-cracks. important in parts loaded in fatigue, like in aerospace.

The classic application: stamping punches and dies, as we saw in chapter 15. Also extrusion dies, gears and splines in hardened parts. Keyways in a part that has already been hardened. Small, precise parts, and very thin walls, because there are no forces to bend them.

And nearly sharp inside corners, which milling can't produce. Wire EDM has design rules too. only through shapes can be cut. A blind pocket needs sinker EDM, in the next chapter. An internal shape needs a start hole, and room for it.

a small tab is sometimes left, and removed at the end. it's needed, because every extra skim cut is more time. Wire EDM has its typical problems too. Wire breakage, from poor flushing or too much power.

stresses are released, mainly in hardened material. Deviation along the height, when the wire vibrates or isn't tensioned enough. And a recast layer that wasn't removed, which weakens the part. What makes wire EDM expensive?

Mainly time: the process is slow, and one part can take hours. The area to cut, meaning length times height, and the number of skim cuts. Wire, water, and machine maintenance. And start holes and preparation.

On the other hand, the machine can run unattended all night, which lowers the cost a lot. And for hardened or complex parts, there's no real substitute. hardness, to an accuracy of microns, with no forces. It's slow, so it's used where other processes can't do the job.

In the next chapter: sinker EDM.

17. EDM sinker

An injection mold cavity, deep narrow ribs, and a blind pocket with sharp corners in hardened steel. Milling can't reach there, and wire EDM can't cut a blind pocket. In sinker EDM, a shaped electrode sinks into the part, and sparks remove the material. In this chapter we'll get to know the electrode, the process, and what makes it expensive.

The principle is the same as wire EDM: sparks across a tiny gap melt and vaporize the material. But here the electrode is a full shape, the mirror image of the cavity you want to produce. conduct electricity, and the oil flushes the particles away. A servo system holds the gap, and the electrode slowly descends into the material.

electrode moves in a small circle, enlarging the cavity under control and improving flushing. The electrode is usually made of graphite or copper. Graphite is light, relatively cheap, and machines fast, so it's common in large molds. Copper gives a better surface finish and finer detail.

spark gap, and that gap differs between roughing and finishing. usually there's one electrode for roughing, and one or two more for finishing. Blind pockets of any shape, at any reasonable depth, in hardened material. Sharp inside corners, as sharp as the electrode allows.

Deep, narrow ribs that no milling cutter can reach. And uniform matte surfaces, which serve as the final finish of the product in molds. shaped like a thin tube, with water flowing through it. This drills small, deep holes fast in hard materials.

It's used for start holes for wire EDM, and for cooling holes in turbine blades. Here too, a thin recast layer is left on the surface, with micro-cracks. In sensitive parts it's removed by fine finishing or polishing. Plastic injection molds are the most common application.

Die-casting and forging dies, as we saw in chapters 1 and 2. Pockets and slots in hardened parts, after heat treatment. And in aerospace, parts made of especially tough alloys. Sinker EDM has design rules too.

electrode, so it's best to give a radius wherever possible. Think about how the electrode will enter, and how the oil will flush the cavity. drawing, because a finer finish takes more time and more electrodes. Sinker EDM has its typical problems too.

Electrode wear, which rounds corners and changes dimensions. process unstable and leaves burn marks on the surface. And wrong dimensions, when the spark gap wasn't calculated correctly. What makes sinker EDM expensive?

The electrodes: design, milling and inspection, and sometimes that's the most expensive part. Time: the process is slow, and one cavity can take hours, even days. The number of electrodes, depending on the number of corners and the required finish. On the other hand, the machine runs unattended, and in a hardened part there's no substitute.

Sinker EDM copies the shape of the electrode into the material, at any hardness. blind pockets and sharp corners in hardened material, there's no substitute. In the next chapter: laser.

18. Laser

Sheet metal parts of any shape, straight from the drawing, with no tooling and no dies. This is laser cutting, one of the most common processes in shops today. light cuts metal, what the laser delivers, and what makes it expensive. A laser beam is focused to a tiny spot, where the energy density is enormous.

The metal melts, and sometimes vaporizes, along the cut line. An assist gas blows the molten metal out through the kerf. metal and adds heat, so cutting is fast, but the edge oxidizes. nitrogen is used: the edge is clean and bright, but gas consumption is high.

And compressed air is a cheap compromise, for thin sheet. efficient, fast, and able to cut even copper and brass, which reflect light. still common for cutting wood, acrylic and non- metals. Steel, stainless steel and aluminum, from thin sheet of half a millimeter up to thick plate.

Powerful machines cut steel 25 millimeters thick and more. The kerf is very narrow, usually tenths of a millimeter. The accuracy is good, usually around a tenth of a millimeter. And the heat-affected zone is narrow, because the heat is concentrated.

On a flatbed machine, the cutting head moves over the sheet, and the motion is CNC controlled. Nesting software arranges the parts on the sheet to leave as little scrap as possible. A pallet changer lets a new sheet be loaded while the machine is cutting. Tube lasers also cut holes and slots in the walls of tubes and profiles.

Fine striations can be seen on the edge, and in thick sheet they're more pronounced. At the bottom, resolidified molten metal can remain: dross. Where the beam pierces the sheet, a small mark is left. And in thick sheet the edge is slightly tapered.

Marking and engraving: serial numbers, logos and codes, with no contact and no ink. Laser welding: a narrow, deep seam, with little distortion. And advanced uses, like cladding and metal 3D printing. Laser cutting has design rules too.

with lower quality, and in thick sheet it's better to drill it. Very small details overheat and can burn. Tiny connections, microjoints, are left to hold the parts in the sheet until cutting is done. Parts with a common line can be cut with a single cut, saving time and material.

oxide layer on the edge, which can interfere with paint and welding. Laser cutting has its typical problems too. Dross at the bottom of the cut, when the gas or the focus isn't right. Burning at sharp corners in thick sheet.

Heat distortion of thin or small parts. And reflective materials, which need a suitable laser. What makes laser cutting expensive? Machine time: the cut length, the sheet thickness, and the number of pierce points.

Gas, mainly nitrogen in large quantities. Sheet utilization: how well the parts are nested on it. And removing dross and burrs, if needed. But with no tools or dies, laser suits prototypes and small to medium batches.

A laser cuts almost any shape from sheet, fast, accurately, and with no tooling. Thickness, gas and cut length set the price. In the next chapter: waterjet cutting.

19. Waterjet cutting

Rubber, stone, glass, composites, titanium and thick aluminum plate. All of them can be cut on the same machine, with water. cuts, what it delivers that no other process does, and what makes it expensive. A pump pressurizes water to an enormous pressure, around 4,000 bar.

The water exits through a tiny orifice in a jewel, and becomes a thin, very fast jet. A pure water jet cuts soft materials: rubber, foam, gaskets, and even food. To cut metal, stone or glass, an abrasive sand is added to the jet, usually garnet. The sand mixes with the water in a narrow tube, and it's the grains that do the cutting.

It's a cold process: no heat-affected zone, no hardening, and no heat distortion. So it suits heat-sensitive materials, like titanium, hardened steel and composites. It cuts almost any material, even very thick, sometimes more than 100 millimeters. And there are no tools: like laser, you go straight from the drawing to the cut.

In thin sheet, waterjet cutting is much slower than laser. The kerf is wider, usually around a millimeter. out tapered, and the jet lags behind and rounds corners at the bottom. Advanced heads tilt the jet and correct the taper.

Good accuracy is around a tenth of a millimeter. And it's a wet, noisy process, with sand to clear away. The part sits over a water tank, which absorbs the jet after it passes through. The cutting head moves under CNC control, and on some machines it also tilts, to cut bevels.

And the cutting speed is chosen by the material, the thickness, and the required edge quality. Gaskets, rubber and foam. Stone and glass countertops. Thick plates of aluminum and titanium.

Composites in aerospace. And hardened steel parts that mustn't be heated. Waterjet cutting has design rules too. An inside corner will always have a radius, about half the kerf width.

In thick parts, account for the taper, or ask for taper correction. risky, because the material can crack at the pierce point. And small parts can drop or tip over, so tiny tabs are left. Waterjet cutting has its typical problems too.

Taper and rounded corners at the bottom, when the cutting speed is too high. A frosted edge on the side where the jet enters. Delamination in composites, at the pierce point. And flash rust on steel that sat in the water.

What makes waterjet cutting expensive? Machine time, which depends heavily on thickness and edge quality. The abrasive, which is usually the largest running cost. Maintenance of the pump, seals and orifices, which work at enormous pressure.

On the other hand, there are no tools, so it suits even a single part. Waterjet cutting suits almost any material, at any reasonable thickness, with no heat. isn't allowed, or the material is special, it's the choice. In the next chapter: plasma.

20. Plasma

Thick steel plate for bridges, ships and heavy machinery. To cut it fast and cheaply, plasma is used. what it delivers, and where it beats laser and waterjet. Inside the torch there's an electrode, and an electric arc forms between it and the part.

Gas is forced through a narrow nozzle, and the arc heats it to more than twenty thousand degrees. At that temperature the gas becomes plasma: an ionized gas that conducts electricity. The plasma melts the metal, and the strong gas flow blows it out. Because the arc passes through the part, the material must conduct electricity.

The gas can be air, oxygen, nitrogen, or special mixtures, depending on the material. cheap and simple, and there are handheld units too. High-definition plasma constricts the arc, giving a better edge and higher accuracy. And there's also underwater cutting, which reduces noise, smoke and distortion.

Steel, stainless steel and aluminum. It works best on plates from a few millimeters up to several tens of millimeters. In thick plate it's much faster than laser and waterjet, and the machine is cheaper. In thin sheet, a laser gives a better result.

The edge comes out slightly beveled, usually a few degrees. The heat-affected zone is wider than with a laser. Dross can remain at the bottom. Accuracy is usually around half a millimeter, and better with high-definition plasma.

And a hole smaller than the plate thickness doesn't come out well, so it's better to drill it. Steel structures and bridges. Shipbuilding and heavy equipment. Preparing weld bevels, with a tilting head.

And cutting pipes and profiles. Plasma has design rules too. Surfaces that must be precise are given a machining allowance. The cut edge hardens from the heat, which can make later machining or bending harder.

Small, precise holes are drilled, not plasma cut. Plasma has its typical problems too. A beveled edge, when the speed or torch height isn't right. Dross at the bottom, when the speed is too low or too high.

Falling quality, as the electrode and nozzle wear. And heat distortion of thin plates. What makes plasma cutting expensive? Consumables: electrodes and nozzles, which need frequent replacement.

Gas and electricity. Cleaning off dross and grinding the edge. And machining allowance, when accuracy is needed. On the other hand, for thick steel plate, it's the cheapest way to cut.

Plasma cuts thick metal plate fast and cheaply, with moderate accuracy. That completes the non-conventional group. In the next chapter we'll start the advanced group: 5-axis milling.

21. 5-axis milling

Impellers, turbine blades, aircraft structural parts, molds and medical implants. Parts like these have complex surfaces that must be reached from every side, at every angle. On an ordinary milling machine that takes many setups, many fixtures, and long tools. With 5-axis milling, most of the work is done in one setup, with short tools and high accuracy.

two working methods, what happens behind the scenes, and what it costs. An ordinary milling machine has three linear axes: X, Y and Z. 5-axis milling adds two rotary axes. The A axis rotates around X, the B axis around Y, and the C axis around Z.

Each machine has two of them, depending on its configuration. the table: the table tilts, and on it sits a rotating table, a trunnion. medium parts: it's rigid and accurate, and the part turns to face the tool. The drawback: the table has to tilt the full weight of the part, so it's limited in size.

head: the head tilts and rotates, and the part stays put. This is the configuration for large, heavy parts, like aircraft structural parts and large molds. and one in the head, a combination of the two approaches. The most common method is called 3+2.

locks the rotary axes, and mills in three ordinary axes. Then it tilts to the next angle, and continues. setup, and only the side the part is held by remains. 3+2 suits angled holes, surfaces at angles, and box parts with many sides very well.

is rigid, because the rotary axes are locked during the cut. In the simultaneous method, all five axes move together, continuously, while cutting. This way the tool follows a curved surface, and keeps a constant angle to it all the way. This is essential for impellers, blades, and any free-form surface.

cutting moves to a better zone of the ball, and the surface improves. the full height of the wall, and get a smooth wall in one pass. of a large circle, barrel cutters, which allow wide passes with a good finish. When a rotary axis moves, the tool tip moves with it in space.

constantly calculates the linear motions that compensate for the rotation. point management, and it lets the path be programmed by the tool tip, not by the machine. where its pivot centers are, so it's calibrated regularly. and 5-axis programming is more complex and takes experience.

translates the path into commands that specific machine understands. There's a risk of collision between the tool, the holder, the head, the table, the part and the fixture. So a full simulation of the machine, with its real model, is run before every cut. rotary axes, and zones where the machine has to rotate very fast to pass a certain point.

In 5-axis milling, the workholding must leave access from every direction. So the part is raised on a narrow fixture, so the head and the tool don't collide with the table. move between machines without losing its position. And often the part is machined from a solid block, leaving a small base that's cut off at the end.

Because everything is done in one setup, the relation between surfaces is more accurate. But the errors of the rotary axes add up, so calibration matters. Heat changes the machine during work, and advanced machines compensate for it. machining, and checks dimensions along the way, without removing it.

Fewer setups: every additional setup can add error, aS we Saw in chapter 5. doesn't need to be long to reach the depth, so it's more rigid and vibrates less. Access to undercuts and angled surfaces that can't be reached in three axes. Better surfaces, and less manual finishing.

And fewer fixtures, fewer transfers between machines, and a shorter lead time. Impellers and blisks: a disc and blades from a single block. Turbine blades, with curved surfaces and thin walls. Aircraft structural parts, with deep pockets and angled walls.

Molds with deep cavities, where a short, tilted tool replaces a long, vibrating one. Medical implants, and bodies with holes at many angles. 5-axis milling has design rules too. Not every part needs 5 axes: if three axes are enough, it's cheaper.

each surface from, and don't create a surface no tool can reach. Plan datums and tolerances so they can be machined in the same setup. needed, because it's the most expensive to program and inspect. 5-axis milling has its typical problems too.

Collision, when the simulation doesn't match the real machine. Marks on the surface, when the rotary axes move in jerks. Dimensional errors, when the machine isn't calibrated. And chatter in thin walls, even with a short tool.

What makes 5-axis milling expensive? The hourly rate is higher, because the machine is far more expensive. Programming and simulation time, which on a first part can be longer than the machining itself. A first part that needs to be inspected and tuned.

Special tools and holders. On the other hand, you save setups, fixtures, transport between machines, and waiting time. So it pays off mainly on complex, expensive parts, in small and medium quantities. 5-axis milling reaches almost any surface, in one setup and with short tools.

3+2 for parts with many sides and angles, and simultaneous for curved surfaces. calibration and workholding, not just on the machine. In the next chapter: mill-turn and Swiss-type.

22. Mill-turn and Swiss-type

A shaft with flats, a keyway and cross holes. A tiny medical screw. A long, slender hydraulic pin. These are round parts, but they also need milling and drilling. milling machine, they're made on a single machine. machines: the mill-turn center, and the Swiss-type lathe.

rotating tools, driven by their own motor inside the turret. The C axis lets the part stop at a precise angle, or rotate slowly during milling. This makes it possible to mill flats and hexes, and to drill cross holes and off-center holes. and pockets that don't pass through the center of the part.

A sub spindle grips the part after parting off, and machines the back side. This way a completely finished part comes out, without anyone touching it. Large machines also have a tilting milling head, the B axis, combining a lathe with 5-axis milling. One setup, so the holes and flats are accurate relative to the axis of rotation.

Fewer transfers between machines, fewer fixtures, and fewer parts waiting between stations. With a bar feeder, the machine can run unattended for many hours. Live tools are weaker and less rigid than the spindle of a machining center. So heavy milling and hard materials are better done on a milling machine.

collision between the turret, the spindles and the part. And the machine is more expensive than an ordinary lathe. Swiss-type is a different kind of lathe, born in the Swiss watch industry. On an ordinary lathe, the part rotates in place and the tool moves along it.

and forth through a guide bushing, which supports it. the part is supported just a few millimeters from the cutting point. twenty times longer than their diameter, without bending. Swiss machines usually work with bar stock up to 32 millimeters in diameter.

They have many fixed tools, live tools, a sub spindle, and many axes working at the same time. And they reach accuracy of microns, in mass production. The bar must be ground to a precise diameter, so it slides smoothly in the bushing. The material left in the bushing at the end of the bar goes to scrap.

For short parts there's a mode without the bushing, which saves scrap. diameter: a very large flange doesn't suit Swiss- type. Medical and dental screws and implants. Connectors and pins for electronics.

Parts for watches and precision instruments. Hydraulic pins, shafts and valves. And on mill-turn centers: shafts, bushings, valve bodies, and flanges with holes. A simple round part, with no milling: an ordinary lathe.

A round part with flats, slots and holes: a mill-turn center. A small, long, slender part, in large quantities: Swiss-type. And a large part, complex from every side: a mill- turn with a B axis, or 5-axis milling. There are design rules here too.

Design holes and flats so the live tools can reach them. Use standard sizes of holes, threads and slots. On Swiss-type, keep the largest diameter of the part close to the bar diameter. And cross holes that meet inside the part leave a burr, so plan how it will be removed.

These machines have their typical problems too. mainly in soft materials, so good chip breaking is needed. Chatter when milling with weak live tools. On Swiss-type: a worn bushing, or an inaccurate bar, causing diameter errors.

And dimensional drift in long runs, because of heat. What makes work on these machines expensive? The price of the machine and the hourly rate. Programming and setup time, especially on Swiss- type, where there are many tools to set.

So in small quantities, the setup can cost more than the machining. are no secondary operations, and in large quantities the cost per part is very low. A mill-turn center produces a complex round part, completely finished, in one setup. parts, with micron accuracy and in large quantities.

In the next chapter: honing and lapping.

23. Honing and lapping

A hydraulic cylinder, an engine cylinder, a gauge block, and a valve sealing face. All of these need a surface more precise and smoother than ordinary grinding delivers. This is where two fine finishing processes come in: honing and lapping. Honing is used mainly to finish bores.

The honing head carries several abrasive stones, which expand outward and press on the bore wall. The head rotates and at the same time strokes up and down. The combination creates a pattern of crossing lines on the wall, a crosshatch. In an engine cylinder, these lines hold oil, and help the piston move freely.

Honing removes very little material, usually a few hundredths of a millimeter, with low heat. Honing corrects the geometry of the bore: roundness, cylindricity and straightness. It gives a very precise diameter, and a smooth surface, usually an Ra of 0.1 to 0.4 microns. But, like a reamer, it follows the axis of the bore, and doesn't correct its position.

that flattens the peaks and leaves the valleys for oil. during the work, and the process stops exactly at size. surfaces that must be flat and parallel to the highest level. Between the part and a lap plate, usually cast iron, there's a slurry of abrasive grains in a liquid.

The part moves over the plate in a constantly changing path, so every point wears evenly. The grains roll and remove material at the level of microns. The result: flatness measured in fractions of a micron, and a very smooth surface. Flatness is checked with an optical flat, which shows bands of light on the surface of the part.

In double-sided lapping, both sides of the part are processed together, giving excellent parallelism. It's important to tell lapping apart from polishing. Polishing improves shine and smoothness, but doesn't correct the form. Lapping improves the form itself: flatness, parallelism and size.

Honing: hydraulic cylinders, engine cylinders, gear bores, and injector parts. Lapping: sealing faces of mechanical seals, valve seats, gauge blocks, and optical surfaces. A small allowance is left, usually a few hundredths of a millimeter. The previous process must be good: honing and lapping correct a little, and can't save a bad part.

the drawing, and for honing, the crosshatch angle if it matters. And cleaning is very important: grains left on the part can ruin the assembly. There are typical problems here too. A bore that opens up at the ends, bell mouth, when the stroke overruns the bore too much.

A tapered bore, when the stroke isn't balanced. Grains embedded in soft material. In lapping: rounded edges, and scratches from an oversized grain that got into the slurry. What makes honing and lapping expensive?

The processes are slow, and remove very little each time. Precise measurement, sometimes in a climate- controlled room. Thorough cleaning of the part after the work. On the other hand, lapping many parts together on one plate lowers the cost a lot.

And often, it's the only way to reach the required geometry and finish. Honing finishes bores, giving them precise geometry and a pattern that holds oil. Lapping finishes surfaces, giving flatness and parallelism at the level of fractions of a micron. In the next chapter, the last in the series: additive manufacturing.

24. Additive manufacturing

So far we've seen processes that remove material, form it, or cast it. In additive manufacturing, the part is built layer by layer, adding material only where it's needed. structures, and single parts replacing whole assemblies. methods, the processing after printing, and what makes it expensive.

We start from a 3D model of the part. Software slices the model into thin layers, and calculates the shape of each layer. The machine builds one layer, lowers or moves the part, and builds the next layer on top of it. metals three main ones: powder bed fusion, directed energy deposition, and binder jetting.

This is the most common method for precise metal parts. A recoater spreads a thin layer of metal powder, a few tens of microns thick. A laser beam melts the powder only in the shape of the current layer. The build platform lowers by one layer thickness, a new layer is spread, and the cycle repeats.

Everything happens in an inert gas atmosphere, usually argon, so the metal doesn't oxidize. Surfaces that overhang at too steep an angle need supports. The supports also conduct heat away, and hold the part so it doesn't warp. The part is fused to the build plate, and at the end it's cut off, often by wire EDM.

There's also an electron beam version, ina vacuum, which suits titanium especially well. is fed straight into a melt pool, created by a laser or an electric arc. The head moves and builds the part, like welding, layer on layer. The method is fast and suits large parts, but it's less accurate.

So the part is built close to its final shape, and then machined. It's also used to repair expensive parts, like turbine blades and molds. In binder jetting, a print head jets binder onto a layer of powder, without melting it. Then the part is sintered in a furnace, and the particles fuse together.

During sintering the part shrinks, by about 20 percent, and the design must compensate for that. The method is faster and cheaper, and suits batches of small parts. There are several methods in plastics too. FDM extrudes a molten plastic filament, and it's common in every shop.

SLA cures a liquid resin with light, and gives fine detail. And SLS melts nylon powder, giving strong parts with no supports. In the shop, the common uses are prototypes, and fixtures and gauges for production. The part that comes out of the machine isn't finished yet.

First, a stress-relief heat treatment is done, even before it's cut off the plate. Then the supports are removed, by hand or by machining. For critical parts, HIP is used: high pressure and high temperature, which close internal porosity. The surface is rough, usually an Ra of 5 to 15 microns, so functional surfaces are machined.

scan, which also sees porosity and internal channels. channels, lattices, and surfaces that can't be machined. wherever it doesn't carry load, and the part gets lighter. Part consolidation: an assembly of ten parts can become a single part.

No tools and no molds, so you can change and try things quickly. channels that follow the shape of the part greatly shorten the cycle time. The process is slow, and part size is limited by the machine size. The cost per part is high, and doesn't drop much with volume.

The properties can differ in different directions, depending on the layer direction. There's a risk of porosity, internal stresses and distortion. And in aerospace and medical, qualifying a printed part takes a lot of testing. Additive manufacturing has its own design rules too.

Surfaces up to about 45 degrees from vertical are built without supports. Avoid large flat surfaces hanging in the air. Internal cavities need holes to remove the powder. A uniform wall thickness is better, so heat spreads evenly.

The orientation of the part in the machine affects time, supports, surface finish and strength. And on functional surfaces, a machining allowance is left. What makes additive manufacturing expensive? Machine time, set mainly by the build height, meaning the number of layers.

The powder, and the inert gas. Post-processing, which can reach half the cost. And inspection, especially for critical parts. On the other hand, several parts in the same build share the machine time.

complex parts, in small quantities, or when there's no other way to make the shape. Additive manufacturing doesn't replace the processes we've learned; it joins them. shape, and finish by 5-axis milling, turning, grinding or EDM. Additive manufacturing builds a part layer by layer, giving design freedom no other process has.

It's slow and costly per part, but on the right part it changes the whole picture. casting and forging, through machining and sheet metal, to the advanced processes. For every process, we saw what it delivers, how to design for it, and what makes it expensive. And the right choice is always a balance of shape, material, accuracy, quantity and cost.