Transcript: Drawing Reading

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. The Drawing as a Contract

On the table lies a drawing of a single part: several views, dozens of dimensions, symbols, notes and a title block. Most people see it as a picture of the part. Someone who reads drawings at a high level sees something completely different: a contract.

In this course we will learn to read that contract all the way through: what it requires, what it allows, and what it does not say at all. Every drawing has at least three parties who read it. The designer writes in it what the part must do.

The manufacturer reads in it what he is allowed to make. And the inspector reads in it the basis for accepting or rejecting the part. If all three read the same drawing and understand the same thing, the drawing has done its job. If each one understands something different, the argument will

come in the end, usually when the parts are already finished. A part that meets every requirement on the drawing is a conforming part, even if it does not work in the assembly. And a part that exceeds a single requirement, even by a hundredth

of a millimeter, is a rejected part, even if it works perfectly. That sounds harsh, but it is the principle that lets a manufacturer on one side of the world make a part that will be assembled on the other. So when a conforming part does not work, the problem is

in the drawing, and the drawing is what gets corrected. And when a rejected part still has to be used, that is a formal decision by whoever is responsible for the design, not a decision of the shop floor. One of the basic rules in ASME Y14.5 is that the drawing

defines the part, without dictating how to make it. The drawing says that a hole must be ten millimeters in diameter, with a certain tolerance and at a certain location. It does not say whether to drill it, mill it or ream it.

The decision of how to make it belongs to the manufacturer. That is what lets him choose the cheapest and fastest process that still meets the requirements. There are exceptions: when the process itself determines the properties of the part, such as heat treatment, coating or welding, the drawing refers to a specification that defines it.

A good drawing reader asks about every requirement: does it define the part, or does it dictate a method to me? And a method is binding only when it is written on the drawing explicitly. One of the things that sets an advanced reader apart is that he also reads what is not written.

A dimension with no tolerance next to it is not a dimension without a tolerance. It takes the general tolerance from the title block or from a general note. All dimensions on the drawing apply at a temperature of twenty degrees Celsius, even if that is not written anywhere.

They apply to the part in its free state, without clamping, unless stated otherwise. And the standard named in the title block defines dozens of rules that are not drawn, and those rules differ from standard to standard. That is why exactly the same drawing can be interpreted differently under

ASME and under ISO, and we will see this in detail later in the course. Another basic rule: you do not measure dimensions from the picture itself. Even when the drawing looks accurately to scale, a dimension that is not written on it is not defined, and you must not fill it in with a ruler.

And if a dimension needed for manufacturing is missing, that is not an invitation to guess. It is a question for the designer. A good drawing defines every characteristic of the part once, in one way, and without contradictions. A dangerous drawing is not necessarily a drawing with an obvious mistake.

Often it is a drawing that can be read in two ways. A duplicated dimension, an undefined surface, a note that contradicts a dimension, or a tolerance that cannot be measured: each one is an opening for an argument. A large part of this course is aimed at exactly that: spotting these openings before they cost money.

The course is built in six parts. In the first part we revisit representation itself at an advanced level: projection systems, sections, conventions and spatial thinking. In the second part we go deep into dimensions and tolerances:

dimensioning philosophy, general tolerances, the envelope principle versus the independency principle, fits and tolerance stack-ups. In the third part we read geometric tolerances within the complete drawing, through the eyes of the datum reference frame.

In the fourth part we cover everything beyond geometry: surface texture, welding, material, heat treatment, coating, threads and special features. In the fifth part we read the drawing as a document: the title block and notes, assembly drawings, critical characteristics, model-based definition and change management.

And in the sixth part we bring it all together: we read drawings through the manufacturer's eyes, find errors, and build a fixed reading method for any drawing. The basis of the course is ASME Y14.5 from 2018, the standard most common in industry. Wherever ISO differs from it in a significant way, we will stop and look at

the difference, because in real work drawings arrive under both standards. All the drawings in the course were built specifically for it. They are engineering-correct parts, but they do not belong to any product or company. A drawing is a contract between the designer, the manufacturer and the inspector.

It defines the part, not the process; it is binding even in what it does not say; and you do not measure from it with a ruler. In the next chapter we start from the basis of every drawing: how a three-dimensional body is transferred

onto a flat sheet, and why confusing the projection angle can turn an entire part into its mirror image. See you in chapter one.

1. Projection Systems

A mechanical part is three-dimensional, and the sheet is flat. Every drawing starts with one question: how do you transfer the part onto the sheet without losing any information? The answer is orthographic projection, and two different systems for arranging the views.

In this chapter we will understand both of them in depth, and see how confusing them produces a part that is the mirror image of what was designed. In orthographic projection, the lines of sight are parallel to each other and perpendicular to the projection plane.

So every view shows only two dimensions: width and height, or width and depth, and never all three. A surface parallel to the projection plane appears in its true size and shape. A surface perpendicular to the plane appears only as a line. And an inclined surface appears foreshortened: it looks smaller than it really is.

That is another reason not to measure from the picture: a length that appears on the sheet is not necessarily the true length. Imagine the part inside a glass box, with one view projected onto each of its six sides. When the box is unfolded onto the sheet, there are two ways to arrange the views,

and that is the whole difference between the two systems. In third-angle projection, common in the United States and in ASME standards, the projection plane is between the eye and the part. So each view is drawn on the side it is viewed from:

the top view above the front view, and the right- side view to its right. In first-angle projection, common in Europe and in ISO standards, the part is between the eye and the projection plane. Then each view is drawn on the opposite side:

the top view below the front view, and the right- side view to its left. systems. Only their position on the sheet is different. And someone who knows only one system will read the other one backwards, without noticing. To remove any doubt, the title block includes a symbol that defines the system.

The symbol is a truncated cone in two views: a side view, which looks like a trapezoid, and an end view, which looks like two circles. The two circles are the view from the narrow end of the cone. In third angle, the circles are drawn next to the narrow end, and the trapezoid points toward them.

the wide end, and the trapezoid points away from them. That is how you identify the system correctly, even if the symbol was drawn mirrored or in an unexpected place. Sometimes, instead of a symbol, the system is written out in words.

Suppose a first-angle drawing arrives, and it is read by someone used to third angle. The part is a plate with a tall wall along the back edge, and a hole near the front right corner. In first angle, the top view is drawn below the front view, and the side closest to the front view is the back of the part.

bottom view, and understands the near side as the front. The result: the wall moves to the front, and the hole moves to the back. The part that is made is the mirror image of what was designed. And the dangerous part: the views stay consistent with each other,

so nothing on the drawing looks wrong. nothing. On a non-symmetrical part it scraps the entire batch. What do you do when a drawing arrives with no symbol and no note? First check the title block and the general notes.

Sometimes the system is defined there, or in the standard the drawing refers to. Then check whether a 3D model is attached to the drawing, and compare against it. But do not rely on the views looking illogical. As we saw, the reversed interpretation is completely consistent.

And if there is still doubt, ask the designer. On a non-symmetrical part, a guess is a bet on the entire batch. The front view does not have to be the front of the part. It is the view that describes the shape best. It is chosen so that it has the fewest hidden lines,

usually in the orientation in which the part is assembled or machined. The number of views is the minimum that defines the part completely. A turned part, such as a shaft, is often defined in a single view, and the diameter symbol replaces the end view.

An unnecessary view is not just wasted space. It is one more place where dimensions can contradict each other. What happens when a part has an inclined surface that is not parallel to any of the three principal planes?

In all the regular views it appears foreshortened, and a hole on it looks like an ellipse. Here we use an auxiliary view: a view projected onto a plane parallel to the inclined surface. In the auxiliary view the surface appears in its true size and shape, and the hole looks round. The auxiliary view is drawn in line with the direction of sight onto the surface,

from the view in which the surface appears as a line. a partial auxiliary view, so as not to clutter the drawing. When a full view is not needed, a partial view is drawn, cut off with a break line. A local view shows only one feature, such as a keyway or a slot, without drawing the whole part.

A detail view marks a small area with a circle and a letter, and draws it separately at a larger scale, for example two to one. And the dimensions in the detail view are still the true dimensions, not the enlarged ones. A view moved from its natural position must be identified: an arrow with a letter

that shows the viewing direction, and the same letter next to the view itself. A view that was moved without being identified is an error in the drawing, because it breaks the rules of projection. Orthographic projection shows two dimensions in each view,

and inclined surfaces appear foreshortened. In third angle the view is drawn on the side it is viewed from. In first angle, on the opposite side. Before reading a single view, check the projection symbol, and if there is no symbol, ask. In the next chapter we will cut the part: advanced sections,

and what each type of section reveals and hides. See you in chapter two.

2. Advanced Sections

A regular view shows the part from the outside. Everything inside appears as hidden lines. In a complex part, the hidden lines pile up on top of each other, and they cannot be read. The section view solves this: the part is cut by an imaginary plane, the near portion is removed, and we look inside.

In this chapter we will get to know the types of sections, their conventions, and what each section reveals and what it hides. Every section starts with the cutting-plane line, drawn in the adjacent view. It shows where the cutting plane passes, and the arrows at its ends show the viewing direction.

The letters at the ends identify the section, for example A, and the section itself is called section A-A. line. Without it, you do not know what you are looking at. The direction of the arrows determines what remains in the view:

the portion the eye sees, not the portion that was removed. A cut surface is marked with hatching: thin parallel lines, usually at 45 degrees. What lies behind the cutting plane is drawn with regular lines, and what is hidden is usually not drawn at all.

A single part has the same hatching in every section on the drawing. In an assembly, adjacent parts get hatching at a different angle or a different spacing, so it is clear where one part ends and the next begins. The hatch pattern does not define the material.

The material is defined in the title block or in the parts list. And a very thin part, such as a gasket or sheet metal, is sometimes shown solid filled instead of hatched. In a full section, the plane passes through the entire part, usually along the axis of symmetry.

On a symmetrical part you can save effort: a half section removes only a quarter of the part, and the view shows half cut and half from the outside. That way one picture shows both the external shape and the internal one. The boundary between the two halves is a center line,

not a solid line, because there is no real edge there. And on the uncut half, hidden lines are not drawn, because the cut half already shows them. Sometimes the important features do not lie in the same plane. In an offset section, the cutting-plane line changes direction

at right angles and passes through all the features. In the section itself everything is drawn as if it were cut in a single plane, and the bends in the cutting-plane line are not shown. So someone who reads the section without checking the

cutting-plane line may think all the features lie in one row. On a round part, such as a flange, the holes usually sit on a bolt circle, not opposite each other. In an aligned section, the cutting-plane line passes through the holes at an angle, and the inclined portion is then rotated into the plane.

That way the holes appear in the section at their true distance from the center. And this is an important point: such a section is not a true projection. It deliberately departs from the rules of projection to show what matters. A flange with three holes, 120 degrees apart,

will look in the section as if it had holes on both sides of the center. The number of holes and their angular position are read in the front view, not in the section. Some things are not hatched even when the plane passes through them. A rib or a thin web cut lengthwise is not hatched,

because hatching would give the impression of a solid, heavy part. nuts, pins, keys and balls are not sectioned lengthwise. They are drawn whole, even when the plane passes exactly through their axis. Someone who does not know this convention may think the

bolt was not cut at all, or that the rib does not exist. And on a part with ribs or spokes that are not on the cutting-plane line, they too are rotated into the plane, as in an aligned section. When only a small internal area needs to be shown, a broken-out section is used.

A small portion of the view is removed and bounded by a freehand break line. A revolved section shows the cross-sectional shape of a long feature, such as a spoke or an arm. It is rotated ninety degrees and drawn on the view itself. A removed section is the same idea, but it is drawn outside the view,

identified with letters, and sometimes at a larger scale. A section reveals the inside, but only where the plane passed. A hole outside the plane will not appear in the section. And since hidden lines are not drawn, it will not appear as a hidden line either.

So a section is never a complete picture. It is read together with the other views. And when a feature seems to be missing, first check whether it simply does not lie in the cutting plane, before assuming it does not exist. Before every section: find the cutting-plane line and the direction of the arrows.

they were in the same plane, even when they are not. Ribs, shafts and bolts cut lengthwise are not hatched, and that is a convention, not a mistake. And whatever is not in the plane does not appear in the section. The section complements the views; it does not replace them.

In the next chapter we will get to know the conventions and simplifications of the drawing: threads, gears, springs, repeated features, and where the drawing simplifies on purpose. See you in chapter three.

3. Conventions and Simplifications

A drawing does not try to be an accurate picture of the part. Accurately drawing every thread form, every gear tooth or every coil of a spring would take hours, and would add no information. So the drawing uses conventions: a shortened,

agreed representation that describes the feature without drawing it. In this chapter we will get to know the important conventions, and the principle behind all of them: when the picture is simplified, the information is in the callout. On an external thread, according to ISO, the major diameter is

drawn with a thick line and the root diameter with a thin line. In the end view, the root diameter is drawn as three quarters of a thin circle, so it will not be confused with a hole or a chamfer. A thick line marks the end of the full thread.

In ASME standards, in the simplified representation, the root diameter is sometimes shown as a hidden line, so you need to know which standard the drawing follows. In all cases, the picture does not define the thread. The callout defines it: type, diameter, pitch and tolerance class.

On an internal thread the picture is reversed: the tap drill diameter, which is the minor diameter, is drawn with a thick line, and the major diameter with a thin line. In a section, the hatching goes up to the thick line, that is, up to the wall of the hole. In a blind hole, both the thread depth and the drill

depth are drawn, and the drill depth is always deeper. And the drill point is drawn as a cone at 120 degrees, even if the actual drill angle is 118. The depth of the hole is measured to the end of the full diameter, not to the tip of the cone. assembly is drawn in section, the two threads meet.

the bolt is drawn in full, and it hides the internal thread. The internal thread appears only in the part of the hole where there is no bolt, and there the hatching again goes up to the thick line. Someone who does not know this may think the hole is not threaded to its full depth.

In the conventional representation, a gear is drawn without teeth: the addendum circle with a thick line, and the pitch circle with a thin center line. Sometimes one or two teeth are drawn, when the position of a tooth relative to another feature, such as a keyway or a hole, must be shown.

And in drawings produced from CAD systems, very often all the teeth are drawn. But even then, the tooth shape in the picture is only a picture. You do not measure from it, and it does not define the tooth. What defines the teeth is in a data table on the drawing: module,

number of teeth, pressure angle, accuracy grade and inspection dimensions. from the drawing, even if the picture looks complete. Splines are usually drawn in a simplified representation, like gears, and their data appears in a table or in a callout according to the standard, for example ISO 4156.

Rolling bearings on an assembly drawing are sometimes drawn as a rectangle with a cross inside, according to ISO 8826. The bearing itself is defined by its catalog number in the parts list, not by the picture. A spring is also drawn simplified: a few coils at the ends, and the rest shown with center lines.

The spring is defined in a table: wire diameter, mean diameter, number of coils, free length, and sometimes a force at a given length. On a spring, the force at a given length is often more important than any geometric dimension. When the same feature repeats several times, it is drawn and defined once.

A callout such as 6X @10 means there are six identical holes. At the other locations only center lines are drawn, and sometimes not even the holes themselves. The number of occurrences in the callout is what is binding. If the picture shows five centers and the callout says six, there is a contradiction, and you ask.

Sometimes EQS, or EQ SP, is added to the callout, meaning equally spaced. When this callout appears, an angular dimension for each hole is not needed. Without it, the angle between the holes must be defined by a dimension. On a symmetrical part, only half, or even a quarter, can be drawn.

According to ISO, two short parallel lines at the ends of the center line indicate that the part is symmetrical about it. A long part with a constant cross-section, such as a shaft or a profile, is drawn shortened using break lines.

The dimension written on it is the true length, not the drawn length. from the picture will get a completely wrong number. A flat surface on a round shaft is marked with two thin crossing lines, to distinguish it from a round surface.

Knurling is drawn on only a small portion of the surface, and the type and pitch are defined in the callout. A small intersection between two features, such as a small hole entering a shaft, is sometimes drawn with straight lines instead of the exact curve.

sometimes drawn with a thin line, or not drawn at all. And in ASME standards, hidden lines are drawn only when they are needed. The absence of a hidden line does not prove there is nothing there. A line of one long dash and two short dashes, a phantom line, shows an alternate

position of a moving part, or an adjacent part that does not belong to the drawing. It provides context only, and it is not part of the geometry the drawing defines. All of these conventions share one principle. The picture shows where the feature is and roughly what it looks like.

The callout, the table and the note define it exactly. So when there is a gap between the picture and the callout, the callout usually governs, but such a gap is always a reason to ask. And someone who does not know a convention will see it as an

error in the drawing, or worse, interpret it as real geometry. The drawing simplifies on purpose: threads, gears, springs, repeated features and long parts. On an external thread the major diameter is thick, and on an internal thread the tap drill diameter is thick.

Gears and springs are defined in a table, and repeated features are defined by the number in the callout. And wherever the picture is simplified, the information is in the callout, not in the picture. In the next chapter we move to the second part of the course: dimensioning philosophy,

and why a good dimension is first of all an engineering decision. See you in chapter four.

4. Dimensioning Philosophy

A dimension on a drawing is not just a number. It is an engineering decision. distance, from which point, and with which tolerance. Exactly the same part can receive two different dimensioning schemes, and end up as two parts that function differently.

In this chapter we will learn to read the intent behind the dimensions, not just the numbers. A functional dimension directly defines what matters for the function of the part. If two holes must match two pins on another part, the important distance is the distance between them.

So it is dimensioned directly, from hole to hole, and not each hole separately from the edge. A dimension chosen for manufacturing convenience can harm the function, even when all the numbers are within tolerance. The standard is aimed at functional dimensioning.

The manufacturing method is chosen by the manufacturer later. There are two main ways to arrange dimensions: as a chain, or from a single baseline. In chain dimensioning, each dimension starts where the previous one ended. With four chained dimensions, each with a tolerance of one tenth,

the position of the last feature can vary by up to four tenths. In baseline dimensioning, every feature is dimensioned from the same edge, and the tolerance does not accumulate. But there is a price: the distance between two adjacent features is

no longer controlled directly, and it can vary by up to two tenths. There is no single right way. The choice tells the reader which distance the designer wanted to keep tight. On drawings for CNC manufacturing you often see ordinate dimensioning:

one zero point, and each feature gets one number on each axis. This is really baseline dimensioning, with the same properties: no accumulation from the baseline, but the distance between two features is not controlled directly. a hole table, with a letter or a number for each hole.

and the tolerances apply to it like any other dimension. A redundant dimension is one that can be calculated from other dimensions on the drawing. A closed chain is the classic example: three partial dimensions, plus an overall dimension that covers all three.

A part can meet three of them and exceed the fourth, and then it is not clear which dimension governs. So a correct chain leaves one segment undimensioned, or marks one of the dimensions as a reference dimension.

And the segment left without a dimension is usually the least important one. That too is a statement by the designer. A reference dimension appears in parentheses, and sometimes with the note REF. It is for information only: it has no tolerance, and it is not inspected for acceptance of the part.

It is there to save the reader a calculation, for example an overall length. A common mistake is to inspect a reference dimension and reject a part because of it. The part is judged by the dimensions that define it. A basic dimension is enclosed in a frame.

It is a theoretically exact dimension: it has no tolerance of its own, and the general tolerance does not apply to it. The tolerance of the feature comes from its geometric feature control frame, for example a position tolerance.

Someone who applies the general tolerance from the title block to a basic dimension is inspecting the part against a requirement that does not exist. And a basic dimension with no geometric tolerance referring to it is an error on the drawing, because then the feature has no tolerance at all.

Instead of a dimension and a tolerance, both limits can be written directly, for example twenty and twenty point zero five. This is convenient for manufacturing and inspection, because no calculation is needed. And some dimensions have only one limit, marked MIN or MAX,

for example a maximum corner radius or a minimum thread depth. determined by the function or by other dimensions. ASME has a symbol called the dimension origin symbol: a small circle at the end of the dimension line, instead of an arrowhead.

It says which feature measurement starts from, and that changes the result when the surfaces are not perfectly parallel. Measuring from the wrong side can accept a part that should have been rejected, or reject a good part.

When a dimension is changed on the drawing without updating the picture, it is marked with a line under the number. The line says: the picture here does not match the number, and the number governs. And that is another reminder of the rule from chapter zero: do not measure from the picture.

The dimensioning scheme is where the designer tells you what matters to him. A direct dimension between two features says: this distance is critical. Dimensions from a single baseline say: this edge is the reference point of the part. And a dimension with a particularly tight tolerance says:

here the function is sensitive, and so is the cost. Someone who reads the drawing this way can plan manufacturing and inspection that protect what really matters. Let's take an example: a plate with a central hole for a shaft, and two holes for bolts.

The designer dimensioned the bolt holes from the central hole, because they must match a flange that sits on the shaft. The manufacturer would prefer dimensions from the edge, because that is where it is convenient for him to fixture and measure.

If the manufacturer converts the dimensions to the edge on his own, the tolerances accumulate, and the distance to the central hole can be exceeded even when all of his dimensions are within tolerance. And if he still wants to work from the edge, he must tighten his

tolerances so that the designer's original dimensions are maintained. That is the principle: you may manufacture any way you like, but inspection is done to the dimensions on the drawing. A dimension is an engineering decision, not just a number.

A chain accumulates tolerances, a baseline holds each feature relative to the edge, and a direct dimension holds the distance between two features. A redundant dimension creates a contradiction, a reference dimension is not inspected, and a basic dimension gets its tolerance only from the feature control frame.

In the next chapter we will talk about the tolerances you cannot see: general tolerances, and what they define when there is no tolerance next to a dimension at all. See you in chapter five.

5. Default Tolerances

Most dimensions on a drawing are written without a tolerance next to them. That does not mean they have no tolerance. It means the tolerance is written somewhere else. Default tolerances govern most of the part's geometry, and most readers never look at them at all.

defined, how to read them, and what they do not cover. Default tolerances appear in the title block or ina general note, usually with the words "unless otherwise specified". They apply to every dimension that has no tolerance of its own.

A dimension with its own tolerance, a reference dimension and a basic dimension do not receive the general tolerance. And if the drawing has no general tolerance at all, dimensions without a tolerance are undefined, and that is a question for the designer.

On drawings to ISO, the general tolerance is usually defined by reference to ISO 2768. Part one of the standard sets tolerances for linear and angular dimensions, in four classes: fine, medium, coarse and very coarse, marked f, m, c and v. The tolerance is not fixed. It grows with the dimension.

In the medium class, a dimension of 20 mm gets +0.2, and a dimension of 200 mm gets +0.5. without checking which range it falls in on the table. the shorter leg, not according to the size of the angle. ISO 2768 also sets tolerances for external radii and chamfer heights:

in the medium class, up to 3 millimeters +0.2, and above 6 millimeters +1 millimeter. That way even a broken corner, or a small radius drawn without a tolerance, is defined. Part two of ISO 2768 set general geometric tolerances: straightness, flatness, perpendicularity and symmetry, in three classes: H, K and L.

A callout such as ISO 2768-mK means: medium class for dimensions, and class K for geometry. In 2021 this second part was replaced by a new standard, ISO 22081, so on drawings you can meet both callouts. Someone who receives a drawing with mK needs to know that the perpendicularity and

flatness of the part are also limited, even though there is no symbol on them. ISO 22081 works differently from part two of ISO 2768. Instead of a table by tolerance type, it usually defines a general profile of a surface tolerance, relative to a datum reference frame that appears in the title block.

So when you see a reference to ISO 22081, look in the title block for both the tolerance value and the datums it refers to. On drawings to ASME, and especially on inch drawings, there is a different convention. The title block defines the tolerance by the number of decimal places.

For example, one place: +0.1. Two places: +0.01. And three places: +0.005. So the same number, written two ways, gets two different tolerances: 1.5 versus 1.500 are not the same requirement. These values are not part of the standard itself. Each company sets them in

its own title block, so always read the title block of the specific drawing. And someone who adds or removes a trailing zero on a dimension changes its tolerance. A typical ASME title block also includes a tolerance for angles, for example +0.5°, and sometimes a note about breaking sharp edges.

And there is a modern trap: a drawing produced from a CAD system, with three decimal places on every dimension. If the title block sets the tolerance by the number of decimal places, every such dimension suddenly gets the tightest tolerance.

That is usually not the designer's intent, but as far as the drawing is concerned it is the requirement, so you ask. General tolerances also apply to what is not dimensioned at all. A right angle drawn without a dimension gets the general angular tolerance.

And holes drawn on the same center line, or features that look symmetrical, have that relationship only within the general tolerances, not exactly. In other words: what looks aligned or perpendicular on the drawing is aligned and perpendicular only within the general tolerance.

There is a principle in ISO 2768 worth knowing. According to the standard, a part that exceeds a general tolerance is not automatically rejected if its function is not impaired. But that is not a decision for whoever is measuring. As we saw in chapter zero,

the decision on a nonconforming part belongs to whoever is responsible for the design. ASME Y14.5 has no similar clause. A dimension out of tolerance is out of tolerance. The general tolerance is chosen according to the normal accuracy of the shop, so that most dimensions will be achieved without special effort.

A general tolerance that is too tight makes the whole part more expensive, because every dimension becomes a requirement. And a general tolerance that is too loose hides a risk: an important dimension that was left without its own tolerance gets a tolerance that does not suit it.

So when you read a drawing, ask about every important dimension: is the general tolerance really enough for it? A dimension without a tolerance takes the general tolerance from the title block. In ISO 2768 the tolerance depends on the size of the dimension,

and the callout mK also limits the geometry. On inch drawings, the number of decimal places is part of the requirement. And what looks perpendicular or aligned on the drawing is limited only by the general tolerance. In the next chapter we reach one of the deepest differences between ASME and ISO:

the envelope principle versus the independency principle. See you in chapter six.

6. Envelope versus Independency

Suppose a shaft is dimensioned with a diameter of twenty, plus or minus five hundredths. The shaft is inspected, and every measurement is between twenty minus five hundredths and twenty plus five hundredths. But the shaft is slightly bent. Is it acceptable? The answer depends on the standard in the title block.

Under ASME it may be rejected, and under ISO it may be accepted. In this chapter we will understand why, and what it changes in inspection and in assembly. ASME Y14.5 has a rule called Rule #1: the envelope principle. The rule says that the size limits of a feature govern

not only its size, but also how much its form may vary. At maximum material condition, MMC, the feature must have perfect form. On a shaft, this means the entire shaft must pass through a perfect cylinder twenty plus five hundredths in diameter.

The thinner the shaft, the more room it has to bend. That is allowed, as long as it stays inside the envelope. So under ASME a feature of size is inspected in two ways. One check is of the envelope: does the whole part fit into the

perfect cylinder, or, for a hole, does a perfect pin fit into it. The second check is of the local size: everywhere along the part, the two-point size does not go beyond the other limit. This is Taylor's long-established principle: a full- form GO gauge, and a two-point NO-GO gauge.

A bent shaft can pass the local measurement at every point, and still be rejected in the envelope check. Take a pin with a diameter of 10 and a tolerance of minus 0.04, Under the envelope principle, the largest pin, exactly ten in diameter, must be perfectly straight.

four hundredths, and still stay inside an envelope of ten. The hole too, at its minimum diameter, must accept a perfect pin ten in diameter. The result: every conforming pin always fits into every conforming hole. That is what the envelope principle guarantees.

Under the independency principle, the same pin can measure ten at every point and be bent by three hundredths. Then it occupies a space of 10.03, and may not fit into a hole ten in diameter. In ISO standards, the default is the opposite.

Under ISO 8015, every requirement on the drawing stands on its own. A size tolerance controls only the size, not the form. default between two points, according to ISO 14405. So our bent shaft meets the size requirement,

because every two-point measurement is within the limits. Its bending is limited only by a straightness tolerance, if there is one on the drawing, or by the general geometric tolerance. ISO 14405 does not stop at two points. It defines several

ways to measure a size, and each one has a modifier. LP is a two-point size, and it is the default. GG is a size calculated by the least-squares method, the way most coordinate measuring machines calculate.

GN is the smallest cylinder that circumscribes a shaft, and GxX is the largest cylinder that fits inside a hole. The E modifier is in effect a combination: GN or GX at the maximum material limit, and LP at the other limit.

And here is an inspection trap: a coordinate measuring machine that calculates a diameter by least squares is measuring something other than what the drawing asked for, unless GG is written. When the function requires an envelope, for example a shaft that must fit into a hole, it has to be requested explicitly.

This is done with the letter E in a circle, after the tolerance, for example @20 h7 ©. Or with a general note, such as ISO 2768-mk-E, which applies the envelope to every feature of size on the drawing. Without the modifier, even a tight ISO 286 fit does not guarantee assembly if the part is bent.

ASME also lets you go in the opposite direction. which cancels the envelope principle for a specific feature. On older drawings you will find a note instead, such as PERFECT FORM AT MMC NOT REQUIRED. And there are cases where the envelope principle does not apply in the first place:

stock material, such as bars and sheets, and non- rigid parts that are measured in the free state. It is also important to understand the limit of the envelope principle. It controls the form of a single feature, but not the relationship between two features. The perpendicularity of a hole to a surface, or the location of a hole relative to an edge,

is not controlled by the envelope principle. For that you need geometric tolerances. Anyone who thinks the size limits ensure that two diameters are on the same axis is wrong under both standards. An ISO drawing read through ASME eyes will lead to rejecting good parts,

or wasting time on inspections that were not required. And an ASME drawing read through ISO eyes will lead to accepting parts that will not go together in assembly. So before inspecting a feature of size, find in the title block which standard the drawing follows.

And if the drawing is to ISO and the part has to fit into another part, check whether there is an E modifier. If there is not, it is a question for the designer. In ASME, the default is the envelope principle: at maximum material condition, perfect form. In ISO standards, the default is the independency principle:

size is checked between two points, and form is controlled separately. The E modifier applies an envelope in ISO standards, and the | modifier cancels it in ASME. And under both standards, the envelope does not control the relationship between features. In the next chapter we will get to know the ISO 286 system of fits:

what H7 and g6 mean, and how to read a fit. See you in chapter seven.

7. Fits · ISO 286

When a shaft goes into a hole, the important question is not only what their diameters are, but how they will behave together. Will the shaft rotate freely, be located precisely, or be pressed in and never move again? The ISO 286 system of fits answers this question with two short designations, such as H7 and g6.

In this chapter we will learn to read these designations, calculate the clearance or interference from them, and understand what they require of manufacturing and inspection. Every fit designation is made of a letter and a number. relative to the nominal size: above it, below it, or around it.

The number is the tolerance grade, IT, and it sets how wide the tolerance zone is. An upper-case letter denotes a hole, and a lower- case letter denotes a shaft. So H7 is a hole tolerance, and g6 is a shaft tolerance. And on an assembly drawing both are written together, with a slash: H7/g6.

Tolerance grades range from IT01, the highest accuracy, up to IT18. The width of the zone depends on the grade and also on the size: the same grade gets a wider zone at a larger diameter. For diameters between eighteen and thirty millimeters, IT6 is thirteen microns,

IT7 is twenty-one microns, and IT8 is thirty-three microns. To get a feel for it: IT6 usually requires grinding or very fine machining, IT7 suits reaming or precise milling, and IT8 to IT9 suit normal machining. Every grade you improve raises the price. That is the economic decision inside the small number.

The letter sets the fundamental deviation: the limit of the tolerance zone closest to the zero line. For an H hole, the lower limit is exactly the nominal size. The hole can only be larger than it. nominal size. The shaft can only be smaller than it. the shaft below the nominal size, and give clearance.

Later letters, such as p or s, raise the shaft above the nominal size, and give interference. already tells the reader which type of fit is intended. Most of industry works in the hole-basis system: the hole is always H, and only the shaft changes. The reason is practical: a precise hole is made with fixed-size tools, such as a reamer,

and checked with a fixed gauge. It is easier to keep such tools only for H sizes. The shaft is easier to make and measure at any size, by external machining. There is also a shaft-basis system, in which the shaft is h. It is used when one long shaft carries several parts with different fits.

drawing knows he is looking at a hole-basis system. Take a hole of diameter 25 H7: from exactly 25 up to 25.021. With a g6 shaft, between 24.980 and 24.993, you get a clearance fit. The minimum clearance is seven microns, and the maximum is

forty-one microns. The shaft will always move inside the hole. With a k6 shaft, between 25.002 and 25.015, you get a transition fit. In a transition fit, depending on the actual sizes, there can be a clearance of up to nineteen microns, or an interference of up to fifteen microns.

Such a fit is chosen for precise location, when the part has to be assembled with a light press and taken apart when needed. With a p6 shaft, between 25.022 and 25.035, you get an interference fit. The minimum interference is one micron, and the maximum is

thirty-five microns. The shaft is always larger than the hole. And the calculation rule is simple: maximum clearance is the largest hole minus the smallest shaft, and minimum clearance is the smallest hole minus the largest shaft. On a part drawing, the designation appears next to the diameter, for example diameter 25 H7.

Many drawings also add the limits themselves in parentheses, so nobody has to look them up in a table. If both the designation and the limits appear, and they do not match each other, that is a contradiction, and you ask.

On an assembly drawing the combination appears, H7/g6, to show the intent of the fit. And on drawings to ASME you sometimes see inch fits of a different kind, such as RC or FN, according to ANSI B4.1. The idea is the same, and the tables are different. An H7 hole is usually checked with a plug gauge:

the GO end at the lower limit, and the NO-GO end at the upper limit. A shaft is checked with a ring gauge or a snap gauge, on the same principle. Measuring with an ordinary caliper at such a grade is hardly enough, because a twenty-micron zone is close to the accuracy of the instrument itself.

And in an interference fit, the assembly itself is part of the process: pressing, heating the outer part, or cooling the shaft. So a fit is also read as an indirect instruction to manufacturing: which finishing process, which gauge, and which assembly step will be needed.

First, the envelope principle: on an ISO drawing, a fit without an E modifier does not guarantee that a bent part will go in, as we saw in the previous chapter. Second, temperature: the dimensions apply at twenty degrees. A shaft measured right after machining, while it is warm, measures too large.

machining, you need to know whether the fit applies before side can turn a clearance fit into an interference fit. And fourth, units: in the ISO 286 tables the deviations are written in microns, and on the drawing in millimeters. A conversion mistake is a mistake of a thousand times.

A fit designation is a letter and a number: the letter sets the position, and the number the width of the zone. H means a hole that starts exactly at the nominal size. In the hole-basis system, the shaft's letter immediately tells

you whether the fit is clearance, transition or interference. Maximum clearance is the largest hole minus the smallest shaft, and minimum clearance is the smallest hole minus the largest shaft. And for every fit, also check the envelope, the temperature and the coating.

In the next chapter we will combine several dimensions: tolerance stack-ups, worst case and RSS, and how to identify on the drawing the dimension that really matters. See you in chapter eight.

8. Tolerance Stack-ups

its own. But in the assembly, the parts meet each other. Several dimensions, each with its own tolerance, accumulate together, and create a clearance, an interference or a location that none of them defines alone. This is a tolerance stack-up, and this is where it is decided whether the assembly will work.

In this chapter we will learn to build a stack-up, calculate it in two ways, and identify on the drawing the dimensions that really matter. dimensions that starts and ends at the same place. At the center of the loop there is a single requirement: a gap,

a thickness, or a distance that must stay within certain limits. This requirement is called the closing dimension. It is not dimensioned directly, and it is the result of all the others. Every dimension in the loop gets a direction: a dimension that increases

the requirement is positive, and a dimension that decreases it is negative. Dimensions that are not in the loop do not affect the requirement, even if they are very tight. So the first step is always to draw the loop, not to calculate. Let's build an example: a bearing housing with a bore fifty deep,

with a tolerance of plus or minus one tenth. Inside it sit a bearing twenty wide, a spacer twenty-five long, and a washer four and a half thick, each with a tolerance of plus or minus five hundredths. The requirement is an axial clearance between the washer and the cover,

which must be between two tenths and eight tenths. The depth of the bore increases the clearance, so it is positive. The bearing, the spacer and the washer fill the bore, so they are negative. minus twenty-five, minus four and a half: half a millimeter.

Half a millimeter is exactly in the middle of the requirement. But the question is what happens when each dimension moves within its tolerance. the dimensions are at their worst limit at the same time. The tolerance of the clearance is simply the sum of all the tolerances.

One tenth, plus three times five hundredths, is twenty-five hundredths. So the clearance can range from twenty-five hundredths to seventy-five hundredths. Both results are within the requirement, so the assembly will always work, with any combination of conforming parts.

This is the safe method, and it is suitable when there are few parts, or when failure is unacceptable in any case. The second method is RSS, root sum of squares. It is based on a statistical fact: the chance that all the

parts reach their worst limit at the same time is almost zero. Instead of adding the tolerances, you add their squares, and take the square root. In our example: the square root of one tenth squared, plus three times five hundredths squared, comes out to about thirteen hundredths.

That means the expected clearance is between thirty-seven hundredths and sixty-three hundredths, much narrower than the worst-case result. The more parts there are in the stack-up, the greater the advantage of RSS. But this method has a price: it assumes that every dimension is distributed around the middle,

and that the processes are stable and independent of each other. lf a manufacturer systematically aims for the edge of the tolerance, the assumption breaks down, and RSS gives an overly optimistic picture. RSS suits series production, with many parts and processes under statistical control.

When a designer relies on RSS, ASME allows the tolerance to be marked with the ST symbol, statistical tolerance. Next to the symbol there is usually a note that requires statistical process control in production. Someone who sees ST on a drawing needs to know: meeting the tolerance alone is not enough.

The distribution of the process is also part of the requirement. And for a single part, or a small batch, RSS is a gamble, and worst case is the right choice. It is not only dimensions that enter the stack-up. Geometric tolerances too, such as position, perpendicularity or runout,

move surfaces, so they are links in the loop. A position tolerance of one tenth diameter, for example, contributes plus or minus five hundredths to the stack-up. Someone who calculates a stack-up from the dimensions only,

and skips the geometric tolerances, gets a result better than reality. Here we return to chapter four: the way a part is dimensioned determines how many links it brings into the stack-up. In a good design, each part contributes only one dimension to the stack-up,

the dimension that directly touches the requirement. If the part is dimensioned in an internal chain, two or three of its dimensions enter the loop, and the total tolerance grows. So when you see a direct dimension between two surfaces that are both part of the loop,

it is usually not a coincidence. It is the critical dimension. And a manufacturer who converts such dimensions on his own changes the stack-up the designer calculated. What do you do when the calculation shows the requirement is not met?

You can tighten tolerances, but that makes every part in the stack-up more expensive. You can add an adjustment component, such as a shim or a washer of selected thickness, that closes the gap at assembly. And you can use selective assembly: sort parts by size, and assemble matching parts together.

Any such solution must appear in the documentation, because whoever assembles needs to know it is part of the process. dimensions around a single requirement, the closing dimension. Worst case adds all the tolerances, and guarantees assembly with any combination.

and requires stable processes, so it is marked with ST. Geometric tolerances are part of the stack-up, and the direct dimension on the drawing is usually the critical dimension. This completes the second part of the course. The next chapter starts the third part:

the datum reference frame. See you in chapter nine.

9. The Datum Reference Frame

In the third part of the course we will read geometric tolerances within the drawing, not each symbol on its own. And we start from the datum reference frame, because every location or orientation tolerance is measured relative to it.

The datum reference frame is the instruction for how to hold the part during inspection, and it is also the designer's statement of how the part sits in the assembly. In this chapter we will learn to read it: what each letter says, why the order matters, and what it reveals about the function.

A part floating in space can move in six ways: three translations along the axes, and three rotations about them. These are the six degrees of freedom of the part. To measure the location of a hole, the part must first be locked,

so that none of these degrees changes during measurement. The datum reference frame does exactly that: it defines which features of the part lock it, and in which order. Without a datum reference frame, a position tolerance is a number with no starting point.

So a feature control frame with no datum letters limits only form, not location. The first letter in the frame is the primary datum. The part rests on it, touching at least three points. This locks three degrees of freedom: one translation and two rotations.

The second letter is the secondary datum. The part is pushed against it at a minimum of two points, and two more degrees are locked. The third letter is the tertiary datum. One point is enough, and it locks the last degree. Three, two, one: this is the principle on which every datum reference frame is built.

In inspection it looks like this: the part is placed on the surface plate, pushed against an angle plate, and pressed against a stop. And the measurement itself is taken from the coordinate system that was created, not from the edges of the part.

The order of the letters is not a matter of convenience. If the primary datum is A, the part sits fully on A, and only then is pushed against B. If the primary datum is B, the part sits on B, and surface A aligns only as far as it can. When the angle between the two surfaces is not exactly ninety degrees,

the two orders give different coordinate systems, and therefore different results. A hole can pass inspection in one order, and fail in the other. So the letters are read from left to right, exactly in the order they are written, and the order is not changed.

There are three concepts worth separating. The datum feature is the real surface on the part, with all its irregularities. The triangle with the letter is attached to it. The datum is a theoretically perfect plane, or a perfect axis, from which measurement is taken.

And between them stands the datum feature simulator: the surface plate, the angle plate or the precision pin, which actually contact the part. Measurement is taken from the simulator, because it is what the part really meets, both in inspection and in assembly.

So a rough or unstable surface chosen as the primary datum will give results that change from one inspection to the next. A good datum reference frame reflects the assembly. The primary datum is usually the surface the part sits

on in the assembly, the largest and most stable surface. The secondary and tertiary datums are usually the features that locate the part: a central bore, a pin, or a wall it is pushed against. When you read a drawing, ask: are the datum features that

were chosen the features that really contact the other parts? If so, inspection will simulate the assembly. If not, a part that passes inspection may not fit in the assembly. And when the datum reference frame does not look functional,

that is a reason to ask the designer, not to change it. On a cast or forged part, the raw surfaces are not true enough to serve as a full datum surface. So datum targets are used: points, lines or small areas defined on the surface. They are shown in a circle divided in two: the size of the area on top,

and the letter and number below, for example A1. Three targets define the primary datum, two the secondary, and one the tertiary, exactly as before. That way both the first raw part and the machined part are inspected from the same targets, and the transition between the processes is preserved.

A datum feature can also be a feature of size, such as a hole or a shaft. Then the simulator is a pin or a ring, and the datum is their axis. When there is no modifier next to the letter in the frame, the simulator adjusts itself to the actual size of the hole, and there is no play.

When the letter is followed by M in a circle, the simulator is a pin of fixed size, at the maximum material boundary. A hole larger than that boundary leaves play, and the part can move slightly on the pin. This is called datum shift, and it is allowed.

That is exactly what happens in an assembly with a pin, so it also makes manufacturing easier without harming the function. When you read a feature control frame, you can reconstruct the entire inspection from it. The letters say what the part is placed on and in which order,

and the modifiers say whether there is play. A common trap is to inspect all the dimensions from the same frame, when different feature control frames on the drawing refer to different datum reference frames. Another trap is to fixture the part for manufacturing

on other features, and then be surprised at inspection. You may manufacture in any fixture, but someone who fixtures the part according to the drawing's datum reference frame reduces the risk from the start. The datum reference frame locks the six degrees of freedom, by the three-two-one method.

The order of the letters determines the result, and it is read exactly as written. Measurement is taken from the simulator, so a primary datum must be stable and functional. On raw parts datum targets are used, and a letter with M in a circle allows datum shift. In the next chapter we will combine geometric tolerances with dimensions,

and find contradictions on a complete drawing. See you in chapter ten.

10. Geometric Tolerances and Dimensions Together

In the previous chapter we read the datum reference frame. Now we will read how geometric tolerances and dimensions work together, on the same feature. A single feature can have a size, a form tolerance, an orientation tolerance and a location tolerance, and they must all be consistent with each other.

When they are not consistent, the drawing contradicts itself, and there is no way to inspect it. In this chapter we will learn to spot such contradictions, read a material condition bonus, and understand tolerances on hole patterns. Geometric tolerances have a natural hierarchy:

location also controls orientation and form, and orientation also controls form. So a position tolerance on a hole already limits its perpendicularity, and a parallelism tolerance on a surface already limits its flatness. An additional tolerance under a wider one is called a refinement. It makes sense only if it is smaller.

For example, parallelism of two tenths and flatness of five hundredths on the same surface: that makes sense. The flatness is refined within the parallelism. But flatness of two tenths under parallelism of five hundredths adds nothing, and that is a sign that something was not thought through.

And the same applies to size: under the envelope principle, a flatness larger than the thickness tolerance of the same part is meaningless. The most common contradiction: a hole located both by a plus-or-minus dimension and by a position tolerance.

and there is no way to know which one to inspect to. When there is a position tolerance, the dimensions that locate the hole must be basic dimensions, ina frame. Another contradiction is an orientation or location tolerance that

refers to a datum that is not identified on the drawing at all. And one more: a tolerance that refers to the same feature it applies to, as if the hole were measured relative to itself. In all these cases you do not choose an interpretation.

You record the contradiction and ask the designer. When the position tolerance is followed by Mina circle, the tolerance applies only when the hole is at maximum material condition, that is, at its smallest diameter. The larger the actual hole, the more it is added to the tolerance,

by the size of the difference. That is the bonus. Take a hole with a diameter of ten and a tolerance of plus one tenth, with a position tolerance of one tenth and Mina circle. A hole exactly ten in diameter gets a position tolerance

of one tenth. A hole 10.1 in diameter gets two tenths. The reason is functional: a larger hole leaves more room for the bolt, so it can be less accurately located and still fit. The worst case is called the virtual condition:

the smallest hole diameter minus the position tolerance. Here it is 9.9. And that is exactly the diameter of the pin on the functional gauge. If the pin goes into all the holes, the part is good. L in a circle works the same way, but in reverse: the tolerance applies

at least material, and the bonus grows as there is more material. It is used when the concern is a thin wall, not assembly. A hole close to an edge, for example, may leave a weak wall. L in a circle guarantees a minimum wall thickness.

the same for every hole size, and there is no bonus. And the choice between the three options tells the reader what the designer was trying to protect: assembly, strength, or precise location. Sometimes you see a position tolerance of zero, with M in a circle.

That does not mean the hole must be in a perfect location. It means all the tolerance was moved to size: a hole at maximum material condition must be exactly in place, and every increase in diameter is position tolerance. That way the manufacturer decides for himself how to split the

tolerance between size and location, and the function is preserved. One frame can apply to several holes together, for example four holes, with the callout four times before the diameter. Then the holes are inspected as a pattern:

both the location of each one, and the distances between them. Sometimes the frame is built of two rows, with one shared position symbol. This is a composite position tolerance. The upper row, the wider one, locates the whole pattern relative to the datums.

The lower row, the tighter one, controls only the distances between the holes and their orientation, not the location of the pattern. In other words: the pattern can move as a block within the wide tolerance, but the holes must hold their relationship to each other within the tight tolerance.

This suits a flange that connects to another part with several bolts: it is more important for the holes to match each other than for the pattern to be in an exact place. In ASME, when several patterns refer to the same datums, in the same order and with the same modifiers, they are inspected as one pattern, all at once.

To separate them, SEP REQT is written, separate requirement. In ISO standards the default is the opposite: each pattern is inspected on its own, and to combine them you must write SIM, or CZ for a combined zone. So exactly the same drawing can require one inspection or several, depending on the standard.

There are a few more differences worth knowing when you read a drawing to a standard other than the one you are used to. In the 2018 edition of ASME, the concentricity and symmetry symbols were removed. Position, profile or runout tolerances are used instead.

In ISO standards both symbols still exist, and you will also find them on older ASME drawings. And in both standards, a cylindrical tolerance zone requires a diameter symbol before the value. planes, and that is a completely different requirement. To avoid missing anything, read every feature in the same order.

First size: what is the dimension, and does the envelope principle apply. Then form, orientation and location, and check that each one is smaller than the one above it. Then the datums: do they exist, and are they in the right order. And finally the modifiers: M, L or nothing, and whether there is a bonus or a datum shift.

If anything in this chain does not add up, itis a question for the designer, not a decision for whoever is measuring. Geometric tolerances and dimensions must be consistent: a refinement is smaller than the tolerance above it, and a position tolerance is located only by basic dimensions.

M in a circle gives a bonus for assembly, L ina circle protects a wall, and on hole patterns a composite tolerance separates the location of the pattern from the relationship between the holes. In the next chapter we start the fourth part: surface texture, and what Ra says and what it does not say. See you in chapter eleven.

11. Surface Texture

Two surfaces can be exactly the same size, and still behave completely differently. One seals, and the other leaks. One wears slowly, and the other fails from fatigue. The difference lies in the surface texture: the small hills and valleys the tool leaves behind. In this chapter we start the fourth part of the course,

and learn to read surface texture symbols, and what Ra says and what it does not say. When you magnify a section of a machined surface, you see three layers of deviation. The overall form, such as a curve or a slope, is controlled by geometric tolerances. Waviness is a long-wavelength deviation, usually caused by vibration or by deflection of the tool.

And roughness is the short wavelength, the marks of the tool itself. Most of the symbol on the drawing deals with it. The tool marks also run in a certain direction, and that is called the lay. The most common parameter is Ra: the average of the

deviations from the mean line of the profile, in microns. Ra is a stable number and convenient to measure, so it appears on most drawings. But it has a weakness: two completely different surfaces can have the same Ra. A surface with sharp peaks and a surface with narrow valleys will give the same average,

even though they behave in opposite ways in sealing and in wear. And a single scratch hardly changes Ra, because it is swallowed by the average. Rz measures the height between the highest peak and the deepest valley in each sampling length, and calculates the average.

So Rz is much more sensitive to individual peaks and scratches. There is no fixed ratio between Ra and Rz. The ratio depends on the process, so you Cannot convert between them with a formula. Someone who replaces Rz with Ra using a conversion

table changes the designer's requirement. And on inch drawings the value is written in micro- inches. An Ra of thirty-two micro-inches is about eight tenths of a micron. The basic symbol is a broken line, like a V with one long leg, touching the surface.

removal is required, that is, the surface must be machined. A circle inside the V says the opposite: material removal is prohibited. The surface stays as it is after casting, forging or pressing. process is allowed, as long as the texture is achieved.

The parameter and the value are written on the long leg, for example Ra eight tenths. A mandatory manufacturing process, a machining allowance, and a lay symbol can also be added. run relative to the line on which the symbol is drawn. The equals sign means parallel, the perpendicular sign means perpendicular,

X means crossed, C means circular, and M means multidirectional. The lay is especially important on sliding surfaces and seals, because it determines whether fluid will flow along the marks or be stopped by them. And the measurement depends on it too: Ra is usually measured perpendicular to the lay.

Measuring parallel to it gives a number that is too low. In ISO, the symbol is now defined in ISO 21920, which replaced ISO 1302 in 2021. In ASME, the symbol is defined in ASME Y14.36, and the form is very similar. On older ASME drawings, a number written next to the symbol without a parameter name is Ra.

And in ISO there is an important rule: by default, up to sixteen percent of the measurements may exceed the value. When max is written after the parameter, no measurement may exceed it. And the cutoff length is set by the size of the value. For Ra between

one tenth and two microns, the cutoff is eight tenths of a millimeter. On most drawings, not every surface is marked separately. Next to the title block a general symbol appears, for example Ra 3.2, followed by a symbol in parentheses.

That means: all surfaces 3.2, except those marked otherwise on the drawing. So when a particular surface is not marked, it is still not free. It takes the general symbol. Every process has a natural range of roughness. Ordinary turning and milling usually give between eight tenths and six microns.

Reaming gives about four tenths to three microns. Grinding usually reaches one tenth to one and a half microns, and polishing or lapping less than half a micron. So the roughness value on the drawing is also an indirect instruction

for the process. An Ra of two tenths almost always requires grinding. And every step toward lower roughness adds an operation, time and cost. There are a few traps worth knowing. On a coated part, you need to know whether the roughness applies

before or after coating, because coating can change it considerably. On a shaft running against a seal, Ra alone is not enough. Turning leaves helical marks that can pump fluid out. And a single deep scratch can cause a leak or a crack, and still not change Ra.

When the function is sensitive to this, the designer needs to add a parameter such as Rz, or an explicit requirement. And if it is missing, you ask. Surface texture is roughness, waviness and lay, and each of them affects the function. Ra is a stable average, but blind to peaks and scratches.

Rz is more sensitive to them, and there is no fixed conversion between them. The symbol says whether material removal is required, prohibited or allowed, and the general symbol appears in parentheses next to the title block. In the next chapter we will get to know welding symbols,

and the differences between the American standard and ISO. See you in chapter twelve.

12. Welding Symbols

The welding symbol is one of the densest symbols on a drawing. One small line encodes the weld type, size, length, side and process. It is also one of the easiest symbols to read backwards, because there are two main standards, and they do not read the side the same way.

Between the American standard, AWS A2.4, and the international standard, ISO 2553, there is also a difference in the meaning of the numbers. In this chapter we will take the symbol apart, and see exactly where the traps are. The basis is a horizontal reference line, with an arrow running from it to the joint.

The weld symbol is drawn on the reference line, with the dimensions next to it. At the other end of the line there can be a tail, a small fork. The process or the specification is written inside it. And where the arrow meets the line there is room for two special symbols: a circle,

meaning weld all around, and a flag, meaning field weld, done during assembly. A triangle is a fillet weld, the most common. A V-shaped symbol is a groove weld with two bevels. A straight line and half a V are a groove with a single bevel.

Two parallel lines are a square-groove weld, with no edge preparation. There are also symbols for U and J grooves, plug welds, spot welds and seam welds. And additional marks above the symbol set the contour of the weld face: flush, convex or concave, and sometimes a letter that says how to finish it, for example G for grinding.

Here lies the big trap. The arrow points to a joint, and the joint has two sides. In the American standard: a symbol drawn below the reference line is on the side the arrow points to. A symbol above the line is on the other side. A symbol on both sides of the line means welding on both sides.

In ISO there are two systems. System A uses a double reference line: a solid line and a dashed line beneath it. In system A, a symbol on the solid line is on the arrow side, and a symbol on the dashed line is on the other side.

ISO system B works with a single line, like the American standard. So when you see a double line, it is an ISO system A drawing, and you read by the solid line, not by above and below. Someone who reads such a drawing with American eyes will weld on the wrong side.

In the American standard, the number to the left of the triangle is the leg size of the fillet weld. In ISO a letter must appear before the number: a for throat thickness, or z for leg length. And the difference is large: a5 means a throat thickness of five millimeters, and a leg of about seven millimeters.

Someone who welds a five-millimeter leg where a5 is written produces a weld about thirty percent weaker than designed. And a number without a letter on an ISO drawing is a question for the designer, not a guess. The weld length is written to the right of the symbol.

With no length, the weld runs the full length of the joint. For intermittent welds, in the American standard, a length and a pitch are written: 50-150, meaning segments fifty millimeters long, every hundred and fifty, center to center. In ISO the notation is different: the number of segments,

times the length, and in parentheses the spacing between segments. is the spacing from end to end, not center to center. Someone who confuses the two gets a different number of segments, and a different total weld length.

In a groove weld, the numbers describe the preparation and the penetration. The number to the left of the symbol is the depth of preparation, and next to it, in parentheses, the effective throat, that is, how far the weld penetrates. The root opening is written inside the symbol, and the groove angle above it.

And when the penetration requirement is missing, it is not clear whether full or partial penetration is required, and that is a huge difference in strength and cost. The welding process is written in the tail, for example TIG or MIG, or an ISO process number, such as 141 for TIG.

The tail often refers to a welding procedure specification, a WPS, which defines all the parameters. The symbol itself does not say how many imperfections are allowed. That is set by a quality standard, such as ISO 5817, with quality levels B, C and D.

And if the drawing does not refer to a quality standard, there is no definition for weld acceptance, and you need to ask. The American standard also has a symbol for nondestructive testing, with the same line-and-arrow structure.

Abbreviations such as RT for radiography, UT for ultrasonic, MT for magnetic particle, PT for liquid penetrant and VT for visual inspection. This symbol says what to test and where, not how to decide whether the weld is acceptable. That too is set by the standard the drawing refers to.

A summary of the welding symbol traps. First: the arrow side. First identify whether the drawing is American or ISO, and whether there is a double line. Second: fillet weld size. In ISO, check whether a or Z is written.

Third: intermittent welds. Pitch center to center, versus spacing between segments. Fourth: the small circle and flag, which are easy to miss, and change the scope of the work. And fifth: a welding drawing is usually an assembly drawing, and every weld refers to two parts that need to be identified.

A welding symbol is made of a reference line, an arrow, a weld symbol, dimensions and a tail. In the American standard, below the line is the arrow side. In ISO system A, the solid line is the arrow side. In ISO, a is the throat thickness and z is the leg length, and a5 equals a leg of about seven.

For intermittent welds, the American pitch is center to center, and the number in parentheses in ISO is the spacing between segments. And quality is set by a separate standard, not by the symbol. In the next chapter we will read the material,

heat treatment and coating on the drawing. See you in chapter thirteen.

13. Material, Heat Treatment and Coating

Two parts can be identical in dimensions, and completely different in strength, hardness and durability. The difference is written on the drawing, but not in the picture: in the title block and in the notes. The material, its condition, the heat treatment and the coating

are part of the definition of the part, just like the dimensions. In this chapter we will learn to read all these definitions, and in which order they apply. The material usually appears in the title block, in the material field. It is written to a particular standard: for example 1.4404

under the European standard, or 316L under the American system. Often a product standard also appears, which defines the form of the material and its properties, for example plate, bar or tube. In many alloys, the temper is part of the material. Aluminum 6061 in the T6

temper is very different from the same aluminum in the annealed condition. And T651 says something more: the material was stretched to relieve stress, and that affects distortion during machining. Someone who substitutes a material that looks equivalent to him, without approval,

changes the part. An equivalent between standards is close, not identical. And a material certificate is usually required too, for example to EN 10204 type 3.1, proving that the actual material is the material on the drawing. Heat treatment appears in a note, and defines what the part must

be after the treatment, not only which treatment to carry out. example forty to forty-five on the Rockwell C scale. For case hardening, such as carburizing or nitriding, the case depth also appears, and the hardness at which that depth is measured.

When only part of the surface is hardened, the area is marked on the drawing with a thick chain line, according to ISO 15787. And the location where the hardness is tested is usually marked as well, because on a large part the hardness is not uniform.

A hardness requirement with no test location is incomplete, because every point on the part can give a different result. There are several hardness scales, and each is measured by a different method. Rockwell C for hard steels, Brinell for softer materials and castings,

and Vickers for thin layers and laboratory measurements. There are conversion tables between the scales, but the conversion is approximate. So when the drawing requires a particular scale, you measure on that scale. enough for acceptance, unless otherwise approved.

The coating too is defined by a specification, not just by a name. Anodizing, for example, can be decorative or hard, dyed or clear, and each one has a different thickness and different properties. So the note usually includes the standard, the type, the class and the thickness.

For zinc plating to ISO 2081, for example, the definition includes the coating thickness and the type of post-treatment. And on stainless steels, a passivation note refers to a standard such as ASTM A967. This is not a coating, but a chemical treatment of the natural passive layer.

A coating adds material, so it changes dimensions. A layer of ten microns on each side increases a shaft by twenty microns, and reduces a hole by twenty microns. penetrates into the material, and half builds up on top of it.

So it is important to know whether the dimensions on the drawing apply before or after coating. This is usually written in a note, and when it is not written, you ask. Areas that must not be coated, such as threads or fit surfaces, are marked on the drawing as areas to be masked during coating.

A coated thread without prior allowance may not go together, and a hole with a tight fit may not accept the shaft. There is one trap that is not just a question of size. In high-strength steels, electroplating can introduce hydrogen into the material.

The hydrogen causes embrittlement, and the part can break without warning, hours or days after assembly. So the specification usually requires hydrogen embrittlement relief baking, shortly after plating. When the drawing specifies a hard steel and electroplating,

and there is no baking requirement, that is an urgent question for the designer. The notes on the drawing also define, explicitly or implicitly, a sequence of operations. Usually: material in a given condition, rough machining, heat treatment, finish machining, and coating only at the end.

Heat treatment after finish machining can distort the part, so a machining allowance is left on the precise surfaces. And when the note says the dimensions apply after heat treatment, the manufacturer has to plan the allowance himself.

Someone who reads the notes as a list and not as a process may carry them out in the wrong order. marking: what to mark, where, and by which method. The method matters: engraving or stamping ona highly stressed surface can create a crack initiation point.

So the location is usually defined in an area that is neither stressed nor functional. An equivalent material without approval. A missing material condition, or one that was misread. Hardness without a test location, or measurement on a different scale.

Coating that was not taken into account in the tolerance of a fit or a thread. And a hard steel with electroplating, without baking. The material and its condition are part of the definition of the part, and they are not substituted without approval.

Heat treatment is defined by its result: a hardness range, a case depth and a test location. A coating is defined by a specification, changes dimensions, and requires knowing whether the dimensions are before or after coating. And all the notes together define a sequence of operations, which must be read as a process.

In the next chapter we go deeper into threads: metric, inch, pipe threads and Helicoil. See you in chapter fourteen.

14. Threads in Depth

In chapter three we learned how a thread is drawn. Now we will learn to read its callout, and that is where most of the information is. A single thread callout gives the diameter, the pitch, the tolerance, the depth, and sometimes also the hand and the number of starts.

And when a metric thread is swapped for an inch thread, or one pipe thread for another, the screw goes in half a turn and jams. In this chapter we will cover metric threads, inch threads, pipe threads and Helicoil holes. A metric callout starts with the letter M and the nominal diameter, for example M10.

When no pitch is written, it is the standard coarse pitch. For M10 it is one and a half millimeters. A fine pitch is always written explicitly, for example M10x1.25. After a dash comes the thread tolerance class, and then the depth. depth, and the tap drill depth, which is always longer.

diameter to a depth of 20, and tap to a depth of 16. Someone who drills only to the thread depth leaves no room for the tip of the tap, and will not get a full thread to the required depth. A thread tolerance is built like the ISO 286 fits:

a number for the tolerance grade, and a letter for the position. An upper-case letter for an internal thread, and a lower-case letter for an external thread. 6H and 6g are the most common combination, and it suits most bolts and nuts. 4h is a more precise thread, and 6e leaves a larger allowance, for example room for plating.

When the part is coated after threading, you must check that the tolerance suits the coating thickness, otherwise the bolt will not go in. And in inspection, the governing dimension is the pitch diameter, not the major diameter. Inch threads are written differently: diameter, threads per inch, series and class.

1/4-20 UNC-2A, for example: a quarter-inch diameter, twenty threads per inch, coarse series, class two, external. UNF is the fine series, and at the same diameter it has more threads per inch. A denotes an external thread and B an internal one.

The classes are one, two and three, and three is the most precise. Small diameters are written as a number, for example 10-32 UNF. And there is a well-known trap: 1/4-20 and M6 look almost the same, and one screw will go into the other a few turns before it jams.

In pipe threads, the number in the callout is not the diameter of the thread. A half-inch pipe thread, for example, has an outside diameter of about twenty-one millimeters. NPT is the American thread: tapered, with a sixty- degree angle, and the seal is made on the thread itself, with a sealant.

In the British system, G is a parallel thread to ISO 228. It does not seal by itself, and sealing is done with a gasket or an O-ring. RIS a tapered external thread, RC a taperea internal one, and Rp a parallel internal one, to ISO Te And the thread angle in the British thread is fifty- five degrees,

so NPT and BSPT are not interchangeable, even though they look similar. Someone who assembles a G thread with sealant on the thread instead of a gasket will get a leak. When threading into a soft material, such as aluminum, a wire thread insert, a Helicoil, is often used.

The drawing shows the final thread, for example M8, and the length of the insert, for example one and a half times the diameter. But the hole itself is tapped with a special, larger thread called STI, with a special tap. Someone who taps a regular M8 instead of STI will not be able to install the insert.

So when you see a Helicoil on the drawing, check exactly what must be drilled, tapped and inserted, and in which order. LH after the callout means a left-hand thread. Without LH, the thread is right-hand. In a multi-start thread, the lead and the pitch are written,

for example Ph3 P1.5, meaning a two-start thread. A chamfer is sometimes shown at the start of the thread, so the screw will start easily. And at the end of an external thread there is sometimes a thread undercut, to standards such as DIN 76, so the thread is full up to the shoulder.

Threads are usually checked with gauges: a plug gauge for an internal thread, and a ring gauge for an external thread. Every gauge has a GO end and a NO-GO end. The GO end must enter the full length of the thread without force.

The NO-GO end is allowed to enter up to about two turns, and no more. And the gauges must be of the same tolerance class as the drawing: a 6H gauge for a 6H thread. A metric versus an inch thread at similar diameters. NPT versus BSPT, and G versus R.

A tap drill hole too short in a blind hole. A coated thread with a tolerance that leaves no room for the coating. A Helicoil without an STI tap. And a left-hand thread that nobody noticed.

In a metric callout: diameter, pitch if it is fine, tolerance and depth. In an inch callout: diameter, threads per inch, series, class, and A or B. In pipe threads, the number is a name, not a diameter, and you distinguish tapered from parallel, and sealing on the thread from sealing with a gasket.

With a Helicoil, the hole is tapped STI, and the drawing shows the final thread. And inspection is with GO and NO-GO gauges, of the same tolerance class as the drawing. In the next chapter we will get to know special features: edge breaks, undercuts, splines and tables on the drawing. See you in chapter fifteen.

15. Special Features

A drawing has small features that take up little space, but define a great deal. An edge, a small groove at the end of a shaft, a spline, or a table in the corner of the sheet can decide whether the part will assemble, hold, and pass inspection. They are usually defined by reference to a standard,

not by a full drawing, so you need to know how to read the reference. undercuts, splines, keyways, center holes, knurling and tables. A note such as break sharp edges is one of the most common notes on a drawing, and also one of the least defined.

How much to break? With a chamfer or a radius? And what is allowed to remain? ISO 13715 gives this a precise language: a symbol next to the edge, and a number with a sign. A positive number means material may remain beyond the ideal edge, such as a burr, up to that value.

A negative number means the edge must be removed, with a chamfer or a radius, up to that depth. And plus or minus means either is allowed, within the limit. A general note to the standard, next to the title block,

defines every edge not marked otherwise, like a general tolerance. At the end of a ground shaft, next to the shoulder, a small undercut often appears. Without it, the grinding wheel or the tool leaves a small radius in the corner, and the mating part will not seat flush against the shoulder.

The undercut is usually defined by reference to a standard, such as DIN 509, with a form and dimensions, for example E1 by 0.2. The letter denotes the form of the undercut, and the numbers the radius and the depth. Someone who replaces the undercut with an ordinary radius changes

the contact length and the stress concentration in the corner. A spline is a shaft with teeth that transmits torque to a hub. representation, and the whole definition is in a data table. The table lists the number of teeth, the module, the pressure angle,

the tolerance class and the fit class, to a standard such as ISO 4156 or DIN 5480. And there is usually an inspection dimension too: measurement over pins on an external spline, or between pins on an internal spline. matters more than any other dimension in the table.

A keyway is a slot for a key, which transmits torque between a shaft and a hub. The keyway dimensions are usually taken from a standard, such as DIN 6885, according to the shaft diameter. system, such as N9 for a normal fit or P9 for a tight fit.

And the depth is sometimes dimensioned from the opposite side of the shaft, not from the surface, so it can be measured directly. Someone who measures the depth from a different point than the one dimensioned on the drawing will get a different number and make the wrong acceptance decision.

On parts machined between centers, the end of the shaft gets a center hole. It is defined to ISO 6411, with a form and diameters, for example A 2.5 over 5.3. And the standard also gives three symbols: the center hole must remain, may remain, or must not remain.

This matters, because a center hole that remains can be used for inspection and repair in the future, or get in the way of the mating part. Knurling is a pattern rolled onto the surface of a shaft, usually so it can be gripped or pressed into another part.

The drawing gives the type of knurl, straight or diamond, the pitch, and sometimes a standard such as DIN 82. Knurling increases the diameter, so when it is used for a press fit, the diameter after knurling is the important dimension.

Tables on a drawing are a way to gather a lot of information in one place. A tabulated drawing, for example, defines several similar parts on one drawing: each row is a part number, and each column is a dimension with a letter. The picture carries the letters, and the table the values for each part number.

the part being made, and only then read dimensions. A mistake in the row is a mistake in every dimension at once. A hole table, a bend table for sheet metal, or a spline data table is read the same way: identify the row, then the column.

A summary of the traps in special features. Break sharp edges with no value is an undefined requirement. A reference to the standard, with a number and a sign, is better. An undercut replaced with a radius changes how the part seats on the shoulder.

On a spline, the inspection dimension over or between pins governs. On a keyway, check from which point the depth is dimensioned. And in tables, identify the right row first. Small features are usually defined by reference to a standard, not by the picture.

Edges to ISO 13715: positive allows material, negative requires removal. Undercuts to DIN 509, keyways to DIN 6885, and center holes to ISO 6411. Splines in a data table, with an inspection dimension over or between pins. And in every table, identify the row, then the column.

In the next chapter the fifth part begins: the drawing as a document. We start with the title block and the notes. See you in chapter sixteen.

16. The Title Block and the Notes

The fifth part of the course deals with the drawing as a document: not only what is drawn, but everything around it. And it starts with the title block, in the bottom right corner of the sheet. Most readers look at it only to find the number. But it defines how to read everything else.

In this chapter we will go through the fields of the title block, the notes, and the documents the drawing refers to. ISO 7200 defines the basic fields: title, identification number, revision, date, sheet number, and the legal owner of the document.

On drawings to ASME, the sheet size, the scale, a CAGE code and the general tolerance block usually appear as well. The drawing number and the part number are not always the same number. One drawing can define several parts, as we saw in a tabulated drawing.

And the sheet number, for example one of three, says there are more sheets, and each of them is part of the definition. Someone who works from one sheet only may miss a dimension, a section or a note that is on another sheet.

The revision is one of the most important fields. It says which version of the drawing is in your hands, and every change to the part raises it. So before starting work, check that the revision on the drawing matches the revision on the purchase order or the work order.

And on a multi-sheet drawing, check that all the sheets in your hands are at the same revision. A drawing at an old revision is one of the most common sources of rejected parts, even though every dimension was made correctly. The scale is written in the title block, for example one to two.

But as we saw in chapter zero, you do not measure from the picture. The scale helps you understand the size, and is not used for measurement. When a particular view is drawn at a different scale, such as an enlarged detail, its scale is written next to it.

The title block also defines the reading rules for the whole drawing. The projection symbol says whether the views are in first angle or third angle. The reference to the tolerancing standard, such as ASME Y14.5 or ISO 8015, says whether the envelope principle or the independency principle applies.

And the units, millimeters or inches, are written there. Someone who assumes the units without checking may make a part twenty-five times too large, or too small by the same ratio. And the general tolerances, the default surface texture and the general edge break usually appear in this area too.

The general notes appear next to the title block. They apply to the whole drawing. There are also flag notes: a number inside a triangle or a flag, which appears next to a particular feature in the picture. notes list, and it applies only where the flag appears.

So when you read a numbered note, look in the picture for every flag with the same number, not just the first one. What happens when notes contradict each other? Usually, a specific requirement next to a feature overrides a

general note. That is what unless otherwise specified means. But when the contradiction is between two specific requirements, or between the drawing and a specification, there is no automatic rule. In that case you do not choose the convenient interpretation.

You record the contradiction, and you ask. A drawing almost always refers to other documents: a material specification, a process specification, an inspection standard, or customer requirements. These documents are part of the drawing in every respect.

Their requirements are binding as if they were written on the sheet. And they have a revision too. When the drawing does not specify a revision of a specification, the current revision usually applies, and that can change. So someone working from a specification saved on a computer

a few years ago may be working to outdated requirements. The title block also carries the approval fields: drawn, checked and approved. A drawing without approval is a draft, even if it looks finished. And in some organizations the document status appears too,

for example for reference only, or released for production. Manufacturing from a drawing that has not been released is working to a requirement that can still change. This gives a simple reading order.

First the title block: number, revision, sheets, units, standard and projection symbol. Then the general notes and the flag notes, and the documents the drawing refers to. And only then the views and the dimensions. them without knowing the rules they were written by.

The title block defines the identity of the drawing and its reading rules. The revision and the sheets determine exactly what is in your hands. Flag notes apply only where the flag appears, and a specific requirement overrides a general one. Referenced documents are part of the drawing, and they have a revision too.

And in the next chapter we will read assembly drawings: parts lists, balloons and tightening torques. See you in chapter seventeen.

17. Assembly Drawings

A part drawing says what one part looks like. An assembly drawing says how the parts come together. It does not redefine the geometry of each part. That is the job of the part drawings. But it defines what is assembled, how many of each, in which order,

with what force, and what must be achieved at the end. So misreading an assembly drawing can reject a whole assembly, even when every part on its own is conforming. In this chapter we will read the parts list, the balloons,

the assembly notes, and the dimensions that appear only in the assembly. An assembly drawing usually includes a view or a section showing all the parts in place. In an assembly section, as we saw in chapter two, shafts, bolts and pins are not hatched, and adjacent parts get hatching at different angles.

That way you can tell the boundary between two parts, even when they are made of the same material. There are few dimensions on an assembly drawing, and they belong to the assembly only: overall dimensions, locations, or dimensions to be achieved after assembly.

The parts list is the table that defines what goes into the assembly. It is defined in standards such as ISO 7573 and ASME Y14.34, and it usually has an item number, a part number, a description, a quantity, and a material or standard. The item number is the number that appears in the balloon,

and the part number is the number of the drawing or of the purchased part. Standard parts are described by their standard, for example an ISO 4762 screw, M8x25, property class 12.9. And for consumables, such as adhesive, sealant or shims,

the quantity is sometimes written as AR, as required. Someone who replaces a standard screw with one that looks identical but has a different property class changes the assembly. A balloon is a circle with an item number, and a leader line pointing to the part in the picture.

When the leader ends in a dot, it points to the surface of the part. When it ends in an arrowhead, it points to its outline. Every item in the list must appear in a balloon at least once. Identical parts that repeat several times get one balloon, and the quantity is written in the list.

And for fastener sets, such as a screw, a washer and a nut, a stack of balloons on a single leader is sometimes used. When there is a balloon with no row in the list, or a row with no balloon, that is an error on the drawing, and you need to ask.

Most of the assembly information is in the notes. A tightening torque, for example twenty-five newton meters, appears next to the screw or in a general note. And it must always come with a condition: whether the thread is dry or lubricated.

The same torque on a lubricated thread produces a much higher clamping force. In a joint with several screws, a tightening sequence sometimes appears too, for example in a cross pattern, and in several steps. Other notes define a threadlocker, lubrication, or a sealant, to a specification.

Someone who tightens without reading the condition may tighten less than required, or stretch the screw until it fails. The assembly drawing often shows the fits between the parts, for example H7/g6 next to a shaft in a bushing.

For an interference fit, the note also defines the assembly method: pressing, heating the outer part, or cooling the shaft. And when the assembly includes an adjustment, such as shims that close a gap, the drawing defines the final dimension to be achieved, not the shim thickness.

That is exactly the solution from the tolerance stack-up in chapter eight: measure at assembly, and select the right shim. Sometimes a part is not fully machined before assembly. A hole for a dowel pin, for example, is sometimes drilled through two parts together,

after they have been assembled, so that they line up exactly. On the part drawing this appears as a note such as drill at assembly, and the dimensions of the hole appear on the assembly drawing. Someone who drills the hole in advance in the single part, to a dimension,

loses the match that drilling them together was meant to give. And there are also dimensions that appear on the assembly as reference dimensions, in parentheses, just to give the picture, without requiring inspection. A large product is usually built like a tree: a top- level assembly, subassemblies, and parts.

Each level has its own drawing and parts list, and a subassembly appears in the top-level assembly as a single item. So when you look for a particular part, you sometimes have to go down several levels. An exploded view, in which the parts are drawn separated along the assembly line,

helps you understand the order, but it does not replace the parts list. And for parts that come in pairs, right-hand and left-hand, the drawing sometimes shows only one of them, and states that the other is its mirror image. A summary of the traps in an assembly drawing.

A balloon with no row in the list, or a quantity that does not match. A standard screw replaced with a different property class. A torque without a dry or lubricated thread condition. A part marked drill at assembly, drilled in advance.

And a shim whose thickness was set in advance, instead of by measurement. To read an assembly drawing, start from the title block and the parts list. Then go through every balloon, and make sure it appears in the list and that the quantity is right. Then read the assembly notes: torques, conditions, sequence, consumables.

And finally the dimensions and fits to be achieved after assembly, and whether there is any drilling or machining done together. Someone who starts assembling before reading the notes may find out at the end that the assembly sequence was part of the requirement.

An assembly drawing defines what, how many, in which order and with what force, not the geometry of each part. The parts list and the balloons must match each other, item by item. A tightening torque always comes with a condition, and sometimes with a sequence.

Adjustment and shims are defined by the final dimension, not by thickness. And drilling at assembly is done only after the parts have been assembled. In the next chapter we will get to know drawings for other processes: casting, forging, sheet metal and plastics. See you in chapter eighteen.

18. Casting, Forging, Sheet Metal, Plastics

Until now we have read mostly drawings of machined parts. But many parts are not born on a machine tool. Casting, forging, sheet-metal bending and plastic injection molding create the shape in a mold or die, not with a cutting tool.

So their drawings include information that does not exist on a machining drawing: draft angles, parting lines, radii, shrinkage and machining allowances. In this chapter we will learn to read this information, and what it tells the toolmaker, and whoever machines the part afterwards.

On a cast part, every wall parallel to the direction in which the part is withdrawn from the mold needs a small draft, so the part can come out. The draft usually appears in a general note, for example a draft of one to three degrees on all walls, not in every view.

The parting line, where the two halves of the mold meet, is marked on the drawing, because a seam can remain along it. And the radii also usually appear in a note, for example all unspecified radii three millimeters. A surface to be machined after casting gets a machining allowance,

and ISO 8062-3 defines both the allowance and the casting tolerance grades. Sometimes there are two drawings: one of the raw casting and one of the machined part. material to be removed is drawn with a phantom line. And raw surfaces are measured from datum targets, as we learned in chapter nine,

because they are not true enough to serve as a full datum surface. Forging also has draft and a parting line, but two more things as well. The first is flash: the excess material squeezed out between the two halves of the die. The drawing defines how much of it may remain after trimming.

The second is mismatch: the distance by which one half of the part is offset relative to the other half, along the parting line. Both have tolerances from standards such as EN 10243-1, and they usually appear in a note. And sometimes the grain flow in the material is marked as well,

because forging orients the grain flow, and that affects strength. Someone who machines a forged part without knowing where the parting line runs may fixture it on the seam, and get an unstable location. On a sheet-metal part, the drawing usually shows the formed part,

and sometimes the flat pattern as well. The bend radius is written explicitly, because it determines the length of the flat pattern and the risk of cracking. It is important to check which side of the bend a dimension is taken to:

the inside face or the outside face. The difference is the material thickness. On the flat pattern, the bend lines are marked, with the direction next to them: bend up or bend down. The rolling direction of the sheet is sometimes marked, because bending parallel to the rolling direction can cause cracks.

And a hole too close to a bend line can distort. So the drawing sometimes defines a minimum distance, or the hole is made after bending. machining, and are usually defined in a general note, to a standard such as ISO 2768 or a dedicated sheet-metal standard.

On an injection-molded plastic part, much of the definition is aimed at the mold. Here too there are draft angles and a parting line, plus a requirement for uniform wall thickness, so the part cools without warping. The drawing sometimes defines the gate location, or an area where it may be placed.

allowed, because they leave small circles on the surface. The dimensions on the drawing are the dimensions of the finished part. The toolmaker adds the shrinkage of the plastic on cooling himself. Tolerances for molded parts are defined in ISO 20457,

which replaced the German standard DIN 16742. And the surface texture is sometimes defined by a mold finish standard, such as SPI or VDI 3400. Some plastics absorb moisture, such as nylon. Their dimensions change with humidity, so the drawing defines when,

and in what condition, they are measured. A note such as measure after conditioning for twenty-four hours at twenty-three degrees is part of the requirement. Someone who measures a part right after molding will get different dimensions,

and may reject a good part or accept a bad one. There are a few things common to all these drawings. A surface left as it came out of the mold is sometimes marked with a surface texture symbol with a circle: material removal prohibited.

Dimensions between raw surfaces get wide tolerances, and dimensions of machined surfaces get machining tolerances. So it is important to identify for each dimension whether it is between two raw surfaces, between a raw and a machined surface, or between two machined surfaces.

A dimension between a raw surface and a machined one is usually the one that determines how much material will be removed, and where the part will be fixtured. A summary of the traps in drawings for these processes. Draft that was not taken into account: a dimension measured at the wrong end of a drafted wall.

A parting line or flash that was not identified, and fixturing on the seam. A sheet-metal dimension measured to the wrong side of the bend. Bending parallel to the rolling direction, even though the drawing marked the direction. And measuring a plastic part before the required conditioning.

On such a drawing, start by identifying the process and its general notes. Then identify the parting line, the direction of withdrawal, and the draft angles. Then identify which surfaces are raw and which are machined, and which points the raw ones are measured from.

And only then move on to the dimensions, with a clear understanding of which type of surface each one belongs to. Someone who reads a casting drawing like a machining drawing will demand accuracy the mold cannot deliver, or miss a requirement that exists only in the notes.

On drawings for molded parts, the shape is created in the mold, and the drawing adds draft, parting lines, radii and machining allowances. In forging, flash and mismatch are defined too, and sometimes grain flow. In sheet metal, the bend radius, the side a dimension is taken to,

and the rolling direction are part of the requirement. In plastics, the dimensions are those of the finished part, and the standard is ISO 20457. For materials that absorb moisture, measure after conditioning. And in every process, identify for each dimension whether it is raw or machined.

In the next chapter we will deal with critical characteristics and inspection: what a KC is, and what a first article inspection is. See you in chapter nineteen.

19. Critical Characteristics and Inspection

A drawing has dozens of dimensions, and they are not all equally important. Some dimensions, if exceeded, still leave a working part. And some, if exceeded, make the part fail, and sometimes put people at risk. The drawing marks these dimensions, and that marking determines how

they are manufactured, how they are inspected, and what is documented. In this chapter we will learn to read critical characteristics, and understand what first article inspection and measurement on a coordinate measuring machine require. A key characteristic, a KC, is a dimension or requirement whose

variation has a strong effect on function, safety or assembly. diamond, a hexagon, a letter in a box, or another symbol. So the meaning of the symbol is always defined in the notes on the drawing, or in the customer's specification.

Many organizations also have a classification of defects: critical, major and minor. A critical defect can cause a hazard, a major defect impairs the function, and a minor defect does not affect use. Someone who does not know the symbol reads a critical characteristic like any other dimension.

with a tolerance. It is a requirement for process control. It usually requires statistical control in production, not just inspection at the end. Sometimes it requires one hundred percent inspection of the parts, not sampling. And it requires documentation: who measured, with what,

and what the result was, for every part or every batch. And sometimes the process that produces it must not be changed without approval, even if the change looks small. A critical characteristic that passes inspection but was not measured according

to the procedure, as far as the customer is concerned, was not inspected. producing a critical characteristic, you measure its capability. Cp compares the tolerance width to the spread of the process: the tolerance width, divided by six standard deviations.

Cpk adds the location of the process: the distance from the mean to the nearer limit, divided by three standard deviations. A process can be narrow enough, but too close to a limit, and then Cp is good and Cpk is low. A common requirement is a Cpk of at least 1.33, and sometimes more for critical characteristics.

So someone who aims for the edge of the tolerance to leave material for rework lowers the Cpk, even when every part is within tolerance. First article inspection, FAI, proves that the process is capable of producing a part that meets every requirement of the drawing.

In aerospace it is defined in AS9102. The standard defines three forms: the first identifies the part and the drawing, the second documents materials, special processes and functional tests, and the third documents every single characteristic.

In the third form, every dimension, every tolerance and every note on the drawing gets a row, with the measured result. And this inspection is repeated after a design change, a process change, a move to another site, or a long break in production.

Someone who changes the manufacturing process and does not repeat the inspection is supplying a part that has not been proven to meet the requirements. For first article inspection to be complete, the drawing is ballooned. Every requirement gets a balloon with a number: a dimension,

a geometric tolerance, a surface texture, and even a general note. Every number is a row in the inspection report, so no requirement can be missed without its row staying empty. Notes such as edge breaks, part marking or coating also

get a number, and are inspected like any dimension. And on a multi-sheet drawing, the numbering runs across all the sheets, not just the first one. A coordinate measuring machine, a CMM, measures points on the part and calculates the geometry from them.

Its program must be built according to the datum reference frame on the drawing: the same datum features, in the same order. A program that builds its axes from other surfaces gives numbers that look accurate, but measure something else.

And the calculation method matters too: least squares, minimum circumscribed or maximum inscribed cylinder, as we saw in chapter six. So a CMM report must state the datum reference frame and the calculation method, not just the number.

The instrument that measures is also part of the result. instrument should be at most one tenth of the tolerance width. And a repeatability and reproducibility study, Gage R&R, checks how much of the spread in the measurements comes from the instrument and the operator, not from the parts.

parts and accept bad ones, and nobody will notice. traceability to a recognized measurement standard. Every measurement includes uncertainty. When a result is close to the tolerance limit, it is hard to know for sure which side of it the part is on.

ISO 14253-1 defines a decision rule: to prove a part conforms, the result must be within the tolerance, reduced by the uncertainty. In other words, the acceptance zone is narrower than the tolerance on the drawing. In some organizations the decision rule is defined in the contract or on the drawing,

and in others it is not. When it is not defined, it is worth agreeing on it in advance. And temperature is part of the measurement too: the dimensions on the drawing apply at twenty degrees, as we saw in chapter zero. A summary of the traps in inspection.

A critical characteristic measured like any other dimension, with no control and no documentation. First article inspection that is not repeated after a process change. A measurement program built from datum features other than those on the drawing. An instrument whose resolution is close to the tolerance width.

And a result right at the limit, accepted without taking uncertainty into account. Critical characteristics are marked with a symbol defined in the notes, and they require control, documentation and sometimes full inspection. Cpk measures both spread and location, and a common requirement is 1.33.

First article inspection to AS9102 checks every requirement on the ballooned drawing, and is repeated after every significant change. And in the next chapter we will get to know the drawing that has no sheet: model-based definition, MBD. See you in chapter twenty.

20. Model-Based Definition · MBD

In every chapter so far, the definition of the part has been a sheet: views, dimensions and notes. In many organizations this is changing. The definition moves into the 3D model itself, and the 2D drawing disappears or becomes secondary. This is called model-based definition, MBD.

In this chapter we will learn to read such a model, and what changes in the rules we have learned, when the model is the contract. be on the drawing is attached to the geometry itself. Dimensions, geometric tolerances, datums, surface texture and notes

are together called PMI: product and manufacturing information. There are two kinds of PMI. Graphical PMI looks like text on the screen, but the computer does not know which surface it belongs to. Semantic PMI is linked to the surfaces themselves, and the computer knows

which tolerance applies to which surface, relative to which datums. Only semantic PMI lets CAM software or a measuring machine read the requirements automatically. Y14.41, and on the international side in ISO 16792.

The rules for such a model are defined in ASME Y14.41, and on the international side in ISO 16792. The symbols themselves have not changed: the same GD&T symbols, the same frames and the same datums, only in 3D space. To transfer a model with PMI between different systems, the STEP AP242 format is used.

And for inspection results and measurement plans there is the QIF format, which links the requirement in the model to the measured result. An MBD model usually includes saved views, which correspond to the views on a drawing. Each saved view shows a particular viewing direction, and only the PMI

that belongs to it, so that not everything appears on the screen at once. When you select a tolerance, the system highlights the surface it applies to and its datum features. So in a good model there is no question which surface a note belongs to, as there sometimes is on a crowded drawing.

Someone who reads a model only through a picture of it loses all this information. Here there is a fundamental change compared to a drawing. In chapter zero we learned not to measure from the picture. In an MBD model, the geometry is the definition, and it is exact.

A dimension that is not written explicitly is queried from the model, as a basic dimension. And its tolerance comes from a general note, usually a profile of a surface tolerance on all surfaces, relative to a datum reference frame. For example: all unmarked surfaces, a profile of five tenths relative to A, B and C.

In other words, in an MBD model every surface is defined, even if there is no number next to it. When the model is the contract, its version matters exactly as much as a drawing revision. The file must be identified with a number and a version, and often with an integrity check of the file as well.

Many organizations add a reduced drawing: a 2D sheet with the important dimensions, the material and the notes, for convenience on the shop floor. But the reduced drawing is usually for reference only, and the model governs. So it is important to check what is stated about the relationship between them,

and which one governs when they contradict each other. Not every 3D file carries the same information. A native CAD file carries everything, but requires the same system. STEP AP242 carries exact geometry and semantic PMI as well.

Older versions of STEP, such as AP203 or AP214, usually carry only geometry, without the requirements. And triangle mesh files, such as STL, are an approximation of the geometry, not the geometry itself.

Someone who receives a model in a format that does not carry PMI receives a shape without tolerances, and that is not enough for manufacturing. The great advantage of MBD is that the same model can be used all the way through. The CAM software builds toolpaths directly from the geometry.

The measuring machine can read the semantic PMI and build a measurement program from it. And first article inspection can be built directly from the list of requirements in the model, instead of from manual ballooning of a drawing. But this requires a tool at every station that can display the model and its PMI.

A worker who has only a picture or a reduced drawing does not see some of the requirements. A summary of the traps in an MBD model. Measuring a surface from the model when its tolerance is defined elsewhere, without checking the general note.

Working to an old version of the model, because the file was saved on a local computer. Saving to a format that does not carry PMI, and losing all the tolerances. A reduced drawing that was not updated after a change to the model. And units: a model built in inches and opened as if it were in millimeters.

Start by identifying the model: number, version, and the status of the reduced drawing. Then the general notes: units, standard, and the general profile tolerance. Then the saved views, one by one, with the PMI of each. And only then queries on the geometry, for dimensions that are not written explicitly.

Someone who starts by measuring the model, without reading the notes, does not know which tolerance applies to what he measured. In MBD, the 3D model is the definition, and the PMI is linked to the geometry. requirements, and STEP AP242 transfers it between systems.

Dimensions that are not written are taken from the model, and their tolerance comes from a general note. And the model version matters like a revision, and the model governs over the reduced drawing. In the next chapter we will deal with change management:

revisions, change orders, and deviations. See you in chapter twenty-one.

21. Change Management

mistakes are discovered, and requirements change. And with every change, the important question is not only what changed, but whether everyone is working to the same definition. Change management is the system that ensures this: who requests, who approves,

from when the change applies, and what is done with what has already been made. In this chapter we will learn to read a drawing that has changed, and to tell a revision, a deviation and a waiver apart. A drawing that has changed has a revision block, usually in the upper corner.

Each row has a revision letter or number, a short description of the change, a date, and who approved it. The rules for this are defined in ASME Y14.35. Where something changed in the picture, a small triangle with

the revision letter sometimes appears, so it is easy to find. And around the border of the sheet there is a grid of letters and numbers, like on a map. The revision block states which zone each change is in. Someone who reads only the latest revision in the block,

and does not look for the markers in the picture, may miss a change that looks small. Not every change gets a new revision. Sometimes it gets a new part number. The rule is interchangeability: can an old part and a new part replace each other everywhere? the parts are interchangeable, and a revision is enough.

If the change affects one of them, for example a hole that moved and will not fit an old assembly, the new part gets a new part number. Otherwise, two different parts with the same number will sit in the stores, and someone will assemble the wrong one.

A change starts with an engineering change request, an ECR, which explains what the problem is and what is proposed. After approval, an engineering change order, an ECO, is issued, which defines exactly what changes and in which documents.

The order also defines effectivity: from when the change applies. For example from a certain serial number, from a date, or from a production lot. And it defines the disposition of what already exists: parts in stock, parts in work, and parts at the customer.

The options are usually: use as is, rework, or scrap. Someone who receives a drawing at a new revision without checking the effectivity may stop production that is still allowed, or continue production that is no longer allowed. There are situations in which the drawing is not changed, and yet it is not met.

A deviation is approval in advance to manufacture differently from the drawing, for a limited quantity or a limited time. For example, a different material because the material on the drawing is unavailable, for one hundred parts only.

A waiver is approval after the fact to accept a part that has already been made and does not meet the requirement. In some standards it is also called a concession. In both cases, the drawing does not change.

The approval applies only to the parts or the period defined in it. Someone who keeps manufacturing under a deviation after the quantity has run out is producing nonconforming parts. When a part does not meet a requirement, a material review board decides what to do with it.

Rework brings the part into full conformance with the drawing. After rework, the part conforms. Repair leaves the part different from the drawing, but usable. So repair requires engineering approval, and sometimes customer approval as well. Someone who calls a repair rework is hiding the fact that the part does not meet the drawing.

When working with a customer, there are changes the customer must approve. A change that affects form, fit, function, safety or cost is considered a Class | change, and requires customer approval. A minor change, such as correcting a spelling mistake,

is considered a Class II change, and sometimes a notification is enough. And a process change too, without a change to the drawing, can require approval, as we Saw with first article inspection in chapter nineteen. On the shop floor, the important question is which copy is in your hands.

An old printed copy is one of the most common sources of mistakes. So printed copies are sometimes marked as uncontrolled copies, or collected when a new revision is issued. A handwritten correction on a drawing, without a change order, is not a change. It is only a note. against the system, not just against the sheet in your hands.

A summary of the traps in change management. Working from an old copy, because it was the one available next to the machine. A handwritten correction treated as an approved change. A deviation used after its quantity or its period has run out.

A new revision, where a new part number was needed. Old stock that was not dealt with, because nobody read the disposition. And a process change, without repeating first article inspection. When you receive a drawing that has changed,

start from the revision block: what changed, and in which zone. Then look for the revision markers in the picture, and compare with the previous revision. Then read the change order: the effectivity, and the disposition of what already exists. And finally check that the related documents were updated too:

work instructions, inspection plans and machining programs. Someone who updates only the drawing, and keeps the old measurement program, will measure a new part to old requirements. The revision block, the markers in the picture and the

zones around the border show what changed and where. A change that breaks interchangeability gets a new part number, not just a revision. A deviation is approval in advance, a waiver is approval after the fact, and both apply only to what is defined in them.

Rework brings the part to the drawing, and repair leaves it different and requires approval. In the next chapter we move to the last part of the course, and read a drawing through the manufacturer's eyes. See you in chapter twenty-two.

22. Reading Through the Manufacturer's Eyes

Until now we have read drawings to understand what the designer requires. The manufacturer reads the same drawing with a different question: how do we make this, how much will it cost, and what can go wrong. This kind of reading is done before the quote and before work starts,

not after the part is already on the machine. In this chapter we will go through the drawing in the order an experienced manufacturer reads it, and see what to look for at each stage. The first pass is the title block: material, condition, quantity, revision and standard.

The material and the overall dimensions determine the stock: which bar diameter, which plate thickness, and how much machining allowance. A material that is not available in the right size changes the price and the lead time before work even starts.

coating, marking, and documents the drawing refers to. Every such reference is additional work, and sometimes an outside supplier and waiting time. The next question is how many setups will be needed. Every side of the part that has machined features is

usually another setup, and every setup has setup time. The datum reference frame says what to locate on: the primary datum feature is usually machined first, and serves as the basis for everything else. Features with a tight tolerance between them are best machined

in the same setup, so as not to introduce a transfer error. When the drawing requires a tight relationship between two sides of the part, you need to plan how the datum is transferred between setups. After that, look for what determines the process and the cost.

The tightest tolerance on the drawing sometimes determines the entire process: grinding, reaming, or a separate finishing operation. A low roughness, or a very small geometric tolerance, also adds an operation. A sharp internal corner in a pocket is a well-known trap.

An end mill always leaves a radius, and a truly sharp corner requires EDM. So when there is no internal radius on the drawing, ask which radius is allowed, before quoting. A deep, narrow hole, with a depth of more than ten times the diameter, requires a special deep-hole drill, with through-tool coolant, and a long time.

And thin walls distort during machining and clamping, and need to be planned for in advance. A long, slender shaft, with a length of more than four times the diameter, will deflect in turning without support. It requires a tailstock center or a steady rest, and that affects the setup and the time.

chatters and limits the speed and the surface finish. A deep internal thread in a blind hole, a narrow groove, or a very small radius: each of them requires a special tool. A manufacturer who identifies all of these in advance quotes correctly and plans correctly.

A manufacturer who discovers them on the machine loses money. As we saw in chapter thirteen, the notes define a sequence of operations. Heat treatment in the middle of the process requires leaving a machining allowance, and planning finish machining after it.

Coating at the end of the process requires knowing whether the dimensions are before or after coating, and masking the areas that must not be coated. Every such outside step adds lead time, so it is part of the planning and of the price. An experienced manufacturer also checks how he will

measure every dimension, before he makes anything. Does he have an instrument with enough resolution for the tightest tolerance? Are there critical characteristics that require statistical control or inspection of every part? Is first article inspection required, and what does it include?

And when inspection requires equipment he does not have, he needs to decide in advance whether to send it out for inspection, or to ask. From this whole pass, a list of questions for the designer is built. Dimensions that contradict each other, missing tolerances,

an undefined datum feature, or a coating with no thickness. Features that cannot be made as drawn, such as a sharp internal corner. And sometimes suggestions too: a larger radius, a wider tolerance that does not harm the function, or a more available material.

But a suggestion is a question, not a decision. As we Saw in chapter zero, a manufacturer does not change the drawing on his own. And a question asked before manufacturing costs much less than one discovered after the part has been rejected.

In a quote, the drawing is translated into time and material. The setup time for each setup is spread over the whole quantity, so in a small quantity it is a large part of the price. The cycle time per part is determined mainly by the tolerances,

the surface finish and the amount of material removed. And special processes, such as heat treatment, coating and testing, come with their own price and lead time. Someone who quotes by geometry alone, without the notes, loses money on every part.

A summary of the traps in reading through the manufacturer's eyes. A quote without reading the notes and the referenced documents. Assuming the general tolerance is loose, without checking the title block. A sharp internal corner, or a deep hole, discovered only on the machine.

and get asked only after the part has been rejected. The manufacturer reads the title block and the notes first, and determines the stock, the material and the outside processes. The datum reference frame determines the setups,

and tight relationships are machined in the same setup. difficult features determine the process and the cost. And every ambiguity becomes a question for the designer, before manufacturing, not after. In the next chapter we will practice everything we have learned ina

diagnostic workshop: drawings with errors, and we will find them together. See you in chapter twenty-three.

23. Diagnostic Workshop

In this chapter we will not learn anything new. We will use what we have learned. We will look at six drawings, and each of them has one error. After each drawing we will pause for a moment. Try to find the error yourself, before we reveal it. And for every error we will ask three questions: what is wrong,

what will come out of it in production, and what do we ask the designer. Here is a plate with three dimensions: forty, eighty, and one hundred twenty for the overall length. Each of them has a tolerance of plus or minus one tenth. What is wrong? The dimensions close a chain. The overall length is defined twice:

once directly, and once as the sum of the other two dimensions. If the two smaller dimensions are at their upper limit, the sum is one hundred twenty point two, and that is already outside the tolerance of the overall dimension. The manufacturer does not know which dimension to honor.

So we ask the designer which of them is a reference dimension, in parentheses. Here is a position tolerance frame, referring to datums A and B. Only datum A is identified in the picture. What is wrong? Datum B is not defined anywhere on the drawing, so the tolerance is incomplete.

Every manufacturer will choose a different surface, and every measuring machine will build a different reference frame. The results will not be comparable. The question for the designer is simple: which feature is datum B? Here is a hole with a position tolerance of one tenth, relative to A, B and C.

Its location is defined by dimensions of thirty and twenty, with a tolerance of plus or minus five hundredths. What is wrong? With a position tolerance, the dimensions that locate the feature must be basic dimensions, in a frame, with no tolerance.

Here there are two contradicting definitions: a square zone from the dimensions, and a round zone from the geometric tolerance. The manufacturer does not know which to inspect. The question for the designer: are the dimensions supposed to be basic dimensions?

Here is a hole with an H7 fit, and a note: zinc plating, eight microns. There is no note about a masked area, and no note on whether the dimensions are before or after plating. What is wrong? Eight microns of plating on each side reduces the hole by sixteen microns,

and that is almost the entire H7 tolerance width at this diameter. If the part is machined to the drawing and then plated, the hole will come out of tolerance. The question for the designer: should the hole be masked during plating, or does the dimension apply after plating?

Here is an M8 thread, sixteen deep, in a blind hole. The tap drill depth is also defined as sixteen. What is wrong? The tap drill hole must be deeper than the thread, to leave room for the tip of the tap. At equal depths, the thread will not be full to the bottom, or the tap will hit the bottom and break.

The question for the designer: what is the tap drill depth, or what full-thread depth is really required? Here is an ISO fillet weld symbol, with a double reference line, and the number five to the left of the triangle. What is wrong?

In ISO, a letter must appear before the number: a for throat thickness, or z for leg length. Without a letter, five can be a throat thickness of five, meaning a leg of about seven, or a leg of five. The difference is about thirty percent in strength. The question for the designer: a or z? In each of these cases, the drawing looks complete at first glance.

The error was not in the picture, but in the relationship between two details: a dimension and a dimension, a tolerance and a datum, a fit and a coating. but checking that the details agree with each other. In every case, the solution was not to choose an interpretation, but to ask.

A manufacturer who chooses an interpretation on his own takes on the responsibility for the result. A good question for the designer is short and unambiguous. It states the drawing number, the revision, and the location on the sheet, by the zone on the border. It describes the problem in one sentence, and offers one or two options.

For example: on drawing number such-and-such, revision C, zone B3, datum B is not defined. Is the bottom surface intended? A question like that is answered quickly, and leaves no room for interpretation. And a question that was asked and answered in writing is

kept with the drawing, so the next production run knows too. A summary of the traps in the workshop. Reading each detail on its own, and not checking the relationship between them. Choosing a convenient interpretation, instead of asking.

Asking verbally, without documenting. And correcting the drawing ourselves, by hand, as if it were an approved change. We saw Six errors: a closed chain, a missing datum, position with ordinary dimensions, plating on a fit, a short tap drill hole, and a weld with no letter.

In all of them the error was in the relationship between details, and in all of them the solution was a question. In the next chapter, the last in the course, we will bring everything we have learned together into a complete reading protocol, step by step.

See you in chapter twenty-four.

24. A Complete Reading Protocol

This is the last chapter of the course. Throughout the course we learned each part of the drawing separately: views, dimensions, tolerances, datums, materials and documents. In this chapter we will bring it all together into one protocol, ten steps, that suits any drawing.

The goal is not to skip any step, and not to discover a problem only when the part is already on the machine. The first step is to check what is in your hands. The drawing number, the revision, and the number of sheets.

The revision must match the one on the order. And also check the document status and the approvals: a drawing that has not been released is still a draft. The second step is to read the rules the drawing was written by.

The units, the projection symbol, and the tolerancing standard, which determines whether the envelope principle or the independency principle applies. And then the general tolerances and the general notes. They apply to every dimension that has no tolerance of its own.

The third step is the material and its condition, the heat treatment, and the coating. And with them, all the documents the drawing refers to: material specifications, process specifications and inspection standards. From here you can already know what the stock is,

which outside processes will be needed, and in which order. The fourth step is to understand the shape. Go through the views and the sections, and build a 3D picture of the part in your head. And pay attention to conventions and simplifications, such as threads,

symmetrical parts and hidden lines, so you do not read them as ordinary geometry. The fifth step is the datum reference frame. Identify the primary, secondary and tertiary datums, and the order between them. The datum reference frame determines how the part is set

up in manufacturing, and how it is fixtured in inspection. The sixth step is to go through every dimension. For every dimension, check what type it is: a toleranced dimension, a basic dimension, or a reference dimension.

Check the dimension chains, and that no dimension is defined twice. whether it is a clearance, transition or interference fit. The seventh step is to go through every feature control frame. In every frame ask: what does it apply to, what is the shape of the zone,

relative to which datums, and is there an MMC or LMC modifier. And check that every datum that appears in the frame is actually identified on the drawing. The eighth step is everything defined by symbols and references. tap drill holes, welds, edges, undercuts and splines.

This is where many of the errors we saw in the diagnostic workshop are found, because they look small. The ninth step is to identify critical characteristics, and plan the inspection. Which dimensions are marked as critical, and what they require:

control, documentation, or inspection of every part. Is first article inspection required, and is there a suitable measuring instrument for every tolerance. The tenth step is to collect everything that is unclear. Every contradiction, every missing tolerance,

and every feature that cannot be made as drawn, becomes a question. The question includes the drawing number, the revision and the zone, and it is sent to the designer before work starts. And the answers are kept in writing, with the drawing.

On an assembly drawing, add the parts list, the balloons, the assembly notes and the torques to the protocol. In an MBD model, the steps are the same, but they are read from the saved views and the PMI, not from a sheet.

And on a drawing that has changed, start from the revision block, and check what changed and what the effectivity is. You might ask why a protocol is needed, if you know how to read a drawing. The answer is that most of the mistakes we saw in this course did

not come from a lack of knowledge, but from a step that was skipped. A revision that was not checked, a general note that was not read, or a datum that nobody noticed was missing. A fixed protocol turns reading into a routine, and routine is what prevents mistakes.

In this course we started from the drawing as a contract, and went through its whole language. Views and sections, dimensions and tolerances, fits and stack-ups, datum reference frames and geometric tolerances. Surface texture, welds, materials and threads, and then the drawing as a document:

title block, assembly, processes, inspection, the model and changes. And at the end, reading through the manufacturer's eyes, a diagnostic workshop, and one protocol that ties it all together. A drawing is a contract. Whoever reads it completely

makes what is required, and asks before making a mistake. Thank you for learning with us. mechanical engineering material, can be found at METAL HUB. Good luck reading your next drawing.

Goodbye.