Designing and building any kind of mechanical system is a complex process that needs to properly account for many different parameters, like cost, materials, and manufacturing techniques. But one of the key challenges is making sure that all of the parts, once manufactured, will fit together and function as intended. And that's why tolerancing is such an important part of the mechanical design process.
The easiest way to define tolerances is using the dimensional approach, where drawings define how much each dimension of a part is allowed to deviate from its nominal value. But dimensional tolerancing doesn't work particularly well in a lot of scenarios because it doesn't really reflect how the part will be used. It doesn't let you specify that you need a surface to be flat because it has to create a seal with another part, for example, or let you control how close to perpendicular the axis of a hole needs to be to the surface it's drilled into.
Geometric dimensioning and tolerancing, usually called GD&T, is a different approach to tolerancing that allows you to control tolerances in a way that reflects the intended function of the part. It complements dimensional tolerancing by letting you control 14 different geometric characteristics, helping you better communicate which aspects of your design are important. These characteristics can be split into 5 categories that control Form, Orientation, Location, Profile and Runout.
Unlike the traditional tolerancing approach that applies tolerances to dimensions, GD&T applies them to features instead. A feature could be a surface, a hole, or a slot, for example. It's important to differentiate between surface features, which are just individual surfaces, and features of size, which are any features that have a defined dimension, meaning that they can be measured with callipers, whether that's a hole, or a feature defined by two opposed parallel surfaces.
This is because in the GD&T world geometric tolerances can mean very different things if they're applied to surface features or to features of size. Geometric tolerances are assigned to features using feature control frames. These little grids contain all of the information needed to fully control a particular geometric characteristic.
They can be applied to features using leader lines, extension lines, or for features of size they can be attached directly to dimensions. Let's look at how they're structured. The first box in the frame contains a symbol that defines which of the 14 geometric characteristics is being controlled.
The next box specifies the tolerance to apply. This value defines the size of a tolerance zone within which the entirety of the feature must be located. The shape of the zone depends on the geometric characteristic being controlled - a diameter symbol can be added to indicate that the tolerance zone is circular or cylindrical.
Next is a series of letters that defines datums, the reference surfaces that need to be considered during inspection. And finally modifiers can be added to either the tolerance or to the datums, to get even more control over tolerancing. We'll talk about datums and modifiers in more detail later on, but first let's look at an example, starting with one of the simpler geometric characteristics, flatness.
The feature control frame for a flatness call-out looks like this. When the call-out is applied to a surface it defines a tolerance zone between two parallel planes that are separated by the distance shown in the feature control frame. All manufactured parts are imperfect – for a part to meet this tolerance all points on the surface must be located within the tolerance zone.
The two planes defining the tolerance zone are parallel to each other, but they don't have to be parallel to any other surfaces. Flatness tolerances are often specified on surfaces that mate with other parts and need to have even contact, like the face of a flange. Flatness tolerances can also be applied to features of size, in which case the tolerance zone applies to the derived median plane of the feature.
The derived median plane is constructed by taking the midpoints of opposite points on the two surfaces that define the feature of size. Since the surfaces are imperfect, the derived median plane will be too. When learning about GD&T it's often useful to think about how a part will be inspected to see if it meets the geometric tolerance.
Flatness of a surface can easily be measured using a dial test indicator. First the part is mounted on three jacks, and the jacks are adjusted so that the indicator reads zero at three defined points. This creates a reference plane.
The indicator is then swept across the surface to identify high and low points. If the distance between the highest and lowest points is less than the width of the tolerance zone, the flatness requirement is met. Another very common inspection approach is to use a CMM, a coordinate measuring machine.
A computerised probe is used to take measurements that are fed into software that then uses algorithms and curve fitting to determine deviations from the perfect size. CMMs are expensive pieces of equipment but can be used to inspect any kind of geometric tolerance. Next in the Form category of geometric tolerances is Straightness.
It's similar to Flatness, but is applied to individual lines instead of to an entire surface. When applied to a surface feature, any line on the surface in the same direction as the line the call-out is pointing at must be within a tolerance zone defined by two parallel lines. For inspection the probe is swept along multiple straight lines instead of being swept across the entire surface.
When straightness is applied to a feature of size instead of a surface, the tolerance zone is cylindrical and it applies to the axis of the feature. You might apply a straightness tolerance to the axis of a pin, for example, to make sure it will engage properly with a hole. The circularity tolerance is used to control how round a surface is.
The tolerance zone is defined by two concentric circles, the radial distance between the two circles being equal to the specified tolerance. Circularity controls the roundness of individual cross-sections completely independently. This means the tolerance zones don't need to be on the same axis, and the diameter of the concentric circles can vary along the length of the feature.
Circularity can be inspected in a few different ways but ideally the part should be rotated and a probe used to measure displacements at several different cross-sections. The measurements are plotted on a polar graph to determine if the tolerance is met. Cylindricity is the last of the four form tolerances.
It's similar to circularity except the tolerance zone is uniform along the full length of the feature. Form tolerances control the shape of a single surface, axis or plane. But most other tolerance types control the geometry of a feature relative to one or more references, that are called datums.
Datums are identified on drawings using a letter and this triangle symbol, and can be attached to features in a few different ways. Datums are usually defined using surfaces, but if the symbol is attached to a feature of size the datum is the corresponding centreline or centre plane. Datums are used to locate features by defining how a part should be immobilised when inspecting a geometric tolerance.
To be accurate with the terminology we need to differentiate between a datum feature, which is the feature on the object that's restrained, a datum, which is the theoretical perfect surface corresponding to that feature, and a datum simulator, which is a real imperfect surface that will be used to immobilise the part to approximate the perfect datum. A part just floating in space is said to have six degrees of freedom - it can translate left and right, up and down, and forward and back, and it can rotate around those three axes. If we hold the datum feature against a datum simulator, three of the six degrees of freedom are immobilised.
The part can now only translate left and right, and up and down, and it can only rotate around a single axis. Restraining one more datum feature constrains another two degrees of freedom. And by restraining a third the part is fully immobilised and can be inspected.
These datums establish a datum reference frame, the coordinate system used to inspect the feature. The order in which the datums are applied is important because all real surfaces are imperfect - using datums in the same order ensures that measurements are repeatable. To see why let's look at an example where we want to measure where the centre of the hole is located.
Since we held the part against datum simulator B first it will have a minimum of three contact points with datum feature B. Datum simulator C will have a minimum of two contact points with datum feature C, and datum simulator F will have a minimum of one contact point with datum feature F. The datums are listed in order in the feature control frame.
If we change the order in which the datums are applied, or if we use different datums, the part will be set up slightly differently for measurement. All of the remaining geometric tolerances use datums. Let's look at the orientation group of tolerances next.
They're used to control the angles between features. Parallelism controls how close a feature is to being parallel to a datum. The tolerance zone is defined by two planes that are parallel to the specified datum.
Perpendicularity works in the same way, but the tolerance zone is at 90 degrees to the datum. And angularity is a more general orientation tolerance that controls the angle between a feature and a datum. When applied to features of size, the orientation tolerances apply to the centre plane or axis of the feature.
The diameter symbol is used in this feature control frame to specify that the tolerance zone for the axis of the feature is cylindrical. To meet the tolerance the axis must be contained within the tolerance zone. Parallelism is inspected in a similar way to Flatness, but instead of mounting the part on jacks the datum feature on the part is placed directly on the datum simulator.
Perpendicularity can be checked in the same way. And angularity can be checked using a sine bar, that allows angles to be measured accurately. There are three location tolerances - position, concentricity and symmetry.
Although they all appear in the ISO standards, the concentricity and symmetry tolerances were removed from the 2018 edition of ASME Y14. 5, so I won't cover them in this video. Position is one of the most commonly used geometric tolerances.
It defines the maximum distance the axis or median plane of a feature of size can be located away from its theoretically exact position. It's often applied to control the location of holes. The theoretically exact position of the feature, called the true position, is defined using basic dimensions, which are enclosed in a box to show that normal dimensional tolerances don't apply to them.
The position tolerance establishes a cylindrical tolerance zone around the true position. To be acceptable the axis of the hole must be contained within the tolerance zone. The position of a hole can obviously be defined using dimensional "plus and minus" tolerances, so you might be wondering why the geometric tolerance approach is any better.
There are a few reasons. One big advantage is that dimensional tolerances define a rectangular tolerance zone, but in almost all cases it makes more sense to use a cylindrical zone, which is evenly distributed around the true position of the hole. Another advantage of the geometric tolerance approach is that it allows you to explicitly define the relevant datums and the order in which they should be considered.
For holes the primary datum is usually chosen to be the datum perpendicular to the axis of the hole, because the hole axis being perpendicular to the mating surface is usually more important than its position on the surface. And finally, using a position tolerance allows a bonus tolerance to be gained by applying modifiers. Modifiers are an important part of GD&T that allow the tolerance zones applied to features of size to be increased by an additional bonus tolerance, depending on how close the feature is to its size limits.
This hole is a feature of size, and its limits of size are defined by dimensional tolerances. The hole has a maximum allowable diameter of 9. 8 millimetres, and a minimum allowable diameter of 9.
2 millimetres. GD&T identifies three different conditions for any feature of size - a maximum material condition, a least material condition and a regardless of feature size condition. The maximum material condition occurs when the feature is at the size limit where it has the most amount of material.
For a hole this is the smallest allowable hole size. And for a pin it's the largest allowable diameter. The least material condition is the opposite case where the feature has the smallest allowable amount of material.
By default geometric tolerances apply at the Regardless of Feature Size condition, meaning that the size of the tolerance zone is defined by the tolerance value in the feature control frame, and it doesn't change. But this behaviour can be adjusted by including a modifier, either the letter M for MMC or the letter L for LMC, next to the tolerance in the feature control frame, which adds a bonus tolerance to the tolerance zone depending on the actual size of the feature. Let's look at an example for MMC, which is the most commonly used modifier.
Here it's applied to the position of a hole. The modifier means that the tolerance zone in the feature control frame applies at the maximum material condition, which is the smallest allowable hole. If the hole is larger than MMC, a bonus tolerance is added to the position tolerance that's equal to the difference between the actual size of the feature and the maximum material condition.
One common use of the MMC modifier is where it's applied to benefit from the fact that a hole is oversized, and so its position can be less accurate and still fit with a mating part. The LMC modifier is less commonly used but works in a similar way. It adds bonus tolerance when the actual size of the feature has more material.
This can be used if you have a hole close to an edge for example, and you need to apply a tight tolerance to the position of the hole to make sure there's sufficient material between the hole and the edge, but you want to relax the tolerance if the hole is smaller. The MMC and LMC material modifiers can be applied to other tolerance types like flatness or perpendicularity, and can even be applied to datums if they're features of size, although that's outside of the scope of this video. Material modifiers aren't the only way that the form of a feature can be affected by its size.
A key concept that appears in the ASME standard is the Envelope Principle, which is also referred to as GD&T Rule Number 1. It states that "the surface or surfaces of a regular feature of size shall not extend beyond an envelope that is a boundary of perfect form at MMC". Let's look at an example to see what this means.
This pin has a nominal size of 12 millimetres with a dimensional tolerance of plus or minus half a millimetre. Rule Number 1 establishes an envelope around the pin based on the maximum material condition, which is the largest possible diameter of 12. 5 millimetres.
According to Rule Number 1, no part of the pin surface is allowed to extend beyond this envelope. This means that the MMC limit of size controls not only the size but also the form of the pin. If the actual size of a manufactured pin is 12.
5 millimetres, meaning that it's at MMC, then it will need to have perfect form to fit into the envelope. If the actual size of the pin is smaller than MMC, the pin doesn't have to have perfect form - it can be slightly bent, or barreled, for example. To be acceptable the pin has to be within the limits of size, be contained within the MMC envelope, and meet any other geometric tolerances that have been defined.
Rule number 1 is the default behaviour in the ASME standard, and its purpose is to ensure that parts will fit together properly. This pin will always fit in a hole that's larger than the MMC envelope. The ISO standard works differently - it uses the Independency Principle by default, where the geometric form and the size of a feature are considered separately.
When using this approach the limits of size do not control form at all. The pin could be completely bent and still acceptable so long as it is within the limits of size. When using the Independency Principle there's no guarantee that the pin will fit in a hole larger than the MMC envelope.
Additional geometric tolerances need to be applied to control how straight the pin is. Modifiers can be used to change the default behaviour. If the E modifier is used on a drawing to the ISO standard, it means that the Envelope Principle applies.
And if the I modifier is used on a drawing to the ASME standard it means that the Independency Principle applies. ASME defines a few other special cases where the Envelope Principle is overwritten - for example if a flatness or straightness tolerance has been called out explicitly for a feature of size. But anyway that's enough about modifiers and the Envelope Principle - let's go through the remaining tolerance types.
Profile tolerances are very versatile and can be used to control the form, orientation and location of features all at the same time. The Profile of a Surface tolerance creates a tolerance zone that follows the shape of the toleranced feature, with a width equal to the specified tolerance. Profile of a Line is similar to Profile of a Surface, but it controls individual line elements of a surface, instead of the entire surface at once.
The inspection of complex profile tolerances can be difficult without a CMM, although it really depends on the application and the complexity of the surface. In some cases profile tolerances can be used instead of other tolerance types. Applying a Profile of a Surface tolerance to a single nominally flat surface without datums, for example, is the same as applying a flatness tolerance.
Finally we have the runout category of tolerances. Runout is a term used to describe the eccentricity of a surface relative to a particular axis. There are two runout tolerances, circular runout, and total runout.
Circular runout controls the roundness of individual cross-sections of a feature relative to a datum axis. In this case the datum axis is defined by datum feature A. The tolerance zone is defined by two concentric circles.
This is similar to the circularity tolerance zone, except that circular run-out uses datums so the tolerance zones must be centred on the datum axis. Like circularity, circular run-out only controls individual cross-sections, so the radius of the tolerance zone can vary along the axis of the feature. Circular runout can be inspected by rotating the part around the datum axis and using a dial gauge to measure deviations.
Total runout, which has two arrows in the symbol, is used to control runout along the axial direction as well, so the tolerance zone is defined by two concentric cylinders. During inspection the dial gauge is moved along the part to see if there are any deviations outside of the tolerance zone. Runout tolerances are often applied to rotating parts like shafts, because any significant eccentricity relative to the axis of rotation can cause unwanted vibration.
GD&T is a pretty complex topic and it's impossible to cover everything in a single video, but hopefully this has given you a solid understanding of the fundamentals. If you enjoyed the video, you might be interested in hearing about Nebula, the creator-built streaming site where you can watch exclusive videos from The Efficient Engineer that aren't on YouTube. There's the video on The Future of Engineering Drwings, for example, that explores recent trends related to engineering drawings, like the move towards model-based design and the use of statistical tolerance analysis.
Or the video on Hydraulic Systems. Or the one on Dimensional Analysis. .
. There's loads of amazing content from other creators on there too, including exclusive videos from Mustard, RealLifeLore and Neo. And all of the videos on Nebula are completely ad-free and there are no sponsor messages, so you can watch without interruption.
To make Nebula even better, we've teamed up with CuriosityStream, who have kindly sponsored this video, to create an unbelievable bundle deal that includes both streaming sites. CuriosityStream is home to thousands of high quality documentaries covering all kinds of different topics, including space, technology, history and the natural world. I've recently been enjoying Oddly Satisfying Science, a really fun series that uses loads of fascinating experiments to investigate interesting science topics like combustion, resonance and magnetism.
And here's why the bundle is such a good deal - if you sign up to any of the CuriosityStream annual plans using this link and enter the code "efficientengineer", you'll not only get a 26% discount, but you'll also get full access to Nebula, for free. The landing page is a little confusing, but if you use the "efficientengineer" code when signing up for any annual plan you'll receive an email from Nebula with instructions on how to set up your free account. That's less than $15 to get access to both sites for a full year.
It really is a great deal. So to get the bundle deal head over to curiositystream. com/efficientengineer, or click the on-screen link, and use the code "efficientengineer".
Every single person who signs up using this link will be directly supporting this channel, helping me continue to create engineering videos. And that's it for this introduction to GD&T, thanks for watching!
