Understanding GD&T

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!