This time around, I’d like to present another “pet peeve” of mine, at least in the world of GD&T. It involves using the position symbol when the only quality being controlled is perpendicularity.
This is very common — it stems from some subconscious notion that if GD&T is going to be used on a hole, it’s got to be the “true position” symbol. NO!
Consider the following example. There is a position tolerance applied to the large hole on the left, and the datum being referenced is A.
But let’s go to the standard and examine how the geometric control called “position” should be used: ASME Y14.5-2009 (and prior editions) state that position’s main job is to control location — meaning that it involves a distance — and perpendicularity often comes along as part of that position control.
Since the large hole given above is already distanced from the edges by plus/minus dimensions, the geometric tolerancing has nothing to do with location. The only relationship that the large hole has with datum A is one of orientation. Therefore, an orientation symbol must be used:
Notice the perpendicularity symbol. This is the correct way to identify this hole, since the hole itself now becomes the datum feature for other features to locate back to.
That said, there are no GD&T police that will haul you to jail if you insist on using the position symbol. But recall that the purpose of geometric tolerancing is to use a standardized language to express the design requirements. So it’s best to stick with the proper terms and symbols if you want to minimize confusion when expressing your requirements!
One final footnote — there are times when a position tolerance may reference only one, perpendicular datum: If a pattern of features (two or more) are being positioned with one feature control frame, then a single datum plane is allowed (because there is the location between the two features that position controls). And another example is that of coaxial features; we may have one diameter positioned to another diameter, and this “coaxiality” is indeed a location control.
Occasionally users of GD&T suggest that everything be simplified by just boiling all 14 symbols down to just two or three. (What, you didn’t know there were 14 symbols? Click here for a handy chart!)
There is some logic to what these people are saying — namely, that many GD&T symbols overlap others, and position and profile can be used in such a way as to cover the others. But as you might guess, there are pros and cons to this.
- First, realize that position always controls two qualities: location and orientation. Location is obvious, but don’t forget orientation — because position extends all the way through the depth of a feature, it will control any tilt or angling of that feature.
- Profile of a surface, if used with datum references and basic dimensions tying it back to those datums, can control all four required qualities: location, orientation, size, and form (shape). Since it covers ALL of these, it can be argued that the other GD&T symbols could be ignored and simply use this one symbol (well, two if you count profile of a line).
But there are two problems with this minimalist philosophy: For one thing, it may sometimes be necessary to really only control a particular aspect, such as parallelism. You wouldn’t want to use position, since we don’t care so much about location. And you wouldn’t use profile, because form control is not needed!
Second, though the minimalist philosophy seeks to simplify drawings, it can actually make it harder for people to decipher what you are trying to say. I mean, come on — if you want something to be perpendicular, what’s so hard about understanding the perpendicularity symbol? Profile might do the same thing, but recall that profile can be applied to any angle, so it doesn’t immediately mean 90º to the reader (although the drawing makes a corner look like 90º, what if it’s an 89º corner and you didn’t look too carefully for an angular dimension?).
So the bottom line is: While it is possible — and often desirable — to use position and profile to control multiple qualities of a feature, we shouldn’t ignore the other symbols, which have a definite role to play in the GD&T world.
Another new feature that was introduced in the 2009 standard (ASME Y14.5-2009) is the option of creating a “non-uniform” tolerance zone for either of the two profile symbols.
Recall that the profile symbols normally specify a uniform boundary or bandwidth that is centered around the “true” or perfect profile. This true profile is first established by basic dimensions on the drawing or by referencing the CAD model, which is the perfect design. Here’s a traditional profile callout:
where the tolerance zone looks like:
Notice that the 2 mm zone follows the exact contour of the intended design — this is how profile tolerances have always been understood, and will continue to be understood if no other indication is made. But the latest version of the Y14.5 standard allows a non-uniform zone, where the feature control frame simply says “non-uniform,” but it is then required that the zone be described in detail on the drawing or by referencing a note or other detailed information. An example:
Notice that each side of the tolerance zone has a different radius; the surface of the actual manufactured part can now deviate anywhere within these two curved planes. There may be various reasons why the designer wishes to do this.
I should also mention that the “non-uniform” profile usage may have a tolerance zone of any shape — it doesn’t have to always be a radial type as given here. Of course, if you have your new copy of Y14.5, you may read more about this in paragraph 8.3.2.
On an unrelated note, I can share with you that our training schedule is getting quite busy for the first half of 2010! Despite the recent economic woes, it seems that many managers are aware of the value in having all their engineers trained in the new standard. So if you haven’t already, please contact us to obtain a detailed proposal to have our seminar offered at your company.
I wrote about this a long time ago, but it’s worth mentioning again as the new year approaches (for people who still do New Year’s resolutions!). Regular GD&T users should be aware of the certification process for GD&T Professionals.
The American Society of Mechanical Engineers (ASME) has established a credential for GD&T proficiency, called GDTP, which stands for ‘Geometric Dimensioning and Tolerancing Professional.’
It is a testing process that measures your ability to interpret and apply tolerances correctly. It is not a license to practice GD&T (no one can legislate that) but it is something that looks nice on your resume!
There are actually two certification levels: the Technologist Level, which measures your ability to read GD&T; and the Senior Level, which tests not only interpretation, but also the application of GD&T to a design. One does not necessarily need to become a Technologist first; some people go right for the Senior Level, although they are required to document at least five years of experience in GD&T (and they have a more difficult test!).
If you decide to pursue either level, be aware that the questions on the test come from all sections of the 1994 Y14.5 standard. (UPDATE — summer 2017: They now offer the exam based on the 2009 standard, or you can still do the 1994 version if you wish.) Each chapter has a “weight” that determines the number of questions from the chapter that appear on the test. This means that there is more than just GD&T; you need to be familiar with the nuances of traditional tolerancing as well as the many definitions contained in that standard. Some questions representative of the Technologist Level:
Sample question #1:
A dimension ‘not to scale’ is symbolized by:
a. placing the number in parentheses
b. placing a line under the number
c. including NTS after the number
d. italicizing the number
Sample question #2:
If a datum feature of size is applied RFS, a datum displacement is:
a. not allowed
b. allowed at MMC
c. allowed at LMC
d. allowed at the resultant condition
Sample question #3:
When applied to planar surfaces, angularity, parallelism, and perpendicularity also control:
d. Rule #1
Sample question #4:
Which of the following datum feature symbols is incorrect?
The GDTP process is not for everybody, but if it’s something that might interest you, contact us for some guidance or you may visit ASME’s website for more detail:
FYI — the answers are: b, a, c, and “Q,” respectively. If you got all those, send a comment and I’ll post some questions from the Senior-level test next time!
OK — time to dive into another item that is new in the world of geometric tolerancing. The standard that was released earlier this year expanded the definition of a “feature of size.” This has an impact in that some GD&T symbols can only be applied to “features of size,” most notably position.
The 1994 standard defined a feature of size as a single entity: “One cylindrical or spherical surface, or a set of two opposed elements or opposed parallel surfaces….” This is just a fancy way of describing things like a hole, pin, a part thickness, or other feature that can be measured directly for size.
A traditional “feature of size”
The 2009 standard now breaks “features of size” into two categories: regular and irregular features of size. The regular feature of size keeps the definition given above. The irregular feature of size is new: it is defined as “a directly toleranced feature or collection of features that may contain or be contained by an actual mating envelope….”
Thus, a grouping of objects can now form a “feature of size.” This allows a geometric tolerance to be applied to the group as if it were one feature. In the example below, I can position the imaginary circle with GD&T, and even allow bonus tolerance as the three pins get closer together (because the external circle created around the three pins will get smaller). This is different from positioning the three pins themselves.
Example of an “irregular feature of size”
For folks who have been around GD&T for a while, this might take some getting used to! But it can make sense for many applications such as in the example shown above.
While everyone is ooohing and aaaahing over the new GD&T standard released in April, there is a rule that dates back to 1994 that very few people know about. And although it’s not something that would be used very often, it’s something that might be worth filing in the back of your brain…
This little-known rule is the idea that the variable tolerance created by an MMC or LMC modifier — often called “bonus tolerance” — can have a limit placed on it. Most GD&T people are comfortable with the notion of bonus tolerance, but recall that the maximum amount of bonus is completely dependent on the tolerance allowed for size. Here’s an example:
The position tolerance of each hole is going to be 0.2 at a minimum, and this happens when the hole is manufactured at 10.8 mm. If you manufacture a hole at 11.4, then the allowable position tolerance is 0.8 (this is the original tolerance of 0.2 plus the bonus of 0.6, which comes from the spread on the hole’s size).
Now suppose that the designer wants to allow extra position tolerance with the MMC modifier, but for some reason can’t let it grow to 0.8. (Maybe there is concern about having a hole drift too close to the edge of the part.) Then the standard allows for the feature control frame to state a maximum tolerance value, thus placing a cap on the bonus tolerance:
Now, the position tolerance will still be 0.2 for a hole of 10.8, but if you make a hole at 11.4, then position tolerance is 0.5 mm.
I mentioned this trick on another GD&T discussion forum recently, and most of the folks who are regulars there hadn’t heard of it. So just think of it as another tool in your design toolbox, even if it is rarely used. If you have a copy of the ASME standard, check out Figure 6-42 in the 1994 edition, or Figure 6-15 in the 2009 edition for their examples of this.
As always, your comments are welcome!
Several times I have heard that a designer is hesitant to use GD&T because he knows that the manufacturer will not understand it. There are several ways to answer this dilemma:
- Too bad; the burden is on them to learn it
- Use traditional tolerancing even though it lacks the benefits of GD&T
- Use a hybrid approach, and make yourself available for guidance if they have GD&T questions
Without sounding callous, the best answer is probably the first option. Even small machine shops go through the process of becoming certified in ISO, so why shouldn’t they be fluent in GD&T? They will be handicapped in their business by not knowing this important tolerancing system.
I don’t know if this is true or a tall tale, but one engineer at our seminar said that he once worked at a small manufacturer that, when bidding on a new job, would count the number of GD&T callouts and multiply it by a cost factor. The thinking was that more GD&T callouts meant a more expensive product to produce! Needless to say, that is nonsense.
Of course, you may want to gently ease into the GD&T waters if you know that a supplier isn’t comfortable with it. (You might not want to throw a “zero tolerance at MMC” at them right away.) But the bottom line is that GD&T provides maximum tolerance at efficient costs, so every manufacturer should become familiar with it to avoid extinction.
Out there in the GD&T world, there is often confusion about parts that have irregular shape. We are told that the theory of GD&T requires datums to be 90º to one another. Sure, that’s great in a textbook where the examples are nice, rectangular, flat plates! But what about those other shapes?
It’s actually very easy. The confusion is that people mistake the term “datum” for “datum feature. The standard defines a datum as a theoretically exact point, axis, or plane. But a datum feature is defined as a physical portion of the actual part from which the datum is derived.
Think about those two terms, and you’ll see that irregularly shaped parts pose no problem. Even something shaped like a blob or a potato chip has a physical surface. It may require using datum targets, but a theoretical plane can still be constructed from those targets.
So again, it’s true that the theoretical datums mentioned in a feature control frame are perpendicular to each other. But those theoretical datums can be derived from any crazy-shaped surface.
If you have the new 2009 ASME standard, see pages 81-90 for some neat examples. (If you have the 1994 edition, see pages 54 and 78-79.) Stay tuned for future entries on the recent changes in the standard!
If you are a regular user of GD&T, you probably know that the ASME standard was recently revised (for details, see the blog entry below dated March 28, 2009). In today’s column, I’d like to introduce you to one of the changes.
The term “maximum material condition” or MMC has been around for a long time. This concept is invoked when the circled M symbol is placed in a feature control frame. Well, a new item for the 2009 standard is something very similar, called “maximum material boundary,” or MMB. Yet it is invoked using the same circled M symbol.
The reason this was introduced was to eliminate confusion when the M symbol is modifying a datum that has its own geometric tolerance. Consider the following example:
The position tolerance references datum feature B with the M symbol. But here’s the key: think about the size of a gage pin that would be inserted into the center hole (it should be attached to a flat plate that simulates datum A). It would not really be simulating the MMC of 22.0; instead, it would be 21.8 in order to accommodate the perpendicularity tolerance of 0.2. Thus the confusion — people would say “MMC” when discussing the datum, but had to understand that it wasn’t really the true MMC that would be simulated.
So the new standard uses the term “maximum material boundary” to differentiate it from the true “maximum material condition.” The picture above would not change, but in talking to someone you would say “the position tolerance of the OD is 0.4 at its MMC, relative to datum A and datum B at MMB.”
I suppose if there were no perpendicularity tolerance on the center hole, then you could interchangeably say “MMB” or “MMC,” since they would be the same (22.0). And by the way, the other choices of LMC or RFS on a datum reference also have their counterparts of “LMB” and “RMB” in the new standard.
In a GD&T class, I often talk about (and sketch) how a sample part can be held in a fixture — this helps people understand the concept of datums, particularly if datum targets are involved.
This does not imply that an inspector must use a customized fixture to check a part. I refer to fixtures and physical gaging in a class simply because people can visualize those concepts, whereas a CMM is more abstract (sometimes CMMs and similar devices are called “soft gaging” as opposed to traditional “hard gaging”).
If you are using a CMM, then you ensure that the probe samples the part at the prescribed datums; this establishes a coordinate system in the computer for other measurements to be made against. But wait: the part isn’t floating around in mid-air! It is still contacting something. Perhaps it is sitting on a granite table. Here’s a key point: instead of sampling three points on the surface of the part to create the datum, you should take three points on the table, since that table simulates the true datum (as derived from the high points of the part surface).
The only tricky part is when datum targets are involved. This is where the designer identifies specific points, lines, or areas on a surface which are to be sampled for constructing a datum in the computer. It’s tricky because those targets have an exact location, which should be dimensioned from other datums (or somehow located in the math model). But you can’t probe all datums simultaneously, so this is where a fixture might help!
Without a fixture, you might sample three pads representing A1, A2, and A3. But if your location for those three pads was off, you won’t know it until you sample B and C. So it’s doable, but it becomes an iterative process; you may have to resample some datum targets until you determine that the sampled points were at the prescribed locations.
Note to engineers/designers: This is one reason why it’s not ideal to place datum targets at random locations! They are not identifiable to the eye. Also, the datum targets should simulate the actual function or contact points, and random locations don’t do that. (But they are sometimes necessary if the functional points are inaccessible or if the geometry of the part is so complex that there’s no other way around it.)