If you’re familiar with the different GD&T modifiers, then you probably know that the circled P creates a “projected tolerance zone.” This is often used on threaded holes to keep any fastener that protrudes beyond the threaded hole from causing interference with a mating part:
Without the “P” modifier, the tolerance zone exists only within the depth of the threaded hole itself. The result is that the threaded hole could tilt, and be passed for position tolerance, yet cause interference:
So “P” is a good thing. However, when this concept is presented in our GD&T classes, someone will occasionally ask if we could — as an alternative to “P” — simply tighten the position tolerance number instead. The dialog might go like this:
“Couldn’t we just change the 0.3 to 0.2 (or 0.1) and achieve the same effect of preventing too much tilt?”
“Yes, that would be legal,” I answer. “But using the P allows us to keep a larger tolerance, while preventing interference.”
“But it has the same effect of tightening the position tolerance anyway,” the student might reply.
This is where we have to be careful. It’s true that projecting the tolerance zone has the effect of tightening the perpendicularity aspect of a position tolerance (because it’s extended higher), but it still permits the threaded hole to use the 0.3 for lateral position. In other words, if the threaded hole doesn’t tilt, then the 0.3 is still allowing the axis to drift left or right within that zone. By eliminating the “P” and dialing the tolerance down to 0.2, we’d be robbing ourselves of some tolerance which might still be helpful in terms of x-y location.
So a projected tolerance zone is not the same as merely tightening the tolerance number. That said, there are times when a projected tolerance zone doesn’t make sense, even on a tapped hole. An example might be for a hole whose fastener doesn’t protrude very far up — such as a bolt that engages the threads for 16 mm but then clears through an adjacent plate of only 4 mm thickness.
But in general, a designer should at least consider the “P” option when imposing GD&T on threaded or press-fit holes.
No matter how good a dimensioning system is — GD&T, anyone? — there will still be errors encountered on drawings, simply because there will always be human beings who are behind the creation of a new drawing. And of course we all make mistakes. But I want to point out a few of the more common mistakes that I encounter in my travels.
• Failure to include a diameter symbol in a feature control frame when needed. I’m thinking particularly of position and perpendicularity. When tagging these tolerances to a hole or pin, you usually need to include the diameter symbol before the number, so that the axis of the feature is contained in all directions.
There are times when a hole’s position tolerance should not use a diameter symbol: if you really only want the tolerance to apply in two directions. But that must be clearly indicated by proper using of dimension arrows.
• The next common error I’d like to review is similar to the first — using a diameter symbol when it shouldn’t be there! I see this in feature control frames for circularity, cylindricity, circular runout, and total runout. It might be tempting, because each of these is applied to a round feature, but the tolerance number given is NOT a distance across a circle (which is the definition of diameter), but a radial bandwidth. This one isn’t as egregious, because there is only one way to interpret these symbols, and thus the meaning isn’t different.
• Another error — probably the most common one I’ll be listing here — is the improper location of the datum feature symbol. Too many times I’ll see this triangle symbol tagged to a center line, because the designer/engineer thinks that the datum will be the center line. And that is TRUE! The theoretical datum is very often a center line or axis. However, the triangle symbol doesn’t identify the true, theoretical datum; it is supposed to identify the physical feature from which the theoretical datum will be derived. Notice the difference!
While that is sometimes easily forgiven, the bigger problem is when this misuse of the datum symbol creates ambiguity, such as this one on the left, and the corrected version on the right:
• The next error is related to quality control and statistics. Many of you may be familiar with the practice of identifying “critical characteristics” which require the inspector to measure something and keep a log or spreadsheet for these measurements. This allows the long-term statistical trends for that dimension/tolerance to be tracked. This gets into things like standard deviation, six-sigma, Cpk values, and other lovely terms from statistics.
When imposing these ideas onto GD&T, however, a common mistake is to flag a basic dimension as a critical characteristic. This shouldn’t be done, because basic dimensions themselves have no tolerance — there is nothing to track! Instead, the real variation to be measured is shown in a feature control frame. That’s where the critical flag should be noted.
• Finally, sometimes you may see the position symbol used on a single feature (a hole, for instance) and then the only datum referenced is a single planar datum that happens to be perpendicular to that hole. In other words, the only thing being controlled is perpendicularity. Don’t use the position symbol, then!
The full explanation of this was covered in an earlier blog entry, found here.
That’s it for now — feel free to send comments/suggestions about these or other common mistakes that you encounter. Happy spring/summer, everyone!
Ah, yes. I remember as a child being told that words are important! And that is certainly true in the world of geometric dimensioning and tolerancing. So many people think that GD&T is just a matter of learning the symbols, and it’s true that that is a key part of understanding the language. But behind the symbols are many rules, acronyms, and definitions that can make a great difference if they are not fully understood.
One of the most significant examples is the confusion about the term concentricity. To a casual beginner, the word “concentric” sounds like a simple idea: two or more circles that share a common center. But in the world of GD&T, concentricity has a very specific meaning that is more specific than what you’ll find in Webster’s Dictionary! FYI — the same confusion applies to the symmetry symbol. (For more about concentricity, see this blog entry from a couple of years ago.)
Here are a few other miscellaneous terms to be careful with:
Datum — Technically, a datum is a perfect plane, axis, or point (or combination of these). So when talking about the actual surface of a part, we shouldn’t call it “datum A,” because that surface may be imperfect: slightly concave, convex, etc. The proper term for the actual part surface is “datum feature A.”
MMC — The “maximum material condition” is literally the size of a feature when it has the maximum amount of material allowed. This is a simple idea that is usually covered near the beginning of any GD&T training. It is invoked upon a geometric tolerance by the circled M modifier after the tolerance number. However, few people are aware that when the same modifier appears after a datum letter, it is not called MMC. Instead, it is referred to as MMB, or “maximum material boundary.” The reason it’s different is that a datum feature may have more than just a size tolerance; it could also have a geometric tolerance of its own, thus making the worst-case boundary different from the true MMC. This is an idea that was clarified in the 2009 ASME standard.
Basic dimension — this one is not a difficult term. But what gets me is that many people confuse it with “reference dimension.” I guess they are a little similar; they both have no tolerance. But the reasons are different. A reference dimension (a number shown in parentheses) has no tolerance because it is not to be checked. It is just for reference, or “nice-to-know” information. A basic dimension, however, is linked to GD&T. A basic dimension (a number enclosed in a rectangle) also has no tolerance — not even from the title block — because it establishes a perfect size, location, or angle from which a geometric tolerance is established.
These are just a few of the dozens of terms that are so important to understanding GD&T. And especially for anyone who is preparing for the official ASME certification test, thorough knowledge of all these terms and acronyms is essential!
If you’ve been keeping track of the new GD&T standard, then you’re probably aware of most of the bigger changes. (Yes, I know that 2009 doesn’t sound “new,” but most people still call it the new standard since it takes a while for companies to switch to a new dimensioning standard.)
The new item I want to show you is pretty easy. It is called the “all over” symbol, and it is very similar to “all around,” which may be familiar to you. Both of these symbols will be found with feature control frames that use profile of a line or profile of a surface. Here’s an example of the “all around” symbol, which has been in use for many years:
The “all around” symbol is the small circle on the elbow of the leader line for the GD&T feature control frame. This means that there is a profile zone imposed around the entire perimeter of the part, but only in the left-hand view. It doesn’t cover the two large faces of the part (this is why the 30 mm dimension still has a ± tolerance on it). Here is the same “all around” profile zone shown in yellow:
OK, but now let’s look at the new one, which is called “all over”:
Notice that there are two circles around the elbow of the leader line — this is a new addition in the 2009 standard (to get the same effect previously, we could have used a text note “ALL OVER”). This means that the profile tolerance extends everywhere! Notice that the depth dimension of 30 must now be a basic dimension. Here is this new tolerance shown in yellow:
So as I said, it’s not a difficult concept. But be careful — all over literally means all over! If there were any holes in this block, the profile tolerance would also cover the walls of the hole (which means the diameter of the hole would have to be given as a basic dimension). So use this new one with caution.
I hope everyone has had a great summer. Here’s a topic that will be helpful even to seasoned experts in GD&T, and it kind of follows the previous blog entry…
Often, when discussing the finer points of GD&T with others, we end up going to the official standard (or standards) that pertain to dimensioning and tolerancing in order to seek guidance. But if you’ve been in the real world, you know that a technical document can’t capture every possible scenario.
So we naturally look for the example or description in the standard that is closest to our real-world situation. However, we have to make a decision whether we can make the leap of logic to say that a proposed design is still within the “spirit” of the standard. This can sometimes be a sticky point!
An aside: The two major standards when it comes to GD&T are ASME Y14.5 and also the ISO series of standards (ISO has an umbrella of several standards that embrace GD&T, not just one book). The predominant standard in North America — and the one I’m most familiar with — is ASME. In some ways the two standards have different philosophies about the depth of coverage: in some areas ASME tries to nail down every option, and in other areas ISO takes the harder line.
There are those who would say that we must make our designs conform to the exact letter of the law, and any practice which is not described in the standard (or an obvious modification of one given in the standard) is not to be used. But others espouse more leeway and say that the concepts given in the standard can be extended to many other areas that might have been unforeseen by the standard writers.
I put myself into the latter camp. The key is to look carefully at the wording of the standard: if the words “shall” or “must” are used, then the door is pretty much closed to bending that principle. But if no prohibition is given — or better yet, if the verb used is “may” — then there are probably other ways to practice the given idea and still be in conformity to the standard.
One concept that can serve as an example is the “tangent plane” modifier. When introduced in the 1994 ASME standard, this modifier was shown for use on the three orientation symbols (when applied to surfaces). Eventually, someone was bound to ask whether the tangent plane idea could be used with profile of a surface. The standard never said this cannot be done, and so my vote would be that it’s OK. Others said, nope, it wasn’t in the standard, so tangent plane wasn’t to be used on profile of a surface. In the 2009 standard, the notion of extending “tangent plane” to profile of a surface is now clearly allowed; although no specific example is given, they added a footnote saying that the concept of tangent plane is equally applicable to “other geometric characteristic symbols where the feature is related to a datum(s)” (see page 103 of the current edition of Y14.5).
Bottom line: GD&T is a language. And like any language, there are certain rules that must always be followed. However, there are many ways to patch together different parts of that language and still say something clear. We shouldn’t be too legalistic and limit ourselves to designs that are only identical to the examples given in the standard. Obviously, this is where training and knowledge of the fundamentals of GD&T are necessary in order to know when the envelope is being pushed to far!
Sorry that it’s been a while since my last blog post! That simply means that our training schedule has been busy. Though a good portion of the U.S. economy is still sluggish, I have definitely seen an uptick in the number of requests for GD&T training. So remember, if you have a group of 4 or more people that need the basics or a refresher in GD&T, don’t hesitate to drop us a line or call for a customized price quote for a group class.
Today I should begin by answering the question posed in the title of this blog entry: No — there isn’t always one right way to tolerance something. Recall that GD&T is a language, and like any language there may be more than one way of accomplishing something. People often criticize prints for “bad” or “misapplied” GD&T. And there are certainly many examples of that. But many times what people are calling “bad GD&T” is simply a different way of doing something! That being said, however, I’d like to present the most common GD&T mistakes which are definite no-nos.
Here are my “Top 5” of the most common GD&T errors:
—Failure to show a diameter symbol in the feature control frame (if a cylindrical zone is desired
—Having parallelism (or perpendicularity) on a surface, and then adding a flatness tolerance of the same amount or greater
—Using the position symbol on a single feature related to a perpendicular datum (use perpendicularity!)
—Using concentricity when position RFS would be adequate (assuming ASME standard is invoked)
—Showing the datum feature symbol on a center line (yes, a center line can be a datum, but the symbol MUST be tagged with a physical feature)
Of course there are others, but if any of these items shows up on your drawings, you should at least be comfortable in raising a question to the designer/engineer. If you aren’t sure what I’m referring to in the items given above, or think that they are OK, then that would make for some good homework for you! Think about why those things don’t make sense; use your GD&T reference books, or if you need further explanation, feel free to add a comment here and I’ll try to address it in a future blog entry.
This website and blog naturally focus on GD&T, but it’s a good time to discuss the importance of simple print-reading skills as a prerequisite to learning GD&T. As I travel around teaching classes on GD&T, you’d be surprised how many people don’t fully understand some of the simple rules of drafting, view layouts, and notation on drawings.
First, note that there can be different terms for this skill; the title of this blog entry mentions “blueprint” reading, but nobody uses actual “blue” prints anymore. (This name was given because at one time they really were blue, due to the chemical process used in producing these drawings; see here for more on the history of this.) I suppose a more proper term today would be an “engineering drawing” but if you want to call them blueprints still, hey, go ahead.
If GD&T is to make sense, then the object being toleranced must certainly be understood first. Most drawings use “orthographic” projection, which is simply a fancy name referring to the straight-on, flat view of a part from a particular angle. Think of a cube: each of the six sides can be flattened out to display six orthographic views. Depending on the part, there may be fewer or more than six orthographic views (in addition to other views such as section views).
Here is a simple example showing three orthographic views of the same part:
The trick is to look at a series of flat pictures and be able to visualize a three-dimensional object from those views. Some people are born with that gift of spatial viewing, others can get it with practice. Plus, on many modern drawings a 3-D “isometric” view is given, which certainly helps to visualize the part.
(Note: the traditional orthographic views are usually laid out in a specific arrangement. Here in North America, the standard arrangement is “third-angle projection,” which places the top view above the front view, and the right side view off to the right side of the page. In Europe and many other countries, the predominant arrangement is “first-angle projection,” where the top view is placed below the front view and the right side view is placed to the left. They are both acceptable, but simply different customs. To be sure, always read the title block or notes to determine which system is being used!)
Here’s one reason why all this is all so important to GD&T: Suppose a surface is labeled as datum A in a certain view. When we look at another view we may see a feature control frame tolerancing another surface back to datum A. But if we make a mistake in the visual interpretation, then we may end up applying the tolerance to the wrong face of the part!
Even if you may feel embarrassed about not being proficient at print reading, don’t hesitate to ask for help or seek out some self-study training materials. Happy new year to everyone…
Several months ago I wrote about the requirements for becoming certified as a “GD&T Professional.” (View that blog entry here.) This time, I would like to present some advanced questions.
There are two levels of certification for GD&T Professionals: Technologist and Senior. You do not need to be certified at the Technologist level in order to take the Senior level exam. But you would need to be sure that you are very familiar with all the tricky nuances of GD&T! (Plus, you must submit a letter of verification that you have been regularly involved with GD&T for at least five years.)
So the following are a few questions that might be representative of the more difficult stuff. Answers are at the end, along with the appropriate paragraph number from the 1994 edition of Y14.5…
Sample question #1:
The derived median plane of a feature can best be described as:
a. a theoretically perfect plane through the center of a part’s actual mating envelope
b. a plane that coincides with the centerplane of the true geometric counterpart
c. an imperfect plane passing through center points of all line segments bounded by the feature
d. an imperfect plane representing the average height of a surface plate used to simulate a datum surface
Sample question #2:
Simulating equalized datums may be accomplished by using:
b. V-type knife edges
c. V-type planes
d. all of the above
Sample question #3:
For the drawing given above, assume perfect form and perfect orientation. The minimum permissible distance between the outside of the part and the edge of a hole is:
Sample question #4:
The dimension line of an angle should be:
a. an arc
b. normal to the extension line
c. parallel to the extension line
d. angled to the extension line
Sample question #5:
For the following print, a part of Ø9.17 would be _______ .
a. a good part
b. a bad part
c. good, only if statistical data is monitored
d. good only if a stack is calculated
Sample question #6:
In the following drawing, the .008, .005, and .002 tolerances control ________ respectively.
a. location & size; orientation; form
b. location & perpendicularity; location; form
c. location; orientation & size; form
d. location & orientation; perpendicularity; size & form
Here are the answers: 1=c (paragraph 1.3.15), 2=d (4.6.6), 3=b (4.5.3 and 5.4.1), 4=a (18.104.22.168), 5=c (2.16), 6=d (22.214.171.124)
More information about the official ASME test can be found at their website:
In my opinion, one of the most underutilized tools in the GD&T toolbox is the tangent plane modifier. It was introduced in the 1994 ASME standard, yet some people still think of it as a new concept. Shown in the example below, the tangent plane modifier (circled T) can save money by only controlling the high points of a surface, rather than every point:
To understand the drawing above, first realize what parallelism controls if no T modifier is given. Regular parallelism requires that every point on the top of the part be within a tolerance zone of 0.2 mm. This means that regular parallelism inherently controls flatness to the same specification.
But there might be times when a designer does not need to control flatness. Perhaps another mating part will contact the top of our part, and we only care about the angle at which the mating part sits. In that case, we don’t need the surface to be flat within 0.2, since our mating part will only feel the high points anyhow.
In that case, the tangent plane modifier makes sense. It does not give us a “bonus tolerance” as the MMC modifier does with features of size, but it does have the advantage of being more forgiving of the surface’s form error. The following is an illustration of the possible error that would be allowed by the tangent plane modifier:
Notice that portions of the surface can actually go below the tolerance boundary; this is because the tolerance is imposed only on the imaginary tangent plane — this can easily be inspected by placing a gage block or a flat plate on the top and then measuring the gage block’s parallelism.
Of course, there are times when this is not desired, such as when there are concerns about fluid leaking between this part and a mating part. And it should also be noted that the tangent plane modifier can be used not just on parallelism, but also on perpendicularity, angularity, and even profile of a surface.
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 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.