Topic: Calculating Tolerances for a Press Fit

Jim,

Had a quick question for you, we're trying to add GD&T to an assembly that gets a bushing pressed in. the hole diameter and bushing are rather large (90-94" DIA), and so what I've done is add cylindricity to the hole and to the bushing and then again another cylindricity to the inner diameter of the bushing after it is installed to ensure no high or low out of cylindrical spots after it's fit in. My question is, how do I calculate the geometric tolerance for the hole and bushing before and after installation? Do the fixed and floating equations work in this scenario?

Adam

Adam,

I’ve read this email a couple of times and I’m not certain what geometric tolerance you are trying to calculate. Cylindricity tolerances control three dimensional form and are contained within the size limits.

So, if the MMC of the hole and the shaft are compatible, all the cylindricity control will do is allow the fit to maintain more surface contact.

If you are trying to calculate some other type of geometric tolerance for each, like their positional tolerances for clearance fits, the fixed and floating fastener formulas will work fine.

If the type of fit you are trying to achieve is an interference fit, then the minimum amount of interference is the difference between the least material conditions of the shaft and the hole. The maximum interference will be the difference between the virtual condition of the shaft (or its outer boundary) and the virtual condition of the hole (or its inner boundary), if they have a geometric tolerance that is not contained within the size limits of each (such as position tolerance or runout tolerance).

If the only geometric tolerance the hole and shaft are being assigned is a cylindricity control, then the maximum interference is the difference between the maximum material conditions of the shaft and the hole.

I hope this helps.

Jim

Topic: Clearance vs. Transition vs. Interference Fits

Jim,

What if the difference between the MMC of the hole and the shaft is larger than the overall size tolerance that we need to impose? Doesn't this defeat the purpose of cylindricity? The reason is simply that when you subtract the MMC of the hole minus the MMC of the shaft you get a negative number is this ok?

Adam

Adam,

That is the nature of an interference fit (or a transition fit, if the difference between the LMC’s isn’t also negative). I don’t think it defeats the purpose of cylindricity. As I said in the last email, what cylindricity does in these situations is to make the surface contact more uniform, as opposed to hitting harder at one end than the other. Cylindricity controls the roundness, straightness and the taper of the diameters, making their interference more uniform.

Still, cylindricity is a far less used control than the usual profile of a surface (which requires a basic dimension for the diameter and tolerances size, shape---and even angle and location if the proper datum references are used) or position (which uses a plus and minus tolerance for the diameter and doesn’t control surface shape, instead controlling angle and location). It all depends on what it is you are trying to accomplish.

 
Jim

Topic: Tolerancing Basic Size Dimensions, What Cylindricity Controls, and Measurement Force

Mr. Meadows,

I hope you don't mind me asking you another question...And this is the type of question I hope your Geometric Dimensioning and Tolerancing book based on ASME Y14.5 2009 will answer... but we have a stainless steel machined hub that will mount to a motor shaft. The hub I.D. is critical and we want it dimensioned so as to insure that it will fit onto the motor shaft with little or no force.

Is it proper to dimension the I.D. as a basic, then add a cylindricity callout to control size?

For example: the current dimension is as follows;

dia. 7.935 +0.025 mm - 0

If I wanted to imply the use of a pin gage to check the hole diameter, could I dimension it this way?

dia 7.96 BASIC concentricity 0.025 @MMC

Would that be a correct method to achieve the tolerance we want?

Also, is there a method to specify that the "GO" pin should fall thru the part on its own weight?

 
Would very much appreciate your advice.

Thanks,

Terry

Terry,

It isn’t proper to give a size dimension as a basic dimension unless you are going to use profile of a surface to tolerance both the size and the form. Also, a gage isn’t suited to easily check the two tolerance zones (inner and outer) that profile generates. It will check one, but not the other.

If you dimension the ID to have a diameter of 7.935 plus 0.025 and minus zero, the GO gage pin would be produced at 7.935 (the ID maximum material condition) and it would have to pass through the hole with zero measurement force (per ASME Y14.43-Dimensioning and Tolerancing Principles for Gages and Fixtures). The least material condition would be inspected at cross sections. The ID would have to be cylindrical per Rule #1 (in Y14.5) to within its size tolerance and you must maintain perfect form (cylindricity) if the entire feature is produced at its MMC.

The more the feature of size departs from MMC (as produced), the greater the form error that is allowed. Still, the variations in form and size may not violate a perfect cylinder that is simulated at its MMC by a GO gage, and the LMC may not be violated at cross-sections. There are exceptions to this rule of “perfect form at MMC must be maintained”, such as for cylindrical features that are:

1. flexible,

2. controlled with straightness of the derived median line,

3. dimensioned and toleranced using the Independency symbol,

4. stock size in the as furnished condition,

5. features given size dimensions and tolerances that are identified as applying as an average (AVG) dimension, and

6. features that are controlled with a feature control frame that includes the least material condition symbol.

Jim Meadows

Topic: Implying or Specifying Measurement Techniques

Jim,

Thank you very much. Just got your book last night and will be doing some studying of it in the near future.

But, in regards to my question below; how would you dimension an ID if you wanted to imply the use of a gage pin to inspect it? Again, this is a hub for a blower wheel that fits onto an electric motor shaft.

Thanks a million,

Terry

Terry,

There is no definitive way to imply a gage pin will be used to inspect an ID. The use of the word BOUNDARY beneath a position tolerance feature control frame is an implication that the virtual condition boundary is to be verified, which is what functional gage pins do. The use of the MMC and MMB symbol in the control (circled M’s after the position tolerance and any datum features of size) would make gages easier to use.
The easiest way to insure the use of a gage pin is to write a note. Something like “SEE NOTE 2” beneath the position tolerance, then note 2 stating that “the position tolerance is to be inspected with a gage pin of the following size and configuration” should do the trick.

Another option is to write a measurement plan that states how the part is to be measured. I’ve got a chapter in my gray book on how to write one (pages 436-441). There is also a B89 standard on Measurement Planning.

I hope this helps.

Jim

Topic: Gages That Measure Positional Boundaries

Mr. Meadows,

I hope you doing well – I really enjoyed the class I took with you in Las Vegas back in March.

I have been tasked with making a gage that checks the outside contour of a hose with several “bend intersections.”  I remember you showing us an example of one of these on the projector at class.

Do you cover the basics of doing one of these in your latest book? I have been wanting to get one of your new books ordered anyways.

If you have any suggestions, or advice you can pass along to me, I would really appreciate it.

Thanks again!

Dave

Dave,

The illustrations below are explained in my GD&T textbook (the gray one on my website www.geotolmeadows.com).

The gage dimensions will come from your CAD model or the complete part drawing requirements. The size of the trough in the gage will be the virtual condition of the outside diameter of the hose (MMC plus the positional tolerance). The tolerance on the trough gage will be all minus on the trough (so that no bad parts will be bought by the inspector). 10% of the part tolerance is recommended for use on the gage. The page numbers for the illustrations I’ve sent you are from the grey textbook. I hope this helps.

Jim

Examples of Specifying Positional Boundary Controls on Hoses, Pipes or Tubes

Gages to Measure Positional Boundaries

 

Jim,

Received your latest GD&T textbook yesterday – browsed through it, and it looks like a great resource. Thanks for the care and hard work you put in to your teaching and textbooks.

Dave

Topic: Independency vs. Envelope Principles and Symbols

Jim,

How’s life been treating you? It’s been awhile since our last contact. I left the company where I took your classes last year and moved to the Salt Lake City area. Are you still in the Nashville area?

The engineers here are having GD&T discussion and I wanted to get a second opinion on something. It has to deal with form control within size and the independency rule in the new Y14.5-2009 standard.

1. Is the circled E symbol now required on prints to enforce the envelope principle of size controls form? I recall this as being an ISO thing, but I’m not up to speed yet on the new Y14.5 standard.

2. What is the rationale behind the circled I symbol? I know you have good stories from the ASME committee. What has the committee’s logic behind the rule? When should it be used?

Thanks for the help and keep in touch.

P.S. I need to get my hands on copy of your latest book. I’ve tried to find other sources for the new GD&T rules, but no one does it better than you.

Brian

Brian,

Yes, still in Nashville. Life keeps on going and business is good. I’ve been to Salt Lake City a few times. It’s clean and the people are nice.

1. The circled E is still an ISO thing. ASME Y14.5 doesn’t use the symbol. Perfect form at MMC is still required (other than the few exceptions; straightness of the derived median line, flatness of the derived median plane-used to be straightness of the derived median plane, stock size in the as-furnished condition, use of the circled L in feature controlled frames, flexible features and now use of the circled I). The circled I symbol stands for Independency, and means that the size tolerance and the form tolerance are independent of one another. It means that size tolerance does not control the form.

2. The rationale behind the circled I symbol was mostly that the virtual condition boundary (when using the MMC symbol) is the functional worst mating boundary and the MMC boundary of perfect form is rendered unnecessary by the virtual condition boundary. So, the use of the circled I is basically to allow inspectors to measure MMC easier (at cross-sections) instead of trying to simulate a GO gage. Since the virtual condition boundary will require verification of the worst mating condition anyway (perhaps even with a functional gage), there is no reason to check the MMC boundary of perfect form. The circled I comes with a warning label. If there is no geometric tolerance that controls the form used with it and no feature control frame that generates a virtual condition boundary, the only control on the form being infinitely bad is that other tolerances (such as part length) might be violated. Think of a shaft that bows like a banana. If it bows enough, eventually the length is very short (and the size limits on the length might be violated).

Thanks for the compliment on the books. It was nice hearing from you and where you ended up. Maybe we’ll cross paths again in the future.

Jim

Topic: Least Material Condition and Least Material Boundary Reference Uses

Hi Jim,

Quick question. In your book on page 275, it shows a 10.7-11.0 diameter with a position tolerance. Imagine instead of MMC it was referenced at LMC. Is that practical: a feature control frame with the geometric tolerance @ least material condition, a primary datum reference, a secondary referenced with least material boundary and a tertiary with least material boundary? I have never seen this.

Hubert

Hubert

It’s used to protect wall thickness, material strength and seals. The seals won’t be uniform, but they will seal. For uniform seals, the RFS and RMB concepts are better. Also, there are many ways to protect material strength and wall thicknesses. The LMC/LMB principle is only one. It makes parts hard to measure. It changes the rule on how to measure size limits from a perfect form at MMC envelope to a perfect form at LMC envelope. MMC is checked at cross-sections, while LMC is checked for an envelope.

I use it for casting drawings, where my major concern is to preserve material to machine away in subsequent machining operations.

Jim

Topic: Positioning Hole Patterns with Basic Angles vs. X and Y Coordinate Dimensions

Jim,

A question has repeatedly surfaced with respect to positioning holes with a single datum reference frame. The confusion is associated with the fact that 5 holes are positioned with basic angles (30) associated with an axis which has not been identified as a datum.

An alternate approach under consideration would be to establish the axis as a new datum via the proper datum feature identifier. A new feature control frame would be implemented (for 5 holes only) with the new datum axis as part of the datum feature references for the angularly positioned holes.

Is it legal and / or sufficient to leave the existing Feature Control Frame positioning all the holes with the basic angles or are two FCFs necessary? I’m not opposed to either format. I just wish to be as accurate as possible and compliant with the intent of ASME Y14.5.

As a side note, I look forward to the possibility of meeting you again at the ASME Y14.5 committee meeting.

Thank you for your consideration.

Frank

Frank,

I thought for certain that I had responded to this, but I can find no record of it. So, I guess I looked it over and answered it in my head, but never wrote it down.

Anyway, the attached drawing that you sent me is well done. Assuming the primary datum feature is A and that A has been considered for a flatness tolerance, B is then controlled to A and C is controlled to A and B. There are basic dimensions traceable from B to all holes and since C generates a centerplane datum, we can surmise the basic location of every hole from datum centerplane C. The 30 degree typical is fine (not something we do much anymore, preferring instead to state the number of times in front of the basic angle that it will be repeated). Then all 12 holes are positioned to A, B and C.

It may have been more clear if the five holes you are referring to had basic dimensions given directly from datum planes B and C, instead of making us deduce their location by giving the basic bolt circle and the basic 30 degree angles. Still, what has been done allows anyone to calculate the basic location dimensions from datum plane B and datum centerplane C. The real question to ask in these situations is, “Can you calculate the basic hole locations from the given information?” I think the answer to that here is clearly that you can. There is no datum axis that anything is being measured from. The basic bolt circle and the basic angles are given as a vehicle to allow one to deduce the basic location from datums B and C. With basic dimensions, there is no accumulated tolerance error unless you switch datums in mid-stream. That hasn’t been done here.

The only thing I would make sure is done is that all of the radii have tolerances on them. Plus and minus tolerances are fine to use. It would also be fine to make the radii on the part periphery basic radii and then give each a profile of a surface tolerance.
To address what options you are considering, I would not choose to make the axis of the (what?) outside FULL Radius a datum feature. Using the datum structure you currently have seems much more stable and repeatable.

I also see no need for two feature control frames. You have 12 holes and they all have the same MMC, LMC and position tolerance (hopefully one that has been calculated using the correct fixed or floating fastener formula). The only reason to use two feature control frames would be if you had two different sets of holes with different sizes or different position tolerances.

This is one of those rare instances I occasionally encounter where the holes have been properly positioned. If some feel uncomfortable with this technique, my only suggestion would be to calculate the basic dimensions that are equivalent to what is currently to be deduced from the basic radii of 4.500 and the 30 degree typical dimensions and put those on the drawing instead. These basic dimensions could originate at datum plane B and datum centerplane C and lead us directly to the center of each hole.

I hope this helps. I’ll see you at the next meeting.

Jim

Topic: Continuation of Previous Discussion and a Tolerance Stack-Up Question with Threaded Holes

Jim,

Thank you very much for your timely response. With 20/20 hindsight, I believe I recall you had mentioned difficulties with your email service, and I should have remembered to forward my note to your jamesmeadows@comcast.net address.

Upon reflection, your discussion is very sound and logical, as your thoughts usually are! This reaffirms my notion that the orthogonal datum planes in the given example are sufficient for the noted positional tolerances and creating an auxiliary datum axis would not be wise. You made a very good point that the “datum feature”, a surface dimensioned by a radius (not even a feature of size!), which would have been used to establish the axis, would be a very poor candidate. The subsequent inspections would have been difficult due to the instability of the part and the datum selections for the datum reference frames.

Another point that I had missed, would be the incursion of tolerance stack up due to the two different datum reference frames employed within the two feature control frames for a hole pattern (5 features).

As a side note, I did finish working all of the problems in the GD&T in 2007 workbook, however, I am still pondering the complexities of the tolerance stack up of the 5 piece assembly of problem 55. The discussion within the text book is exceptional (chapter 25), however, the notion that the 4 threaded holes should be considered at their LMC to accommodate the analysis perplexes me at this time. Let it be noted that I haven’t given up, just taking a little more time!

Thank you once again,

Frank

Frank,

You’re welcome.

As far as the tolerance stack-up problem you refer to. It’s not the LMC of the threaded hole. It’s the LMC of the screw mounted in the threaded hole. As my long deceased teacher used to say, “Threaded holes controlled with a position tolerance and a projected tolerance zone aren’t to be considered holes in a tolerance stack up analysis. They are considered vehicles to move screws around.” In other words, he was saying to look at threaded holes and consider them shafts. They are screws that are allowed to move by the projected position tolerance of the threaded holes they are mounted into. I call them mounted screws. In this situation, what we are looking for is the clearance between the smallest screws and the clearance holes that fit over them and also the movement that is allowed by the position tolerance of the threaded holes.

As a side note, the threaded holes are, in theory, allowed some bonus tolerance due to the circled M in the position control, but that amount is hard to quantify because of the self-centering effect of the screw entering the threaded hole, the depth of the threaded hole and the class of fit. It is a negligible amount that we usually don’t try to put a number on. If we did try to calculate the bonus, it wouldn’t be based on the size of the screw’s outside diameter. It would be based on the holes allowed pitch diameter growth and how much that allowed the mating screw’s pitch cylinder to move.

Nice to hear from you again.

Jim

Topic: Formed Tools and Countersinks

James,

I wanted to ask you a question on formed tools.

If you have a hole with a countersink on both sides of that hole and it is created by a formed tool (the tool creates both countersinks and the hole at the same time), do you apply the same controls as if it were create by individual tools or is there some kind of expression/note that you attach to the datum of that hole?

Thanks,

Alvin

Alvin,

It can be treated as though it was a counterbored hole. There are three ways we usually deal with them.

One is that we show the diameter of the pilot hole and its countersink size and size tolerance specifications together, then beneath that we show one position tolerance that applies to both.

Two is that we show the pilot hole’s diameter and its size tolerance with a position tolerance below (for example to A, B and C) and then we add a datum feature symbol below that states that the pilot hole is a datum feature (for example D). If there are four pilot holes, we write 4X INDIVIDUALLY after the datum feature symbol (D). Then we show the countersink with a position control that positions it to D and below that we write 4X INDIVIDUALLY. This is to note that there are four different D’s and that each counterbore or countersink is positioned to its own D. It would also be allowable to call each pilot hole a different datum feature letter (for example D, E, F and G) and position each counterbore or countersink to its own datum feature.

The third way is to spec the pilot hole and the counterbore separately and give each its own position tolerance to whatever datums you want (usually to the same datums-for example A,B and C). This allows you to use different amounts of position tolerance for the pilot hole and the counterbore or countersink.

Some say that a countersink should be controlled with a profile control, as we would control other tapered diameters, with basic angles and basic sizes and profile of a surface tolerance to a datum reference frame. I personally think that is overkill, but it wouldn’t be wrong.

Jim

Subject: Gauge Design Question

Hi Jim,

I am working with a gauge designer that wants to do something unconventional with the datum- feature relationship in this absolute pessimistic gauge and I would like to get your take on it. The picture below shows a portion of the inspected part drawing with the feature we are trying to inspect for position and the datum it is called out to.

Inspected Part

Normally, we would call out the datum B gauge to have a VC boundary of .2760. The gauge designer wants to widen it (see below) and subtract the widened amount from diameter that measures the feature. Although we understand that this will reject more good parts, we are not sure if this is capable of accepting bad parts. We also came across a section in your book that states only the VC or MMC of a datum should be used and thought you might be able to tell us why.

Proposed Gauge

Any assistance is greatly appreciated. Please call or email if anything is missing or unclear.

Best,

Rebecca

Rebecca,

It’s an interesting approach that he wants to take. It’s also not correct. The Y14.43 standard states that with an absolute gage the tolerance on the gage holes may only be minus from the virtual condition or the MMC or maximum material boundary (MMB) as applicable. Your gauge designer wants to go one way on the datum feature simulator (plus only) and the other way on the gauge element that simulates the constrained feature (starting the size at a smaller size than the virtual condition and giving it a plus tolerance also, but not enough to make it exceed the .501 virtual condition).

I have no idea why he or she wants to do that. It’s creative, but there is a much simpler and more correct way to do it. Just make the datum feature simulator a diameter of .276, its MMC, and make the diameter of the larger gage hole a diameter of .501. Make the size tolerance on each all minus tolerance (as much as 10% of the total tolerance on the feature being simulated). For example, the datum feature simulator could be a diameter of .276 and have no plus tolerance, but a minus tolerance of as much as .0001. Then make the other simulator hole a diameter of .501 with no plus tolerance and a minus tolerance of .0003, with a position tolerance of zero at MMC and the datum feature referenced at regardless of material boundary (or as it’s called in the older 1994 Y14.5 standard, regardless of feature size).

This gage would be capable of measuring the MMC of the datum feature and the position tolerance of the larger part diameter. The gage he or she has designed could accept a part with a datum feature B that is oversized. Also, what he’s trying to do involves transferring some of the tolerance on the larger diameter to the datum feature simulator. This gets tricky when the diameters aren’t produced just out-of-coaxiality, but are produced at angles to one another. Notice the datum feature is a lot longer than the larger diameter. If the diameters are out-of-parallel to one another, transferring tolerance from one to the other won’t be calculated as a one-to-one proportion. It will be trigonometric.

The ASME Y14.5-1994 standard had a similar math error in its formulas for calculating position tolerance for multi-diameter mating features, but when I pointed it out (as described above) they changed it in the ASME Y14.5-2009 standard.

Hope this helps.

Jim

Jim,

Thank you, that is in line with what I was thinking and I appreciate the confirmation.

Best,

Rebecca

Rebecca,

One more thing. The gage I described uses a zero position tolerance at MMC. That makes it a Practical Absolute gage, which could, in a far-fetched theory, allow a bad part to pass.

To make it an Absolute gage that won’t even in theory accept a bad part, call out the gage position tolerance as zero at LMC. Or start the size of the gage element at .5007 and then give it a minus only size tolerance of .0003 and a position tolerance of zero at MMC. That would make the outer boundary of the gage hole .5007 (LMC) plus .0003 bonus position tolerance equals .501 (which is the same as you would get if you called the gage hole out with a .501 LMC and a zero position tolerance at LMC).

In either case, they are both Absolute gages.

Jim

Subject:  Some Other Trainer Wrecked Our Design Manual

Jim,

About a year ago, we asked you for a quote to come to our company and train a large group of our employees in GD&T. Ultimately, we decided go with one of your competitors. This guy came in and trained our people, but during the training in which he was supposed to be using the Y14.5 standard’s rules and symbols, he said the Y14.5 committee had made many errors and he had a better way of doing things. So, he proceeded to teach us symbols and rules he had apparently made up.

Then he talked our management into “correcting” our internal design manual’s tolerancing section by inserting these rules and symbols which don’t appear in any standard we can find. After our designers created a bunch of new design drawings that used what he’d taught, we sent our part drawings out for bid, and none of our suppliers knew what any of the symbology we used meant.

In short, this guy taught us wrong and changed our design manual to be wrong and we made a lot of new product drawings that are wrong. And they are so wrong that our suppliers say they are meaningless.

You’ve got to do something about this! We want to know what you plan to do to correct this mess.

Brian

Brian,

Just so I understand. You hired someone other than me. He wrecked the tolerancing section of your design manual and taught your employees rules and symbols he plucked out of mid-air. Now, none of your new drawings can be interpreted by your suppliers. And you want to know what I’m going “to do to correct this mess”?

I’m going to advise you to choose your trainers more wisely in the future, and to ask me for another quote to correct the problems the other guy created.

Jim

Subject: Weldment Question

James

I would like your opinion on the GD&T for a weldment. I have a roof that is welded together with two different sheet metal parts and I would like two rectangle opening to line up after welding so we can install an air duct. See attach PDF for my idea on how to line up the rectangle openings. The more that I look at it the more that I think that it is not right. Also attach is a BMP of the Solidworks assembly. What do you think?

Thank You

Chris

Chris,

Alignment is location. You’ve assigned perpendicularity controls everywhere, and although this will make the sides well oriented, it doesn’t do anything for where they are. If it is warping that concerns you, complying with the flatness and perpendicularity controls after welding would help, but if these controls apply only at the stage before they are welded, even they don’t help much. The rule since Y14.5-1994 is that tolerances only apply at the level of the drawing they are depicted. They don’t apply to the part at other stages, such as after welded.

It seems to me that you need to consider applying alignment controls, such as position before and after welding. Working assembly drawings are allowed to contain information regarding size, form, orientation and location tolerances that can’t be described before assembly.

I hope this helps.

Jim

Subject: Step Datums, Continuous Features, Compound Datum Features and Patterns of Datum Features

Dear Mr. Meadows,

My name is Brad, and I’ve taken the GD&T course and the Tolerance Stack-up course from you at University of Milwaukee of Wisconsin. You mentioned that if we have GD&T questions to contact you and I’d like to take you up on that. I have two questions at this time.

The first has to do with combined datums (ie, B-C, or whatever the proper term for it is) within a feature control frame. But, I guess me basic question is, does B and C have to be coplanar along one axis or another? I have an electrical board designer that wants to put them in opposite corners of a board and an engineer that says they both need to be along the x-axis or y-axis. I tried to find an example in your 2009 book, but couldn’t find anything.

The second question has to do with continuous feature of size. In the 2009 text book on page 177 you specify to inspect the CF (continuous feature) MMC with a GO GAGE. Does this mean that the surface being specified needs to be the maximum surface of the part in order to use CF? I have a heatsink that has 50 fins on one side, but only 45 of them mount a PCB, which are below the height of the remaining 5 fins. To me, these lower 45 fins are the critical surface and need to be controlled, but they are not the MMC surfaces. Can I still use the continuous feature of size callout for the 45 fins? Or what would be the best way to control these to be coplanar? Let me know if you’d like an example, ie. 3d step file, 2d drawing pdf, etc.

I hope things are going well for you and your family and are surviving the storm battles there in Tennessee.

Thank you,

Brad

Brad,

It’s perfectly legal to call out two features that are not coplanar or coaxial to each other as a compound datum. In terms of two non-coplanar surfaces it is called a step datum. In a fixture, it requires one fixturing block to be taller than the other. In terms of two holes or shafts that are not coaxial, it is exactly the same as calling both holes or shafts a datum feature pattern (for example positioning both holes to other datum references or just to each other and then hanging a datum feature symbol below the position control that states both features comprise datum feature pattern B).

As for the continuous feature type of control, they can be any group of features of size (widths or diameters) that you would like to be treated as one continuous feature of size. They don’t have to be the outermost (largest) features of size on the width. On the other hand, if you just want the tops of the fins to be coplanar, profiling them all might be the best way to accomplish that.

Thanks for the concern. My wife and I are fine. This group of storms didn’t do us any serious damage.

Jim

Subject:  I Need to Prove My Boss Wrong

Jim,

My boss thinks I don’t know anything. He treats me like a hangnail. He belittles my work, my clothes, the way I talk and even makes fun of the way I look. He said my eyes are so far apart I look like some sort of alien sea life. He says I walk like a penguin with jock itch. He said if my head was any bigger, it would need its own zip code.

What with jobs being so hard to find these days, I’m keeping my mouth shut. I’ve got two masters degrees and he’s treating me like I wear my underwear on the outside (which come to think of it is kind of a trendy thing to do now). I need to impress this guy. I’m thinking that our company product drawings (and CAD models) are somewhere near the technical correctness of drawings on a cave wall. If I could pass the ASME Geometric Dimensioning and Tolerancing Professional exam and be certified as a GD&T expert, I think that would change his attitude toward me.

Do you have any advice or materials on how best to pass this exam? I hear it isn’t easy.

Harry

Harry,

I think the way to pass any test is to study the material. Take GD&T courses. Read GD&T textbooks. Buy a copy of the Y14.5 standard and take it everywhere you go for a few months and read from it every chance you get.

The senior level exam was 100 questions when I took it. The technologist level exam was 125 questions. Recently, I was asked why I didn’t teach a course on how to pass the GDTP exam. I told the person that it wouldn’t be possible to teach such a course, unless you told exactly what was on the exam and taught the students the answers. That, of course, is not something ASME would look kindly on.

Someone later asked what materials might be possible for me to create that would make a good study guide. It got me to thinking. So, what I did was to write a test that is more than three times as long as the test ASME gives. The test and its answer book are for sale on my website. I sincerely believe that if someone can pass my test, they can easily pass the ASME exam.

Good luck with the exam and with your boss.

And when you get a chance, send me that zip code.

Jim

Close Window