GDT for round parts 3

[cooblacrouse]

My company manufactures predominantly hollow round parts. I am fairly new to the field and have been seeing inconsistencies in historical drawings when it comes to geometric dimensioning and tolerancing. The only answers I seem to get in house is to copy what was done on previous drawings. As I have studied on my own I have yet to find an example of an ID feature called out, using concentricity or runnout, in reference to and OD datum. Does anyone have any input or resources I can use? Examples I find in text books seem to be exclusively done on shafts, OD to OD.

Thank you,

Bob

 

[Viktor]

There is no difference. A datum for round parts is normally (though there are some exceptions) the axis of the surface and the runout is set with respect to this datum. Note that for a round part where the datum is the axis of the surface of revolution, the prime feature that makes sense is runout – no perpendicularity, parallelism, etc. Another important feature is concentricity which can be actually expressed through runout. For datum itself, cylindricity may have some sense. In any case, the selection of the proper datum(s) is the most important. One should realize that there are four basic types of datums: design datums, manufacturing datums, metrological datums and working datums. (sometimes the storage, transportation and assembly datums may also be considered). For example the AXIS of the center holes is usually taken as the design datum for a shaft (or an axel). It is also serves as the manufacturing and metrological datums. However, it has nothing to do with the working datum because these holes play no role (at least, normally) in shaft performance. Therefore, to understand what are the actual numbers to put when assigning shape tolerances, you have to start with the working datum(s) and then, step by step in reverse order, re-calculate these numbers to the design datum. In the case of a shaft with gears – you have first to understand what is the class of gears you need to select to meet the requirements (torque, noise, reliability, etc), then open a reference book on gear tolerances (AGMA) and find actual tolerances on gears, then, using these numbers, re-calculate them to the shaft shoulders, then go down to the axis of the center holes to assign runout between say the bearing and gear shoulders.


Unfortunately, I never seen this topic covered properly in the design books although I taught design.
Viktor

http://viktorastakhov.tripod.com

 

[cooblacrouse]

Victor,

Thank you for your response. An essential part of my problem is the establishment of datums, I do not necessraily agree with what has been done historically in the company. I under stand design datums and manufacturing datums and being in a small company I have to work with closely with manufacturing to give them what they need to make the part and still retain form, fit and function of the design. I have not read any material on metrological datums and working datums and would like to learn more about this. Do you have any recommended books that define and explain their use.

I have also not come across a proper method for checking total runnout in parts which cannot be put on centers. And the industy seems to want to go away from concentricity.

 

[drawoh]

Victor and Cooblacrouse,

I have recently taken a course on ASME Y14.5M-1994 Geometric Dimensioning and Tolerancing.

You cannot use a centre axis as a datum in YT14.5M. It does not exist. Apparently, you can use it in ISO GD&T, but I am not familiar with the standard. Presumably, there is some means for defining where the centreline is.

On round components, I tend not to use things like cylindricity and concentricity, because they are limited in what they specify. In many cases, you can select a flat base and one round surface as datums A and B, then use the positional tolerance to locate everything else.

For further reading, I suggest ASME Y14.5M-1994 Dimensioning and Tolerancing. It is pretty readable.

 

[Viktor]

Dear Optech

Unfortunately ASME Y14.5M-1994 “Geometric Dimensioning and Tolerancing” is a collection of mistakes and errors similar to many other ASME standards. When you put a shaft on the center holes (for manufacturing or inspection), you AUTOMATICALLY use the axis of this hole as THE DATUM. THERE IS NO OTHER OPTIONS. When you hold a cylindrical surface in a 3-jaw chuck – you use the axis of this surface, defined by three points, as the datum and thus you measure say runout with respect to this datum. ISO defines it very precisely when you can use a surface and when the axis of this surface as the datum – as such, in ISO it is clearly indicated on a drawing. ASME Y14.5M-1994 dropped this feature because “genius” or should I say “genies” from ASME did not understand the its meaning. I do not know how many years are still needed to realize that this is one of the most important issues defining quality of products. You can introduce 6sigma (10 sigma, 10000sigma) + black belts (or even green or blue noose) – it is not going to help. Quality begins from the drawings as the prime documents and manufacturing laws. Until ASME and others understand this issue, people in this country will continue to buy Japanese and European cars (those who can afford though – even huge tax on imports is not working) and machine tools (Cincinnati Millicron – where are you?) etc. Look at these drawings from our automotive industry – most do not have ANY datum! Look at design books – “ DATUM” is a “forbidden” word – it does not present even in the index. Not to mention that these books do not consider another important issue – calculations of dimension stackings (loops, chains whatever) – this is a shame. And the country is still playing in 6 sigma game!
Viktor

http://viktorastakhov.tripod.com

 

[drawoh]

Victor,

As I noted, I haven't seen the ISO GD&T standard, so I do not know how they define their centreline. I know ASME Y14.5M, so this is how I think it through.

On a moderately complex part, there are five or ten different ways I can define a centreline. As the designer, I don't want to provide this flexibility to anyone else. I dictate which features are used as datums. My decision is based on the functionality of the part and on how I intend to inspect it.

When I identify real features as datums, I dictate how the part will be jigged up for manufacturing and inspection.

The problem you are describing is bad drafting. Lots of people sitting at CAD stations have no idea of how to prepare fabrication drawings. They do not understand tolerances. They do not know how to or do not bother to apply tolerances. The result is dimensions that are unfabricatable as specified, and/or that cannot be expected to meet requirements.

When your fabricator comes back and tells you he is making a "best effort", you have lost control over your process.

The lack of proper datums does not affect ASME Y14.5M. The standard tells you how to interpret the drawing, datum or no datum. Of course, many drafters will be surprised as hell when they find out what they specified.

JHG

 

[Viktor]

Optech

This is exactly my point – a designer should say it all – no guesses or best efforts. I use to teach my student – you cannot staple your tongue to your drawing. Therefore it should say it all (like Molson Dry – it says it all since…). Unfortunately, this is not a case today. Look at the job descriptions – there are designer and separately engineers. This is nonsense. A good designer should possess multidisciplinary knowledge on the machine functioning, materials selection, heat treatment and other metallurgical procedures, manufacturing, assembly, reliability etc. And this is even without engineering degree as required by formal job descriptions? And then we are talking about design for manufacturing – one needs to know manufacturing and industrial metrology to follows this trend.
I also agree with you that datum selection is the signature of the designer (I won a number of court cases as a technical expert using this personal signature issue to compare drawing produces by different companies). It fully defines his/her qualification, experience, and engineering judgment. Proper selection of datums may save a tons of many to a company.

Unfortunately, this issue is the most neglected one in the current design practice where a fashion trend of 3D modeling give apparent filing of reality. Any nice 3D color drawing is still a picture done by a free painter unless it has proper set of datums.
Viktor

http://viktorastakhov.tripod.com

 

[GregLocock]

Without disagreeing with the many important points you are raising, might there not be multiple sets of datums?

The first 'natural' set is those which are natural to the production process - eg the axis between centres on a turned shaft, or the split line of a casting.

The second is those that can be used by the inspection facility.

There is also a third set, those defined by the function of the part.

A robust design would establish some relationship between the three sets of datums. Cheers

Greg Locock

 

[Viktor]

The first and foremost one is the design datims. If say a designer set lengths of shoulders starting from the left one, it does not mean that this part will be produced the same way. When a designer sent the datum for the bolt hole in a flange, this datum is not normally used in manufacturing. Moreover, the design datum account for MMC which is idealization – in manufacturing and inspection you already have the actual material condition and thus the tolerance is re-calculated using the actual material condition.

Therefore, basically we have four sets of datums: design, manufacturing, inspection, and working. It is highly desirable (for simplicity) to unify these datums. However, it is rarely possible so there should be the re-calculation of tolerances for manufacturing and inspection.
Viktor

http://viktorastakhov.tripod.com

 

[drawoh]

GregLocock,

There cannot be a multiple set of datums, at least, not in the context of a engineering drawing. In the GD&T course I took, I was told that the datums are the required mounting points for manufacturing and inspection.

I thought this was all extreme. If the part comes back from manufacturing and meets all my specifications, I don't care how it got fabricated. If the fabricator thinks he needs an intermediate datum, then I guess he needs one. His job is still to meet my specifications, and I won't be adding his datums to my drawing.

There is no guarantee that the next fabricator that comes along would use the same intermedate datums.

JHG

 

[GregLocock]

OK, so in your philosophy you have aligned two of the sets of datums, manufacturing and inspection. This seems slightly mysterious to me as the end user, I don't care what the manufacturing and inspection guys get up to, what I want is a part that meets my functional spec, which may be based around some entirely different 'datum'. It is the job of the designer to align these requirements, but it is an actual part of the design process, and should be recognised as such.



Cheers

Greg Locock

 

[diamondjim]

Bob,
This discussion is enlightening. The function of
your part seems to dictate how the datums should
be specified. With hollow parts, is concentricity
an issue? It is just basically a pipe of some sort?
It is a hollow shaft or tube that is taking multiple
loads like torque, axial loading, radial loading
and such? With hollow parts, the id or od seems to
be the only logical datum unless it is so thin that
it will not maintain shape and cannot be chucked or
centered by tapered cones. You have not mentioned why
you are concerned. Do the parts have internal stesses
and you are concerned about the cross sections of the
tubes be symmmetrical? You can put datums everywhere,
but are they true planes or the best guess of the plane
etc.? How do you establish the plane? Take for example
parallelism, it seems that the interpretation is that
there are two supposed planes perfectly symmetrical or
offset from the datum plane. If the physical part is
not perfectly flat and nothing is, how do you establish
the true datum plane? I just asked 4 guys all who have
been exposed to Y14.5M the basic question is that
if two parallel surfaces on the drawing are each flat
within .001 are the parts parallel within .001 or .002
to each other? 3 out of 4 say .002. Is the majority
right as to what is meant? Or does the standard imply
only one answer? Obviously not.
So again what is the function that you are trying to
control? Uniform thickness between od an id and not
really concerned about roundness? I am certain that you
have seen the pipe expanders to round up and expand
the necessary mating parts so they can fit together.
Datums are fun and the designers responsibility. The
hard part is knowing what your plant can actually make
verses what they want to make or control or if you are
really being realistic in asking for certain features
that are beyond the normal shop procedure. Have fun.

 

[drawoh]

Greg,

This discussion is awkward without some sort of graphics tool to use as a reference.

Let's take the case that you require a part with feature C aligned accurately to features A and B. The ideal case is that I will use features A and B as my primary and secondary datums on my drawing, and that the fabricator and inspector will use these featues for their fixturing. You will have a relatively high level of confidence about the resulting part meeting all of your requirements. This happens a lot.

An alternate case is that feature A is not a good fixturing surface. It is not poassible to verify your required alignment through direct measurement.

Usually, there is a feature D, that feature A can be located from. In this scenario, my primary datums are D and B. Features A and C each are located from these. My tolerances must be twice as accurate, since I am working with two positional tolerances instead of one.

The very worst case is that I will have to design feature D into the system so that I can use it as a datum.

Your ultimate requirement is for a part that works, but this is not possible unless I can write up specifications that can be fabricated to, and inspected.

Diamondjim,

If the datum is a surface, that surface is defined by the three points that make contact with your granite reference table. This is explained fairly clearly by ASME Y14.5M-1994.

JHG

 

[Viktor]

GregLocock and Optech

This is a strange situation where you are both right. I would agree with Optech that our discussion is awkward without graphics.

Greg – definitely you should specify on your drawing only the design datums to assure accuracy required for part performance. However, a good designer should keep in mind a possible way of part production (this we call DESIGN FOR MANUFACTURING). For example, if you specify the axis of center hole as your design datum, you automatically tell the manufacture: you have to produce these two holes; you have to machine this part using these holes; you have to inspect this part using these holes, etc. However, you don’t need these two holes for part performance. So you indirectly suggested the way of manufacturing.

The manufacturing datums can be very different from the design datums. As mentioned by Optech, the design datums may not be suitable for the fixturing. Here another closely related topic called the principles of locating should be involved. A manufacturing engineer preparing the original design drawing for production, should decompose it for many manufacturing drawings for each operation. Each of these manufacturing drawing should indicate the clamping surfaces – manufacturing datums (if a part to be fixed then clamping should take away 6 degrees of freedom), dimensional accuracy, shape and positional tolerances particular for this operation. As such, this manufacturing engineer should re-calculate the tolerances assigned by the designer for all intermediate operations. Moreover, according to the requirement of quality standards, each operational quality control station as well as the final should have a sketch of the part where the metrological datums (clamping features) should be indicated and the way to measure the required accuracy should be clearly shown. Again, this will depend on what kind of measuring tool is available. Clearly, it will be different for inspections by calipers and CMM. Anyway, it is a responsibility of the manufacturer to meat the quality requirements assigned by the drawing. And he does it accounting for the available technological and inspecting equipment available.

Optech
Your statement “If the datum is a surface, that surface is defined by the three points that make contact with your granite reference table. This is explained fairly clearly by ASME Y14.5M-1994.”
I cannot agree with this statement – it is incomplete.
Common surface have the forms of planes, cylinders, and cones. Sometimes special types of surfaces are found. The surfaces occur in many arrangements. A block may be made up of perpendicular planers; a shaft may have one or more cylindrical surfaces in its length, bounded by planes, with conical surfaces or round holes in the ends; and a gear may have inside and outside cylindrical surfaces, planes, and involute surfaces. To cope with the many possibilities, many datums means have been devised, but the key to all of them is found in the principles of locating. According to these principles, the choice of locating points must take into consideration:
1. The six possible degrees of freedom and the criteria of their restrictions.
2. The relative merits of available points for location.
3. The condition of the locating surfaces.
4. The shape of the part.
5. The surface to which registration is required.

Viktor

http://viktorastakhov.tripod.com

 

[drawoh]

Victor,

My statement was incomplete. I should have refered to a _flat_ surface.

ASME Y14.5M-1994 describes a circular datum as follows...

"Primary Datum Feature - Diamter RFS. The simulated datum is the axis of the true geometric counterpart of the datum feature. The true geometric counterpart (or actual mating envelope) is the smallest circumscribed (for an external feature) or largest incsribed (for an internal feature) perfect cylinder that contacts the datum feature surface. See Figs 4-11 and 4-12."

Figs 4-11 and 4-12 are hard to described in text, but they show a perfect cylinder and a perfect hole coming into contact with a with rough hole and rough cylinder, respectively.

I have never tried to inspect for something like this. It looks challenging.

Still, when I apply a datum symbol on my drawing, the standard explains what it means.

None of what we have discussed around here gets us around the need for competent design and drafting. To apply useful tolerances onto a manufacturing drawing, the designer must understand the manufacturing process as well as the final requirements, and the drafting standard.

JHG

 

[Viktor]

Dear JHG

I fully agree with your statement:

“None of what we have discussed around here gets us around the need for competent design and drafting. To apply useful tolerances onto a manufacturing drawing, the designer must understand the manufacturing process as well as the final requirements, and the drafting standard.”

However, “Huston, we have a problem.” The problem is how to achieve this. The standard is does not answer a number of vitally important questions (and it actually should not). There should be a number of good design books with examples of datum selection, re-calculating tolerances between different datums (including manufacturing rough and final datums), etc. Otherwise, it is next to impossible to teach engineering students what the design is all about.

Life is very good even without knowing and understanding the datum and principles of locating. Moreover, modern CAD programs, can do the job in just a few seconds.

In my opinion, engineering students have been taught to rely far too completely on computer models, and their lack of old-fashioned, direct, hands-on experience can be disastrous. By the 1980th, engineering curricula had shifted to analytical approaches, and visual and other sensual knowledge of the world seemed much less relevant. Computer programs spewed out wonderfully rapid and precise solutions of obviously complicated problems, making it possible for students and faculties to believe that civilization had at last reached a state in which all technical problems were readily solvable.
As faculties dropped engineering drawing and shop practice from their curricula and deemed plant visits unnecessary, students had no reason to believe that curiosity about the physical meaning of the subjects they were studying was necessary.
Despite the enormous effort and money that have been poured into creating analytical tools to add precision to the design of complex systems, a paradox remains. There have been a harrowing succession of flawed designs with fatal results (For example one famous automotive company could not calculate the location of the center of gravity on its popular SUV so many life were lost due to this “innocent” misfortune). Those failures exude a strong scent of inexperience or bad habits or both and reflect an apparent ignorance of, or disregard for, the limits of stress in materials and people under chaotic conditions. Successful design still requires expert tacit knowledge and an intuitive “feel” based on experience; it requires engineers steeped in an understanding of existing engineering systems as well as in the new systems being designed.
An excellent outlook on design failures may be found in a book titled “Engineer Is Human: The Role of Failure in Successful Design” written by Professor Henry Petrovski. (I strongly recommend that you to read this book). Petrovski uses the 1978 collapse of the modern “space-frame” roof of the Hartford Civic Center under a snow load as an example of the limitations of computerized design. The roof failed a few hours after a basketball game that had been attended by several thousand people, and, providentially, nobody was hurt in the collapse. Petrovski explains the complexity of the space frame, which suggested mammoth Tinkertoys, with long, straight steel roads arranged vertically, horizontally, and diagonally. To design a space frame using a slide rule or a mechanical calculator was a laborious process with too many uncertainties for nearly any engineer, so space frames were seldom built before computer programs became available. With a computer model, however, analysis can be made quickly. The computer’s apparent precision, says Petrovski - six or more significant figures - can give engineers “an unwarranted confidence in the validity of the resulting numbers.”

Who made the computer model of a proposed structure is of more than passing interest. If the model is worked out on a commercially available analytical program, the designer will have no easy way of discovering all the assumptions made by the programmer. Consequently, the designer must either accept on faith the program’s results or check the results - experimentally, graphically, or numerically - in sufficient depth to be satisfied that the programmer did not make dangerous assumptions or omit critical factors and that the program reflects fully the subtleties of the designer’s own unique problem.
To understand the hazards of using a program written by somebody else, Petrovski quotes a Canadian structural engineer on the use of commercial software: “Because structural analysis and detailing programs are complex, the profession as a whole will use programs written by a few. These few will come from the ranks of structural ‘analysis’ and not from the structural ‘designers.’ Generally speaking, their design and construction-site experience and background will tend to be limited. It is difficult to envision a mechanism for ensuring that the products of such a person will display experience and intuition of a competent designer. More than ever before, the challenge to the profession and to educators is to develop designers who will be able to stand up to and reject or modify the results of a computer-aided analysis and design.”
The engineers who can “stand up to” a computer will be those who understand that software incorporates many assumptions that cannot be easily detected by its users, but that affect the validity of the results. There are a thousand points of doubt in every complex computer program. Successful computer-aided design requires vigilance and the same visual knowledge and intuitive sense of fitness that successful designers have always depended on when making critical design decisions. If we are to avoid calamitous design errors, it is necessary for engineers to understand that such errors are not errors of mathematics or calculation, but errors of engineering judgment, a judgment that is not reducible to engineering science or mathematics.
Here, indeed, is the crux of all arguments about the nature of the education an engineer requires. Necessary as the analytical tools of science and mathematics most certainly are, most important is the development in students and neophyte engineers of sound judgment and an intuitive sense of fitness and adequacy.
No matter now vigorously a “science” and computerization of design may be pushed, the successful design of real things in a contingent world will always be based more on art than on science. Unquantifiable judgments and choices are the elements that determine the way a design comes together. Engineering design is simply that kind of process. It always has been. It always will be.


Viktor

http://viktorastakhov.tripod.com

 

[cooblacrouse]

Diamondjim,

Bear with me I am but a lowly designer with but a high school diploma and a 1 year certificate in CAD. However I have had some limited experience with machining and inspection. My concerns are mainly for what is the proper tolerance, what is can be inspected and what can be manufactured. For example, take a simple internal ring gear with rabbets on either side for the purpose of sandwiching it between housings. The rabbets and the ID, blank dia of gear teeth before gear cutting (we do not use a topping cutter), must all be have a common axis. For manufacturing the OD of the part is made the primary datum because it is held in a hydraulic fixture for gear cutting. The rabbets and the ID are all different set-ups, therefore clamping forces could be on different parts of the OD. In the past, more than 8 years ago, concentricity was used exclusively on these parts but it was being inspected in a vee-block, which did not give true concentricity but circular runnout. A decision was made to change all concentricity to total runnout, which was not necessary in all cases. The only examples I have found for checking total runnout is between centers on a shaft. In this case we need to check the rabbets and the ID against the OD. The part was put in a vee-block on the OD and an indicator run along the rabbets and the ID respectively, which measures circular runnout not total runnout. To me concentricity is the correct tolerance in this case because I am not concerned about taper or differences in roundness being at the same place in the part. I want the axes to be the same. Enter the CMM. The machinists, I found out, are now using a CMM to check these parts and are really checking concentricity. Then when the parts get to inspection they could fail for total runnout due high and low points being at different places and causing an increased indicator movement without effecting the concentricity. On top of this, our inspector just went through a course in GDT and was told that concentricity should not be used because it is purely theoretical and too hard to inspect.

You see my quandry, I have no examples of how to properly inspect an ID to an OD for runnout and I do not feel runnout is the right tolerance for the part in all cases.

Thank you,

Bob

 

[docholliday]

Just in case anyone else has been searching the web for the book that Viktor mentioned - which sounds like a really worthile read - and not seeing worthwhile results, I've noticed (thanks to Amazon.com)that the author is actually Henry Petroski.

Mike

 

[drawoh]

Cooblacrouse,

One option you have with ASME Y14.5M-1994 is to apply datum targets. Instead of defining the OD as your datum, you define three points, A1, A2 and A3. Three points define the circle you want everything located to, and they define where the fabricator and inspector ought to be clamping for each of their processes. This takes care of out-of-roundness problems with your OD.

Concentricity is not supposed to be used much anymore. Probably, you should be using the positional tolerance, which controls a few more features.

Are you inspecting your gear before or after you cut the teeth?

If before, you need to leave sufficient material that each gear tooth will be completely fabricated. Consider the following specification for your ID...

Datum A is the flat surface on one side of the gear
Datum B is the OD, defined using datum points.
Positional tolerance: 0 at least material condition

Make the diameter tolerance sloppy. Specify whatever minimum diameter should not cause problems for the gear cutter.

Note what I have done here. You need material to cut the gear out of. The maximum allowable ID is the minimum inside diameter of the gear, located exactly at the gear centre, and precisely round. If your ID is 0.1" too small, it can be located 0.05" off centre, and it can have out of round bulges extending to the maximum ID. At maximum material condition, you don't care how round the hole is, as long as it does not pass outside the maximum diamter.

Outside of CMM, there is no completely reliable inspection strategy. As an alternative to runout, I could consider jigging the gear with Datum A vertical. Locate the datum points to get Datum B. Measure to the bottom and top points of the ID. Rotate the gear and do it again.

All of this assumes that you are inspecting the ID prior to gear cutting. This is how I would solve this particular problem.

JHG

 

[cooblacrouse]

optech,

The ID of the part before gear cutting is the top of the tooth after gear cutting. Also note that our gear teeth are very small, ie. .015" high on a 2" pitch circle. The ID is inspected before gear cutting.

I do not understand how you would specify datum targets on a round part. How can you tell where the target points are to clamp in the same place every time? The part is a steel ring, do you need some type of timing mark?

If true position is used how is it inspected? If the CMM finds the theoretical axis of the datum, OD, by averaging a specified no. of hits and then does the same for the ID and gives you the variance it seems similar to how it calcualtes concentricity.

Bob