Recommanded tolerance for datum features 2

[supergee]

Hello all,

As some of you might know, I am teaching GD&T at the college level. I was wondering if there was a rule of thumb about the value to give for datum tolerances. I got a tip about that a few years ago from someone in the aerospace industry. The rule of thumb was to make the datum 10 times more precise than the least tolerance referencing that datum.

This would mean a flatness of .0005" for a datum when a hole position tolerance is .005". That seems to make perfect sense in the aerospace business, but .0005" is very precise for many companies.

While I am in favor of teaching the best practices of the industry, I want to teach the students not only the best but also what is reasonable after doing a cost-benefit analysis. For instance, 10x more precise if people's lives might be at risk, such as critical components with significant impact in case of failure (e.g., aircraft engines), and 5x more precise for noncritical components with low impact (e.g., low-cost washing machines).

Is there some standard or reference on this subject you might know?

Gee

 

[mfgenggear]

OP
The standard is experience.
It all depends on the product and application.
Eg ground shafts, gears, critical complex details, sheet metal details, rough castings forgings,

 

[supergee]

Thanks for your input, mfgenggear.

As a teacher, my job is to take existing experiences and summarize them so that students don't start from scratch. My predecessors used to teach GD&T symbols and their meanings.

I try to teach them the effect of GD&T on practical cases: I don't want them to just read GD&T, I want them to design with GD&T.

That is why I need real-life scenarios. I actually give them an oral exam, where they need to explain WHY they chose the tolerances and datums on their homework. Ever since, most of my students have been able to explain when and why they should use certain tolerances and even the values for location. The datum value is a recurring question, which is why I ask here.

Gee

 

[3DDave]

There is a fundamental flaw that is not discussed in the ASME Y14.5 standard.

The standard makes a promise that nothing is allowed to cross the boundary of the datum; that the datum is absolute and that the True Geometric Counterpart" or "Datum Feature Simulator" is a suitable stand-in, themselves taken as sufficiently perfect.

The flaw is that that the datum is held to be representative of the limitation imposed by the mating part, but the reality is the mating part is irregular.

This irregularity isn't mentioned.

A simple stack calculation based on the AME of mated parts may give the same as the AME of the mated parts, but will often be less.

In ASME Y14.5: 2+2 <= 4

It is also possible for the mating of irregularities to allow unaccounted for rotations.

This can cause an additional datum shift that isn't otherwise accounted for.

Making the datum features excessively precise is one way to deal with the problem. The other is to make the extent of the datum features so small that the effect is minimized.

There is also another factor - QC wants their job to be easier and throughput to be higher. Not dealing with irregularities does that. If the form of the feature is nearly perfect they don't need to spend time looking for high and low spots; they might be able to choose a single CMM hit to represent an entire surface. The conflict with those who make the parts is obvious.

Just keep in mind that setting a part on the surface plate will contact high spots. Those spots aren't necessarily what the mating part will contact.

 

[mfgenggear]

3d Dave very good.

OP
The answer is complex. I will try to give examples.
Keep ot simple, give tolerances of ÷/- 010 and +/- .005. In general. True position .010 and .005 when possible.
My specialty is gears. Gear shafts.
On shafts manufactureers like between centers, and datum at each end. You can give .0005 runout and .0005 diameter tolerance. Yet give. 0005 tolerance and run out on other ground diameters to the datuma. And it is done often.

As a manfacture they tighten those tolerances due to stack up of tolerances as machining . This is also done often.
Place the AANSIY14 procedures. But tolerance to perform the following.
Given enough tolerance so the manufacture
Can machine at the most cost efficiency.
Yet maintain the requirements and integrity
Of the detail or assembly.
It's a fine line.
I recommend when possible send out drawing for concurrent engineering and manufacturing review.

 

[Ryan6338]

I agree 100% with all the replies. There's really no general rule that can be applied here. The drawing should be designed to guarantee fitment and function with the widest tolerance possible. The idea of increasing a tolerance just because something is safety critical doesn't really make sense. When it comes to tolerances, the goal is always to maximize tolerance zones while still meeting all functional requirements. Sometimes this results in a tight tolerance, and sometimes it doesn't. On the contrary to your example, it's often much more expensive to design things with wide tolerance zones.

Things like aircraft parts may be given a tighter tolerance just because the increased costs of high-tolerances is negligible compared to other factors of the design and the quantity isn't high enough to justify significant time spent on cost-reduction by widening tolerances as much as possible. Products that need to be low-cost may require significantly more design effort to reduce their cost as much as possible. They end up getting a wide tolerance at the cost of significant engineering effort ensuring everything will work using the cheapest possible manufacturing methods.

 

[jassco]

Hi, Supergee:

Designers of a product should be familiar with its manufacturing processes which control economical precision for a feature. If your students are not familiar with process, they can look at standard tolerances for typical manufacturing processes. If you are in US, you can look into ANSI standard tolerances B4.1. IT grade number (4 to 13) is a good starting point. If you deal with special processes, your best bet is to find tolerances from vendors who is going to make the product or components.

Although ASME or ISO standards don't recommend specifying manufacturing process for a product or component, the designer needs to have knowledge of processes in order to design it.

Best regards,

Alex

 

[ctopher]

I have seen young engineers switch careers, burn out, change from mech to other engineering, because they are taught GD&T and how to tolerance parts. They want to only design a 3D model and move on.
The ones I find that stick with it are the ones that are taught machining practices, they get experience in the shop.
Teaching them GD&T is great, but also teach them why and how it's used in the machine shop. Show videos, visit shops.
My son is an engineering professor, he also sees the same as I do.

 

[drawoh]

supergee,

I assume you are discussing Features Of Size (FOS) datums.

There is a crude rule of thumb that your inspection fixture should be ten times as accurate as whatever it is your are measuring. If your datum feature of size is accurate enough, you can ignore its tolerances and material conditions. If your datum feature is sloppy, you can call it out at MMC. Regardless, you have all sorts of fixturing problems you need to think through.

I did a GD&T presentation at work, and I prepared some drawings to use for it, one of which I goofed up. I did not bother to fix the mistake. The drawing made a useful discussion tool. What you can do is prepare a drawing with a sloppy FOS datum feature, and discuss fixturing with your students. Rules of thumb are not cast in stone. Maybe the sloppy feature works!

 

[supergee]

Thank you all for your replies. Honestly, they're all quality answers.

• 3DDave, as usual, you demonstrate excellent comprehension of the standard.
• mfgenggear, jassco, and, well, everyone else, I don't remember reading replies from you before, but you make very valid points, and I thank you.
• yan6338, I like your input about the relative cost of added precision to an already expensive aerospace part. I will mention it.

I do understand why we need to control the surface. Below are three PowerPoint slides I show my students to help them understand why a part that works on a surface plate might not work when used. It's in French, but the images are explicit (I am in the French part of Canada and I teach ASME). I was wondering about what value is reasonable, if any.

So, in conclusion, I will tell my students that:

• There are no standards about how to determine datum feature precision.
• The vast majority of times, but not always, the precision on the datum is much lower than the precision of the feature related to the said datum.
• There's a rule of thumb of 1/10th of the precision for the datum, but this might differ depending on the application and risk factor.
• Like with everything, when they start their career, they should ask an experienced colleague about what they do and why. (Though, in my career, I found a LOT of experienced colleagues who know little about GD&T... I mean colleagues that check parallelism with a micrometer )

If you feel there's more to add, feel free to write back.

Gee

 

[Garland23]

Interesting that you're using inches. I thought you guys were ahead of us Americans in using SI units

 

[CTengIS]

There is no 1/10 rule of thumb for qualifying the datum features. The 1/10 rule of thumb is for the gages and fixtures (datum feature simulators) that are used at inspection.

Just like other features of the part, the datum features are controlled by tolerances to make sure they are useful for their function. Remember that when you control a surface that is not a datum feature by a geometric tolerance such as angularity or profile relative to datums, you are also controlling its flatness within the same tolerance value. However, If there is no flatness tolerance for a primary datum feature, then its form is uncontrolled. Then it may not function well as an interface feature in the assembly. The tolerance value can be driven by how much stress/deformation, or rocking, or maybe in some cases fluid leakage, your design can tolerate at the interface.

 

[jassco]

Hi, Supergee:

What you are after is qualification of datum features to make sure they are repeatable. There are tolerance and cost involved. You need to let your students know how to compromise them. I used to teach design of precision machine tools. I always use something similar to IT grades. For example, you have a flat datum feature A. You want to make sure that it is reasonably flat. How do you do that? Well, you look up standard tolerances for the process that creates the feature and determine flatness based on size of the surface.

Best regards,

Alex

 

[3DDave]

IT grades are per ISO 286, for those interested.

I suspect it is better to determine what variation in the datum features is acceptable and then find a process to produce it than the other way around.

If the process is forced on the designer then make the design as insensitive to the process variation as possible if that variation is too much.

 

[Wuzhee]

Although ASME or ISO standards don't recommend specifying manufacturing process for a product or component, the designer needs to have knowledge of processes in order to design it.

I come across this almost daily in our R&D group. My coworkers like to overthink and they want to establish definitive manufacturing processes on the drawings.

Then theres's the other group who can't comprehend modern machining techniques and are stuck with 2-axis turning and 3-axis milling.
It really narrows down the paths one could take because the lack of process knowledge.

 

[dgeesaman]

I've never heard of a relationship between the tolerance of form for a datum and the tolerances of features that reference it as a datum.

On a practical level, most parts have several features of similar high precision ('high' is relative to the function and manufacturing method of the part). So I find my datums are of similar tolerance of form as the other key features.

If you're making a functional gauge, it would make sense to have your datum-facing feature on the gauge be 5x or 10x better than the datums resting against it. Just like you might select a suitably flat granite table or suitably accurate gauge pin for a hole. But gauge tolerances are a different matter than the tolerances of the part itself.

Also as a general comment, I've been coached and rewarded in real life for tolerancing my drawings to maximize the tolerance against functional limits. I will always try to learn the capabilities of the manufacturing process that is in use and why it's the current practice, but I try to not add notes or requirements that would exclude other methods or processes that could produce a satisfactory component. The goal is to design the part with the widest possible tolerances and in a configuration that allows as many manufacturing methods as possible.

I think good tolerancing is one of the hardest things to learn in industry - not because it's intellectually difficult - but because it requires a deep knowledge of many things that do not live on an engineer's desk. And few companies have engineers operating in an environment where the necessary interaction and feedback is available. And I think many design engineers simply ignore this part of their functional responsibilities.

 

[rimag]

There might be a difference between ASME and ISO here how datums are associated and established from datum features, but for ISO atleast, the form/location/orientation of a datum feature is important as it will affect the measuring uncertainty of the tolerance zone of features referencing the datum system.

If tolerances of datum features is more generous than the features that references the datum you introduce more measuring uncertainty.
I work in the aerospace industry with mostly machined precision components, and a flatness tolerances of the primary datum reference in the area of 0.005" is not unusual as it might be needed for the function, but also to be able to inspect and verify features of tight tolerances in the part.

From my experience from inspection reports, the flatness is often much finer than specified and It comes down to an understanding of the machining process to know whether a certain tolerance is "tight" or not for the specific part/and datum feature.

 

[Wuzhee]

.005" is only 0.127 mm. I wouldn't call that *precision machining*. Anything below 0.05 (~ .00196 in) is what I call precision requirement.
We require 0.02 regularly which isn't a big deal at all.

 

[mfgenggear]

in the gear and gear shaft components.
USA tolerances day in and day out .0003 - .0005. typical diameters and runout.
and it's not unusual to obtain .00005-.0001.
of course ground surfaces. including surface and I'd and od grinding. not including lapped. which is more precision. one has to consider
accumulative dimension stack up while manufacturing.

 

[rimag]

.005" is only 0.127 mm. I wouldn't call that *precision machining*. Anything below 0.05 (~ .00196 in) is what I call precision requirement.
We require 0.02 regularly which isn't a big deal at all.

You see, I am not used working with inches . I agree, and my point was just that, normally obtaining a tight flatness is not a big deal.