Engineers Handbook - Different Clearance Holes 5

[greg2835]

I have noticed in the engineers handbook (30th ed) there are a few instances where clearance hole sizes are tabulated for inch fasteners. For instance, in the section Fasteners -> Metric Threaded Fasteners -> Clearance Holes for Bolts, Screws, and Nuts (p. 1659) there is a table that uses ASME 18.2.8 for clearance holes. In another section, Fasteners -> Cap and Set Screws -> Drill and Counterbore Size (p. 1733) the clearance holes for the counterbores are listed from ASME B18.3 and are different than the previous table. Furthermore, in section Threading -> Tapping and Thread Cutting -> Tapping Drill Sizes -> Clearance Holes (p. 2093) the listed clearance holes are different than the previous two tables.

I noticed that my CAD program (SolidWorks) uses the third mention table for all clearance holes (simple hole, counterbore, countersink) and so do most other tables and posters I see in shops. I'm just looking to see if anyone can provide some clarity as to why there is a variety listed. For instance, why does ASME state different clearance holes in B18.2.8 and B18.3?

Thanks in advance,

Greg

 

[MintJulep]

The great thing about standards is that there are so many to choose from....

 

[JohnRBaker]

Well there are different classes of 'fits' when it comes to fastener clearance holes.

John R. Baker, P.E. (ret)
EX-Product 'Evangelist'
Irvine, CA
Siemens PLM:
UG/NX Museum:

The secret of life is not finding someone to live with
It's finding someone you can't live without

 

[greg2835]

@MintJulep Ha! Very true

@JohnRBaker yes and they each list different classes of 'fits'. The first table lists Close, Normal, and Loose fit. The second table lists Close and Normal fit. And the third table lists Close and Free fit. But the majority of them don't match up. Below is an example for a #4 screw clearance hole (drill sizes listed)


Close Normal (Free) Loose
Table 1 #31 #30 #27
Table 2 1/8 #29
Table 3 #32 #30


I know they are all pretty close, just wondering if anyone knew the reasoning - or if it is as simple as we just have a variety of the same standard

 

[greg2835]

Sorry I thought my table was going to look more like a table :/

Table 1:
Close = #31
Normal = #30
Loose = #27

Table 2:
Close = 1/8
Normal = #29

Table 3:
Close = #32
Free = #30

 

[CWB1]

Simple, different fastener types have different threads. Set screw threads for example are commonly a class 3 fit whereas most everything else is a class 2. In a similar vein, cut threads are geometrically slightly different than formed threads, hence the difference in strength.

 

[Jboggs]

"just wondering if anyone knew the reasoning"
It has to do with all the related considerations such as: how precisely you want the holes to position the screws, what kind of tooling and skill levels are available, how many holes there are in the pattern, and many others. For example, let's you have a lot of holes in a pattern. If you know they will be laid out by hand with a tape measure, you might go with larger clearance holes just to allow absorption of the unavoidable inaccuracies and variations, so the assembly guys don't have to spend half the day filing out and resizing holes just to get them to fit. If however you know the layout will be done on a CNC, then you know the positions will be more accurate, and you can go with smaller clearance holes. The various "standard" just assist the engineer in applying his judgment to the particular situation. That's why standard clearance holes in structural steel work and in tool and die work are two very different things. Think of the environment (tools, skill levels, assembly practices) in which they are created and used.

Standards are very important, but they should not replace the human judgment of the engineer.

 

[greg2835]

Very good, thank you to everyone for your input. @Jboggs I couldn't agree more. The size of the hole must meet design intent as well as manufacturing and other capabilities.

 

[BiPolarMoment]

The great thing about standards is that there are so many to choose from....

This is why you just do your testing first and write your protocol afterwards...

 

[tbuelna]

ASME B18.3 "Socket Cap, Shoulder, Set Screws, and Hex Keys (Inch Series)" is a standard more applicable to dimensions of the fasteners and associated tools. ASME B18.2.8 "Clearance Holes for Bolts Screws and Studs" is a standard listing recommended fastener clearance hole sizes in 3 classes (close, normal, loose) designed to utilize existing standard drill bit sizes.

 

[CWB1]

I disagree.

B18.2.8 and B18.3 control different types of fasteners with different threads and the necessarily different clearance holes as mentioned above. It may seem arbitrary to many engineers who have little/no background on the shop floor, but the couple thou difference in major diameter between a class 2 and class 3 thread of the same pitch can create all manner of issues downstream of design if standards are applied improperly.

 

[Sparweb]

It's always fun to arrive late to a discussion like this one that is approaching a resolution and throw a confusion grenade.

In aerospace we classify holes by the application, and some of us actually refer to holes as "class 1" through "class 4" or "5" depending on which reference you're looking at (I can see MintJulep pointing his/her finger already). For any given standard fastener size there are then given a min/max to specify in the tolerance limits, suitable for a particular application. For instance, if installing a structural part with shear-loaded 1/4" fasteners, a Class 1 or Class 2 hole might be called for, leading to a tolerance approximately [0.250/0.254] inch, but if the application is a light bracket that could be removed repeatedly or has lots of holes that must all freely line up, then a class 4 hole would be applicable, and then the drawing has a tolerance on the hole more like [0.265/0.274]. Not only is the hole larger but the tolerance band is looser, too. Know when you can make the part cheaper.

Notice how we are not specifying the drill size to be used. We are relying on manufacturing to select the right drill for the job.
What we are actually providing here is the pass/fail criteria to our inspectors who will use the drawing to accept/reject the finished part.
To be a bit more pointed about it: we are not taking responsibility for telling manufacturing how they should make the hole.
If they want to use a router with a 1/16" pin to cut a circular path, then by all means they can, but a short sharp E bit will do, too.
They sometimes complain because we are not telling them step-by-step what to do, but if we give in, we will be tying their hands and they'll complain about that even more.

STF

 

[CWB1]

Different industries do operate differently, however the important thing to realize here is that not all fastener types are commonly manufactured to the same thread class until you get into nonstandard fasteners. A common hardware store 1/4-20 hex bolt print callout would be 1/4-20 UNC-2A. The common set screw in the next bin OTOH would be 1/4-20 UNC-3A. The major thread diameter is different so the corresponding clearance hole necessarily is too along with the callout, strength, and a host of other design considerations, hence different applicable standards. Not sure why there is any confusion on this issue, this is freshman year design 101 that anybody touching a design or print should be well aware of. Mistaking otherwise is paramount to specifying a pilot drill on a threaded hole callout.

 

[3DDave]

The difference between the 2A and 3A max OD is 0.0011 inch. Not much reason to change a clearance hole.

Specifying the tap drill is an explicit way to get the finished hole one wants. There is enough range to allowable minor diameters that several different standard drills can be used to get the desired combination of thread strength and ease of tapping. One might go with a larger drill with slightly lower strength requirements to speed tapping and increase the rate of production/minimize the wear rate of taps. Alternatively, go with a smaller drill to maximize the strength. It should not be left to a factory floor guy to become an ad hoc part of the engineering design process.

As for the original question, I noted that the tolerances for drilled holes in the Machinery's Handbook chart indicated it was from drilling a hundred holes of each size into iron and measuring them. Which means they really don't apply to other materials, such as aluminum, but people use the same tolerances as if they do. The chart also fails to mention if this was a 3-sigma range or just the range they got for that sample. Doesn't matter - people copy and paste and don't read the fine print.

I expect the same is true of the clearance hole charts. Someone did some experiment, gathered some data, and it got published. If the actual reasoning/method is not part of the chart, then the contents fall back to a default of not being so bad that people stop using it. Without backing the particular values are otherwise meaningless.

Required clearance is a matter of all the factors that affect the structural need for the fastener, too many to care to list, and manufacturing capability. The chart just gives an out for avoiding evaluating the situation. If the fasteners don't fit, they'll just drill the clearance holes bigger anyway.

 

[CWB1]

Yes, the difference in thread classes is very small however to an end user that tiny bit of difference often means fasteners backing out, galling, failing, and a host of other concerns, hence different standards and geometries that every designer and draftsman should be well aware of. Personally I wouldn't doubt the difference in clearance holes to be vital somewhere in standard manufacturing or usage.

It may seem trivial to office staff but as parts must be made to print or rejected, nonstandard combinations of tap/drill/clearance/head/point geometry create all manner of issues that quickly drive up cost. Many production shops use combination tools, spec something nonstandard and the drill, tap, and clearance geometry become three separate operations with three separate tools rather than one. Even if the shop runs individual tools/operations, spec'ing a nonstandard hole often means additional machine setup time to change tools and certainly will mean additional inspection, again time and cost. It also increases the risk of mistakes causing scrap and most suppliers will charge accordingly, 30% premiums on parts that need special manufacturing is very common as is additional charges like material profit markups, tool markups, etc that would not be charged otherwise. Internally, manufacturing engineering may decide to spec a pilot drill or tooling for various reasons but they will do so on manufacturing markups and process sheets, not on the design print in case the part is outsourced in future years.

Standards are meant to simplify life throughout the value stream and help keep costs low. You're welcome to deviate to improve the design but there are many risks associated with doing so and its not something that should be done as a matter of habit or laziness or you are needlessly adding cost and risk.

 

[3DDave]

Backing out and galling and failing have little to do with clearance holes. I think those troubles can't have much to do with the class of thread, since threads are non-interfering regardless of Class over short (10 turn) engagements. Poorly made threads that probably don't meet class have problems, as do threads in incompatible materials.

If the risk is from working with a 1-sigma shop (30% fail rate) then that's an avoidable one. If forced to work with such a shop, then nothing will help. I say that as having worked with a shop of that capability. One time they broke two taps in a hole. It was tap-drilled for a 1/4-20 hole. Then they grabbed some 1/4-20STI taps. No fixing that on the drawing.

 

[JohnRBaker]

Hole clearance, or class-of-fit, is also an issue when considering the specified dimensional tolerances that are going to be applied, which is dependent on what sort of manufacturing processes are going to be utilized when creating the parts that will be fastened together.

John R. Baker, P.E. (ret)
EX-Product 'Evangelist'
Irvine, CA
Siemens PLM:
UG/NX Museum:

The secret of life is not finding someone to live with
It's finding someone you can't live without