M8 tapping drill

When I was young, and knew no better, I gauged a tapping drill by holding up to the tap and picking a drill a bit bigger than the tap root.

Many of the Metric taps I mainly use have the tapping drill stamped on, and for M8 it always says 6.8 drill.

Chris Gunn

Group Captain Harry Day had a perhaps relevant quote but I don't wish to seem rude

Rod

Looking at the DIN standards the tolerance for NUT threads is 6.647 - 6.912mm.

Bearing in mind that MOST materials other than brass have some extrusion.

Interestingly there doesn't seem to be any DIN standard for threaded holes in things athat are not Nuts or threaded inserts. Yes I have searched the list of DIN standards.

Neil

It took me a few moments to find but it's very apt

I used to think that, now I'm not so sure.

The last thing I did on the threaded hole I made above was to check whether the 7.1mm drill fitted after tapping. I was expecting it to not fit, or at least be tight. Instead it went through smoothly without any problem. I wonder if modern HSS ground taps are better performance than older taps and are less prone to extrusion? After all extrusion implies that the tap is not cutting, but is pushing material out of the way.

Andrew

Neil, the whole point of what I said was that for standard applications the drill size is dictated by the DIN standard - by definition of the minor diameter D1 for external threads. If you drill it bigger the D1 dimension will no longer meet the standard. Regarding the use of the word Nut in the standard, it is there to clarify the difference between internal and external threads I think. The standard still applies to threads even if they are not in a nut or on a bolt. By that definition the standard would only apply to bolts (being threaded over a portion of it's length rather than screws with full length threads!

To add to your last post try this link **LINK** you can look at the thread class and see what changes happen. I don't know if it is accurate (it is a good idea to be careful with random information on the Internet). It should also give you an indication of the measured diameters you can expect for the thread class you have.

Rod, that seems very apt - it might also follow that another quote may be in order from Plato? (a wise man knows he knows not). At any rate, I have been saying all along that it is up to the personal preference in your own workshop. (Neil, this applies to one of your earlier posts regarding DIN standard, you can do what you like if you know what you are doing - just don't call it a DIN standard any more).

Mark

And on the subject of showing yours, here are mine....

the second picture shows the markings on the tap - and you can also see the abuse it has had! If you don't tighten the chuck enough for M8 it will slip..... especially on the mill

Mark

PS. this set was 48 quid last year - on offer in local machine factors. 7 taps and 7 drills to suit = average at 3.48 an item.... can you afford to buy cheap junk by comparison?

Edited By Mark C on 12/10/2016 17:52:49

I just looked at my tapping/drill set and the drill is 6.8mm.

That means the OP is likely in even more trouble with his cheap tap set. On another line, I am wondering if his tap ''set'' is a set of three per thread size or a box set with a single tap for each thread size. If it is the latter, they are not of much more use than thread chasing.

No, not done it yet, my tap set is a pile of *****. I have no recollection of where it came from, but it was quite a few years ago. There is one tap per size which looks to be a first tap. Most of the dies struggle with steel and tear aluminium. I am replacing them as I can! My Volker M6 taps are really rather nice.

I expect I'm not the first novice to snap up a bargain which promptly snaps!

Iain

Rod, thanks for your contribution, it certainly would help the OP to solve his problem, is there any need to be insulting?

Rough rule of thumb for Metric Coarse is to use a tapping drill (Nominal size minus thread pitch)

May be applicable to all 60 degree thread forms?

Can't claim that "To the pure, all things are pure" applies to me, so WHAT did Rod write that was insulting? Nothing that I could see, but have never heard of Harry Day, and prefer to exchange knowledge, rather than try to enter into arguments on the Forum.

Howard

Edited By Howard Lewis on 12/10/2016 19:32:55

Edited By Howard Lewis on 12/10/2016 19:33:41

Howard, problem with a simple question that acquires 5 pages of replies is that little simple tips like that (it is in my first reply - 7th post on first page) get lost!

I belive it would work with any 60 degree thread but only the metric ones are listed by pitch, all the others are in threads per inch or something similar.

I belive the quote goes along the lines of "fools follow rules without question" hence my use of the Plato quote (or Socrates?) you would need to look it up.

Mark

PS, it works for all metric as long as you have the pitch

Edited By Mark C on 12/10/2016 19:43:03

Harry Day is reputed to have said: "Rules are for the obedience of fools and the guidance of wise men"

Is it foolish to insist that the correct size drill for tapping is what is written on the tap if there is a better alternative that fits a particular situation?

I don't know. What I do know is that industrial practise is not necessarily the best approach to engineering in the home workshop.

If I have insulted you then I apologise. I do not think you are a fool and I am, clearly, not particularly wise.

I think we need to go down the pub and have a pint together

best wishes,

Rod

Edited By Roderick Jenkins on 12/10/2016 19:54:25

Mark,

I can see where you are coming from. The problem is everyone is assuming a 6.8mm drill is too small. In fact perhaps we are all right.

Kennametal say:

"Suggested Percentages of Full Thread in Tapped Holes

This is what Guhring say:

"Percentage of Thread and Tap Drill Selection:

Many variables affect the performance of threaded holes and the taps used to generate them. One very important factor is the drill size used to produce the hole that will be tapped. Most tap drill charts call out only one tap drill size, and that will produce an approximate 75 percent thread. In general, tap tool life can be increased significantly by using a lower percent of thread and we suggest using values between 60% and 70% for most applications. Thread strength is not directly proportional to percent of thread. For example a 100% thread specification is only 5% stronger than a 75% thread specification but requires 3 times the torque to produce.

Metric threads of the International Standards Organization (ISO) have the same 60-degree thread form as UN threads, though the diameters and pitches are not interchangeable. Metric tap drill charts have the same drill size problem in that they use the same formula as that employed for the obsolete AS threads. In both ISO and UN thread series, having a range of useful drill sizes allows designers and machinists to tailor effective thread depth for long holes, various materials and thread strength requirements. It also allows for the combining of inch and metric taps and drills where convenient to do so. "

Together with a useful drill size calculator: www.guhring.com/Tech/TapDrill/

So Kennametal sing the praises of 50% engagement and even Guhring's 60% is outside DIN specification.

Dormer's view is more conservative, they recommend a 6.8mm drill for M8 with the proviso that is you use one of their advanced rill bits that has less of a tendency to cut oversize, you should use a 6.9mm drill. In other words they expect a normal 6.8mm drill to make a hole at least 6.9mm in diameter...

Sandvik Coromant remind us:

Thread height in %, is the ratio between actual height and maximum height of the internal thread. The example below applies to ISO & UTS standard – 60° threads.

Example, M8x1,25
Maximum thread height according to standard is 6/8 H.
H = 0.866 x P
(H = Basic triangle height)
(P = thread pitch)

Maximum thread height is:
6/8 * (0.866 x 1, 25) = 0.811 mm
Actual thread height at a core hole of Ø6.9 mm:
(8 - 6,9) / 2 = 0.55 mm

Thread height is then (0.55 / 0.81) x 100 = 68%

I think, perhaps, we have lost sight of the fact that a 6.8 hole only provides 74% engagement, and that a 6.9mm hole is only 68% thread engagement, and closer to what most of us will get with a 6.8mm drill.

That 6.9mm hole with 68% engagement is within DIN specification.

Finally Fuller are erring on the side of caution and broken taps - they recommend a 6.75mm drill but warn that "All information is strictly informative".

Me? Now I'm fully informed I'll probably use a 7mm drill knowing that the 61% engagement will strip the external thread before it fails, with a safety margin*

Neil

*Just as well as most of use would rather replace a stripped stud than fix a stripped out hole in a workpiece.

<edited for typos>

Edited By Neil Wyatt on 12/10/2016 20:02:15

Neil, how do you arrive at "everyone" quite a few people in this thread have said 6.8 is their prefered size including me?

I had to google it too Rod. Brilliant but the thread will go on, and on, and on and........................................

A perfect world also springs to mind.

John

-

Tally Ho chaps, bandits at 9 o'clock. It might have been Douglas Bader...

Interesting calculator Neil

100% 6.4mm

90% 6.5mm

80% 6.7mm

70% 6.9mm

75% 6.8mm

Change the 8mm to 8.1mm which is what the tap is likely to be and 75% comes out at 6.9mm. 80% comes out at 6.8mm.

Add the undercut that a typical die will give and ...............

I bough some reasonable quality M8 dome head socket screws recently. Diameter 7.8mm

Drills on the other hand when I measure them are usually undersized. I only usually measure low diameter ones though up to a few mm to decide which slot to put them in. As they go in 0.1mm steps it's not unusual for some to go into slots that do not match the size that was supplied.

John

-

I agree with you Jason, perhaps we should just listen to the most vocal minority given the majority probably can't be ar......

Neil, did you notice what make my taps are along with the drill size supplied?

Mark