What drill size do you use for form tapping M8?

Finegrain

Diamond

Joined

Sep 6, 2007

Location

Seattle, Washington

• Aug 22, 2021

• #1

Hi guys,

I'm looking at my tooling for M8 (standard 1.25mm pitch) form tapping, and am having some trouble deciding what drill to use. The form tap drill size chart I use says that a 65% thread needs a 7.45mm drill. That's hard-to-find metric size, and is right in between L and M letter drills. L (.290") would be ~73% thread, and M (.295") would be 60% thread.

Regards.

Mike

 

G

gregormarwick

Diamond

Joined

Feb 7, 2007

Location

Aberdeen, UK

• Aug 22, 2021

• #2

7,4 is near enough. I do lots of M8 in 17-4 and I use 7.4 most of the time.

 

Rick Finsta

Stainless

Joined

Sep 27, 2017

• Aug 23, 2021

• #3

I use 7.5mm but have used M drills in the past. Only in 6061.

 

Ox

Diamond

Joined

Aug 27, 2002

Location

Northwest Ohio

• Aug 24, 2021

• #4

Depends on the material, and maybe even the lube.

In 6061 with oil, I have ran all the way down to [max] pitch D on drills all day long in a multi-spindle screw machine.

If you are in 17-4, something a wee bit bigger may be a good idea.


-------------------

Think Snow Eh!
Ox

 

Finegrain

Diamond

Joined

Sep 6, 2007

Location

Seattle, Washington

• Aug 24, 2021

• #5

Ox said:

Depends on the material, and maybe even the lube.

Click to expand...

For now, 1018 cold rolled. Coolant is Blaser 935 soluble oil at ~10%.

Regards.

Mike

 

S

sirAIG

Aluminum

Joined

Jan 10, 2019

Location

State College

• Aug 24, 2021

• #6

FWIW Maritool chart lists m8x1.25 at a letter "M" drill. .2950"

 

Finegrain

Diamond

Joined

Sep 6, 2007

Location

Seattle, Washington

• Aug 24, 2021

• #7

sirAIG said:

FWIW Maritool chart lists m8x1.25 at a letter "M" drill. .2950"

Click to expand...

Probably because that's the nearest commonly available drill size. "M" would be slightly less than 60% thread, IF it drilled right on-size. I usually see a little oversize hole in 1018 -- if the "M" makes a .001" oversize hole, that's going to be only ~55% thread.

Regards.

Mike

 

H

Houndogforever

Hot Rolled

Joined

Oct 20, 2015

Location

Boring

• Aug 24, 2021

• #8

7.4mm is my standard for aluminum for either 5/16-24 or M8 x 1.25.

 

S

sirAIG

Aluminum

Joined

Jan 10, 2019

Location

State College

• Aug 24, 2021

• #9

Finegrain said:

Probably because that's the nearest commonly available drill size. "M" would be slightly less than 60% thread, IF it drilled right on-size. I usually see a little oversize hole in 1018 -- if the "M" makes a .001" oversize hole, that's going to be only ~55% thread.

Regards.

Mike

Click to expand...

Understood, I am not well educated in form threading at that level. What chart do you have that calculates the percentage of thread engagement? That would be handy to have!

 

S

SeymourDumore

Diamond

Joined

Aug 2, 2005

Location

CT

• Aug 24, 2021

• #10

Do you need to hit specs, or just want a functional thread?
If the former, then you're stuck with finding a size that produces the correct minor after tapping.
If the latter, then see Balax's charts: Hole Size Charts | Balax Inc.

 

Ox

Diamond

Joined

Aug 27, 2002

Location

Northwest Ohio

• Aug 24, 2021

• #11

Doo to the "M" formation of a formed thread, your 55% formed thread is not nearly as strong as a 55% cut tapped hole.

Just so's y'all understand that.


Most ref to formed threads are really ref to "rolled" threads on the OD, which are rolled up to full crest, and yes, those are stronger than cut.

But a "formed" ID thread is seldom ever near "crest", and thus has a hole in the middle..

It doesn't take much to strip out low % ID formed threads.

BTDT and I don't use form taps nearly as much as I did 20 yrs ago.


--------------------

Think Snow Eh!
Ox

 

G

gustafson

Diamond

Joined

Sep 4, 2002

Location

People's Republic

• Aug 24, 2021

• #12

Ponder what your actual hole size is.
If like me you are mowing into stuff, the hole can be slightly oversize, so on the small tapped holes I do in 6061 I use a very particular slightly undersized drill.

So if you were center drilling, peck drilling and running slow and careful, maybe an on size drill if good. IF you are blasting in 10000 holes and want to get through it, you can run couple thou under and your actual hole diameter will end up where you want it
Anyway, ponder the difference between drill size and hole size, as it matters in roll taps

 

TheBigLebowski

Aluminum

Joined

Sep 9, 2018

• Aug 24, 2021

• #13

Finegrain said:

Probably because that's the nearest commonly available drill size. "M" would be slightly less than 60% thread, IF it drilled right on-size. I usually see a little oversize hole in 1018 -- if the "M" makes a .001" oversize hole, that's going to be only ~55% thread.

Regards.

Mike

Click to expand...

Assuming that the hole drills 0.001" oversize - a 7.4 mm drill will put you within 0.001" of your target hole size erroring in the minus direction.

It looks like both McMaster and MSC carry HSS 7.4mm drills at $5ish a pop - so no worries about expensive carbide tools.

 

A

AARONT

Stainless

Joined

Feb 19, 2013

Location

Madison, WI

• Aug 24, 2021

• #14

sirAIG said:

Understood, I am not well educated in form threading at that level. What chart do you have that calculates the percentage of thread engagement? That would be handy to have!

Click to expand...

I like to use Guhring's calculator. It's treated me well. Tap Drill Calculator - GUHRING