1. Plastic
Join Date
Sep 2005
Location
Iowa
Posts
19
Post Thanks / Like
Likes (Given)
0
0
Hi all:

I did a search but didn't come up with any good links.

I am looking for a thread depth chart. Not the calc of .75 divided by threads/in. I mean the actual depth of the threads or the "minor external diamension" subtracted from the "major external dimension".

I don't always cut with the compound, but just use the cross.

Thanks,

Jake

2. Diamond
Join Date
Jan 2006
Location
Houston, TX
Posts
6,087
Post Thanks / Like
Likes (Given)
565
1027
Do you have a "Machinery's Handbook" ?

Invest in one... even an OLD one...

3. Divide one by the threads per inch and then multiply by .866

1/16 = .0625

.0625 x .866 = .054 single depth of thread

If you need a chart, work the formula above for all the common threads and make your own chart.

4. Cast Iron
Join Date
Nov 2002
Location
Southern Indiana
Posts
465
Post Thanks / Like
Likes (Given)
0
1
Hi Jake,
I have a thread gage (sometimes called a fishtail)that has the double depths listed for most of the threads. If you don't have one, I suggest getting one. They're handy for grinding and setting up thread tools too.

If that isn't available, I just work from the one that I have memorized; 20 TPI = .065 double depth.

As an example, say that you want to cut 16 TPI.
20/16 = 1.25
1.25 X .065 = .081
16 TPI = .081 double depth.

Works for me anyway.

Mike

5. Aluminum
Join Date
Oct 2002
Location
Los Angeles, CA, USA
Posts
140
Post Thanks / Like
Likes (Given)
0
0
that looks like this...

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

Threads per inch [20] ? 16
Compound rest angle [29 deg] ?

{compound feed at compound angle = 29.0 deg}

(A) dot sharp crest - sharp root = 0.05413 in {0.06189 in}
(B) dot flat crest - flat root = 0.03383 in {0.03868 in}
(C) dot sharp crest - flat root = 0.04059 in {0.04641 in}
(D) dot flat crest - sharp root = 0.04736 in {0.05415 in}
(E) double dot sharp crest - sharp root = 0.10825 in

For American National (60 deg) thread form, subtract 0.0406 in from
major diameter (assumes p/8 flat on crest) to obtain pitch diameter

use any line on threading dial
----------------------------

Regards, Marv

Home Shop Freeware - Tools for People Who Build Things
http://www.myvirtualnetwork.com/mklotz

6. Diamond
Join Date
Jan 2006
Location
Houston, TX
Posts
6,087
Post Thanks / Like
Likes (Given)
565
1027
Wich one is right?.. Is EITHER RIGHT???

Divide one by the threads per inch and then multiply by .866

1/16 = .0625

.0625 x .866 = .054 single depth of thread
OR.........
As an example, say that you want to cut 16 TPI.
20/16 = 1.25
1.25 X .065 = .081
16 TPI = .081 double depth.

7. SND
Diamond
Join Date
Jan 2003
Location
Posts
10,743
Post Thanks / Like
Likes (Given)
4557
2914
Well I'll add another one in there.

I normaly use this little formula. I'm not sure exactly why its this number works. I think it takes care of the normal root and crest sizes. Anyway, simple as can be. Only 1 number to remember, .625

.625 devided by whatever TPI #

.625/16 = aprox .040" depth per side. These numbers are only meant to get you somewhere close, pretty much just like looking at it. When its getting close to a true V shape, you're almost there and should get out the 3wires/ gages, or the mating part.

I also use this formula for undercuts and I add a bit more for clearance. I never had any complaints.

8. Diamond
Join Date
Jan 2006
Location
Houston, TX
Posts
6,087
Post Thanks / Like
Likes (Given)
565
1027
So far NOBODY agrees... this is NOT funny....
but somehow I sorta expect it...

Do any of you make threads to the BOOK ?

Get a "Machinery's Handbook"

Every one of you would be royally Pi\$\$ed if the spark plugs you bought were made using your methods...

9. Plastic
Join Date
Sep 2005
Location
Iowa
Posts
19
Post Thanks / Like
Likes (Given)
0
0
So what does the Machinery Handbook say?

Jake

10. --------------------------------------------------------------------------------
Wich one is right?.. Is EITHER RIGHT???

quote:
--------------------------------------------------------------------------------
Divide one by the threads per inch and then multiply by .866

1/16 = .0625

.0625 x .866 = .054 single depth of thread

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

OR.........

quote:
--------------------------------------------------------------------------------
As an example, say that you want to cut 16 TPI.
20/16 = 1.25
1.25 X .065 = .081
16 TPI = .081 double depth.

--------------------------------------------------------------------------------
So far NOBODY agrees... this is NOT funny....
but somehow I sorta expect it...

Do any of you make threads to the BOOK ?

Get a "Machinery's Handbook"

Every one of you would be royally Pi\$\$ed if the spark plugs you bought were made using your methods...
Why don't you get your BOOK out and see which one is right?

11. Cast Iron
Join Date
Nov 2002
Location
Southern Indiana
Posts
465
Post Thanks / Like
Likes (Given)
0
1
Gary E,
By the time you have the thread data found in the handbook, The thread could already be cut! It just isn't all that technical.

I stand by my "formula". I use that because I happen to be able to remember it.

Another way to do it:
Pitch X 1.3 = double depth (Handbook worshippers will probably want to use 1.299 in place of 1.3)
These numbers are not for a pointed tool, but rather for a tool that has a proper flat at the tip. I think that this is where the descrepency comes from. The single depth of a thread with a sharp root is indeed .866 X pitch. These threads are weaker though.

Incidently, all this was derived from the "Greenfield Screw Thread Manual" which I believe is still in print.

Mike

12. Plastic
Join Date
Sep 2005
Location
Iowa
Posts
19
Post Thanks / Like
Likes (Given)
0
0
Well, I must say I have calculated each of your formulas including the DOT program and none of you are the same.

Since I don't have a handbook, what does it say?

Jake

13. SND
Diamond
Join Date
Jan 2003
Location
Posts
10,743
Post Thanks / Like
Likes (Given)
4557
2914
It says it doesn't matter how you want to calculate it as long as the end result is good.

Going with only a calculated depth without checking with 3wires or a ring gage is NOT acceptable in normal production where many parts have to interchange.

14. Aluminum
Join Date
Oct 2002
Location
Los Angeles, CA, USA
Posts
140
Post Thanks / Like
Likes (Given)
0
0
Here you go...

http://homepages.tesco.net/~A10bsa/uncpro.htm

Regards, Marv

Home Shop Freeware - Tools for People Who Build Things
http://www.myvirtualnetwork.com/mklotz

15. Aluminum
Join Date
Oct 2002
Location
Los Angeles, CA, USA
Posts
140
Post Thanks / Like
Likes (Given)
0
0
Here you go...

http://homepages.tesco.net/~A10bsa/uncpro.htm

Addendum: Note that, from the above page,

hn = 0.54127/16 = 0.033829

which agrees exactly with what my program calculates for
dot-flat crest to flat root.

Regards, Marv

Home Shop Freeware - Tools for People Who Build Things
http://www.myvirtualnetwork.com/mklotz

16. Cast Iron
Join Date
Nov 2002
Location
Southern Indiana
Posts
465
Post Thanks / Like
Likes (Given)
0
1
SND,

Good point. A formula is only good for getting you in the ballpark. Always stop feeding in a few thou shy of the calculated position and start gaging for the last bit.

17. .130 / number of threads per inch

example .130 / 12 = .01083333333

18. Plastic
Join Date
Sep 2005
Location
Iowa
Posts
19
Post Thanks / Like
Likes (Given)
0
0
JS:

That is sounding good. My fishscale says .93 for 14tpi.

so 13/14 = .92857

.92857/2 = cross slide depth

Correct?

Jake

19. Stainless
Join Date
Sep 2004
Location
south SF Bay area, California
Posts
1,917
Post Thanks / Like
Likes (Given)
108
564
Jake --

The Theoretical Single Depth of Thread for either the Unified or ISO Metric threadform -- which are both 60-degree threads with a 1/8 Pitch flat at the Major Diameter and a 1/4 Pitch flat at the Minor Diameter -- can be calculated easily from the Thread Pitch:

Theoretical Single Depth = (5/8) x Pitch x Cos (30 degrees)

Working a numerical example for a Unified threadform of 1/16 inch Pitch:

Theoretical Single Depth = (5/8) x 1/16 inch x Cos (30 degrees)

= 0.625 x 0.0625 inch x 0.866

= 0.0338 inch

Working a numerical example for an ISO Metric threadform of 1.25 millimeter Pitch:

Theoretical Single Depth = (5/8) x 1.25 millimeter x Cos (30 degrees)

= 0.625 x 1.25 millimeter x 0.866

= 0.677 millimeter

The Unified and ISO Metric threadforms are modified (truncated) V screwthreads with a 60-degree included angle between the flanks. In a 60-degree Sharp-V screwthread, the measured-along-the-flank length would be exactly equal to the Pitch. The flats at the Major and Minor Diameters on the Unified and ISO Metric threadforms result in a reduction of the measured-along-flank length to 5/8 that of a same-pitch Sharp-V screwthread. [This means that the Theoretical Along-Flank Infeed of a compound / top slide set at 30 degrees to feed along the flank can be calculated as (5/8) x Pitch, which for a Unified threadform is exactly equal to (5/8) / Number of Threads per Inch.]

The Single Depth of the screwthread is the measured-along-flank length of the screwthread times the Cosine of one-half of the V angle.

Ok, the arithmetic says you can combine the 5/8 and Cos (30 degree) factors to create a "magic number", but doing so is a BAD idea. It would be far better to learn the fundamental geometry of the Unified / ISO Metric threadform well enough that you can re-derive the equations whenever you need them.

That geometry really is pretty straight-forward, and once your understand it, the terms 5/8 and Cosine (30 degree) will come to mind far more readily and reliably than will magic numbers.

John

20. I'm the only right one here. I hardly ever calculate thread data. I cut threads until they look like a thread then gage them with the nut or male thread, mike them over wires, or thread mike them if they're in range of the thread mikes I have.

I also cut threads with the standard root flat P/4 to P/6) on the tool tip. Never cut threads with a pointy tool.

All the thread data and the NIST formulae it takes to derive it from scratch are in Machinery's Handbook.

#### Posting Permissions

• You may not post new threads
• You may not post replies
• You may not post attachments
• You may not edit your posts
•