[4]

Cutting Threads, Depth Of Cut

[3]
[10] Like what you see?
Click here to donate to this forum and upgrade your account!

RJSakowski

H-M Supporter - Gold Member
H-M Supporter - Gold Member ($25)
Joined
Feb 1, 2015
Messages
4,344
Yesterday, I had to thread some 5/16" stainless rod and did not have a chart of thread depths handy. This morning, I decided to make one based on the definition of unified National thread geometry. The external thread geometry consists of a 60o vee shape with the top of the vee truncated to a width of P/8 where P is the thread pitch and the bottom truncated with a radius which is tangent with thread at a distance of P/4 along the thread face from the bottom of the vee.

If using a threading tool ground to a sharp point and advancing the tool using the compound, the distance along the thread face from the major diameter to the bottom of the vee is P -1/8 * P = 7/8 * P = .875 * P. If the compound is set at an angle of 29.5o, the distance is slightly less or .995025 * 7/8 * P = .87065 * P.

If a tool is ground to conform to the specification (i.e., with a radius), the distance traversed by the compound will be less yet and equal to .79167 for a 30o compound angle and .78773 for a 29.5o compound angle.

The chart gives the compound distance for a 29.5o compound angle setting for cutting the standard UNC, UNF, and UNEF threads.

Bob
Note the chart was removed due to an error. A corrected chart is shown in a following post.

Thread Geometry.JPG Thread Cutting Chart.JPG
 
Last edited:

ch2co

Grumpy Old Man
H-M Supporter - Gold Member ($25)
Joined
Jan 9, 2013
Messages
985
Great layout and easy to follow graphic and table. This one will end up in the shop. Thanks

Chuck the grumpy old guy
 

RJSakowski

H-M Supporter - Gold Member
H-M Supporter - Gold Member ($25)
Joined
Feb 1, 2015
Messages
4,344
Don't want to step on your toes but here is an easy one to follow. Less complex info for newbies. I keep this hanging by my lathe.
Not a problem. It would have saved me some work. I like the incremental cut depths designed to provide uniform cutting pressure as the width of cut increases.

It appears as though there is an implied radius on the tip of the threading tool (which would be required to make a thread to spec.). A threading tool ground to a sharp point would not cut deep enough.

When threading, tool geometry and tool deflection will impact the cut thread. A thread mike, thread wires or mating part should be used to verify the final thread.

As I reviewed my original post, I noticed an error in the formula for the depth of cut for a conformal tool (the last line in the sheet). The depth of cut for a 30 degree compound angle should have been p - 1/8*p - 1/6*p =17/24*p. The corrected chart is below.

Thread Cutting Chart.JPG
 

Bamban

Active User
H-M Supporter - Gold Member ($25)
Joined
Jul 13, 2014
Messages
819
I am trying to understand the 2 charts and deciding which one to print and use for a guide, am I reading them correctly that one charts calls for 0.036 depth of cut for 24 TPI and while other 0.028?

Thank you.
 

JimDawson

Global Moderator
Staff member
H-M Platinum Supporter ($50)
Joined
Feb 8, 2014
Messages
7,939
Try both, use the one that works for you.
 

RJSakowski

H-M Supporter - Gold Member
H-M Supporter - Gold Member ($25)
Joined
Feb 1, 2015
Messages
4,344
I am trying to understand the 2 charts and deciding which one to print and use for a guide, am I reading them correctly that one charts calls for 0.036 depth of cut for 24 TPI and while other 0.028?

Thank you.
I saw a discrepancy as well. It appears that the Seko chart is intended for use with their inserts which most likely have a specific non zero radius at the tip. In use, you would touch off on the O.D. of the thread and zero your dial there. With a radius, the tool does not need to cut as deep to correctly form the thread. The mystery to me was it appears that the same Seko tool is used for all threads pitches instead of being proportional to the pitch.

It was for that reason that I suggested not plunging blindly into the threading but measuring your cut thread to determine your progress.

The drawing below shows an external 10 tpi thread drawn to specification with some dimensions. The blue line represents the threading tool, the red line is the external thread. As you can see, a conformal threading tool would not have to cut as deep to make the thread. When I grind a threading tool, I usually just slightly break the point instead of putting a specific radius. The thread is not to spec. and is not as strong as a to-spec. thread but it usually works for my purpose.

All the dimensions are proportional so a 24 tpi thread would have a .0365" depth of cut for a sharp pointed tool and a.0295" depth of cut for a conformal tool.

Since the Seko chart show a less deep cut, it is most likely "steel safe" (takes off less material rather than more). I would recommend using their numbers to start.

Bob
10 tpi Thread Geometry.JPG
 

atunguyd

Active User
Registered
Joined
Jun 9, 2014
Messages
176
RJSakowski, any chance of making up the same table for metric sizes? Or if you want please provide the excel file and I will add metric to that, it would be great to have one excel file that has all the threads needed.
 

RJSakowski

H-M Supporter - Gold Member
H-M Supporter - Gold Member ($25)
Joined
Feb 1, 2015
Messages
4,344
RJSakowski, any chance of making up the same table for metric sizes? Or if you want please provide the excel file and I will add metric to that, it would be great to have one excel file that has all the threads needed.
 

RJSakowski

H-M Supporter - Gold Member
H-M Supporter - Gold Member ($25)
Joined
Feb 1, 2015
Messages
4,344
I couldn't post the excel spreadsheet but I can send it to your e-mail. It should be a simple task to convert.

Bob
 

Bamban

Active User
H-M Supporter - Gold Member ($25)
Joined
Jul 13, 2014
Messages
819
I saw a discrepancy as well. It appears that the Seko chart is intended for use with their inserts which most likely have a specific non zero radius at the tip. In use, you would touch off on the O.D. of the thread and zero your dial there. With a radius, the tool does not need to cut as deep to correctly form the thread. The mystery to me was it appears that the same Seko tool is used for all threads pitches instead of being proportional to the pitch.

It was for that reason that I suggested not plunging blindly into the threading but measuring your cut thread to determine your progress.

The drawing below shows an external 10 tpi thread drawn to specification with some dimensions. The blue line represents the threading tool, the red line is the external thread. As you can see, a conformal threading tool would not have to cut as deep to make the thread. When I grind a threading tool, I usually just slightly break the point instead of putting a specific radius. The thread is not to spec. and is not as strong as a to-spec. thread but it usually works for my purpose.

All the dimensions are proportional so a 24 tpi thread would have a .0365" depth of cut for a sharp pointed tool and a.0295" depth of cut for a conformal tool.

Since the Seko chart show a less deep cut, it is most likely "steel safe" (takes off less material rather than more). I would recommend using their numbers to start.

Bob
View attachment 109044

Bob,

Thank you. Appreciate the work you put into this discussion, very informative to pre-kinder guys in the machining world like me.

I am using the Warner threading tool and bit, my guess they qualify for sharp pointed tool.


nez
 

chip maker

Active Member
Registered
Joined
Dec 7, 2013
Messages
138
This was a great post for the people that are confused about cutting threads ( Me Included ). The charts are easy to look at and get you were you need to be. Again a lot of good info on this site. Thanks to all who share their information with others to put into use.
 

hackley69

H-M Supporter - Gold Member
H-M Supporter - Gold Member ($25)
Joined
Feb 20, 2014
Messages
79
Great information! Thanks for posting.
 

doco

Active User
Registered
Joined
Feb 25, 2012
Messages
50
Yesterday, I had to thread some 5/16" stainless rod and did not have a chart of thread depths handy. This morning, I decided to make one based on the definition of unified National thread geometry. The external thread geometry consists of a 60o vee shape with the top of the vee truncated to a width of P/8 where P is the thread pitch and the bottom truncated with a radius which is tangent with thread at a distance of P/4 along the thread face from the bottom of the vee.

If using a threading tool ground to a sharp point and advancing the tool using the compound, the distance along the thread face from the major diameter to the bottom of the vee is P -1/8 * P = 7/8 * P = .875 * P. If the compound is set at an angle of 29.5o, the distance is slightly less or .995025 * 7/8 * P = .87065 * P.

If a tool is ground to conform to the specification (i.e., with a radius), the distance traversed by the compound will be less yet and equal to .79167 for a 30o compound angle and .78773 for a 29.5o compound angle.

The chart gives the compound distance for a 29.5o compound angle setting for cutting the standard UNC, UNF, and UNEF threads.

Bob
Note the chart was removed due to an error. A corrected chart is shown in a following post.

View attachment 108742View attachment 108743
Just curious, what percent engagement are you looking for? Machinery's Handbook gives a handy formula easily remembered, to calculate on-the-fly.

MinDiam = MaxDiam - ((1.29904*Engagement)/pitch)

EG.
1/4 20 TPI @ 75% engagement
0.250 - ((1.29904 * 0.750)/20)
0.250-0.048714=~0.201 or a #7 drill ( 13/64 would be 0.002" larger)


doco
 
[5] [7]
Top