Guide for odd threads

[Johnny Larue]

so you gotta make those .391 X 27 odd threads in machinist handbook...but maybe customer says I like .393 X 32 threads instead....NO PROBLEMO....heres a quick tip for dialing em in....I had a nut supplied by customer but no gauge for this....or sometimes you have to match one piece to another. whatever. so ya do the G76 thing but your missing some info...so a general rule of thumb is this....use the numbers of nearest thread...in this case its the .391 X 27.....so you use the minor diameter of the 27's which is .343....and you need the P which is single depth of thread...and SAVE THIS you'll use it a lot...you take .61343 / threads per inch = single depth of thread...which is .61343 / 32 = .01916and this figure...you take half of that and add to the X offset POSITIVE which is .009....so that you can come down to tight size if needed...leaving it ZERO might undercut the threads since you used nearest threads numbers if they are smaller....I used a NTK2 top notch profiling carbide tip since they are tiny threads....so with that in mind you would program and figure it this way...also I was cutting 303 SS which is kinda hard...now a lot will disagree but try this also...I ALWAYS run 100RPM's....theres a reason why but its complicated...the only time I vary this is if huge force is needed....like a 3 inch X 4 threads per in SS...then I had to run like 300...all tapping on a mill or threading on a lathe is GENERALLY LEFT AT 100RPM's....theres exceptions of course for all the captain obviouslies including plastics (word police disclaimer here) ...if you want to know why I will tell you...but in another thread...make these and ye shall see...use 100...see how nice they are...use any material...see how nice they are...nuff said...turned the boss to .385 for threads by .35 long....this way can be used for many threads...and of course it can be modified...but try it my way first and with these tiny cuts....it will only take a minute longer but you will see no burrs or not much...I do rub it with like 400 wet or dry or stone off tops of threads and make pretty...don't alter the RPMs until you actually try it...once I explain to you why you'll have a machining revolutional moment...and might give yourself a..... DOH....ENJOY

M98 P999 (SAFE RETRACT)
G04 T303 (DWELL AND CHANGE TOOL AT SAFE RETRACT)
S100 M13
G00 X.42 Z.5 (Z IS GENERALLY LEFT AT .5 POSITIVE OR 3 THREADS FOR CONTROL TO CATCH UP INCASE YOU USE THIS FOR PLUG AND PLAY AND DO BIG THREADS AND FORGET)
G76 P020029 Q00200 R.0003
G76 X.343 Z-.348 P01916 Q00150 F.03125
G00 Z.5
M98 P999
M30



1st G76 line is 02 finish passes pull straight out and compound infeed at 29 degrees
Q is first pass
R is stock left for finish pass per side

2nd G76 line P is single depth of thread and is ALWAYS POSITIVE
Q depth for each pass
F threads per inch.....1 divided by 32 in this case

 

[doug925]

Or..... You pick up a copy of ME Thread Pal for $100, and you will have the ~exact~ thread data for ANY imaginable thread you can come up with.

In the case of a Ø.393 - 27...


Doug.

 

[Johnny Larue]

Or..... You pick up a copy of ME Thread Pal for $100, and you will have the ~exact~ thread data for ANY imaginable thread you can come up with.

In the case of a Ø.393 - 27...

View attachment 178195
Doug.

yes...but what if your apprentice with no money yet? or you don't have internet access or a computer near by....and this is good for beginners to learn also since the chart doesn't tell you to add to the X offset....as always...most of us know the ordinary way...so this is another tip

PS...look at that chart...the minor diameter has a wide range...if your new at threading a lot of guys would wonder what number they use...love the avatar BTW...stella fo me my friendski

side note...I see you use PURIFORMS DEFRAGGLER...and CCLEANER....wise choice...but spybot is not needed any more unless you like to run just that....I would suggest AVAST instead...PURIFORM also makes RECUVA which is excellent....I know you know your stuff just by several program icons....LOL

also the repair techs use FILEHIPPO.com for all program downloads...no bloatware...if you take your machine to geek squad they go to filehippo and use ccleaner and malwarebytes and others that are free and then charge you 150.....DOH...dats gonna leave a mark

 

[Booze Daily]

Doubt many apprentices are programming CNC lathes.

100 rpm? I don't even tap that slow.

 

[angelw]

M98 P999 (SAFE RETRACT)
G04 T303 (DWELL AND CHANGE TOOL AT SAFE RETRACT)
S100 M13
G00 X.42 Z.5 (Z IS GENERALLY LEFT AT .5 POSITIVE OR 3 THREADS FOR CONTROL TO CATCH UP INCASE YOU USE THIS FOR PLUG AND PLAY AND DO BIG THREADS AND FORGET)
G76 P020029 Q00200 R.0003
G76 X.343 Z-.348 P01916 Q00150 F.03125
G00 Z.5
M98 P999
M30

1st G76 line is 02 finish passes pull straight out and compound infeed at 29 degrees
Q is first pass
R is stock left for finish pass per side

As pointed out to you in another Thread, if you specify 29 as the angle with the P address of the first G76 Block, the in-feed will be a compound in-feed of 14.5degs from perpendicular to the Thread axis, not 29deg.

Q is the clamp value for Minimum DOC, not first pass DOC

2nd G76 line P is single depth of thread and is ALWAYS POSITIVE
Q depth for each pass
F threads per inch.....1 divided by 32 in this case

Q is the DOC for the First Thread Pass and the value used as a constant in the calculation for successive DOCs, not the DOC for each pass. However, as the First Pass DOC in your second G76 Block example is smaller than the Minimum DOC specified in the First G76 Block, all passes will be made at the Minimum DOC specified in the First G76 Block. Not a clever use of the G76 Cycle.

 

[yardbird]

so you gotta make those .391 X 27 odd threads in machinist handbook...but maybe customer says I like .393 X 32 threads instead....NO PROBLEMO....heres a quick tip for dialing em in....I had a nut supplied by customer but no gauge for this....or sometimes you have to match one piece to another. whatever. so ya do the G76 thing but your missing some info...so a general rule of thumb is this....use the numbers of nearest thread...in this case its the .391 X 27.....so you use the minor diameter of the 27's which is .343....and you need the P which is single depth of thread...and SAVE THIS you'll use it a lot...you take .61343 / threads per inch = single depth of thread...which is .61343 / 32 = .01916and this figure...you take half of that and add to the X offset POSITIVE which is .009....so that you can come down to tight size if needed...leaving it ZERO might undercut the threads since you used nearest threads numbers if they are smaller....I used a NTK2 top notch profiling carbide tip since they are tiny threads....so with that in mind you would program and figure it this way...also I was cutting 303 SS which is kinda hard...now a lot will disagree but try this also...I ALWAYS run 100RPM's....theres a reason why but its complicated...the only time I vary this is if huge force is needed....like a 3 inch X 4 threads per in SS...then I had to run like 300...all tapping on a mill or threading on a lathe is GENERALLY LEFT AT 100RPM's....theres exceptions of course for all the captain obviouslies including plastics (word police disclaimer here) ...if you want to know why I will tell you...but in another thread...make these and ye shall see...use 100...see how nice they are...use any material...see how nice they are...nuff said...turned the boss to .385 for threads by .35 long....this way can be used for many threads...and of course it can be modified...but try it my way first and with these tiny cuts....it will only take a minute longer but you will see no burrs or not much...I do rub it with like 400 wet or dry or stone off tops of threads and make pretty...don't alter the RPMs until you actually try it...once I explain to you why you'll have a machining revolutional moment...and might give yourself a..... DOH....ENJOY

M98 P999 (SAFE RETRACT)
G04 T303 (DWELL AND CHANGE TOOL AT SAFE RETRACT)
S100 M13
G00 X.42 Z.5 (Z IS GENERALLY LEFT AT .5 POSITIVE OR 3 THREADS FOR CONTROL TO CATCH UP INCASE YOU USE THIS FOR PLUG AND PLAY AND DO BIG THREADS AND FORGET)
G76 P020029 Q00200 R.0003
G76 X.343 Z-.348 P01916 Q00150 F.03125
G00 Z.5
M98 P999
M30



1st G76 line is 02 finish passes pull straight out and compound infeed at 29 degrees
Q is first pass
R is stock left for finish pass per side

2nd G76 line P is single depth of thread and is ALWAYS POSITIVE
Q depth for each pass
F threads per inch.....1 divided by 32 in this case

"if you want to know why I will tell you...but in another thread."

Thanks Johnny! I would greatly appreciate that.

Brent

 

[litlerob1]

"if you want to know why i will tell you...but in another thread."

thanks johnny! I would greatly appreciate that.

Brent

hahaha lmfao

 

[Johnny Larue]

As pointed out to you in another Thread, if you specify 29 as the angle with the P address of the first G76 Block, the in-feed will be a compound in-feed of 14.5degs from perpendicular to the Thread axis, not 29deg.

Q is the clamp value for Minimum DOC, not first pass DOC



Q is the DOC for the First Thread Pass and the value used as a constant in the calculation for successive DOCs, not the DOC for each pass. However, as the First Pass DOC in your second G76 Block example is smaller than the Minimum DOC specified in the First G76 Block, all passes will be made at the Minimum DOC specified in the First G76 Block. Not a clever use of the G76 Cycle.

angleW...I really hate to break this to you but you've been wrong on this...and I will let you and your sidekicks above read it for the class so they learnt someting...otay...first...and these will all be STRAIGHT FROM THE BOOK seeing as how you wouldnt believe me if I told ya....so if you learn something WHEN I show you been wrong....then try to not be a Debbie downer on stuff and addressing me after this otay? Use SIR

read this section and remember what you say about the 14.5 degrees....I'm pretty sure it might come to you....the others...not so much....LOL...now take SPECIAL CARE when reading the word NOTE and that line in it...then remember back into that slope and bring that 14 back up front again...LOL....then we will go to page 2...tell me if ya notice anything important...LMAO...well get to Q next

 

[Johnny Larue]

now for the Q and the word P and all the angles you can do...I want you all to focus now....on each angle you can input....over here...theres no squirrels....focus

PS...wrap your slopes around that 14.5 degrees that's actually means a 29 degree included thread tool...and those other numbers that you say we should use....like the 60...that's like 30 right...lets go back to the note again class...for the 4 stooges shall we...hey this is fun...gotta run until tommorrys next lesson BOYS...later...larue

 

[Johnny Larue]

o oh.....do you hear someting

 

[Booze Daily]

Don't know what book that is, but EVERY lathe I've ever used the programmed infeed angle is the included angle of the thread form.
ie 29 for acme, 55 whitworth, 60 vee,etc.

 

[JNieman]

Don't know what book that is, but EVERY lathe I've ever used the programmed infeed angle is the included angle of the thread form.
ie 29 for acme, 55 whitworth, 60 vee,etc.

Ditto.


(Except HAAS... had their own 'simplified' P settings)

 

[Vancbiker]

So if the thread you described in the first post corresponds to Figure 7.8 and the sample program in one of the pictures you posted, you meant to be cutting a 29 degree included angle thread form?

 

[implmex]

Johnny Larue, i hate to break it to you but I've got the REAL Fanuc book (the one written in Japlish) open at page 146 and ....You're Wrong!!
The book clearly shows the commanded angle as the INCLUDED angle of the tool tip, so 60 for a 60 degree vee thread.

Notice please, in the example from your own book that the 55 degree Whitworth thread is programmed Pxxxx55 on the first G76 line.
So: Pxxxx55 for a 55 degree included angle thread....Pxxxx60 for a 60 degree included angle thread.

Angelw is correct...you owe him one.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
www.vancouverwireedm.com
Clarus Microtech Inc. | Facebook

 

[gregormarwick]

Don't know what book that is, but EVERY lathe I've ever used the programmed infeed angle is the included angle of the thread form.
ie 29 for acme, 55 whitworth, 60 vee,etc.

Ditto.


(Except HAAS... had their own 'simplified' P settings)

You can add Anilam and Gildemeister EPL (maybe heidenhain too?) to that list.

However, every Fanuc ever, including Johnny's (lol,lmao, etc.), uses the final included angle of the thread form.

Notice please, in the example from your own book that the 55 degree Whitworth thread is programmed Pxxxx55 on the first G76 line.
So: Pxxxx55 for a 55 degree included angle thread....Pxxxx60 for a 60 degree included angle thread.

What Johnny Genius is too stupid to realise is that his book confirms everything that the rest of us already know. Note, "tool nose angle" very specifically printed below his grubby digit.

But because the final outcome will be the same in any case, and because he runs so sloooowly with a stupid tiny DOC, he couldn't possibly tell the difference.

 

[yardbird]

later...larue

View attachment 178272

Notice the rpm in the program example posted.

Brent

 

[TeachMePlease]

If we all pitched in, we could buy this guy a keyboard with punctuation that works.


Don't think any of us make enough to buy him a clue.

 

[angelw]

angleW...I really hate to break this to you but you've been wrong on this...and I will let you and your sidekicks above read it for the class so they learnt someting...otay...first...and these will all be STRAIGHT FROM THE BOOK seeing as how you wouldnt believe me if I told ya....so if you learn something WHEN I show you been wrong....then try to not be a Debbie downer on stuff and addressing me after this otay? Use SIR

read this section and remember what you say about the 14.5 degrees....I'm pretty sure it might come to you....the others...not so much....LOL...now take SPECIAL CARE when reading the word NOTE and that line in it...then remember back into that slope and bring that 14 back up front again...LOL....then we will go to page 2...tell me if ya notice anything important...LMAO...well get to Q next

View attachment 178269 View attachment 178270

Gosh, what can I say. Oh, I know. You're not often right but you're wrong this time; again!
The sad thing is that you're such a cretin that you don't realize that the note in the pages you Posted do nothing to support your erroneous understanding of the G76 Cycle.

Following is a Cut and Paste form a Fanuc digital manual.

G76P (m) (r) (a) Q (Δd min) R(d);
G76X (u) _ Z(W) _ R(i) P(k) Q(Δd) F(L) ;

m = Repetitive count in finishing (1 to 99)
This designation is modal and is not changed until the other value is
designated. Also this value can be specified by the parameter No.
5142, and the parameter is changed by the program command.

r = Chamfering amount
When the thread lead is expressed by L, the value of L can be set from
0.0L to 9.9L in 0.1L increment (2–digit number from 00 to 90).
This designation is modal and is not changed until the other value is
designated. Also this value can be specified by the parameter No.
5130, and the parameter is changed by the program command.

a = Angle of tool tip
One of six kinds of angle, 80°, 60°, 55°, 30°, 29°, and 0°, can be selected,
and specified by 2–digit number.
This designation is modal and is not changed until the other value is
designated. Also this value can be specified by the parameter No.
5143, and the parameter is changed by the program command.

(Example)
When m=2, r=1.2L, a=60°, specify as shown below (L is lead of thread).
Pm r a
P02 12 60

Δdmin = Minimum cutting depth (specified by the radius value)
When the cutting depth of one cycle operation (Δd –Δd –1) becomes
smaller than this limit, the cutting depth is clamped at this value. This
designation is modal and is not changed until the other value is
designated. Also this value can be specified by parameter No.
5140, and the parameter is changed by the program command.

d = Finishing allowance
This designation is modal and is not changed until the other value
is designated. Also this value can be specified by parameter No.
5141, and the parameter is changed by the program command.

i = Difference of thread radius If i = 0, ordinary straight thread cutting
can be made.

k = Height of thread
This value is specified by the radius value.

Δd = Depth of cut in 1st cut (radius value)

L : Lead of thread (same as G32).

 

[angelw]

now for the Q and the word P and all the angles you can do...I want you all to focus now....on each angle you can input....over here...theres no squirrels....focus

PS...wrap your slopes around that 14.5 degrees that's actually means a 29 degree included thread tool...and those other numbers that you say we should use....like the 60...that's like 30 right...lets go back to the note again class...for the 4 stooges shall we...hey this is fun...gotta run until tommorrys next lesson BOYS...later...larue

From your own example pictures Johnny. See your pictures below where I have taken the liberty of outlining the data that is relevant to the discussion, so that you might gain an understanding.



Do these examples mean that you're wrong again? Heavens.

You really need to take a breath and actually learn something about the subject before you preach about it.

I suspect that Reading Comprehension 101 is an available education stream still. That may help!

Warning to Newbies
1. Read Johnny's Posts
2. Disregard the content completely
3. Seek information on same subject Posted by Forum Members that actually know something of the subject.
or,
4. Read relevant sections of manual relating to the subject.

 

[angelw]

Notice the rpm in the program example posted.

Brent

Hello Brent,
I suspect that some unscrupulous carbide sales guy has indoctrinated Johnny with the tip destroying cutting data Johnny preaches, to boost his sales. Heck, even a Newbie 5 minutes in would have learned that excessively slow surface speed results in Edge Build Up and accelerated Edge Chipping. Surely one wouldn't use such cutting data out of free choice.


Regards,

Bill