Haas G76 Threading problem....very puzzling.

[wrustle]

Can anyone explain to me why my first cut on this threaded part is nearly .060" deep??

Cutting an 1-3/4-6 thread. 1.750" Dia. C1144 Stressproof material.

I have checked and double checked my tool offset with the tool setter and it's good.

Yet it still takes a tremendous cut on the first pass. No clue why.....it's as if it's not even seeing the "D" value.

2014 Haas ST20

G00 G54 T1212 (1.75-6 FP THRD)
S600 M03
G00 Z0.1
G00 X1.838 M08
M24 (THREAD CHAMFERING OFF)
G76 X1.543 Z-6.43 I-0.0035 K0.051 D0.0127 F0.1667
M09
G00 G59 X0.

Best Regards,
Russ

 

[chucker]

You have a K.051 I thought K was single depth of the thread looks like your thread depth is closer to .095 You can play with the D to get the amout of passes

 

[Bluejeep]

I think K should be .108 ? 6 pitch thread depth.

 

[Bluejeep]

I think what its doing is starting at your short thread depth plus the .012 peck depth which would equal about .069 doc in the 1st pass.

 

[wrustle]

You know....I do threading on here all the time with zero issues.

Always use a full profile insert, great results.

My programs for threading are set up with templates to ease the process and remove the chance for errors, but this just isn't working. The template is below.

G0 G59 X0. Z0.
G0 G54 T1111 ( THREAD FULL PROFILE INSERT)
G0 G54 T1111 ( THREAD PARTIAL PROFILE INSERT)
S1000 M3
G0 X Z.3 M8
G76 X Z- K D F0.
(X = MINOR DIA.)
(Z = THREAD LENGTH)
(K = MAJOR DIA. MINUS PITCH DIA. DIVIDED BY TWO)
(D = 1ST CUT DEPTH = .25 TIMES K VALUE)
(F = FEED = PITCH = 1 DIVIDED BY PITCH)
G00 X Z0.3
M9
G0 G59 X0. Z0.



The part in the picture above was the setup piece, and it took several adjustments to get it dialed in after the first horrendous pass.

The next part....placed in the chuck, pressed cycle start.....and same exact thing.....HUGE first chip, tremendous scream from the machine, and chatter marks you could measure with a scale!

I set my "D" value at .003" for the first pass, and here's how deep it cut. The part is another scrap set up piece......but getting thin on those now.

1st pass with the "D" value set at .003".

 

[drewboyer]

Your K should be at least K.101". Your major diameter is around 1.745 and your minor is programmed at 1.543" which makes your total diameter difference .202" which makes the thread height at .101". You're telling it that the thread height is half of that at .051".

 

[doug925]

Wrustle,

It IS your K value. On a Haas lathe, the K value is the TOTAL height of the thread, from crest to root.
On your part, that would be a K.102
Think in terms of the K being a radial amount.
The control starts cutting at the [minor diameter + (2K) - the D value]

So....
X1.543 + .204 -.003 = X1.744 is the first pass

Right now you are using this:
X1.543 +.102 -.003 = X1.642

Doug.

 

[wrustle]

Your K should be at least K.101". Your major diameter is around 1.745 and your minor is programmed at 1.543" which makes your total diameter difference .202" which makes the thread height at .101". You're telling it that the thread height is half of that at .051".

I get what you're saying, but the Haas "K" value is a radius measure, and all our threading programs are done in that respect. This for some reason is not working.

I'm going to program it using a G92 to get the job done and give Haas applications a call in the morning.

 

[drewboyer]

wrustle should post a picture of his drawers after that first pass.

WUUUUURRRRRRRRRRAAAAAAAAGGGGGHHHHHEEEEEEEEEEKKKK!!!

 

[drewboyer]

I get what you're saying, but the Haas "K" value is a radius measure, and all our threading programs are done in that respect. This for some reason is not working.

I'm going to program it using a G92 to get the job done and give Haas applications a call in the morning.

ok, what is the radius for .202"?

 

[david n]

It's the K x3.

What Ø are you holding on to in the collet? I'm surprised it didn't spin with that first deep cut............................

 

[wrustle]

OK.....I SEE IT NOW!

What a moron I am.........my template is wrong.


It is my K value as a bunch of you have stated. I was subtracting the pitch dia. from the major diameter and dividing by two. It has never caused an issue with all the smaller threads I've done, but this one......HELLO!!!


Thanks guys!! I'll post pics and maybe some video in the morning!

To be continued...............love it!

 

[Bluejeep]

From the Hass resource center, K - Thread height, defines thread depth, radius measure, basically major dia - pitch dia. (not divided in half) wow a lot of people responded while i was typing....

 

[Atomkinder]

Thanks guys!! I'll post pics and maybe some video in the morning!

To be continued...............love it!

 

[HuFlungDung]

Reminds me of one of my favorite witticisms :

The difference between theory and practice, is that in theory there is no difference, but in practice there is.

 

[wrustle]

It's the K x3.

What Ø are you holding on to in the collet? I'm surprised it didn't spin with that first deep cut............................

It did spin Dave, but thankfully this is just a setup piece.

The small dia. is .750" and with the two undercuts on that diameter, it's not grabbing by much!

The threads did come out really nice though. I just hope the remaining 45 pcs come out like this one did.

Later,
Russ

 

[SeymourDumore]

basically major dia - pitch dia. (not divided in half) ..

Uhmm... yeah, divided in half indeed!
Dia-Dia is still dia.

 

[cnctoolcat]

Pitch diameter and minor diameter are two TOTALLY different things.
Glad you figured it out Russ!
All that g-code stuff looks like Chinese arithmetic to me...compared to sweet Mazatrol.
ToolCat

 

[angelw]

Can anyone explain to me why my first cut on this threaded part is nearly .060" deep??

Cutting an 1-3/4-6 thread. 1.750" Dia. C1144 Stressproof material.

2014 Haas ST20

G00 G54 T1212 (1.75-6 FP THRD)
S600 M03
G00 Z0.1
G00 X1.838 M08
M24 (THREAD CHAMFERING OFF)
G76 X1.543 Z-6.43 I-0.0035 K0.051 D0.0127 F0.1667
M09
G00 G59 X0.

Best Regards,
Russ

Hello Russ,
The control is doing exactly what you've requested it to do.

Based on the given OD of the thread of 1.75 and the specified Minor diameter in the G76 Block of X1.543, the K value (Thread Height - Radius Value) will be K0.1035, not K0.051.

As the OD of the Thread is calculated by the machine in the following manner:

Thread OD = X + K x 2

the Major Diameter of your Thread, as far as the control is concerned, is 1.645, not 1.75

Accordingly, the control will apply the first depth of cut, D0.0127, from an OD of 1.645. Based on those figures, your first depth of cut will be as follows:

(1.75 - 1.645) / 2 = 0.0525

First Depth of Cut = 0.0525 + 0.0127
First Depth of Cut = 0.0652

Because the depth of cut (D) is diminished by, in very rough terms and for the sake of the explanation, each successive cut being divided by 2, on threads with large Thread Heights the D address should be as large as possible. Obviously the first depth of cut can only be as great as the Tool, Workpiece and setup will handle. One strategy to have a large D value (this is the value used by the control to calculate every successive Depth of Cut), and have an Actual First Depth Of Cut that isn't going to be too great for the tool and setup, is to overstate the K value. By making the K value greater than the Actual Thread Height, the control calculates a larger Major Diameter (External Thread) than actual, and therefore, some of the larger than normal D value is taken up by fresh air and the control has a bigger D value to calculate each successive Depth of Cut.


Regards,

Bill

 

[Bluejeep]

Uhmm... yeah, divided in half indeed!
Dia-Dia is still dia.

.

I usually just use 1/2 of the double depth of thread from my little arrow head gauge, but to double check what wrustle had written in his template I looked it up in the machinery handbook. In the chart for external threads for a 1 3/4-6 thread, major dia. max = 1.7475, pitch dia. max = 1.6392 ....... subtract those 2 #'s and you get .1083... the radial thread depth ... So now I'm curious and have looked it up and found out why. The pitch dia. is the middle dia. between the theoretical thread "sharp V" top and bottom dia... so that is how a dia. - dia can give a radius... sort of