1. ## G76 thread on Fanuc oi-t control

I need some help cutting a G76 thread on a Kia lathe
.428 x 9.17 tpi. with .312 minor dia.

Tried a G76 code but I kept getting an improper decimal point error!

2. Internal Thread Cutting Cycle Example.

(Diameter Designation, Metric Input).

NØØ9Ø.......... ;
NØ1ØØGØØ X27.9 Z5.Ø ;
NØ11ØG76 PØ4ØØ6Ø Q1ØØ RØ.Ø4 ;
NØ12ØG76 X3Ø.Ø Z-4Ø.Ø P92Ø Q2ØØ F1.5 ;
NØ13Ø.......... ;

OUTSIDE

N310 T0326
G00 X8.0 Z1.2 G97 S500 M03
X1.844
M24
G92X1.7243 Z0.5 F0.0625
X1.7103
X1.6963
X1.6843
X1.6783
X1.6763
GOTO350

The G76 command contains, within two blocks, all the information required to generate a standard thread form and pitch.
A G76 uses one edge cutting to reduce the load on the tool tip.

Show G76 Canned Cycle General Diagram.

A G76 command is written in the following format:

G76 P (A) / (B) / (C) Q (Min) R ;
G76 X(U) Z(W) P (DEP) Q (1st) F ;

where,
P (A) is the number of thread finishing passes (1 to 99).
P (B) is the chamfer amount. This is the angle at which the tool leaves the billet, at the end of the thread cutting cycle.
P (C) is the angle of the tool tip (8Ø°, 6Ø°, 55°, 3Ø°, 29° and Ø°). Note - (A), (B) and (C) are all specified at the same time by the address P, eg, PØ36Ø6Ø = number of cuts is Ø3, chamfer amount of 6Ø and tool angle of 6Ø°.
Q (Min) is the minimum cutting depth (in microns). When the depth of the cut calculated by the CNC control becomes less than this limit, the cutting depth is clamped at this minimum value.
R is the finishing allowance. This is the final, or finishing, cuts applied to the thread. The number of stages to complete this finishing allowance is determined by the value of P(A), ie, the value of R divided by the P(A) number of finishing passes equals the value of each finishing allowance stage.
X(U) is the end position of the thread in the X axis (the core diameter).
Z(W) is the end position of the thread in the Z axis.
P (DEP) is the depth of the thread as a radius value (in microns).
Q (1st) is the depth of the first pass as a radius value (in microns).
F is the size of the thread pitch.

3. G76 General Notes Page.

Note 1.
When incremental dimensions are used, their signs (+ or -) are defined as follows :

U and W = Plus/Minus (determined by the direction of the tool path).
R = Plus/Minus (determined by the direction of the tool path).
P = Plus (always).
Q = Plus (always).

Note 2.
Four symmetrical patterns can be considered depending on the sign (plus or minus) of the X and Z axis movements.

Note 3.
It is possible to cut internal threads with the G76 command.

Note 4.
Thread cutting is repeated along the same tool path from rough cutting through to the final finishing cut, so the spindle speed must remain constant. The G96 command for constant surface speed must not be used when the thread cutting cycle is active, otherwise the pitch of thread could be incorrectly machined.

Note 5.
When possible, allow a 5mm run-in at the start of the thread pass, to allow for any lag in the machine drive system, etc.... Without a sufficient run-in the start of the thread could be machined with an incorrect pitch.

Note 6.
The feedrate override on the CNC control panel will be ineffective, ie, it is set at a fixed value of 1ØØ% during the entire thread cutting cycle.

Note 7.
Although the spindle override feature is not disabled whilst a thread is being cut, it should not be activated since an incorrect thread pitch will be generated.

Note 8.
The cycle stop key will not operate during a thread cutting cycle. The thread cutting operation can only be stopped using either the [RESET] key on the CNC controller panel or [EMERGENCY STOP] button.

Note 9.
The machine can be set to read one block at a time by pressing the [SINGLE BLOCK] key on the CNC controller panel. When operating in single block mode, one press of the [CYCLE START] key will activate one complete threading pass (cut on, thread pass, cut off and rapid back). If single block mode is activated during a threading operation, the tool motion will stop at the beginning (cut on) of the next complete threading pass.

4. G92 General Notes Page.

Note 1.
G92 can be used to cut both internal and external threads.

Note 2.
Plunge cutting is used with G92 to generate a thread, from the first pass to the last finishing pass.
Plunge cutting involves the tool approaching the billet at 9Ø degrees to its surface, rather than approaching the billet at a run-in angle. Effectively, this means greater stresses are placed on the tool since both edges will be cutting. As the tool cuts further into the material, more surface area is in contact with the tool tip.

Note 3.
The same notes on thread cutting in G76 regarding speed, run-in, feed hold etc. are also relevant to G92.

5. Why not post your code here so we can see it?

6. Personally I stick with G92 for Threading. It allows for more control

7. Originally Posted by dcoupar
Why not post your code here so we can see it?
+1 for Mr. Coupar. Kind of hard to trouble shoot a canned cycle without seeing your code. Then we could tell you exactly what is wrong without having to explain the meaning of every value in the cycle.

8. Tried the g76 on the Kia with no decimals in P and Q and it worked well! Thanks Ski-doo. I'll try to post the code tom. Still got a few bugs in.

9. I work with six YUNDAI-KIA machine
SKT300
SKT300-MS
SKT460