Thread: Fanuc 10T

Could someone show me a Fanuc 10T thread canned cycle. I am working on a post and needed some information about the cycle and it's format.

Al

Originally Posted by aldepoalo

Could someone show me a Fanuc 10T thread canned cycle. I am working on a post and needed some information about the cycle and it's format.

Al

There are a number of threading cycles available, but the most popular is the Multi Repetative G76 cycle. The Fanuc Series 10 control uses the single line format, now deemed Series 15 format and can be set via parameter on late model controls.

The G76 format is as follows:

G76 X.... Z.... I.....K.....D.....A.....P.....F.....Q(?)

Where
X = Minor Diameter when cutting external thread, Major Diameter when cutting internal thread
Z = Finish coordinate of thread in Z axis
I = Taper amount, this can be omitted if a parallel thread
K = Height of thread, radius value
D = Depth of cut for the first threading pass
A = Included angle of thread form, or angle of tool nose, from 0 to 120 deg in 1 deg steps; the default is zero
P = Cutting method (Both edge threading with constant cutting amount by default, or for P0)
P1:One edge threading with constant cutting amount
P2:Both edge zigzag threading with constant cutting amount
P3:One edge threading with contant depth of cut
P4:Both edge threading with constant depth of cut

F = Lead of thread

Q = Thread start angle shift, from 0 to 360 degrees in steps of 0.001 degrees. This was available on some 10T controls, but not all. It was for use in cutting multi start threads. Cutting multi start threads can be cut without this feature by changing the Z start position by the pitch of the thread (Thread Lead divided by Number of Starts).

Regards,

Bill

Real good example, Angel.
All of the Canned Cyles on the 10T, the 6T and also the 15T are similar, they each have one line, are easy to learn and use.
I have several examples on my website, if you want to learn from them, look at
www.doccnc.com
Good job, Angel.

Thank you so much!

That was just what I was looking for.

Al

When I run the cycle I have a problem.

The tool his not going to clearance from pass to pass. so what ends up happening is the tool is dragging across the threads and it comes back to the start posting to make the next pass.

1) There is no retract value in the code so is the retract defined on the controller somewhere?

2) How does the start position effect the retract?

I am thinking this issue has something to do with my start position, I am just not sure what I am doing wrong.

Is this the code I wrote:

%
O0001
(JOB 5 THREAD CYCLE )
(TOOL #12 60 DEG. 1/8 0.003 RAD THREADING )
G80 G40 G54
T1212
M41
G50 S500
G97 S500 M03
M08
G00 X.725 Z.1734
G01 X.625 F.0909
G76 X.5266 Z-.605 I0. K0492 D0030 A60 P1 F.090909
M09
G00 X10.
G00 Z5.
G97
M01
M09
M05
M30
%

take out that G1 line right before the G76 line!!!

Yup that's what is was. It's working now.

Thank You

Al

Originally Posted by aldepoalo

When I run the cycle I have a problem.

The tool his not going to clearance from pass to pass. so what ends up happening is the tool is dragging across the threads and it comes back to the start posting to make the next pass.

1) There is no retract value in the code so is the retract defined on the controller somewhere?

2) How does the start position effect the retract?

I am thinking this issue has something to do with my start position, I am just not sure what I am doing wrong.

Is this the code I wrote:

%
O0001
(JOB 5 THREAD CYCLE )
(TOOL #12 60 DEG. 1/8 0.003 RAD THREADING )
G80 G40 G54
T1212
M41
G50 S500
G97 S500 M03
M08
G00 X.725 Z.1734
G01 X.625 F.0909
G76 X.5266 Z-.605 I0. K0492 D0030 A60 P1 F.090909
M09
G00 X10.
G00 Z5.
G97
M01
M09
M05
M30
%

Further to allen3944's suggestion, and by way of an explantaion, following is how the control deals with the G76 cycle:

Practically it does matter, but theoretically it doesn't matter how large an X coordinate (for a male thread) the tool starts from. In software, the control takes the X (minor diameter) value passed in the G76 cycle and adds K x 2 to determine where the major diameter of the thread is. D x 2 is then subtracted from this value to establish the X coordinate for the first threading pass. Accordingly, any X value greater than Xi + 2K (Xi being the X value passed in the G76 cycle) will give a retract that will clear the top of the thread. Obviously don't make it to close, give the tool some room to pass safely past the top of the thread when returning to the Z start point.

In your code listing, I note that the first depth of cut is only 0.003 (D0030). When using P1 mode, the depth of cut will progeressively become less to maintain the constant cutting amount, down to a minimum depth of cut that is clamped via a parameter setting. I would be surprised if the value set in the parameter is this small. You may like to look this parameter up and check the value set. Basically, the depth for the first pass should be as large as practical, as it has a direct bearing on the total number of passes to complete the thread. Also, the K value can be written with a decimal point.

Regards,

Bill