**Fanuc**

**programming that hopefully we give an even clearer picture of the uses and commands for these cycles.**

*( and therefore Haas )*

*We do have some Okuma Programming Notes at the bottom of this post.*The examples will use the same shape ... but will illustrate the to main Fanuc cycles for bar stock roughing ... G71 -Turning and G72 - Facing.

G71 will produce a cutting motion along the Z axis ... generally referred to as a turning motion. The G72 cycle will produce a cutting motion along the X axis ... or a facing type motion.

The way we position our Points A - B - C will also determine the motion as illustrated below. The general rule of thumb is to describe the cutting motion through the finish contour code in a motion that moves from A to B along the contour to C. This description will assist you in placing Points A - B - C in their correct location in relation to the part and the contour.

___________________________________________________________

**Example #1 :**

**OD Cutting Along the Z axis - Turning**

(1) First we established our points A - B - C and using a clearance amount of .100 in X and .050 in Z.

(2) In our program ... the first step is to rapid to point A ... N1000 = our P call in the canned cycle block.

(3) Then command the Canned Cycle Call

(4) Then rapid to point B and proceed around the part contour to point C ... N1100 = our Q call in the canned cycle block.

G96S650M03

G00X11.0Z1.0M08

G00X10.3408Z0.05

G71P1000Q1100U0.01W0.01D0.1F0.012

N1000G00X4.8729.0Z0.05

G01X4.8729.0Z0.0F0.012

G01X4.8729Z-1.2967F0.012

G01X6.9769Z-1.998F0.012

G01X6.9769Z-3.4277F0.012

G01X10.2409Z-3.4277F0.012

N1100G00X10.3408Z-3.4277

G00X10.3408Z0.05

___________________________________________________________

**Example #2 :**

**OD Cutting Along the X Axis - Facing**

By re-arranging Points A - B - C ... and using the G72 cycle ... we can change the cutting direction from turning to facing. The basics of the format and steps in the program are the same ... move from A to B along the contour to C ... and this will help us position Points A - B - C.

G96S650M03

G00X10.1000Z1.0M08

G00X10.3408Z0.05

G72P2000Q2100U0.01W0.01D0.1F0.012

N2000G00X10.3408Z-3.4277

G01X10.2408Z-3.4277F0.012

G01X6.9769Z-3.4277F0.012

G01X6.9769Z-1.998F0.012

G01X4.8729Z-1.2967F0.012

G01X4.8729Z0.0F0.012

N2100G00X4.8729Z0.05

G00X10.34Z0.05

___________________________________________________________

**Example #3 :**

**ID Rough Cutting Along the Z Axis Turning**

Now let's turn things to focus on ID cutting. Again ... the same procedures and rules apply ... flip Points A - B - C to reflect cutting the ID rather than the OD. The same rule applies ... move from A to B along the contour to C.

G96S650M03

G00X.9717Z1.0M08

G00X0.9717Z0.05

G71P1000Q1100U-0.01W0.01D0.05F0.012

N1000G00X2.7117Z0.05

G01X2.7117Z0.0F0.012

G01X2.7117Z-0.8633F0.012

G01X1.7622Z-1.6563F0.012

G01X1.0717Z-1.6563F0.012

N1100G00X0.9717Z-1.6563

G00X0.9717Z0.05

___________________________________________________________

**Example #4 :**

**ID Rough Cutting Along the X Axis - Facing**

And again ... by re-positioning Points A - B - C and using G72 ... we can perform the rough cutting using cutting from the centerline out in a facing motion.

G96S650M03

G00X1.0Z1.0M08

G00X0.9617Z0.05

G72P2000Q2100U-0.01W0.01D0.05F0.012

N2000G00X0.9617Z-1.6563

G01X1.0717Z-1.6563F0.012

G01X1.7622Z-1.6563F0.012

G01X2.7117Z-0.8633F0.012

G01X2.7117Z0.0F0.012

N2100G00X2.7117Z0.05

G00X0.9617Z0.05

___________________________________________________________

**Okuma Programming Notes :**

Okuma OSP controls refer to the cycles as illustrated above as LAP cycles. The format and use is pretty basically the same as described for Fanuc / Haas controls with some modifications. If you can understand the outlines above ... the notes below should get you through the differences between the Fanuc / Haas format and that required by OSP controls.

- For motion for both turning and facing ... command a G85 as the canned cycle command. The variables in the G85 line are outlined in Part 1 of this series.
- On the line immediately following the G85 call ... command a G81 for turning or G82 for facing. This G code should appear on a line by itself with no other code on the line.
- The N number command on the G85 line should refer to the N number of the line where the G81 / G82 is commanded.
- At the end of the sequence that describes the finish contour ... command a G80 on a line by itself to signify the end of the finish profile sequence.

The Fanuc / Haas code from example #1 above has been transposed for the Okuma OSP format below :

G96S650M03

G00X11.0Z1.0M08

G00X10.3408Z0.05

G85 N1000 U0.01 W0.01 D0.1 F0.012

N1000 G81

G00X4.8729.0Z0.05

G01X4.8729.0Z0.0F0.012

G01X4.8729Z-1.2967F0.012

G01X6.9769Z-1.998F0.012

G01X6.9769Z-3.4277F0.012

G01X10.2409Z-3.4277F0.012

G00X10.3408Z-3.4277

G80

G00X10.3408Z0.05

___________________________________________________________

They say a picture is worth a thousand words ... hopefully the illustrations here will help you solidify your programming of these powerful and important canned cycles.

If anyone notices any errors in this post ... please leave a Comment below and straighten it out ... to benefit anyone stopping by ... and Thanks in advance.

*Happy Chip Making in 2013 !!*

*Check out our*__Real World World__machine shop software at www.KentechInc.com
Conversational CAD/CAM

Quoting & Estimating

G Code Conversion

CNC Training

.... and MORE !!!