Fanuc G68 in different planes (5 axis) on a 16M?

[Dowty123]

Does anyone know if it's possible with this control, I looked in the books but can't seem to find anything. I would like to use drilling and boring cycles even if the machine don't have the RTCP option.

 

Thanks in advance!

 

Simon

[Guest CNC Apps Guy 1]

According to the manual(pp 257 and 258 in B-63534EN_02 16i Operators Manual), Canned Cycles are not limited during Coordinate Rotation Mode (G68).

[Dowty123]

Thanks James, I can't find the book anymore (will continue searching) do you mean 'are possible' by 'are'nt limited'. Anyway, I'll give it a try direct on the machine.

 

Thanks again!

 

Simon

[Guest CNC Apps Guy 1]

From the FANUC Manual...

quote:

---

Coordinate conversion about an axis can be carried out if the center of

rotation, direction of the axis of rotation, and angular displacement are

specified. This function is very useful in three–dimensional machining

by a die–sinking machine or similar machine. For example, if a program

specifying machining on the XY plane is converted by the three–

dimensional coordinate conversion function, the identical machining can

be executed on a desired plane in three–dimensional space.

---

quote:

---

N1 G68 Xp x1 Yp y1 Zp z1 I i1 J j1 K k1 R α ;

N2 G68 Xp x2 Yp y2 Zp z2 I i2 J j2 K k2 R β ;

Three–dimensional coordinate conversion can be executed twice.

In the N1 block, specify the center, direction of the axis of rotation, and

angular displacement of the first rotation. When this block is executed,

the center of the original coordinate system is shifted to (x1, y1, z1), then

rotated around the vector (i1, j1, k1) by angular displacement α. The new

coordinate system is called X’Y’Z’. In the N2 block, specify the center,

direction of the axis of rotation, and angular displacement of the second

rotation. In the N2 block, specify coordinates and the angle with the

coordinate system formed after the N1 block in Xp, Yp, Zp, I, J, K, and

R. When the N2 block is executed, the X’Y’Z’ coordinate system is

shifted to (x2, y2, z2), then rotated around the vector (i2, j2, k2) by angular

displacement β . The newest coordinate system is called X’’Y’’Z’’. In the subsequent N3 block, coordinates in the X’’Y’’Z’’ coordinate system are

specified with Xp, Yp, and Zp. The X’’Y’’Z’’ coordinate system is called

the program coordinate system.

If (Xp, Yp, Zp) is not specified in the N2 block, (Xp, Yp, Zp) in the N1

block is assumed to be the center of the second rotation (the N1 and N2

blocks have a common center of rotation). If the coordinate system is to

be rotated only once, the N2 block need not be specified.

---

quote:

---

If one of the following format errors is detected, P/S alarm No. 5044

occurs:

1. When I, J, or K is not specified in a block with G68

(a parameter of coordinate system rotation is not specified)

2. When I, J, and K are all set to 0 in a block with G68

3. When R is not specified in a block with G68

Specify absolute coordinates with Xp, Yp, and Zp in the G68 block.

---

quote:

---

Three–dimensional coordinate conversion can be applied to a desired

combination of three axes selected out of the basic three axes (X, Y, Z) and

their parallel axes. The three–dimensional coordinate system subjected

to three–dimensional coordinate conversion is determined by axis

addresses specified in the G68 block. If Xp, Yp, or Zp is not specified,

X, Y, or Z of the basic three axes is assumed. However, if the basic three

axes are not specified in parameter 1022, P/S alarm No. 048 occurs.

In a single G68 block, both a basic axis and a parallel axis cannot be

specified. If this is attempted, P/S alarm No.047 occurs.

(Example)

When U–axis, V–axis, and W–axis are parallel to the X–axis, Y–axis, and

Z–axis respectively

G68 X_ I_ J_ K_ R_ ; XYZ coordinate system

G68 U_V_ Z_ I_ J_ K_ R_ ; UVZ coordinate system

G68 W_ I_ J_ K_ R_ ; XYW coordinate system

---

quote:

---

The following G codes can be specified in the three–dimensional

coordinate conversion mode:

G00 Positioning

G01 Linear interpolation

G02 Circular interpolation (clockwise)

G03 Circular interpolation (counterclockwise)

G04 Dwell

G10 Data setting

G17 Plane selection (XY)

G18 Plane selection (ZX)

G19 Plane selection (YZ)

G28 Reference position return

G29 Return from the reference position

G30 Return to the second, third, or fourth reference position

G40 Canceling cutter compensation

G41 Cutter compensation to the left

G42 Cutter compensation to the right

G43 Increasing tool length compensation

G44 Decreasing tool length compensation

G45 Increasing the tool offset

G46 Decreasing the tool offset

G47 Doubling the tool offset

G48 Halving the tool offset

G49 Canceling tool length compensation

G50.1 Canceling programmable mirror image

G51.1 Programmable mirror image

G53 Selecting the machine coordinate system

G65 Custom macro calling

G66 Continuous–state custom macro calling

G67 Canceling continuous–state custom macro calling

G73 Canned cycle (peck drilling cycle)

G74 Canned cycle (reverse tapping cycle)

G76 Canned cycle (fine boring cycle)

G80 Canceling a canned cycle

G81 to G89 Canned cycle

G90 Absolute mode

G91 Incremental mode

G94 Feed per minute

G95 Feed per rotation

G98 Canned cycle (return to the initial level)

G99 Canned cycle (return to the level of point R)

---

quote:

---

In the three–dimensional coordinate conversion mode, the rapid traverse

rate in drilling of a canned cycle equals the maximum cutting feedrate.

If tool length compensation, cutter compensation, or tool offset is

specified with three–dimensional coordinate conversion, compensation

is performed first, followed by three–dimensional coordinate conversion.

Three–dimensional and two–dimensional coordinate conversion use

identical G codes (G68 and G69). A G code specified with I, J, and K is

processed as the command for three–dimensional coordinate conversion.

A G code not specified with I, J, and K is processed as the command for

two–dimensional coordinate conversion.

Coordinates on the workpiece coordinate system are assigned to system

variables #5041 to #5048 (current position on each axis).

If a reset occurs during three–dimensional coordinate conversion mode,

the mode is canceled and the continuous–state G code is changed to G69.

The absolute coordinates based on the program or workpiece coordinate

system can be displayed in the three–dimensional coordinate conversion

mode. Specify a desired coordinate system in the DAK bit (bit 6 of

parameter 3106).

By specifying the rigid tapping command in three–dimensional

coordinate conversion mode, tapping can be executed in the direction of

the angle programmed by the three–dimensional coordinate conversion

command.

In three–dimensional coordinate conversion mode, ”Position Error Z”,

displayed on the spindle adjustment screen, is taken from the longitudinal

tapping axis after three–dimensional conversion.

Positioning in three–dimensional coordinate conversion mode must be

linear interpolation positioning (the LRP bit (bit 1 of parameter 1401) is

set to 1).

Three–dimensional rigid tapping cannot be executed for an axis under

simple synchronous control.

---

quote:

---

Three–dimensional coordinate conversion does not affect the degree of

manual intervention or manual handle interrupt.

Three–dimensional coordinate conversion does not affect positioning in

the machine coordinate system (e.g. specified with G28, G30, or G53).

Specify linear rapid traverse when three–dimensional coordinate

conversion is executed. (Set the LRP bit, bit 1 of parameter No.1401, to

1.)

In a block with G68 or G69, other G codes must not be specified. G68

must be specified with I, J, and K.

Programmable mirror image can be specified, but external mirror image

(mirror image by the mirror image signal or setting) cannot be specified.

Three–dimensional coordinate conversion is carried out after the

programmable mirror image function is executed.

To display the absolute position when three–dimensional coordinate

conversion is executed, set bits 4 to 7 of parameter DRL, DRC, DAL, and

DAC No.3104 to 0.

Canned cycles G41, G42, or G51.1 must be nested between G68 and G69.

G68 X100. Y100. Z100. I0. J0. K1. R45. ;

G41 D01 ;

G40 ;

G69 ;

---

quote:

---

N1 G90 X0 Y0 Z0 ; Carries out positioning to zero point H.

N2 G68 X10. Y0 Z0 I0 J1 K0 R30. ; Forms new coordinate system X’Y’Z’.

N3 G68 X0 Y–10. Z0 I0 J0 K1 R–90. ; Forms other coordinate system X’’Y’’Z’’.

The origin agrees with (0, –10, 0) in

coordinate system X’Y’Z.

N4 G90 X0 Y0 Z0 ; Carries out positioning to zero point H’’ on

coordinate system X’’Y’’Z’’.

N5 X10. Y10. Z0 ; Carries out positioning to (10, 10, 0) on

coordinate system X’’Y’’Z’’.

---

 

Hope this helps.

[MMT-USA]

Just a heads up..

 

3d Coordinate conversion (G68) is an option not to be confused with Coordinate Rotation (G68) in the same class.

 

If you do not have this option you cannot specify the axis rotations (I,J,K).

 

True 5-axis coordinate conversion is done using (G68.2/G53) TWP, allowing kinematic error to be accounted for.

[Dowty123]

Thanks a lot, I did'nt expect that much. I'll go on the machine and keep you informed. Sorry for the delay, we're pretty busy at the moment. Hope it lasts.

 

Thanks again!

 

Simon