Drilling with a right angle head on Okuma horizontal with 5th axis table

[maestro]

We have 2 Makino horizontals with 5th axis rotary tables. My post for these works perfectly for drilling and milling with a right angle head. We just purchased a new Okuma MA600 horizontal with the same 5 axis tables. We need to be able to drill with a right angle head the same way as we do on our Makinos. Okuma does not use G98, G99 in their canned drill cycles. They use G53 and G54 on the line before the line with a canned cycle to control the retract hieght. It seems that no matter what I try, I get alarms when trying to change planes and dill holes in X axis. Does anyone have an idea on what the code should look like to accomplish this. No problem on our Fanuc control machines. We do aerospace structural components and drill tons of pilot holes at lots of varying angles and in tight quarters.

[within a thou]

Isnt M53= G98 and M54=G99. I forget what the actual entire block should look like I haven't been fortunate to touch a okuma in years

[maestro]

That is correct, but it goes on the line before the line with the drilling cycle.

[YoDoug®]

You can put the M53/M54 in the line with the cycle call and on any point position line there after. M54 works like a G99 in a Fanuc. The M53 retracts to a specified point called like so

 

G71 Z0.5 ( USED FOR RETRACT PLANE - USED WITH M53/M54 )
G81 Z-0.15 R0.05 P0.237 F0.0056 M53

[maestro]

YoDoug, you are correct, but when I try this with a G19 plane change, I get alarms.

[YoDoug®]

Look in the special functions manual at the section called; Axis Name Designation. This function allows you to call a temporary rotation of the axis label. Example

 

G14 X3 Y2 Z1 ( the XYZ are the desired program code for drill cycle plane,IE XY drill points with Z drilling, The 321 are the corresponding machine axis with 1 meaning X, 2 Meaning Y, 3 Meaning Z. For reversal use a negative, example; X-3 Y2 Z1

[Greg Williams]

You need to use UVW for the plane and check the below parameter. See below from the programming manual, Section 7 - Fixed cycles

 

 

2-1. Determining the Positioning Plane and the Cycle Axis

(1) Determining the positioning plane and the cycle axis by commands

The positioning plane may be determined by selecting a plane using G17, G18, and G19. The

cycle axis is then chosen as the axis which is vertical to the selected positioning plane or the

axis parallel to it.

Xp = X- or U-axis

Yp = Y- or V-axis

Zp = Z- or W-axis

Due to the nature of the cycle axis as described above, once the positioning plane is

determined, only two axes can be selected as the cycle axis. To determine the cycle axis to be

used, specify the address of the desired axis in the block that contains a fixed cycle G code

(G73 - G89).

 

(2) Determining the positioning plane and the cycle axis by parameter

It is possible to fix the cycle axis as the Z-axis by the setting for NC optional parameter (bit) No.

17, bit 0. Accordingly the positioning plane can only be selected by designating G17 (X-Y

plane).

G Code Positioning Plane Cycle Axis

G17 Xp-Yp plane Zp

G18 Zp-Xp plane Yp

G19 Yp-Zp plane Xp

W-axis is selected as the cycle axis.

Movements in the positioning plane

 

(Wrong) G17 X__Y__

G18 X__Y__Z__W__R__F__

 

An alarm occurs since the cycle axis cannot be determined

(two possible axes, Z and W, are specified).

 

(Correct) G17 X__Y__

G18 X__Y__U__V__W__R_

[maestro]

Okuma apps guys finally got back with me. Ran this on machine and works good. Prety close to the Fanuc code on our Makino's. Changing the G71 line to an X dimension is what solved my problem.

 

N80

(.098 DRILL IN RIGHT ANGLE HEAD )

(DRILL PILOT HOLES LEG 1)

M21 (UNLOCK

M27 (UNLOCK C)

T80 M6

M51

G0 G15 H2 G90 X-12.525 Y0 C0. B0. S4000 M3

M20 (LOCK

M26 (LOCK C)

G56 H80 Z10.

G19

G71 X-12.525

G81 X-11.4 R-11.675 F5. M54

Y-1.

Z11.

Y0

G0

G130

M9

M5

G30 P1

/M60

M30