G78-threading cycle help please

[CHANDRU]

Friends,

Recently after commissioning a cnc with oi-TC controller we had G78 Threading cycle problem.

While machining after few passes the spindle was stopping and the tips were breaking.Later we found that there was some G-CODE missing in the program like G90,G53 and G97.

Following is the G78 threading cycle program.

Any mistake pl identify them.

G90 G53 T0505:
G97 S500 M04:
G0 X135.0 Z20.0:
G0 Z5.0 M07:
G01 Z20.0 F1.0:
G78 X132.6 Z-25.0 F4.233:
X132.4:
X132.2:
X132.0:
X131.8:
X131.6:
X131.4:
X131.2:
X131.0:
X130.8:
X130.6:
X130.4:
X130.2:
X130.0:
LIKE THAT
UP TO X128
AND FROM X128.0
X127.95:
X127.9:
X127.85:
X127.8:
X127.767:
G0 Z20.0 M09:
T0000
G0 X0 Z110.0 M05:
M01:

Similarly while doing internal threading cycle with g78 after few passes the tool is digging.

IAM NOT FAMILIAR WITH PROGRAMMING SO PL HELP ME.

Thanks

CHANDRU

[YBMach]

Hello Chandru,

For the O-T model of fanuc, you need to use G76 for a canned threading cycle. If you want to do it line by line, use G92 or G32 code. Second, do not use G53. This is a work offset. Unless you are using the same tool on different chuck, I would recommend never to use G52 to G59 on a lathe.

Hope it helps.

YBMach

[sml]

Hi
Please check this cycle for threading
and use G54 and don't use G90. I hope that is work good.

G76 P(m)(r)(a) Q(△dmin) R(d)
G76 X(u) Z(w) R(i) P(k) Q(△d) F(L)

m: Number of replication for finish maching（1 to 99）
This command is state command.It will not change before a value is specified. FANUC system
parameter（NO.0723）specifing.
r: Quantity of chamfer
This command is state command.It will not change before a value is specified. FANUC system
parameter（NO.0109）specifing.
a: Angle of tool nose：
You can select 80 degree、60 degree、55 degree、30 degree、29 degree、0 degree，and specify
it with 2 digit.
This command is state command.It will not change before a value is specified. FANUC system
parameter（NO.0724）specifing.For example：P（02/m、12/r、60/a）
△dmin: Minimum of cutting depth expressed by radius.
This command is state command.It will not change before a value is specified. FANUC system
parameter（NO.0726）specifing.
d: Allowance for finish
i: Semidiameter of threaded portion
If i=0,it is seen as normal linear thread cutting.
k: Height of thread expressed by radius value.
△d: Cutting depth for fist time（radius value）

[g-codeguy]

Originally Posted by YBMach

Hello Chandru,

For the O-T model of fanuc, you need to use G76 for a canned threading cycle. If you want to do it line by line, use G92 or G32 code. Second, do not use G53. This is a work offset. Unless you are using the same tool on different chuck, I would recommend never to use G52 to G59 on a lathe.

Hope it helps.

YBMach

G54-G59 are work offsets on a lathe. We use G53 on a Mori SL-35 with an MF-T6 control to move the turret to a clearance point.....such as G53X-8.Z-14. G53 does not use tool geometry as part of the move. Nor does it have anything to do with a work offset. It is a machine position.

No idea what a G52 is on a lathe. G50 is used on some old lathes. I suggest you NOT use it except as a last option. Can get in trouble if not careful. Newer lathes have much more friendly ways of moving your workshift, sorry, work offset.

Apparently you don't program for subspindle lathes or make multiple parts with one barstop. Otherwise you would not recommend never using G54-G59.

I am not familiar with any G78 code on a Fanuc control. This is not to say that a machine builder couldn't assign it to any option/operation.

I can't help with the oi-TC control. We do have some O-T control lathes.

[angelw]

Originally Posted by CHANDRU

Friends,

Recently after commissioning a cnc with oi-TC controller we had G78 Threading cycle problem.

While machining after few passes the spindle was stopping and the tips were breaking.Later we found that there was some G-CODE missing in the program like G90,G53 and G97.

Following is the G78 threading cycle program.

Any mistake pl identify them.

G90 G53 T0505:
G97 S500 M04:
G0 X135.0 Z20.0:
G0 Z5.0 M07:
G01 Z20.0 F1.0:
G78 X132.6 Z-25.0 F4.233:
X132.4:
X132.2:
X132.0:
X131.8:
X131.6:
X131.4:
X131.2:
X131.0:
X130.8:
X130.6:
X130.4:
X130.2:
X130.0:
LIKE THAT
UP TO X128
AND FROM X128.0
X127.95:
X127.9:
X127.85:
X127.8:
X127.767:
G0 Z20.0 M09:
T0000
G0 X0 Z110.0 M05:
M01:

Similarly while doing internal threading cycle with g78 after few passes the tool is digging.

IAM NOT FAMILIAR WITH PROGRAMMING SO PL HELP ME.

Thanks

CHANDRU

Hi Chandru,
The other replies you've received are based on a control that is set to G Code System A. There are three G Code Systems available with the Fanuc Control selectable via parameter.

The G78 Code you're using and the way its implemented in your program indicates that your control is set to use G Code System B. G78 in G Code System B is the same as G92 in System A. Overwhelmingly, System A is used with Turning Centre, and unless you have some particular reason for using the control set to System B, you will gain more help from Forums such as this, by setting the control to use G Code System A. In your control, setting bit 6 and 7 of parameter 3401 both to "0" will set the control to System A. Currently, the settings of your control should be 0 and 1 for bit 7 and 6 respectively for it to use G Code System B. Bit numbers run 0 to 7 from right to left. Accordingly, its the two leftmost bits have to be set to 0.

With regards to the problem with the spindle stopping after a few passes, there's nothing in your listed code that would do that.

G53 is used to set the Machine Coordinate System. G54 to G59 are used to set the Workpiece Coordinate System. From a programming perspective, using G54 to G59 is a better proposition.

G97 is correct for all G Code Systems to command constant RPM. G76 is also the correct code in System A and B for the Multi Repetitive Threading Cycle, its G78 in System C.

Where is the Reference Return position on your machine. I note that the penultimate block is a move to X0 Z110. X0 on a lathe is generally the centre line of the machine.

Regards,

Bill