Problem- Fanuc 18T Hardinge T42 Grooving G-Code

[rwpbrian]

Hello
I started a new job running a Hardinge T42 lathe/turning center. A lot of the parts i have been doing have o-ring grooves machined in the parts O.D. The guy running the machine before me has only programmed the grooves from point to point. No one in the shop has any clue where the manual has gone too. There has to be a g-code grooving cycle.
Any help would be great!
Thanks Brian

[angelw]

Originally Posted by rwpbrian Hello I started a new job running a Hardinge T42 lathe/turning center. A lot of the parts i have been doing have o-ring grooves machined in the parts O.D. The guy running the machine before me has only programmed the grooves from point to point. No one in the shop has any clue where the manual has gone too. There has to be a g-code grooving cycle. Any help would be great! Thanks Brian

Hi Brian,
The two cycles you require are G74 and G75 for Face and Diameter (inside and outside) drilling/grooving respectively. See the attached pictures.


Regards,

Bill

[fordav11]

The grooving cycle is really only useful for roughing simple square grooves.
I always program grooves long hand. There's certainly nothing complicated about a groove anyway and doing it long hand means you can rough and finish it and put nice chamfers/rads on the top of the groove making it a much more professional looking job.

Here's an example groove 6mm wide and 6mm deep with chamfer at top and rad at bottom.
OD diameter is 100mm. End Z position of groove is 50mm from the face.


G50 S500
G0 T0101 (3MM WIDE GROOVING TOOL)
G96 S100 M3
G0 X101.0 Z-48.5 M8
G1 X88.2 F0.1 (PLUNGE MIDDLE)
G0 X101.0
Z-51.0
G1 X100.0
X98.0 Z-50.0
X90.0
G3 X88.0 Z-49.0 R1.0
G1 Z-48.5
G0 X101.0
Z-46.0
G1 X100.0
X98.0 Z-47.0
X90.0
G2 X88.0 Z-48.0 R1.0
G1 Z-48.5
G0 X101.0
X300.0 Z300.0 M9
T0100 M5
M1
M30

[tanvon]

hi, may be this cnc blog post might help
CNC Fanuc G74 Peck Drilling Cycle for Simple CNC Lathe Drilling
There are multiple programming examples related to Fanuc and Sinumerik 840D CNC Blog*|*CNC Programming CNC Machine and CNC Setting Blog

[fordav11]

The G74/G75 instructions in Fanuc manuals are a bit cryptic.

The above site doesn't have a G75 example.

Here is a multiple groove roughing example.....

Fanuc 15-series format.....
G75 X0.5 Z-0.675 I0.055 K0.125 F0.004

Referring to the diagram below,
X is the final X dim at the bottom of the groove
Z is the final end Z position
I is the peck amount in X
K is the step over amount in Z

If K was 0.060 then you would get a big wide groove
If K was 0 then you would get only one groove that is the same width as the grooving tool

Fanuc 0/16/18-series format
G75 R.025
G75 X0.5 Z-0.675 P0.125 Q0.055 F0.004

R is how much the tool will retract after each cut
X is the final X dim at the bottom of the groove
Z is the final end Z position
P is the Z step over amount
Q is the peck amount in X

Omit P for a single groove

However when using a G75 there is no chamfering or finish cut. At my company if a job was machined using a grooving cycle and came out sharp with no chamfers it would not be accepted by our quality control and I'm sure our customers would not be pleased either.
Programming at least the finish cut long hand ensures total tool control and allows for a finish cut and chamfers or any other non-standard groove profile.

[g-codeguy]

Don't know where (which manual) forday11 got his information for the G75 cycle from, but the lathes we have (using Fanuc 0, 16, 18, or 21i controls) use P for the depth of cut and Q for the Z axis increment. Therefore omit the Q for a single pass in Z.

Not saying his information isn't right for the lathes he runs. It's not right for the ones I program for tho.

EDIT: We are running 4 Hardinge T42s with 18-T controls, one Conquest 42 and one Conquest 51 with O-T controls & 3 of their EMAGs with 18i-T controls.

Also I'm not sure if decimals in P and Q will work. Never tried them as examples in our various manuals don't show the use of decimals for these values so I've never tried using one.

[rwpbrian]

Wow thanks for all the info guys!
I'll give it a try tomorrow and let you know how it turns out
Thanks again
Brian!

[fordav11]

yeah the P & Q could have been reversed. I personally have zero interest in using G75 and even less (negative) interest in using 2-line fixed cycles so I never tested it or looked into it further.

[g-codeguy]

Originally Posted by fordav11 yeah the P & Q could have been reversed. I personally have zero interest in using G75 and even less (negative) interest in using 2-line fixed cycles so I never tested it or looked into it further.

I don't use G75/G74 unless I need to break the chip. It is faster than manually programming the movements, and lends itself to easily experimenting with the DOC for pecking before retracting if necessary. The cycles add too much time if your not having a problem with the chip.

[fordav11]

I use G74 a lot for peck drilling in Z using Sandvik 805 drills with deep holes (~20" deep) in sh*t material that won't chip but never used G75.