Need Help!- Helical Programming on Fanuc 6M

[mdm714]

I need to program a 3 axis machining center to cut a
helical tool path. I use BobCAD to generate G-Code, but
the software will not generate code for this control.

Is this control (Fanuc 6M) capable of this function?
Do I need to turn on parameters for this function.
What is the G-code for XYZ plain?

Will someone Please give me an example or formula?

[dcoupar]

G17 is XY Plane.

The following should cut a 1" radius circle while feeding down 0.1 in Z.

G90 G00 X1.0 Y0 S2000 M03
G43 Z0.1
G91 G02 I-1. Z-.1 F10.0
G90 G0 Z0.1

[beege]

You may not have any Helical on your machine. If not, could bobcad generate a code that is a series of very short linear moves? Otherwise, maybe someone could suggest a formula for a macro that would include a DO/WHILE loop, to make very short G01 moves ( a few tenths at a time) to simulate a helical form...

[dcoupar]

You may not have macros, either.

[hendikch]

yes you need to turn on options parameter on fanuc 6m to make it enable helical interpolation. and the program would be the same with using G3 or G2 for hellical with 3 axis moving at one time

[Stu_M3]

If you have macros enabled her is a macro I use for bores on an OM control

%
O0001(***HELICAL MILL*****)
(z=depth,Q=PECK/REV,D=DIAM,C=ALLOWANCE,R=RAPID HT)
(C IS THE OFFSET FROM THE BORE FOR THE START OF THE RAMP )
G00G90G40G80G54
G90X0.0Y0.0
G91
G28Z0.0M5
G90
M6T1
S1600 M3
X-100.00 Y0.000
M8
G65 P9021 Z-10.0 Q1.0 D30.00 C0.5 R50.0 F300
G0X100.000 Y0.0
G65 P9021 Z-10.0 Q1.0 D30.000 C0.5 R50.0 F300
G0Z100.0M5
M09
G91G28Z0.0
G90
M30
%




09021( HELICAL MILL SUB PROG:S.CANTY 2004)
#100=FUP[#9/3.]
#101=#4001
#102=#4003
G04P5
#120=[100+#4120]
G04P5
#26=ABS[#26]
#17=ABS[#17]
#105=FUP[#26/#17](N_PECKS)
#106=[ROUND[#26/#105*1000.]]/1000.(PECK)
#114=[ROUND[#106/4.0*1000]]/1000.(PECK/2)
#106=#114*4.0
#107=#106*#105(PECK*PASSES)
#109=#7/2.0(RADIUS)
#110=#109-#3(RAD-OFFSET)
G0 Z#18(Z_RAPID)
G01 Z2.0 F1000
#108=#107-#26(Z_START)
#112=#106/4.0
#113=#112+#108(Z_START)
Z#113 F#100
G91G01
G41Y-#110D101 F#9
G1X#3
G03 X#110 Y#110 Z-#112 I0.0 J#110 F#9
WHILE[ #105 GT 0]DO1
#105=#105-1.0
X-#7 Y0.0 Z-[#106/2.0] I-#109Y0.0
X#7 Y0.0 Z-[#106/2.0] I#109J0.0
END 1
X-#7 Y0.0 I-#109 J0.0
X#7 Y0.0 I#109 J0.0
X-#110 Y#110 I-#110 J0.0
G01 X-#3 Y0.0
G40 Y-#110
G#101G#102
G90
G0Z#18
M99

[ikneb]

I wrote a macro to do a helix but I dont have it here at home but this is how I do one on a control without macro programing (OMC)
1.75 inch hole 1 inch deep

M6 T21
S35714 M13
G0 G90 G54 X0 Y0
G43 H21 Z.1
G1 Z.0098 F53.565
G91 G41 D21 X.875
G03 X-1.75 Z-.0459 R.875
X1.75 Z-.0459 R.875
X-1.75 Z-.0459 R.875
X1.75 Z-.0459 R.875
X-1.75 Z-.0459 R.875
X1.75 Z-.0459 R.875
X-1.75 Z-.0459 R.875
X1.75 Z-.0459 R.875
X-1.75 Z-.0459 R.875
X1.75 Z-.0459 R.875
X-1.75 Z-.0459 R.875
X1.75 Z-.0459 R.875
X-1.75 Z-.0459 R.875
X1.75 Z-.0459 R.875
X-1.75 Z-.0459 R.875
X1.75 Z-.0459 R.875
X-1.75 Z-.0459 R.875
X1.75 Z-.0459 R.875
X-1.75 Z-.0459 R.875
X1.75 Z-.0459 R.875
X-1.75 Z-.0459 R.875
X1.75 Z-.0459 R.875
X-1.75 R.875
X1.75 R.875
G40 G1 X-.875
G0 G90 Z.1
G0 G91 G30 Z0

with macro on OiMB/OiMC

M6 T21
S3571 M13
G0 G90 G54 X0 Y0
G43 H21 Z.1
G113 R.875 Z-1.0 Q.1 S.01 C.1 D21 F53.565
G0 G91 G30 Z0


G113(made a G code for it I use it so much)R.875(radius of hole)Z-1.0(end point absolute)Q.1(max depth of cut per rotation)S.01(start point this point is adjusted by the control so the the end point is ALWAYS corect)C.1(point it Z that it rapids out of the hole to) D21(geom+wear)