G71,73,70 equivalent's for Milling ?

[iMisspell]

Aside from using a sub-program are there any profiling & roughing cycles like G71, G73 and G70 for a lathe which would do the same for a mill or will these work for both ?

Would like to key in a dia. and depth path, set how much would like to take off per-pass and how much to leave for a finish pass. With the ease of changing one varable we would like to change the DOC from .125 to .093 and have the control cal. how many more passess it will need to take.

For a lathe its a snap with a G73, looking for some like that with a Mill, possable ?

Heres a clip incase im not being clear...

N004 X2.562 Z.5
G71 U.093 (DOC .093)
G71 P666 Q668 U.02 W.01 F.010
(LEAVE .02 on DIA. AND.01 ON LENTH)
(ROUGH AT F.01)
(START LINE IS N666)
(FINISH LINE IS N668)
N666 G0 X1.
G1 Z.0 F.01
X1.3589 F.005
X1.4955 Z-.0683 F.002
Z-.281 F.005
X1.5124
X1.63 Z-.343 F.002
X1.6958 F.005
X1.9699 Z-.3803 F.002
X2. Z-.3953 F.005
N668 G00 X2.562
N005 G70 P666 Q668 (FINISH PASS)


Ahhh... after seeing that, maybe this will work on a mill ??? (gonna try at work tomarrow)

Simple fake facing example...
Make one swoop at 4in dia, move out a 1/16 and then another swoop at a 2.5in dia.
Then jump in a Z amount and use the G70 to loop the path from before.
Finish the 1/16 as Z0

G0 X0 Y6 Z.25
Z.125
N100 G1 Y4 F40.
G3 J-4 F60.
G1 K.062 F40.
Y2.5
G3 J-2.5 F60.
G1 Y4.032
N200 G0 Y6
Z.062
G70 P100 Q200
Z.0
G70 P100 Q200
Z-.062
G70 P100 Q200
G0 G53 Z0...

If that does work, you would have to use K for the Z cause its incremental, correct ?


_

[Geof]

"are there any profiling & roughing cycles like G71, G73 and G70 for a lathe which would do the same for a mill or will these work for both ?

This is a darn good question; when you find one let me know .

Haas have pocketing routines that you can fake a bit and do zero depth pockets but I just wrote my own template programs using subroutines. I use a mix of absolute and incremental for square and rectangular facing and for circular facing I use a single G02 in a subroutine and use different tool diameters with tool compensation to change the radius of the circle.

[thogib]

The only way to to that on a mill is with macro programs. No simple G or M codes for a mill, unless your machine tool maker pre-wrote them for you.
Don't ask why when you have a machine with a Y axis, I would think that would have been easy enough to transfer over from a turning controller to a mill controller?
Tom G

[ajl6549]

Simple sub programs work as well. Like prog. an incrementle routine that would mill a rec. pocket the repeat it with an " L " count.

[tobyaxis]

This is only "Hear Say", but someone told me Fadal like the HAAS has a Pocketing Macro/Canned Cycle. Anyone else know anything about this? The Yasnac Control found on Matsuura VMC's has a G12/G13 Canned Cycle close to what your asking for Imisspell. It's a circular spiral cycle. It won't do rectangular boxes though.

I have a book that has a pocketing macro that I'll post here when it is located. Maybe someone here with more knowledge of macro type programming can try it to see if it will work.

[dertsap]

[QUOTE=tobyaxis]This is only "Hear Say", but someone told me Fadal like the HAAS has a Pocketing Macro/Canned Cycle.
QUOTE]

this was the only thing that i liked about the fadals , there are some nice little sub routines

[tobyaxis]

[QUOTE=dertsap]

Originally Posted by tobyaxis This is only "Hear Say", but someone told me Fadal like the HAAS has a Pocketing Macro/Canned Cycle. QUOTE] this was the only thing that i liked about the fadals , there are some nice little sub routines

Thanks for the info Dertsap.
I wonder why other Machine Tool Builders didn't follow up on this? I only got to use older controls. The newest control was a Fanuc 1LE on a 6 axis Swiss Screw Machine and it only had standard Lathe Canned Cycles with a few extras for cross drilling. Can't say how many times a pocketing cycle would have helped out. With all the advances with CAD/CAM I doubt anyone will be offering much in options anymore. Then again most newer controls handle 3D solids with their own intergraded CAD/CAM. Who started that trend, Mazak?

[tobyaxis]

Originally Posted by iMisspell Aside from using a sub-program are there any profiling & roughing cycles like G71, G73 and G70 for a lathe which would do the same for a mill or will these work for both ? Would like to key in a dia. and depth path, set how much would like to take off per-pass and how much to leave for a finish pass. With the ease of changing one varable we would like to change the DOC from .125 to .093 and have the control cal. how many more passess it will need to take. For a lathe its a snap with a G73, looking for some like that with a Mill, possable ? Heres a clip incase im not being clear... N004 X2.562 Z.5 G71 U.093 (DOC .093) G71 P666 Q668 U.02 W.01 F.010 (LEAVE .02 on DIA. AND.01 ON LENTH) (ROUGH AT F.01) (START LINE IS N666) (FINISH LINE IS N668) N666 G0 X1. G1 Z.0 F.01 X1.3589 F.005 X1.4955 Z-.0683 F.002 Z-.281 F.005 X1.5124 X1.63 Z-.343 F.002 X1.6958 F.005 X1.9699 Z-.3803 F.002 X2. Z-.3953 F.005 N668 G00 X2.562 N005 G70 P666 Q668 (FINISH PASS) Ahhh... after seeing that, maybe this will work on a mill ??? (gonna try at work tomarrow) Simple fake facing example... Make one swoop at 4in dia, move out a 1/16 and then another swoop at a 2.5in dia. Then jump in a Z amount and use the G70 to loop the path from before. Finish the 1/16 as Z0 G0 X0 Y6 Z.25 Z.125 N100 G1 Y4 F40. G3 J-4 F60. G1 K.062 F40. Y2.5 G3 J-2.5 F60. G1 Y4.032 N200 G0 Y6 Z.062 G70 P100 Q200 Z.0 G70 P100 Q200 Z-.062 G70 P100 Q200 G0 G53 Z0... If that does work, you would have to use K for the Z cause its incremental, correct ? _

Yes K should the parallel axis to Z It's X(U) Y(V) Z(W) on a Lathe. On a Mill it's X(I)Y(J)Z(K)

[tobyaxis]

Here is the Macro I promissed. This one was written in a machine manual and I have not had a chance to test it, so be very carefull.

Pocket Macro Call (Yasnac MX1)

G65 P9061 X.. Y.. Z.. R.. I.. J.. K.. T.. Q.. D.. F.. E..

Where

X, Y The absolute coordinate value of the start point (the lower left hand corner of the pocket)

Z The absolute position of the bottom of the pocket.

R The absolute position of the rapid traverse tool return

I, J X-axis and Y-axis lenghts of the pocket (unasigned)

K Finish allowance (left-over allowance, unasigned) Default value is 0 (zero)

T Cut width rate (designated in %)Cut width = tool radius * T/100

Q Z-axis cut depth for each cut

D Tool Offset number

F Feedrate in the X,Y plane (G17)

E Feedrate in the Z-axis (Plunge feedrate in Z)

User Macro Body

O9061
#10 = #[2000 + #7].....Tool radius
#11 = #6 + 1.0 + #10
#12 = #5 - 2 * #11
#13 = 2 * #10 * #20/100...Cut Width
#14 = FUP [#12/#13]....X-axis cut count:-1
________________________

#27 = #24 + #11
} X, Y coordinates of the machining start point
#28 = #25 + #11
_______________________

#29 = #26 + #6 .......... Z-axis coordinates of cut bottom
#30 = #24 + #4 - #11
#15 = #4003 ......... Read of G90/G91
G90 ..... ABS Programming
G00 X#27 Y#28
G00 Z#18
#32 = #18 ........#32 cut bottom in execution
DO1
#32 = #32 - #17
IF [#32 GT #29] GO TO 1
#32 = #29
N1 G01 Z#32 F#8
G01 X#30 F#9
#33 = 1
WHILE[#33 LE#14] DO 2
IF [#33 EQ#14] GO TO 2
G01 Y[#28 + #33 * #13]F#9
GO TO 3
N2 G01 Y[#25 + #5 - #11]
N3 IF[#33 AND 1 EQ 0] GOTO 4
G01 X#27
GO TO 5
N4 G01 X#30
N5 #33 = #33 + 1
END 2

G00 Z#18
IF[#32 LE#29] GO TO 6
G00 X#27 Y#28
G01 Z[#32 + 1.0]F[4 * #8]
END 1

N6 #11 = #11 - 1.0
#27 = #27 - 1.0
#28 = #28 - 1.0
#30 = #30 + 1.0
#31 = #25 + #5 - #11
G00 X#27 Y#28
G01 Z#32 F#8
G01 X#30 F#9
Y#31
X#27
Y#28
G00 Z#18
G00 X#24 Y#25 ......Return to start point
G#15 ...........Restore of G90/G91
M99