Spiral Pocket Milling SV24-12 Super Mini w/ Fanuc Oi Mate-MC

[RonRoy2004]

Hello,

After a year and a half I haven't had any luck finding info thru Sharp so am asking here, I can use the pocket functions to make a circular pocket, if I want it to step straight over then make the loop, however I am attempting to make a pocket by feeding to depth, then spiraling out to finish size to ease cutter load and have a precise finish by ramping in and out rather than plunging.

Does anyone know of a macro for this that works? or am I stuck remote programming this with BobCad?

The macro sharp provided makes rectangular pockets and even it steps out in one axis, lol.

Thank You
Ron Riekens II
ronroy2004@comcast.net

[leggazoid]

From leblond makino world of macros book. Look for book on ebay. Wish someone had it in pdf.

%
:0113 (SPIRAL MACRO)
#26= ABS[#26]
#17= ABS[#17]
#22=#17
IF [#26 EQ #0] GOTO 1 (Z)
IF [#17 EQ #0] GOTO 1 (Q)
IF [#18 EQ #0] GOTO 1 (R)
IF [#4 EQ #0] GOTO 1 (I)
IF [#7 EQ #0] GOTO 1 (D)
IF [#20 EQ #0] GOTO 1 (T)
IF [#3 EQ #0] GOTO 1 (C)
IF [#19 EQ #0] GOTO 1 (S)
IF [#13 EQ #0] GOTO 1 (M)
IF [#26 EQ #17] GOTO 2 (Z LESS THAN E)
#33= #4001
#32= #4003
#31= #[2000+#7]
#30= [3.82*#19]/[2*#31]
IF [#30 GT #13] GOTO 8
S#30 M3
#29= #30*#20*#3
GOTO 9
N8 S#13 M3
#29= #13*#20*#3
N9 #27= #18/12
#10= #5041
#12= #5042
#5= #5043-#5083
#16= 0
G17
N7 #14=#17
WHILE [#26 GE #14] DO 1
IF [#31 GE [[#11/2]-.05]] GOTO 4
#28= [#11/2]-#31
G91 GO Z-[.1+#17]
G90 X[[#10+#28]-.05]
G1 X[#10=#28] F#29
GOTO 5
N4 G91 G1 Z-[.1+#17] F[#29/2]
#28= 0
N5 #15=[[#4/2]-#28-#31]/#18*360
#1=30
#28= #28+#27
WHILE [#15 GT #1] DO 2
#24= #10+#28*COS[#1]
#25= #12+#28*SIN[#1]
#2= [#28/[#28+#31]]*#29
G90 G3 X#24 Y#25 R#28 F#2
#1= #1+30
#28= #28+#27
END 2
#28= [#4/2]-#31
#24= #10+#28*COS[#15]
#25= #12+#28*SIN[#15]
#2= [#28/[#28+#31]]*#29
G3 X#24 Y#25 R#28 F#2
X#24 Y#25 I-[#28*COS[#15]] J-[#28*SIN[#15]]
#15= #15+15
#24= #10+#28*.98*COS[#15]
#25= #12+#28*.98*SIN[#15]
X#24 Y#25 R[#28*.98]
IF [#26 EQ #17] GOTO 6
IF [#26 EQ #14] GOTO 6
IF [#16 EQ #1] GOTO 6
G91 GO Z.1 G90 X#10 Y#12
#14= #14+#17
END 1
#17= [#26-[#14-#17]]
#16= 1
GOTO 7
N6 GO Z#5 X#10 Y#12
#17= #22
GOTO 3
N1 #3000= 0(SPIRAL POCK. COMMAND INCOMPL.)
N2 #3000= 0(E EXCEEDS Z)
N3 G#33 G#32 M99
%

[christinandavid]

Have been writing a macro to perform these kind of motions in an incremental linear fashion to allow freedom using rotation (to suit our milling head attachment).

Was surprised to find that I can use it to describe virtually any kind of motion - facing, pecking, involute (pocketing), helical (polygonal, not just circular) and trochoidal.

Pocket-wise, you can start wherever you want. Slot-wise, you can oscillate the feedrate to reduce air-cutting. I have also added a start/finish angle which can be used to reduce cutter engagement in the corners. I can post it to you with an explanation once I've perfected the cutter-comp.

DP

[dcoupar]

leggazoid,

Thanks for posting this. I don't suppose they had any examples of calling the macro?

[mactec54]

Hi RonRoy2004

Here is a 2.0 hole .600 deep with a arc-on & arc-off, Macros are great if you know how to do them or you want to spend the time to learn how to do them, as well your control has to support them, not all can

[leggazoid]

Yes they did have an example of calling it with 2 pictures that explained it. This program is written for inch programming only. I don't have access to these right now but I will try to explain the g65 call...

Start at Z.1 above part.

z = final z depth
q = z increment
d = cutter comp offset
s = sfm
r = ?
i = diameter of finished hole
t = # of teeth
c = feed per tooth?
m = maximum spindle speed

Can someone with macro experience help with r?

[skullworks]

I wrote a macro to ADD G13 to our Mori Seiki SV50B and based it on the Yaznaq implementation which is sparse compaired to the Haas implementation.

At the time I wrote it I had not had to stoop to running Haas machines in production.

The G13 macro was assigned O9013 and became a fully functional G-code cycle like G83.

I used alot of machine variables to plug in the last active F, D, current position etc. I also have many error tests that will cause an alarm if you don't use it properly.

The G13 can be used for circle cleaning/finishing or a full spiral pocket. My macro does EVERYTHING at a fixed Z, Meaning you have to position to hole/pocket center and plunge to depth BEFORE doing the G13 cycle. Also its up to the programmer to retract the tool once the pocket is done. It was a bit rushed and could use some refinement but it has worked fine for us.

I will try to grab a copy.