Milling macros

Can someone with an 0i control for a mill post these macros?

Thanks


Custom Macro B Canned Cycles
The Custom Macro B canned cycles are fully tested examples of macros that
you can use immediately, or copy and modify to implement your own custom
cycles.

O9170 Outside frame milling
O9171 Inside frame milling
O9172 Pocket frame milling
O9173 Face milling
O9174 Outside circle milling
O9176 Inside circle milling
O9177 Pocket circle milling
O9179 Slot milling
O9180 Row pattern drilling
O9190 Rectangular frame drilling
O9280 Bolt-hole circle drilling

%
O9170 (G170 OUTSIDE FRAME MILL)
#2=#4003 (G90/G91 MODE)
#130=#5041(INITIAL X POS)
#131=#5042(INITIAL Y POS)
#132=#5043(INITIAL Z POS)
#133=#[2000+#4107](ACTIVE RADIUS)
IF [#2 EQ 91] GOTO 3 (INCREMENTAL MODE)
#130=0
#131=0
#132=0
N3 #130=#130+#4 (FINAL X POSITION)
#131=#131+#5
#132=#132+#6 (FINAL Z POS - R PLANE)
IF [#13 NE #0] GOTO 4
#13=0
N4 #7=#7-2*#9 (LENGTH - RADIUS)
#8=#8-2*#9 (WIDTH - RADIUS)
#9=#9+#13 (RADIUS+FINISH ALLOWANCE)
IF [#14 NE #0] GOTO 5
#14=#12 (FINISH FEED)
N5 IF [#15 NE #0] GOTO 10
#15=0.5*#12 (PLUNGE FEED)
N10 IF [#16 EQ #0] GOTO 20 (STEP DEPTH)
IF [#16 EQ 0] GOTO 20
#23=#10/#16
#17=FIX[#23] (ROUND OFF)
#23=#10-#17*#16
IF [#23 EQ 0] GOTO 25
#17=#17+1 (NO. OF STEPS IN DEPTH)
GOTO 25
N20 #17=1
#16=#10
#23=0
N25 G90 G00 Z#132 (MOVE TO R PLANE)
G00 X#130 Y[#131-#8/2-#9-#11] (START POSITION)
G41 G91 G01 X#11 F#12
G03 X[-#11] Y#11 R#11
(START OF MILLING CYCLE)
N1 WHILE [#17 GT 0] DO 1
IF [#17 GT 1] GOTO 18
IF [#23 EQ 0] GOTO 18
#16=#23
N18 G01 Z[-#16] F#15(PLUNGE)
G01 X[-#7/2] F#12 (MILL)
G02 X[-#9] Y#9 R#9
G01 Y#8 (WIDTH)
G02 X#9 Y#9 R#9
G01 X#7 (LENGTH)
G02 X#9 Y[-#9] R#9
G01 Y[-#8]
G02 X[-#9] Y[-#9] R#9
G01 X[-#7/2]
#17=#17-1
END 1
N19 IF [#13 EQ 0] GOTO 30 (START OF FINISH CYCLE)
#9=#9-#13 (DECREASE RADIUS BY FINISH ALLOWANCE)
#11=#11+#133 (ADJUST CLEARANCE BY TOOL RADIUS)
G03 X[-#11] Y[-#11] R#11
G01 X[2*#11+#13]
G03 X[-#11-#13] Y[#11+#13] R[#11+#13] F#14
G01 X[-#7/2] (FINISH)
G02 X[-#9] Y#9 R#9
G01 Y#8 (WIDTH)
G02 X#9 Y#9 R#9
G01 X#7 (LENGTH)
G02 X#9 Y[-#9] R#9
G01 Y[-#8]
G02 X[-#9] Y[-#9] R#9
G01 X[-#7/2](END FINISH CYCLE)
#11=#11-#133(ADJUST CLEARANCE BY TOOL RADIUS)
N30 G03 X[-#11-#13] Y[-#11-#13] R[#11+#13] F#14
G40 G01 X[#11/2]
G90 G00 X#130 Z#132(Z MOVE UP)
G#2 (PUTS BACK INTO G90/G91 MODE AS FOUND)
M99
%

Nice macros ! I would love to have these for slot milling. Anyone ?

Quote:

---

Originally Posted by pitri

Nice macros ! I would love to have these for slot milling. Anyone ?

---

I do not currently have any slot milling macros, but would you be interested in trying out one of my 3D custom macros. Here is the first macro I ever wrote and it can machine 1/2 a sphere or cap any size radius on any size diameter.

O7777(CAP 0-90 DEG FULL RAD. OD PART)
(ABSOLUTE SURFACING MACRO)
(START OF TANGENT/ TOP OF PART)
(END OF TANGENT/ OD OF PART)
(WORKS)

(FORMAT G65/G66 CDTSKRZF)
(C = #3 - CUSP HEIGHT/ DEG. OF ROTATION)
(D = #7 - TOOL DIAMETER)
(T = #20 - TOOL RADIUS/ BALL OR BULL)
(S = #19 - PART DIAMETER)
(K = #6 - PART CORNER RADIUS)
(R = #18 - R PLANE)
(Z = #26 - Z START ZERO)
(F = #9 FEEDRATE)
(******************************)

IF[[#19/2]LT#6]GOTO1000
#100=0
#101=#6+#20
#102=#3
IF[#102GT15.]THEN#102=15.
#102=ROUND[90./#102]
#102=90./#102
#103=#5001
#104=[#103-.1]-[[#7/2]+[#19/2]]
#105=#5002
#113=#105
#115=[#105+.1]+[[#7/2]+[#19/2]]
#145=0
IF[#7EQ[#20*2]]GOTO1
#105=#105+[[#7/2]-#20]
#145=#145+[[#7/2]-#20]
N1G0G90X#104Y#115
Z[#26+.1]
G1Z#26F#9
#106=#5003-#101
WHILE[#100LE90.]DO1
IF[#100GT90.]GOTO100
#107=#105+[SIN[#100]*[#101]]
#147=#145+[SIN[#100]*[#101]]
#108=#106+[COS[#100]*[#101]]
IF[#6EQ[#19/2]]GOTO10
#107=#107+[[#19/2]-#6]
#147=#147+[[#19/2]-#6]
N10#100=#100+#102
G1Z#108F#9
G41Y#107
X#103
G02J-#147
G03X[#103+.1]Y[#107+.1]J.1F[#9/2]
G0Z[#108+.1]
G40X#104
END1
N100G0G90Z#18
X#103Y#113
M99
N1000M00( PART CORNER RAD. TOO BIG )

Hi everyone,

So I have been wanting to create a macro for pocketing starting in the center of the pocket, and I'd like to dedicate variables for certain call outs, such as pocket length in x, pocket length in y, z depth, tool stepover, pass per depth, corner radius, etc.. My problem is I'm struggling with how to start out my sub routine so my cutter starts on center and my tool will stepover the amount I specified in a variable. Below is what I will be calling out for variables. Any help or thoughts on this would be greatly appreciated.

#124= #24 ( X CENTER )
#125= #25 ( Y CENTER )
#126= #26 ( Z CENTER )
#104= #4 ( I OR X LENGTH )
#105= #5 ( J OR Y WIDTH )
#106= #6 ( K OR Z DEPTH )
#118= #18 ( R OR CORNER RADIUS )
#117= #17 ( Q OR DEPTH OF EACH PASS )
#121= #21 ( U OR DEPTH OF FINISH PASS )
#120= #20 ( T OR TOOL NUMBER )
#109= #9 ( F OR CUTTING FEED RATE )
#108= #8 ( E OR PLUNGE FEED RATE )
#107= #7 ( D OR PERCENT OF CUTTER DIA )

Newbee!
Is there such a thing as macros for dummies?
I also need help with using the Renishaw probe on my Haas VF-5, can anyone point me in the right direction?

DynoDean

what do you need help with on the probe?

Hello James
That is a nice 1/2 Sphere Program you have got there. Is there any chance you can do a Mach 3 friendly version. As it stands Mach 3 doe's not like the IF statement in the program.

hy pkcnc, i have many parametric codes ... if you wish, i can create one for you :)

i don't have experience with mach 3, but i can start by generating the toolpath, then customize it with mach 3 g-code syntax ( considering that you provide it )

Quote:

---

doe's not like the IF statement

---

this means that you can not write all the logic inside the machine program, thus i guess that mach3 uses only linear code

so, all the logic has to be somewhere else, like in a software application ... no problem, consider it done :) to begin, i need to know part shape before and after operation + tool shape

Hello
Basic shape is 1/2 a sphere, diameter is 100mm. Using a ball endmill 12mm diameter. Would be great if it can be done. The sphere is machined from a block 120 x 120 x120mm.

so you wish for half a sphere, with diameter 100 ? tool o12 ? ok :)

if i give you the toolpath in xyz, can you make it work on your machine ? because i can't, i don't know the g-code for mach3 :)

also, please choose a strategy :
... cut a circle, then make a step in Z, cut another circle, then make a step in Z, and so on
...... or
... continous helix

Quote:

---

The sphere is machined from a block 120 x 120 x120mm.

---

i can deliver a parametric for the finishing

for roughing it would take me longer ... hmm ... what do you say ? are you ok only with finishing ? kindly :)

Hi Toolpaths will be fine. Z step strategy for roughing out. And the continous helix for finishing if you can. Thanks.

I posted this in 2017, I just got a responce this week and it was to the post below this one?
Anyway I am looking for a soft wear program to use my Renishaw probe on my VF-5 for reverse engineering parts. A point cloud that can be turned into a solid.
I want to output from the Haas controler to my laptop drawing program (BOB/CAD CAM)

Quote:

---

Originally Posted by DynoDean

I posted this in 2017, I just got a responce this week and it was to the post below this one?
Anyway I am looking for a soft wear program to use my Renishaw probe on my VF-5 for reverse engineering parts. A point cloud that can be turned into a solid.
I want to output from the Haas controler to my laptop drawing program (BOB/CAD CAM)

---

Hi,

I think MeshLab can do the job, and its free !

You have to create a valid .xyz file from your point cloud, then search for the following page : "How to Create an STL file from a XYZ file in MeshLab" which give the procedure to obtain an stl from the point cloud.

The resulting stl can be imported in any CAD i think.

Quote:

---

Originally Posted by DynoDean

Newbee!
Is there such a thing as macros for dummies?
I also need help with using the Renishaw probe on my Haas VF-5, can anyone point me in the right direction?

---

Only 5 years too late to the party, but maybe a help for someone else. Get the book CNC Programming Using Fanuc Custom Macro B by S. K. Sinha. He does an excellent job of explaining Macro B programming and gives some useful examples.

Quote:

---

Originally Posted by PKCNC

Hi Toolpaths will be fine. Z step strategy for roughing out. And the continous helix for finishing if you can. Thanks.

The sphere is machined from a block 120 x 120 x 120

---

hy pkcnc :) please check attached : roughing from square + helix finishing

but z step finishing may be better, because it requires only g2/3, while helix finishing will break a g2/3 in many linear segments

sorry for the late reply, only recently i remembered this / kindly :)