Bolt Circle Programming

[Isureamcael]

Hi Folks!

I just got my first professional job as an Adjunct CNC Instructor, and Im in need of some refreshers. Im trying to remember some ways to program bolt hole circles using g-code. Im working with fanuc controls - and want to use a g81 canned cycle... but am rusty on how to set up the block. Any suggestions?

Thanks!

(p.s. the more suggestions the better!)

[Mitsui Seiki]

Here is a custom macro that machines a bolt hole pattern.
O0008 (Main program)
N005 G54 G90 S800 M03 T02 (Select coordinate system, absolute mode, start spindle, get next tool ready)
N010 G00 X3.0 Y2.5 (Rapid to center of bolt hole pattern)
N015 G43 H01 Z.1 (Instate tool length compensation, rapid up to workpiece)
N020 G65 P1008 X3.0 Y2.5 Z0 R1.75 D0.75 A45.0 H8.0 C81. F5.0 (Machine entire bolt hole pattern with drilling cycle)
N025. . . . . .


X - Position in X for center of bolt hole pattern
Y - Position in Y for center of bolt hole pattern
Z - Surface in Z into which holes are machined
R - Radius of bolt hole pattern
D - Depth of holes
A - Starting angle (0 is three o'clock position, plus is ccw)
H - Number of holes
C - Cycle type (81 is for drilling, 84 for tapping, etc.)
F - Feedrate for machining
Here's the actual custom macro (program O1008).

O1008 (Custom macro to machine bolt hole circle)
#101=1 (Initialize counter)
#102=#1 (Initialize current angle to A)
#103=360 / #11 (Constant for incremental angular distance between holes)
#104=#26 + 0.1 (Constant for rapid approach plane)
#105=#26 - #7 (Constant for Z bottom position of hole)
N1 IF [#101 GT #11] GOTO 99 (Test if loop is finished)
#110=#24 + COS[#102] * #18 (Calculate X position for current hole based on current angle)
#111=#25 + SIN[#102] * #18 (Calculate Y position for current hole based on current angle)
G#3 X#110 Y#111 R#104 Z#105 F#9 (Machine current hole)
G80 (Cancel cycle)
#101=#101 + 1 (Step counter)
#102=#102 + #103 (Step current angle)
GOTO 1 (Go back to test at loop beginning)
N99 M99 (End of custom macro)

[mrainey]

I'd recommend you have a look at some basic training resources. It sounds like you're likely to have some more CNC questions.

CNC Concepts has great information.

http://www.cncci.com

[holbieone]

it's going to be a little different for each control type
T1M6 ;TOOL CALL
S1000M3 ;CW SPINDLE 1000RPM
N100G81X1.Y2.C.1D-.75F6. ;G81 CANNED CYCLE + FIRST HOLE ,POSITION ,CLEARANCE PLANE AND DEPTH
N200X-1.Y2. ;SECOND HOLE
N300X-1.Y-2. ;THIRD HOLE
N400X1.Y-2. ;FORTH HOLE
N500G80 ;CANCEL CANNED CYCLE

(G81) DRILLING CYCLE (DRILLS FROM CLEARANCE PLANE TO DEPTH IN FEED MODE THEN RETRACTS TO CLEARANCE PLANE IN RAPID MODE)

(X,Y) POSITION OF HOLE TO BE DRILL

(C) CLEARANCE PLANE

(D) DEPTH (IN ABSOLUTE POSITIONING THIS WOULD BE FROM PART ZERO ,INCREMENTAL FROM CLEARANCE PLANE )

(F) FEED RATE (IPM) (CHIP LOAD = FEED RATE / RPM) / 2 PER TOOTH

(X,Y) OTHER HOLE POSITIONS

(G80) CANCEL CANNED CYCLE

HOPE THIS HELPS

KEVIN

[Mitsui Seiki]

You can use G16(Polar coordinate system)


G16(PCS on)
G81 X2 Y0 R0.1 Z -0.1 F3
X2 Y60
X2 Y120
X2 Y180
X2 Y240
X2 Y300
G15(PCS off)
X is radius, Y is the angle.

[psychomill]

Not to be rude, but this probably will be.....

How do you get a job (or go looking for one) as a "cnc instructor" and not understand something so generic as a G81 cycle?... even if its for "bolt circle"... What exactly is it that the course you're instructing consist of?

Curious........??

[Andre' B]

And on a machine the does not do polar.

G0X0.0 Y0.0 Z0.1
G81 R0.1 Z -0.1 F3 L0
X[2*COS[0]] Y[2*SIN[0]]
X[2*COS[60]] Y[2*SIN[60]]
X[2*COS[120]] Y[2*SIN[120]]
X[2*COS[180]] Y[2*SIN[180]]
X[2*COS[240]] Y[2*SIN[240]]
X[2*COS[300]] Y[2*SIN[300]]
G80
G0 X0.0 Y0.0 Z0.1


(OR WITH A LOOP)
G0X0.0 Y0.0 Z0.1
G81 R0.1 Z -0.1 F3 L0
#100=45(START ANGLE)
#101=3(RADIUS)
#102=15(ANGLE INCREMENT)
(* ------------- *)
#103=#100+360
WHILE[#100LT#103]DO1
X[#101*COS[#100]] Y[#101*SIN[#100]]
#100=#100+#102
END1
G80
G0 X0.0 Y0.0 Z0.1

[ChattaMan]

and a shorter version for one that does do polar...........

G16 G81 X2 Y0 R0.1 Z -0.1 F3
G91 Y60 K5 (increments 60degrees, 5 times)
G15 G90 G80

X is radius, Y is the angle.

Just another way of doing the same thing ;-)

[oldjohn]

Mate. Do you know how dangerous this s**t is if you don't know what you're doing? I wouldn't like to be in your class.

John

[Bluesman]

Originally Posted by psychomill Not to be rude, but this probably will be..... How do you get a job (or go looking for one) as a "cnc instructor" and not understand something so generic as a G81 cycle?... even if its for "bolt circle"... What exactly is it that the course you're instructing consist of? Curious........??

Not Rude Psycho, But an excelent question. I was asking the same one to myself. How in the world do you get a job as an "INSTRUCTOR" and then have to go into this forum for something as simple as that. Hmmmmmmmmmmmm
Just for future reference, The green button is usaully "ON" and the big red one is the "E STOP" (Probobly need that one the most)

Bluesman

[holbieone]

Originally Posted by Bluesman Not Rude Psycho, But an excelent question. I was asking the same one to myself. How in the world do you get a job as an "INSTRUCTOR" and then have to go into this forum for something as simple as that. Hmmmmmmmmmmmm Just for future reference, The green button is usaully "ON" and the big red one is the "E STOP" (Probobly need that one the most) Bluesman

at least he knows what he doesn't know

he may have put the horse in front of the cart but at least he's trying ,someone has to

you can't knock someone for trying

[Bluesman]

Originally Posted by holbieone at least he knows what he doesn't know he may have put the horse in front of the cart but at least he's trying ,someone has to you can't knock someone for trying

Dude, He is the instructor he should be beyound trying

Bluesman