COSTOM DRILL CYCLE?

[slyym]

How do you set up a costom drill cycle? I am drilling a hole -5.5" deep and my r plane is z-4.5". What I want to do is retract to z zero like every 10 pecks but retract to z -4.5" the other 9. Is that possible?

[chip]

I don't think custome drill cycles are for that. Mabe, I have set up custome 1 for i.e. a machine that uses tap matic different code and another for standard tap cycles.

 

Mabe try drilling at different depths i.e. Z-5. G80 Z-6.0 G80 R-4.50 in each cycle.

Oh and G98.

[Steve Biehl - Cimquest Inc]

you could set up a Custom drill cycle to do that. You can use the fields under the cycle dropdown for variables to do what you what.

 

For instance, the first field below the dropdown is the 'peck1' variable. You could use that to represent the count before full retract.

 

The bigger problem would be that you have no such 'canned cycle' on the machine control to do that, so you need to post out long hand code or do like chip said, multiple operations to different depths.

[chip]

quote:

---

you could set up a Custom drill cycle to do that. You can use the fields under the cycle dropdown for variables to do what you what.

---

+1

 

Fields??

[slyym]

Your a genius Chip. Steve, how would you post a drill cycle in long hand?

[mayday]

quote:

---

how would you post a drill cycle in long hand?

---

slyym,

he means no canned cycle, in other words your drill cycle would be all G01 and G00 moves for every move you want the Z to do. will be a long prg to do a hole

[JG]

If that dosen't work for you, maybe you could use a macro in the control?

[slyym]

Chips idea is exactlly what I need, but thanks to everyone.Yall are awesome!

[chip]

quote:

---

Your a genius Chip

---

I don't think so......I wish! I learned from the best out here. There's a lot I learn here just want to give back. Some of these 5 Axis Rocket scientists deserve that credit!

 

[Guest CNC Apps Guy 1]

How is this???

 

code:

---

O9004(REDUCING PECK MACRO)

(THIS PROGRAM IS DESIGNED TO RUN FROM A PRE-DRILLED HOLE)

(USED FOR A DEEP HOLE WHERE TWO DIFFERENT DRILL LENGTHS ARE NEEDED)

(#18 "R" RAPID PLANE)

(#4 "I" 1ST PECK)

(#17 "Q" MINIMUM PECK)

(#26 "Z" FINAL DEPTH)

(#5 "J" REDUCTION MULTIPLIER)

(#9 "F" FEEDRATE)

(#3 "C" PECK RETRACT COUNT)

(#100 INITIAL PLANE STORAGE)

(#101 REMAINING DISTANCE CHECK)

(#102 "Z" TARGET VALUE)

(#103 "Z" FEED/RAPID VALUE)

(#8 "E" SUB RAPID PLANE)

#10=#4

(ERROR CHECKS)

IF[#3EQ#0]GOTO5

#3=FIX[#3]

GOTO6

N5#3=1

N6IF[#26EQ#0]GOTO50

IF[#18EQ#0]GOTO51

IF[#9EQ#0]GOTO52

IF[#4EQ#0]GOTO53

IF[#18LT#26]GOTO54

IF[#5NE#0]GOTO7

#5=1

N7IF[#5GT1]GOTO55

IF[#17GE.2]GOTO8

#17=.2

N8#100=#5003(STORE CURRENT Z POSITION)

G0Z#18(RAPID TO R PLANE)

#101=ABS[#5003-#26](CHECK FOR REMAINING DISTANCE #101=FINAL DEPTH)

#103=#18(SET 103 TO R PLANE, #103=NEW "R" IN PART)

WHILE[#101GT[#4+.02]]DO1(TEST 101 FOR FINAL DEPTH)

#149=0

WHILE[#3NE#149]DO2(CHECK FOR RETURN TO "R")

G0Z#103(RAPID INTO NEW "R" PLANE)

IF[#101LE[#4+.02]]GOTO2

#103=[#5003-#4](NEW DEPTH)

G1Z#103F#9(FEED TO "Z")

#101=ABS[#5003-#26](RECALIBRATE DISTANCE TO GO)

#103=#103+.1(RETURN PECK IN "R" PLANE)

G0Z#103(RAPID TO NEW "R")

#4=[#4*#5](RECALCULATE FEED DISTANCE)

#149=#149+1(INCREMENT COUNTER)

IF[#4GT#17]GOTO1(CHECK FOR MINIMUM PECK)

#4=#17(SET TO MINIMUM PECK)

N1END2

G0Z#18(RAPID TO ORIGIONAL "R" PLANE)

END1

G0Z#103(RAPID TO PECK RETURN PLANE)

N2G1Z#26(FEED TO FINAL Z)

GOZ#18

N3G0Z#100

#4=#10

GOTO4

(ERROR STATEMENTS)

N50#3000=1(NO VALUE IN Z)

N51#3000=2(NO VALUE IN R)

N52#3000=3(NO VALUE IN F)

N53#3000=4(NO VALUE IN I)

N54#3000=5(R IS DEEPER THAN Z)

N55#3000=6(J VALUE MUST BE LE 1.)

N4M99

---

[Mike Whitten CAD/CAM Contractors]

That's Hardcore James!

 

Thanks,

Mike

[Guest CNC Apps Guy 1]

I believe this was originally written by Mike Hubbard of Programming Unlimited.

[Mike Whitten CAD/CAM Contractors]

I never got real good with Macros but sometimes they are the only way to go.

 

Mike

[Tim Johnson]

Note For people wanting to use the drill macro;

You must use G65/G66 macro call to use the program.

 

code:

---

M06T45( 3/8 TAPERLENGTH DRILL)

M08

G00G90X11.73Y-10.246G54

G43H45Z6.S1000M03

G66P9004R?I?Q?Z?J?F?C?E?

(#18 "R" RAPID PLANE)

(#4 "I" 1ST PECK)

(#17 "Q" MINIMUM PECK)

(#26 "Z" FINAL DEPTH)

(#5 "J" REDUCTION MULTIPLIER)

(#9 "F" FEEDRATE)

(#3 "C" PECK RETRACT COUNT)

(#8 "E" SUB RAPID PLANE)

X10.Y-9

X6.5Y-6.5

G67

G91G30Z0.

M01

---

If drilling one hole G65 may be used instead of G66. Just remove the G67 also.

[Mike Whitten CAD/CAM Contractors]

Thanks Tim