Rapid override on 1 tool

[Programinator]

I have a long cycle and 1 drill in the cycle needs to be at 25% rapid. It is a g83 cycle on a Haas control. Is it possible to code it so only that tool is 25% rapid and the rest of the program runs at 100%?

[Bruce Gibson]

How about posting the drill cycle out "longhand" and change the G0's to G1's with an appropriate feed rate?

[Programinator]

Ya that would work......but.....is that the only way to do it?

[Tony35]

you could do the same as bruce said but write a drill cycle macro so the program is not so long and you can control the rapid with a feed variable

 

HTH

[Programinator]

Thanks for the input. Looks like the only way is to do it long hand with g1's

 

this is my canned cycle:

 

G83 Z-3.6181 R-.38 K.06 I2.2 J2.14 F7.4

 

Would someone that has a macro for what im trying to do be able to post it out for me. Im not sure how to do a macro.

 

Thanks.

[Tony35]

shawn

i would write the macro for you but i am only working a half day so i dont have the time but if you look in your haas manual it will give you the basics plus look at how the canned cycle is defined in the manual and pass that info to variables and just write out the math functions needed. it sounds harder than it is. if this job is going to be running a while i would use common variables vs local. call up a sub program(for drilling) so you can save this macro for future use all you would have to do is change the variables. G83 is nothing more than a macro that is hidden. i wish we had access to them

 

happy writing

[Tony35]

shawn here is something i found on the web for ya

change as needed for haas and you dont need the alarm logic if you dont want to something to start with

 

%

O9013 (CUSTOM G83 DEEP HOLE CYCLE)

 

(ASSIGN G-CODE G83)

(SET PARAMETER #6053 = 83)

(CALL MACRO DRILLING CYCLE)

(G83 X0.0 Z0.0 W1.0 R0.1 Q0.1 K0.01 F0.008)

(X0. -HOLE LOCATION IN X)

(Z0. -HOLE LOCATION IN Z)

(W1.0 -INCREMENTAL HOLE DEPTH - ALWAYS POSITIVE)

(R0.1 -INCREMENTAL CLEARANCE PLANE AMOUNT - ALWAYS POSITIVE)

(Q0.1 -INCREMENTAL PECK DEPTH - ALWAYS POSITIVE)

(K0.1 -INCREMENTAL RETURN FROM RETRACT CLEARANCE - ALWAYS POSITIVE)

(F0.008 -FEEDRATE)

 

#6=ABS[#6] (FORCE K TO ABSOLUTE VALUE)

#9=ABS[#9] (FORCE F TO ABSOLUTE VALUE)

#17=ABS[#17] (FORCE Q TO ABSOLUTE VALUE)

#18=ABS[#18] (FORCE R TO ABSOLUTE VALUE)

#23=ABS[#23] (FORCE W TO ABSOLUTE VALUE)

#1=[#26+#18] (ASSIGN START POINT W/ R-PLANE TO VARIABLE)

#3=[#26-#23] (ESTABLISH FINAL Z POSITION)

 

(ALARM LOGIC)

IF [#23 EQ 0.0] GOTO 9991 (INVALID W)

IF [#18 EQ 0.0] GOTO 9992 (INVALID R)

IF [#17 EQ 0.0] GOTO 9993 (INVALID Q)

IF [#17 GT #23] GOTO 9993 (INVALID Q)

IF [#6 EQ 0.0] GOTO 9994 (INVALID K)

IF [#6 GT #17] GOTO 9994 (INVALID K)

IF [#9 EQ 0.0] GOTO 9995 (INVALID FEED)

 

G00 Z[#1] (RAPID TO Z START W/ R-PLANE)

G00 X[#24] (RAPID TO X START)

N1000

#4=[#5002-#17] (CHECK IF PECK IS FARTHER THAN FINAL DEPTH)

IF [#4 LE #3] GOTO 2000 (IF PECK IS FARTHER THAN FINAL DEPTH, GOTO N2)

G01 W-[#17] F[#9] (PECK DRILL)

#2=#5002 (STORE CURRENT Z DEPTH)

G00 Z[#1] (RETRACT TO START POINT)

G00 Z[#2+#6] (RETURN FROM RETRACT WITH CLEARANCE K)

GOTO 1000

N2000

#4=#3

G01 Z[#4] F[#9] (DRILL TO FINAL DEPTH)

G00 Z[#1] (RETRACT TO START POINT)

M99

 

 

(ALARMS)

N9991

#3000=1(INVALID W-DEPTH!)

GOTO 9999

 

N9992

#3000=2(INVALID R-PLANE!)

GOTO 9999

 

N9993

#3000=3(INVALID Q-PECK!)

GOTO 9999

 

N9994

#3000=4(INVALID K-RETRACT!)

GOTO 9999

 

N9995

#3000=5(FEED F NOT SPECIFIED!)

GOTO 9999

 

 

N9999

M30

%

[Programinator]

Thanks Tony

[Tony35]

i know it looks confusing just go through it step by step and it will start to make sense

 

good luck

[EazyE]

Probably a little late but might help in the future. Variable #3004 is a variable that overrides certain functions.. I believe if #3004=0 then it will override the feedrate % off setting in the control to on. just be sure to call it again as #3004=2 so it changes back.. Under the variables section in the HAAS manual browse till you find the #3004 there is a list of 1-6 options that this variable controls...

[Programinator]

quote:

---

Probably a little late but might help in the future. Variable #3004 is a variable that overrides certain functions.. I believe if #3004=0 then it will override the feedrate % off setting in the control to on. just be sure to call it again as #3004=2 so it changes back.. Under the variables section in the HAAS manual browse till you find the #3004 there is a list of 1-6 options that this variable controls...

---

I just got done doing it the long way as bruce suggested but i will look at this option tomorrow.

 

Thanks

[Dave Ball]

I don't run a Haas but I think that just turns off/on the buttons on the control panel to prevent operator adjustments, I dont believe it actually shuts off/on rapid movements.

[Programinator]

quote:

---

Probably a little late but might help in the future. Variable #3004 is a variable that overrides certain functions.. I believe if #3004=0 then it will override the feedrate % off setting in the control to on. just be sure to call it again as #3004=2 so it changes back.. Under the variables section in the HAAS manual browse till you find the #3004 there is a list of 1-6 options that this variable controls...

---

I dont see anywhere in the manual for a variable for rapid overide. I do see feedrate but not rapid. Im going to try to ask THE ANSWER MAN

[kunfuzed]

In your control def under Machine Cycles/Mill Drill Cycles uncheck "Peck Drill - Full Retract

 

In the feed options check "Convert Rapid To Maximum Feedrate

 

In your Machine Def under Axis Feedrate Limits/Linear Axis Transverse Rate set Maximum Feed to whatever you want it to feed at.

 

Why doesn't this work? I still get "G0 Z.1" in my longhand.

[kunfuzed]

I thought I had a good idea but couldn't get it to work.

 

In your control def under Machine Cycles/Mill Drill Cycles uncheck "Peck Drill - Full Retract

 

In the feed options check "Convert Rapid To Maximum Feedrate

 

In your Machine Def under Axis Feedrate Limits/Linear Axis Transverse Rate set Maximum Feed to whatever you want it to feed at.

 

Why doesn't this work?

 

 

EDIT: Sorry for the double post.

[Programinator]

sounds like it should work. Thanks for trying

 

I just tried it and it didnt work for me either.

 

[ 12-24-2008, 08:45 AM: Message edited by: Shawn @ All-Tool ]

[kunfuzed]

Yeah, I'd really like to know why that doesn't work.