1. ## Parametric Looping problem

I'm counterboring a .843 dia hole at .490 deep "rough".There is always a hole in these parts that very. In this case the thru hole is .283.The depth finishes at .500 and is constant. So I need a variable that I can change for the thru hole which can be changed and I need to LOOP the last .01 at .002 each pass to create a very sharp edge at the intersection of the bore and the bottom of the .5 face.The boring bar needs to cut up from the inside of the bore to the .843 dia..I've created this loop b4 but for some stupid reason I'm knockin my head against the walls...............Help would be appreciated.....Thx....

2. Is this a fanuc controlled machine?

3. Yes fanuc 21i On a hardinge conquest gt

4. you can use #500 or what ever variable is free for your through hole diameter. you can set the variable in the controller or set the variable in the program(#500=.25.
G0 X#500;
G0 Z____;
G1 X.843;

for the loop you can do this many different ways. I hope this jogs you brain.

(FINISH CYCLE)
#510=-.490(Z START)
#511=.010(FINISH DEPTH)
#512=.002(DEPTH OF CUT)
#513=[#511/#512](MATH FOR # OF PASSES)
#514=0
WHILE[#514LT#513]DO1
#514=[#514+1]
G0X#500
G0Z-[.490+[#514*#512]]
G1X.483
G1Z-.490
END1

G0X#500
G0Z.1

I WORTE THIS ON THE FLY SO THERE MAY BE A MISTAKE PLEASE DOUBLE CHECK ME.

I hope this helps

5. For a simple application such as this, you can even use G94 five times (in this case).
You would need to vary only start X for G94, to suit different initial bores, for which you can use a variable.

The posted macro looks ok, but would not work when the number of passes comes out to be a fractional value (not in this case, of course). And, read G1X.483 as G1X.843.

6. I knew I messed up somewhere. I guess I have never used a G94 before. Is G94 a face turning cycle?

7. Yes.
It has some similarity with G90 cycle.
G90 is used for diameter turning / taper turning.
G94 is used for facing / taper facing.
This is for G-code system A.

8. ## looping macro

Haven't worked much on looping macro but going to today. I've got it to loop but keep getting an error when it goes to retract. Any help?

9. Didn't quite understand that last post. Are you using the macro or the g94?

10. You can even use G94 inside a macro.
My advice is, first try to master the canned cycles. In many cases, these would serve the purpose, and the program would be simple. Macro programming should be the next step.

11. Originally Posted by gtrrpa
Haven't worked much on looping macro but going to today. I've got it to loop but keep getting an error when it goes to retract. Any help?
Can you tell us the alarm number and possible post the code in which you are getting the alarm??

Stevo

12. ## Looping program

Sorry guys,My 1st statement was wrong. I'm not using a Macro (G65) I'm trying to use a looping program like houstonsamuel wrote. Sorry, I'm still having problems with having it retract? Hmmmmm I'll send you alarm and program...Thanks all

Page 1 of 2 12 Last