G83 Peck Drill on Fanuc 18-T

[JerryH]

Having trouble getting this cycle to run, machine keeps giving me a "#10 bad g code) error. Anybody see any problems here?

My tool block:

T1010
S1500 M03
G00 Z.1
G00 X0
G83 Z-3.0 R.100 P0 Q1000 F.006
G00 G80 Z.25
G28 U0
M30

FYI - Parameter 5101, Bit 2 = 1 (I guess this is the parameter that determines if the peck is high speed or regular.)

Thanks!

[APACHE]

GOO XO.OO YO.OO ( LOCATION )
Z.3 R PLANE TO MAVE HOLE TO HOLE
G83 X0.00 Y0.00 Z-00 Q.25 F5. R.1 ( RAPID .1 ABOVE WORK)
G00Z1.
G80
G28Z2. ( WITH ABSOULTE INCODER) OR G91G28Z0.
G49

[JerryH]

Sorry, should have specified this was a lathe program.

[Mitsui Seiki]

I think G80 is "to close " to G83.Put two "blind blocks" between the G83 line and the G80 line.

G83 Z-3.0 R.100 P0 Q1000 F.006
;
;
G00 G80 Z.25

[wganders]

You don't need the "blind blocks", just cancel the drill cycle with the G80 directly after the G83, THEN, move in Z.

[wganders]

The G80 would be in the line immediately after the G83, then after the G80, the next line would be the Z move. My first post was a little confusing.

[cnc-king]

get rid of the P0 or at least assign a value to it for the drill to pause at the bottom of the hole, that is where your error is coming from. had the same problem on a daewoo s2000sy

[theemudracer]

Originally Posted by JerryH Having trouble getting this cycle to run, machine keeps giving me a "#10 bad g code) error. Anybody see any problems here? My tool block: T1010 S1500 M03 G00 Z.1 G00 X0 G83 Z-3.0 R.100 P0 Q1000 F.006 G00 G80 Z.25 G28 U0 M30 FYI - Parameter 5101, Bit 2 = 1 (I guess this is the parameter that determines if the peck is high speed or regular.) Thanks!

No P address is needed.
R is the distance from the start position wich is Z.1
So it will retract to Z.2 with a R.100 with the intial Z set of .1

set R0. and it will use the Z.1 as the retract plane.

let us know what you figure out. I run a 18-iTB lathe my self.

[JMS4287]

Out of curiosity Is by chance the G83 option not turned on....I'll Believe You'll get that same alarm if you don't have that option....???>

[machinemike]

What does your manual say about the alarm? We have a few Tsugami's that don't have enough memory on the backside so we have to change the depth of cut. I'd start messing with the values just to see if it'll run.

[jorgehrr]

I will do it like this:

G83B-.3R.1Q1000F.005
B machine completion point
R distance from zero to approach point (usually .05 or .1 )
Q peck control (not decimal point)
F feed

Cheers

Jorge

[lshingleton]

Try this------i found drilling cycles or can cycles on lathes--always where unreliable so this way you make your own-have a good day

(DRILLING)
G00G28U0
T1000
G00T1010X0.0Z1.0S1500M03
G00Z.1
()
#10=31 (===3.1--IN/.1 TRAVEL)
WHILE[#10GT1]DO1
G01W-0.1F.006
(G04 X1.0) (ENTER DWELL IF NEEDED)
G00W.2
G00W-.2
#10=#10-1
END1
()
G00Z.25
G00G28UO
M30