[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]

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

[g-codeguy]

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!

What machine are you running this on? Have you ever run a Hardinge lathe? Hardinge gives you a deep drilling subprogram that is excellent. Don't tell Hardinge Brothers, but I use it on all our lathes with Fanuc controls.

Drilling operation would look like this:

T1010S1500M3
G0X0Z.5M8
G65P9136K-2.375B.02F.006W.5C.2A.2
G28U0M9
M30

K= Z-axis final depth
B= distance drill rapids to from previous cut
F pretty self explanatory
W= depth of first cut
C= minimum DOC (until last one)
A = dwell at retract point (Z.5)

So above example would drill to Z-.5 on first pass, and rapid to Z.5, dwell .2 second, rapid to Z-.48, and drill at feed rate, etc. This program increments from .5 DOC to .2 DOC as determined by the 9136 program.

Say you had previously drilled a larger hole .6 deep, or were running a casting with a counter bore that was .6 deep. You would add a Z-.6 at the end. The drill would rapid to Z-.58 before feeding.

Course you need the 9136 program! Sound interesting? Would you like to try it? PM me if you do.

[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) -Any macro number can be used
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

[cinomarra]

try this

T1010
S1500 M3
G0 Z.100
X0.0
G83 Z-30000 R-00500 Q01000 F.006
G80
G0 Z.25
G28 U0.
M30

Z-30000 IS 3" TOTAL DEPTH
R-00500 IS .050" FROM INITIAL Z START POINT
Q01000 .100" PECK DEPTH

[g-codeguy]

I work in a job shop. Time is money. Seconds matter. Drilling is one place that can save time. Which is why we use a lot of carbide drills for smaller holes and insert drills for the larger ones. Sure we still use spade, HSS, and Cobalt drills. Insert drills are expensive. Tougher materials usually get a spade drill. Long parts get a spade drill if size permits. Since our parts are usually small, quite often I can avoid pecking small holes in short parts by using a carbide drill. Long, small diameter holes get an HSS or Cobalt drill.

Don't know what drill cycle programs the other gentleman has used, but I've been running the Hardinge deep drill cycle on Hardinge, Daewoo, Mori Seiki, Takisawa, and Nakamura Tome lathes for at least 20 years with never a problem. At least not one that could be blamed on the program.

I know your drill is a reasonable size from the feedrate. Pecking every .1 is a waste of time. Not if there is another alternative. I NEVER use this type of cycle unless it is my only choice, such as on a machine that doesn't have Macro B.

However, to each his own. Personally I enjoy writing programs and subroutines with variables. Just not going to waste my time on a deep drill cycle when there is already one in the control that works great.

[lshingleton]

The place i work at has 270 active cnc in one facility and thers 37 facilitys-i also have been doing this since 1985-Both cnc and robotics--------i suggest the program above because every time i go to a machine more than 5 yrs old someone has lost he parameters somehow and canned cycles dont work anymore and i spend half of a day trying to fix them------the program can be used on any machine and can be customised to do what you want not what some machine builder trys to sell there latest and greatest programming software has put in it -i absoluty cannot stand working with easy nc fanuc-converstional brother programs or mazak --what a was of time and money
I do agree that a peck cycle should be at least diameter value of the drill and high speed pecking cycles for small tools---robo drills are awesome at these
Have a great day

[g-codeguy]

every time i go to a machine more than 5 yrs old someone has lost he parameters somehow and canned cycles dont work anymore

Whoa!! Sounds like a personnel problem. Better start (chair) a few. We are a small job shop. 29 cnc lathes, 2 programmers. Mills are handled by a couple other guys. We both also do a lot of set-ups. No one but me changes any parameters in the lathes. Don't think the other programmer knows enough about them to try changing one. I don't make any drastic changes. Just a few simple ones, mostly for programming purposes, and to put subroutines in the M-call and G-call parameters.

The deep drill cycle is a protected 9000 program. Not sure what parameter would affect a G65 call. No operator or set-up man should be turning off the protection and deleting, or changing, a 9000 program. Otherwise (chair) (chair) . Same thing for parameters. A big no-no.

One thing we try to do is download the parameters and ladder info on all our new machines in case something happens to the machine.

I started here in May 1985. Never have used a conversational program, tho our only Okuma has the capability. All manual programming at first, but we have had Mastercam for quite a few years. I use it as a supplement for my manual programming. Use the G75 groove, and G74 face groove only when I need to break up the chips. Otherwise the G76 threading cycle and the aforementioned deep drill cycle were the only canned cycles I used.

Lately I have been making much more use of the G71 rough turning cycle so that I only have to write one program for a part instead of 4 or 5 because of using different size material. I use another G65 call to figure DOC, feedrate, and set such things as maximum RPM and SFM.

Where do you work that has that many machines? China? I work in NJ. Our shop use to be small, but is now considered one of the bigger ones. Why? Because any shop of size move out-of-state or out-of-the-country.

EDIT: Currently our oldest cnc lathe is about 20 years old. Nothing wrong with the parameters, or my 9000 programs I put in it.

[lshingleton]

HI G-code guy
I work just north of the border for the second largest automotive supplier
I am usually the guy they send in to make very large problems disappear
You are totally correct on the canned cycles----to me and yourself with lots of years we can get around these issues but to most new people they struggle and people like us are getting fewer every year
When a shop is smaller and controled well with manufacturing tecs your procedures are right on------get the machines downloaded when new and keep backups and keep them at the machine with a disc in the control panel
To give you a scope of the size of this company we have 130 toyoda cnc horz-mills in one faciltiy about 50 makino 55/88s and 150 mazak and okuma howa lathes----- controls ;ages of machines i cant even remember the number anymore
I find this an interesting site and always willing to pass on information to help people and learn some things on here to
Whatever floats you boat as the irish say
Have a good week guys and hope your problem goes away

[I_flungdung]

I peck drill on a Nakamura TW-20 on a cast round surface using HSS and it works great!