OSP5000LG ERROR WITH DRILLING CYCLES. PLEASE HELP

HI
I have a lb25 lathe
have been using fusion360 to create some programs and have got the programs into the machine but it alarms up at multiple places in the code on the drilling
cycles
its spitting out a g182 xo z-25 etc followed by a G180 to end the cycle but it doesnt like this
G73 also doesnt work
i have tried everything i can think of in the way of drilling cycles
everything seems to alarm
getting quite frustrated now.
i also run an okuma mc4vA mill at work and have never had any issues with this in the 12 years i've used it with cam and inbuilt igf.
it also spits out a G17 which once removed is no issue
am i missing something in the code below ?


(DRILL1)
N31 M1
N32 T050505
(13.5MM DRILL)
N33 M8
N34 G94
N35 G97 S500 M3 M41
N36 G0 X0. Z11.5
N37 G17
N38 G0 Z6.5
N39 G182 X0. Z-25.056 R5. F75.
N40 G180
N41 Z11.5
N42 M9
N43 X9999.
N44 G0 Z9999.

thanks daniel

i am looking at the manual for a osp 5020L/ osp500L-g
G182 Machine Compound Fixed Cycle: boring (it is optional)


G74 Transverse Grooving Compound Fixed Cycle should be your drilling cycle


G74X0.Z-1.250D.375K.150L.375F.006

D=DEPTH OF CUT IN FEED AMOUNT
K= SHIFT AMOUNT IN Z AXIS
L= TOTAL IN FEED FOR WITHDRAWAL

N38 G0 Z6.5
N39 G182 X0. Z-25.056 R5. F75.
if there is no pecking then just use (this looks to be less than 3 times the dia. it may not need pecking)
G01 X0. Z-25.056 F75.


the G17 should be removed as you should be in x/z (g18)

hy guys :)

Quote:

---

its spitting out a g182 xo z-25 etc followed by a G180 to end the cycle but it doesnt like this

---

just like rcs said, g182 is a boring cycle; uses C axis, and M orientation

Quote:

---

G73 also does work

---

it works because g73 = grooving

Quote:

---

i have tried everything i can think of in the way of drilling cycles
everything seems to alarm

---

try g code :
... home position
... t505
... s500 m42 m08 m03 ( m42 is ok for drill o13.5; is it hss ? )
... g00 x0 z6.5
... g01 z-25.056 f<0.15 g95 ( use a lower feed )
... z-25.056+0.3
... g00 z6.5
... home position
* writing all these is done in few seconds, a minute, etc ... maybe 2 days :)

Quote:

---

it also spits out a G17

---

rad comp planes :
... g17 xy
... g18 xz
... g119 cxz

Quote:

---

it also spits out a G17 which once removed is no issue

---

is no issue = code still does not work :) if i may, consider to replace "is no issue" with "is same sh**t"

Quote:

---

am i missing something in the code below ?

---

no, code is just fine ... you are missing the programing manual; pls find it attached

if you will search inside it, you will find all what was discussed : g182 74 73 17, etc

now, you should configure your cam to use the correct g-codes

Quote:

---

i also run an okuma mc4vA mill at work and have never had any issues with this in the 12 years i've used it with cam and inbuilt igf.

---

12 years of cam&igf, without g-code, can't help one to achieve higher control or debug; i have met persons with 10years+ of g-code, and they can easy switch to cam&igf

if you still have time, i will tell you a story : one day, a cam guy, after years of programing, came down into the production area, to ask for a center drill, so to have a clue what is it, because it's cam was always asking for a center drill before drilling

but i believe that you can relax, because i doubt that future machining is about g-codes/ kindly :)

ok thanks ill try that next week and see how it goes.
is there a reason why okuma felt the need to combine drilling and grooving into one cycle option ?
their description in the book is very vague.
thanks again for your assistance,

try g code :
... home position
... t505
... s500 m42 m08 m03 ( m42 is ok for drill o13.5; is it hss ? )
... g00 x0 z6.5
... g01 z-25.056 f<0.15 g95 ( use a lower feed )
... z-25.056+0.3
... g00 z6.5
... home position
* writing all these is done in few seconds, a minute, etc ... maybe 2 days
deadly kitten.

i can read and edit gcode no problem on fanuc and on the 4va
but they dont combine drilling cycles with god knows what else.

writing it out in longer code was the next option as the next cycle is a 13mm hole and over 140mm deep so pecking was required
for that not really necessary for the 13.5 drill.

as for the g73 , cnc cookbook lists it as a peck drilling cycle as well as a roughing canned cycle.

G Code Purpose Peck Retract Bottom of Hole
G73 High-speed Peck Drilling for Shallow Holes

so i tried it also along with g81 g83 etc that the okuma mill uses.

Quote:

---

is there a reason why okuma felt the need to combine drilling and grooving into one cycle option ?

---

hy, off course, both can use same code, because required motions are pretty identical; if you use the code with :
... drill+x_offset_0 it will drill
... face_grooving_tool+x_offset_<>_0 it will groove

Quote:

---

their description in the book is very vague

---

pls ask whatever you feel :)

Quote:

---

as for the g73 , cnc cookbook lists it as a peck drilling cycle as well as a roughing canned cycle.

---

leave that cookbook, i shared for you the programing manual in my last post :) if you would look inside it, you will find "Longitudinal Grooving Fixed Cycle (G73)"

Quote:

---

so i tried it also along with g81 g83 etc that the okuma mill uses

---

aren't you tired of trying ? kindly :)

Yes I was abit sick of trying on that day
I posted this after I'd tried all of those things
I have edited the 2 programs to suit with the g74 now and will test early next week
I do have all the original books for the machine about 10 of them in total
Thanks for the added Okuma file (I did find it rather amusing that the definitions on the cycles are identical to my books from 1980s in 2014 )
Proves they must do their job I just have to get my head around them now.
Thanks Daniel

hy ... i have all the manuals in pdf format, arround 20-25manuals/per single cnc

if i wish to search for something, i use an in-file search, going through all in just few seconds

i sync my pc from work with an externall hdd, so, if i need to write a code, i may write it at home, and when i reach work i may only run it, in order to test it

Quote:

---

is there a reason why okuma felt the need to combine drilling and grooving into one cycle option ?

---

there is much more to this, because many types of operations can be grouped as sharing same motions; depends how you see things :)

a few years ago, i had one operator on a machine, that involved a hole : drill + ream + chamfer, and my code was parametric ... and he told me that i may use same code for all those operations

meanwhile, code extended, being able to take care of particular situation, with minimal edit time; for example, for your deep hole :

Quote:

---

13mm hole and over 140mm deep so pecking was required

---

... z-20 raise_rpm
... z-60 , go_to_z_clearance in rapid , go_back_inside in feed
... z-100 , go_to_z_clearance in rapid , go_back_inside in feed, decrease rpm
... z-125 , go_to_z_clearance in rapid , go_back_inside in feed
... z-140 , decrease rpm to dead_slow, go_to_z_clearance in rapid

is like a rubic cube, for live tools, and is optimized compared to a g-code :
... it avoids delays inside blind holes, by reversing feed direction
... it has all clerances parameterized
... it may reverse the spinning sense, in order to clear the chips
... uses ctr & can handle as many monitoring values as you wish, with less downtime then activating a single monitoring value in the classic style ( if i remember, is 10-20x faster when it comes to vlm** execution time )
... it is monitoring entire motion, including rapids, thus is not using m216

there is more to it, and i will show it one day; until then, it is growing, by being able to handle whatever particular case appears / kindly :)