Drilling G83 help please!

[JoeTall69]

Hi Guys,

I am trying to run a test part with a drill followed by inside bore, the drill cycle gets the bit to the front face of the piece, then skips to the end of the cycle,
it then skips the boring cycle, and goes straight to the next cycle.

Anyone see what i'm doing wrong?#

(Okuma OSP U10L)

(DRILL3)
N103 M1
N104 T080808
N105 M8
N106 G94
N107 G97 S3000 M3 M42
N108 G0 X0. Z15.
N109 Z5.
N110 G83 X0. Z-38. R0. Q1. P300. F300. L38.
N111 Z15.
N112 G97 S3000 M3 M42
N114 M9
N115 X200.
N116 G0 Z200.

(PROFILE ROUGHING3)
N117 M1
N118 T060606
N119 M8
N120 G95
N121 G97 S3000 M3 M41
N122 G0 X0. Z5.
N123 G50 S3000
N124 G96 S200 M3 M41
N125 G0 Z-1.5
N126 X13.
N127 G85 NAT4 D1. U-0.2 W0.1 F0.5
NAT4 G81
N128 G0 X23. Z-1.5
N129 G1 Z-2.
N130 X22. Z-2.5
N131 Z-9.
N132 X14.
N133 G80
N134 G0 X0. Z-1.5
N135 Z5.
N137 G97 S3000 M3 M41
N138 M9
N139 X200.
N140 G0 Z200.

Similar Threads:

• solidcam naming drilling geometry to drilling radius automatically
• Drilling using a Gun Drilling tool on HBM
• Need Help!- G87 wrap drilling or cross drilling
• Need Help!- Spot Drilling/Center Drilling Steel 55 HRC
• drilling and drilling cycles tutorial

[Prayer]

Maybe you should try g80 after drilling cycle. But not sure, not much of a okuma-guy

[JoeTall69]

Thanks for that - G80 got it to go to the IB cycle after, so one prob solved.
Still not actually running the drilling cycle past getting to X0 Z5

[deadlykitten]

hy joe, if you wish to customize your post, you need good working codes, so to use them as a reference

if you wish, i will provide you samples for drilling, id boring and id finishing, and whatever else, general, or on a specific part pls follow this link for the programming manual ( https://we.tl/t-gQmeES0Z25 ), but i recomand you to build your post from a good code, that i will gladly share, then searching portions of code through the manuals, which is time consuming

it's easier to build from a good code, than sharing and hoping that someone will spot an error; debugging a code is more mind demanding than rewriting it

in most cases when someone complains about a machine not performing as expected, i always re-write the code / kindly

[JoeTall69]

That would be amazing! Im struggling with the Okuma turning post in Fusion spitting out crap code TBH, i have to re-write sections on every program.
Happy to pay for a re-write too :-)

[deadlykitten]

ok, tomorrow morning, i will send you some igf generated codes, that are really close to what okuma official codes looks like

until then, think what you need, maybe share a drawing, demand whatever operations, etc / kindly

[deadlykitten]

hy , pls check attached

there may be required some minimal modifications, since the code is for a newer machine

really, should be minimal, since okuma codes are tough build, with almost none timeline changes

[broby]

Hi Guys,

I am trying to run a test part with a drill followed by inside bore, the drill cycle gets the bit to the front face of the piece, then skips to the end of the cycle,
it then skips the boring cycle, and goes straight to the next cycle.

Anyone see what i'm doing wrong?#

(Okuma OSP U10L)

(DRILL3)
N103 M1
N104 T080808
N105 M8
N106 G94
N107 G97 S3000 M3 M42
N108 G0 X0. Z15.
N109 Z5.
N110 G83 X0. Z-38. R0. Q1. P300. F300. L38.

Need G0 or G80 here


N111 Z15.
N112 G97 S3000 M3 M42
N114 M9
N115 X200.
N116 G0 Z200.

(PROFILE ROUGHING3)
N117 M1
N118 T060606
N119 M8
N120 G95
N121 G97 S3000 M3 M41

The X value on this line (N122) needs to be your hole size, not the centre of the job.
N122 G0 X0. Z5.
N123 G50 S3000
N124 G96 S200 M3 M41
N125 G0 Z-1.5
N126 X13.

Finish allowances need to be Positive values, not negative values, even for ID operations.
N127 G85 NAT4 D1. U-0.2 W0.1 F0.5

NAT4 G81
N128 G0 X23. Z-1.5
N129 G1 Z-2.
N130 X22. Z-2.5
N131 Z-9.
N132 X14.
N133 G80

X value on here should be the same as on N122,
Machine will ALWAYS return to the start point on X and Z when ROUGHING, not when finishing though.
So leaving the X0 here would make the machine return to the roughing start point and then rapid to X0, probably scaring the crap out of the operator.
N134 G0 X0. Z-1.5
N135 Z5.
N137 G97 S3000 M3 M41
N138 M9
N139 X200.
N140 G0 Z200.

Hope these suggestions help.
Brian.

[OkumaWiz]

It looks like the bulk of the post issues are that there is no " cancel commands" after an operation, ie; G00 or G80 when finished. Get the post fixed using the IGF code kitty sent as a reference and you'll save yourself a lot of time and effort.

Broby did a nice job explaining where things went wrong for you. (he always does, so trust him...)

Start points and reference points are very important to the Okuma control. They determine what direction a roughing cycle is going and where the depth of cut starts from, so pay attention when choosing them. Clearances are also determined by them inside a canned cycle, so you want to be sure they are in the right places. For example when turning an OD, your reference point should be > or = your start point in Z and definitely < in X. If the Z is = it will rapid down, but if it is not and is < then it will feed down.

BTW you do not need to go to G94 for drilling (or live tooling) if you do not want to. The control can feed in IPR using the spindle or live tool rpm for the calculation.

Best regards,