Okuma drill cycle

[Camdude®]

Okumas gurus,

here's my dilemma.

part has a C'Bore 2.25 deep

part needs to be drilled 3.5 deep

i would like the drill to start at a depth of 2.15 deep and peck at .05" while retracting up to Z.1 for chip clearance. i am using the Okuma G74 drill cycle but cannot get the retract value to go to Z.1.

Here is the code:

N5 G50 X20. Z20.

N10 T0101

N15 G97 S1279 M03 M41

N20 G0 X0. Z.1 M08

N25 Z-2.15

N30 G74 X0. Z-3.25 D.05 L.1 E.13 F.003

N35 G0 Z.1

N40 M09

N45 G0 X20. Z20.

N50 M05

N55 M02

 

the problem i am having is that the drill is only retracting by the "L" value instead of completely clearing the hole.

The programming manual also has a "DA" value.

is this value used to retract the tool back to the initial retract plane in front of the part.

BTW it is a lathe part

[metalmilita]

This is what i do in those situations.

 

G1 Z-2.15 F20.

G0 Z.1

Z-2.05

G1 Z-2.25 F5.

G0 Z.1

Z-2.15

G1 Z-2.35

G0 Z.1

Z-2.25

G1 Z-2.45

G0 Z.1

Z-2.35

G1 Z-2.55

G0 Z.1

Z-2.45

G1 Z-2.65

G0 Z.1

Z-2.55

G1 Z-2.75

G0 Z.1

Z-2.65

G1 Z-2.85

G0 Z.1

Z-2.75

G1 Z-2.95

G0 Z.1

Z-2.85

G1 Z-3.05

G0 Z.1

Z-2.95

G1 Z-3.15

G0 Z.1

Z-3.05

G1 Z-3.25

G0 Z.1

Z-3.15

G1 Z-3.35

G0 Z.1

Z-3.25

G1 Z-3.45

G0 Z.1

Z-3.35

G1 Z-3.5

G0 Z.1

M5

M30

 

HTH

[Camdude®]

that's what i wound up doing,

but there has to be better way!

[Rick Henrickson 65]

Camdude there is a better way it is called change of rough cut conditions you can use DA DB DC etc I do not have my cheat notes here at work but I do have them at home

 

the line gets to long I remember and you have to use a & sign and continue the line

 

this works on drilling, grooving

[Rick Henrickson 65]

are you using IGF to post your code?

[Camdude®]

Rick, don't know about IGF but my Machinist says he uses it a the machine when doing MDI. i'll check with him tomorrow as they leave at 3:00 our time.

[Rick Henrickson 65]

I will get the change in rough cut conditions notes and put them up here tomorrow

[Camdude®]

Rick, thanks for pulling my bacon outta da fire!

[Avs_Fan]

Here is a generic format I use for Okuma lathe. I think it will do exactly what you want.

 

N__(_/_" DRILL X/Z=0 P=0)

G97 S___ T___ M3M8M42 P__

G0 X0 Z_._

G74 X0 Z_._ D._ L._ DA=.01 K0 E.1 F.00_

G0 Z_._

X20. Z20. M1

[*> THE FOLLOWING ARE OMISSABLE: L._ DA=.01 K0 E.1 <*]

[*> "L" RETRACT,"DA=" RETURN,"K" SHIFT,"E" DWELL <*]

[Avs_Fan]

Carrying this 1 step further, change your code to the example below.

 

"Original Code"

N5 G50 X20. Z20.

N10 T0101

N15 G97 S1279 M03 M41

N20 G0 X0. Z.1 M08

N25 Z-2.15

N30 G74 X0. Z-3.25 D.05 L.1 E.13 F.003

N35 G0 Z.1

N40 M09

N45 G0 X20. Z20.

N50 M05

N55 M02

 

"New Code"

N5 G50 X20. Z20.

N10 T0101

N15 G97 S1279 M03 M41

N20 G0 X0. Z.1 M08

(N25 Z-2.15)>>>>>>>>>>>>>>>>>> Delete this line

N30 G74X0.Z-3.25D.05L.1K2.25DA=.01E.13F.003(Edit as shown)

N35 G0 Z.1

N40 M09

N45 G0 X20. Z20.

N50 M05

N55 M02

 

This will start at Z.1, shift in to Z-2.15, peck .05, retract .01, peck another .05, then retract to Z.1, rapid back in within .01 of the previous depth, & then repeat until Z-3.25 is reached. Then dwells for .13 second (?) & retracts to Z.1 & goes home.

[Camdude®]

Avs_Fan,

that cycle worked great thanks for the help. now i can configure my post to do it for me.

[Avs_Fan]

You're welcome.

I've received a lot of help from this forum. Glad I could give a little back.

[DODGERFAN]

Hey guys,   Can someone post a sample of a drill program with a dwell?

Thanks.