Okuma LB25 program

[Fox Trott]

Hey everyone,
I am learning how to run a LB25 Okuma lathe and need a little help. I don't have much machining experience and am trying my best.
I need to make a basic program for drilling and tapping blind holes into rod ends. The controller I have is a 5020L
What I want to do is spot drill a shallow countersink, drill 1.00" with 27/64 bit, then tap 0.75" deep with a 0.50 NC tap

Any help would be greatly appreciated

-Jackson

 

[Booze Daily]

Do you have any other programs that you could use as a reference?

 

[Fox Trott]

The memory ran out on the machine, other machinist tried to clean it up and it deleted all the files. Machinist left this week so I'm trying to middle through

 

[Booze Daily]

N1 (Spot Drill)
T010101
G97 S1000 M3
G0 X0 Z.1 M8
G1 Z-.1 F.005
G0 Z.1
X20 Z20
M1

N3 (27/64 Drill)
T030303
G97 S600 M3
G0 X0 Z.1 M8
G74 X0 Z-1.14 L.1 D.1 F.005
G0 Z.1
X20 Z20
M1
N5 (1/2-13 Tap)
T050505
G97 S100 M3
G0 X0 Z.1 M8
G77 X0 Z-.9 F.0769
G0 Z.1
X20 Z20
M30

Go slow.

 

[nscele]

Was beaten to it!

Here is a sample of the spot drill operation
G50 S2500
M90
G0 X280 Z150
N0100 (T8 SPOT DRILL)
G97 S2000
G0 X0 Z5 T080808 M3 M8 M66 S2000
G0 Z1
G74 X0 Z-5.0 D7 L7 F.08
G0 X100 Z80

 

[Booze Daily]

First line should be G50 S1000

There’s more to running a lathe than the code.

Be safe.

 

[plastikdreams]

In before the "I ran the drill and turret I to the part" post

 

[nscele]

If you're still learning loose the M66 as well!

 

[bradleyk]

Don't forget gear selection... M41 and M42. If M41 is active and you program S1000 without an M42, you won't be getting up to 1000 rpm.
I'd agree with losing M66. Your machine may not even have that option (cycle time reduction feature).

 

[DouglasJRizzo]

Here's how I program mine with a floating holder:

G0 G97 X20. Z20. F.008 S750 T0101 M3 M8 M42 M86
X0 Z.15
G1 Z-.43
G4 F1.
G0Z20.
X0 Z.15 S600 T0303 M87
G74 X0 Z-1. D.25 L.25 F.008
G0 Z20. M5
X0 Z.25 S250 T0505 M3 M41
G31 Z-.75 F.0769
M5
M4
G31 Z.25 F.0769
G0 X20. Z20. M5 M9
M2
%

 

[Fox Trott]

So the spot drill and the pecking drill work well, the only problem I am running into is the tapping. I need to feed in, reverse chuck, and retract

 

[Fox Trott]

Should state that I'm using a fixed tap, not a tapping "clutch" holder

 

[DouglasJRizzo]

@Fox Trott Yes, sorry, my error.

When tapping -
G97S200M3
X0Z.25
G31 Z-.75 F.0769M5
G31 Z.25 F.0769M4
M5

Try this cutting air first.

 

[camhead420]

I have an Okuma, never had to tap on it yet.
What's up with the M5 on the first line?

 

[DouglasJRizzo]

On many OSP, the M code is executed after the rest of the line has completed.
So, On my OSP5000, the spindle would stop once the tool has gone to the bottom of the bore.

 

[nscele]

Here is the code I use for tapping an M10 x 1.5 thread, 20mm deep.
N0400 (T7 M10 X 1.5 FORM TAP)
G97 S315
G0 X0 Z4 T070707 S315 M3 M8 M66
G77 X0 Z-20 F1.5
G0 X100 Z100