Need Help!- mori SL-15 canned cycle

[Prospot]

we have a mori Sl-15 w/Fanuc 10t control there is no option for G83
is there any way to use G74 and have full retract out of the hole?
or does anyone know what pram it is to turn on the option for G83
Thanks Sam

[littlerob]

It is an impossibility that the control won't support G83.

What is happening when you try to use it? Alarm? Sitting? What function are you trying to use it for? C axis drill or lathe drill?

[dcoupar]

Originally Posted by littlerob It is an impossibility that the control won't support G83. What is happening when you try to use it? Alarm? Sitting? What function are you trying to use it for? C axis drill or lathe drill?

Why is it an impossibility? G83 was an option, and Mori didn't include it with the machines.

[dcoupar]

Originally Posted by Prospot we have a mori Sl-15 w/Fanuc 10t control there is no option for G83 is there any way to use G74 and have full retract out of the hole? or does anyone know what pram it is to turn on the option for G83 Thanks Sam

The only parameter I can find for G74 is 6217 (Return amount). Could you do it with a coolant feeding drill?

[littlerob]

HUH? No peck drilling? Sorry I was wrong.

Robert

http://www.cnczone.com/vb...cycles-152872/

[chucker]

Here is a link to a custom macro drill cycle that could help you do the same thing.

CUTTING TOOL ENGINEERING Plus | Pecking Order

[dcoupar]

Originally Posted by chucker Here is a link to a custom macro drill cycle that could help you do the same thing. CUTTING TOOL ENGINEERING Plus | Pecking Order

Most of those old Mori's didn't have the Custom Macro option turned on either.

[g-codeguy]

Originally Posted by dcoupar Most of those old Mori's didn't have the Custom Macro option turned on either.

But the good thing about being "old" is that they can be turned on. Not that I am advocating it. Fanuc needs to make money too!

[Perfect Circle]

This is what I came up with for a full retract.
Hope it helps you in some way.
%
O00001 ( FANUC 10T)
N01 G18 G20 G40 G80 G90 G98
N02 G00 G28 U0. W0.
(JOB 1 DRILLING CYCLE )
N03 T0707
N04 M01
N05 G50 S400
N06 G97 M04
N07 G54 X0. Z.1 M08
N08 G97 S400
(DRILL FACE - G74)
N09 G74 X0. Z-3. I0. K.2 F.01
N10 G40
N11 Z5.
N13 T0700
N16 M09
N17 M05
N18 G28 U0. W0.
N19 M30
%

[g-codeguy]

Originally Posted by Perfect Circle This is what I came up with for a full retract. Hope it helps you in some way. % O00001 ( FANUC 10T) N01 G18 G20 G40 G80 G90 G98 N02 G00 G28 U0. W0. (JOB 1 DRILLING CYCLE ) N03 T0707 N04 M01 N05 G50 S400 N06 G97 M04 N07 G54 X0. Z.1 M08 N08 G97 S400 (DRILL FACE - G74) N09 G74 X0. Z-3. I0. K.2 F.01 N10 G40 N11 Z5. N13 T0700 N16 M09 N17 M05 N18 G28 U0. W0. N19 M30 %

See post #4 by Mr. Coupar. G74 is not a full retract cycle unless you want to change parameter 6217 for every drill cycle.

[Perfect Circle]

Aye ...well I guess that param. is changed on my control, works for me Sorry.

[g-codeguy]

Originally Posted by Perfect Circle Aye ...well I guess that param. is changed on my control, works for me Sorry.

No need to apologize to me. If it works for you, then great. I'm not about to call you a liar. I don't know a tenth of what some of these guys know. What machine/control are you using? We have OT, 6T, 10T, 16TT, 18T & 21i-T controls on Hardinge, Mori, Daewoo, Takisawa, and Nakamura Tome lathes and it doesn't fully retract on any of them. How far does the tool clear the part on retraction? Is it always the same distance in front of the face? As I understand it, I would have to change that parameter for every drill cycle that used a different drill depth because it is a fixed amount.

I almost never use a G74 for anything other than a chip break cycle for face grooves. I use the deep drill cycle that comes in Hardinge lathes in all our Fanuc controlled lathes. Well...with a few personal modifications of my own.

EDIT: I notice you use a single block call. I assume your machine is an older one. All ours but one use the 2-block call. It is an older Mori Seiki. On 16i-/18i-TA controls the retract parameter for the G74 cycle is 5139. This is why it is critical to know your machine well before attempting to change any parameters. You could wind up in deep doodoo otherwise.