Broaching on okuma lathe

[DODGERFAN]

Soooo.

This is my first attempt at broaching on our new okuma lb300 ex lathe.

The machine is reading the code with no alarms but it's just not feeding after the approach command. Any ideas?

[jlw™]

Mcode to allow feed move with spindle 0?

[DODGERFAN]

The G50 is a limit for the spindle, without a G50 the machine will alarm out and never get past that line.

[DODGERFAN]

Also the g94 makes it inches per minute so no spindle movement is required. 

[Colin Gilchrist]

No, you need to tell the Okuma that "it is OK to move XYZ while the Spindle is not Turning".

M130 / M131

 

[Colin Gilchrist]

Put the M130 before your S0 / M05.

Put the M131 after the tool completes the motion.

[DODGERFAN]

Thanks Colin, I'll let you know how it works. 

[DODGERFAN]

Nothing changed. I checked those commands and for okuma M130 is a chucking error detecting OFF

the M131 is ON. 

[Colin Gilchrist]

Oh, those are for Mill Machines. You'll need to look in your Programming Manual for the Lathe equivalent.

[Colin Gilchrist]

It might be M807 / M808

M807 - Cutting feed interlock release OFF

M808 - Cutting feed interlock release ON

[DODGERFAN]

I'll try that too.  I know it's gonna be something simple, just not sure what.  LOL....  I'll let you know.

[Colin Gilchrist]

Another one you can try is "M904". That is a "non-modal" M-Code, so it is only active on the line you enter it on. (enter it at the end of your G71 line...)

M904 - Machine mode interlock release

[DODGERFAN]

M808 didn't work. Trying 904 now.

[Metric]

At my company we use :

M5; G94; F(per minus). I think you need to use G1 instead of G71 cannel cycle.

Hope this is work for you.

MDT

[DODGERFAN]

I'm gonna need a drink.....LOL.

I know it can be done, we did it at my last job. 

[crazy^millman]

Does the machine have a C axis? If so have you put the machine in C Axis milling mode to do the broaching?

[DODGERFAN]

Ron,

It has c axis lock, but no milling. I've been able to program it long hand and it does through the motions, but it wants to feed in rapid even with the G94.

[crazy^millman]

This doesn't feed?

G94

G1 Z-1.0 F13.5

If not you need to get a hold of you local apps guys and have them explain what is wrong since that should feed in inches per minute. Unless the Feed needs to be in a different format.

[DODGERFAN]

That is correct ron. 

[mkd]

PM sent

[Colin Gilchrist]

Well, the M-codes go up to 1500. So there are quite a few that "could be it".

Try getting away from CSS.

G97 S0

M5

G71

That should work. Again, you might need to activate C-Axis mode.

[Werktuigbouwer]

In the Okuma control G71 is a canned threading cycle. It will probably not feed because the encoder is not reading the start position. At my company we use just a macro program, something like:

(Broaching program)
N1 (ACTIVATE VARIABLES)
V1 = 1.475 (START VALUE X)
V2 = 0.75 (START VALUE Z)
V3 = 1.6 (END VALUE X)
V4 = -1.0 (END VALUE Z)
V5 = 0.002 (DEPTH OF CUT ON DIAMETER)
V6 = V1 (DEPTH COUNTER)
X20. Z20.
T0101
G50S500
G94
M5
M19
N1111 G00 X=V1 Z=V2
G00 X=V6
G01 X=V6 Z=V4 F13.0 (INSERT FEED HERE)
G00 X=V1
G00 X=V1 Z=V2
IF[V6 EQ V3] N8888
V6 = V6-V5
IF[V6 GT V3] N1111
V6 = V3
GOTO N1111
N8888 G95
X20. Z20.
M2

Be aware that I have not tested this program. This is a derivative of a program that we use, for more complex shapes.

[mkd]

Just a plug for DuMont:

If you buy a broach from them you can get an awesome Macro from them that uses a similar variable setup, as shown above^^^^^