[TommyCNCGuy]

Hi Guys,

Having a bit of a problem trying to machine a part using just the C axis in a Okuma LB2000 Space Turn lathe with an Okuma OSP P200L control. I have a stationary cutter that is mounted in the turret which I want to move down into the part (while it is at a certain rotation in the spindle) and then I want to rotate the C axis back and forth while moving the turret into the part in the Z axis. This will shave a one sided chamfer on some lugs inside the part. The problem is that unless the spindle is rotating the linear moves are not allowed. Not sure how to disable this spindle interlock. I have designated my M110 to put the machine into C Axis Joint (allow C axis control) but don't know how to get the particular sequence of G or M codes to allow the spindle to rotate back and forth. It will turn the C axis into position in the G00 mode, but once a G01 move is made it just stops. It shows the current rotation, shows that it has a certain rotation it wants to go to, shows the destination it wants to go to but won't move as it is waiting for a code to allow this to happen.

I have attempted to use G140, but that is to be used with a sub spindle, I have tried M153 but that doesn't have any affect. Searching through the book, I can't find any M or G codes that will apply, or appear to apply.

Here is the code so far:

IF[ABS[V1]GT.003]N803
IF[ABS[V2]GT.003]N804
/IF[ABS[V3]GT.01]N805
TLID

G90G0X[0.+V1]Y[0.+V2]T0101
M8


M110
M141
C9.25(ORIENT TO ALLOW BROACH TO PASS THRU BROACHED SLOTS IN THREADS)
Z.5
G0Z.1F100.
()
V4=.035(STOCK AMOUNT TO BE REMOVED)
Z[-.905+.051+V4+V3]F100.




N101
G1Z[-.905+.051+V4+V3]F100.
IF[[V4]LT 0]N102


C[[V5]-5.]F3000.

Z[-.905+.021+V4+V3]F100.
C[V5]F3000.(ORIENT TO START CUTTING)
G4F.1
G1C[[V5]+15.]Z[-.905-.0746+V4+V3]F3000.
G4F.1
V4=V4-.00122
GOTO N101
M109
()




N102
C9.25F3000.(ORIENT TO ALLOW BROACH TO RETRACT THRU BROACHED SLOTS IN THREADS)
G4F.2
V6=V6+1
G1Z1.F100.
()
N999
M9


G0Y7.Z2.C-22.5


M109
()
GOTO N9999
(ERROR MESSAGES)
N803 M0(V1 IS GREATER THAN +-.003)
N804 M0(V1 IS GREATER THAN +-.003)
N805 M0(V3 GREATER THAN +/-.010)


N9999
M30

It stops at the C rotation in the N101 sequence, changing the C value to a numerical value and removing the feedrate, have no affect, does the same thing. Variable V5 is -8.5

Any help or suggestions would be appreciated,

Thanks

Tom

[OkumaWiz]

I don't see a G94 anywhere to switch into feed per minute mode. Is it active?

Best regards,

[fordav11]

to get C to move a small amount forward and back you need to set the rotation direction to +ve or -ve and continually change it from one to the other. if you dont change the direction the C axis will do a full rotation to the next angle position. probably easiest using a loop in user task 2
C axis +ve = M15
C axis -ve = M16

here's a simple broaching example that goes from +2 degrees to 0 then -2 degees and back to 0 then +2 degrees

M16
G1 C2.0 F100
Z-1.0
Z0
C0
Z-1.0
Z0
C-2.0
Z-1.0
Z0
M15
C0
Z-1.0
Z0
C2.0
Z-1.0
Z0
M16
G0 Z10.0
C0
X10.0

etc

[TommyCNCGuy]

I did have a G94 in there. I was screwing around adding and removing things, so this might be a snippet where it wasn't present. I also tried it with and without feed which made no difference. I have added this to the beginning so it is active in my current code (which still doesn't move).. That was one of my first thoughts is that it was stuck on trying to figure the feed but I think it's waiting for an M or G code to disable the spindle interlock before moving and I'm kind of stumped on what that is.

[TommyCNCGuy]

to get C to move a small amount forward and back you need to set the rotation direction to +ve or -ve and continually change it from one to the other. if you dont change the direction the C axis will do a full rotation to the next angle position. probably easiest using a loop in user task 2
C axis +ve = M15
C axis -ve = M16

here's a simple broaching example that goes from +2 degrees to 0 then -2 degees and back to 0 then +2 degrees

M16
G1 C2.0 F100
Z-1.0
Z0
C0
Z-1.0
Z0
C-2.0
Z-1.0
Z0
M15
C0
Z-1.0
Z0
C2.0
Z-1.0
Z0
M16
G0 Z10.0
C0
X10.0

etc

fordav11,

I had tried playing around with M16 and M15 in the beginning also but it didn't seem to make a difference, it didn't move at all, let alone move all the way around. In your code I see with the M16, it turns in the negative direction to 2 degrees, goes into the part 1.0, backs out, then goes to C0. But since M16 is still active doesn't it have to go all the way around in the negative direction to C0. as it is being told to go in the negative direction only? wouldn't a M15 be required after the initial retract back to Z0. and so on?
I will definitely add some directional M codes eventually, I guess but my biggest problem at this point is that I can't get it to move at all as it somehow wants me to disable the spindle interlock that doesn't allow linear moves if the spindle isn't spinning. I was thinking somehow i could use an M Tool type code and give it a bogus spindle speed so it thinks the tool is turning but since this particular tool is not on a live adapter it wouldn't spin but I'm also not sure of the right combo. Ideally I'd like to figure out a G or M code that would disable this interlock.

Thanks

[fordav11]

the code works. it's copied/modfied from one of my working programs that does deburring of a hole using a live tool and only C and Z. my program goes from +6 degrees to -6 degrees then back to +6 degrees while the tool moves small amounts in Z.

try writing a program to do some simple milling using a live tool just cutting air. it should work.
then run it again but with the live tool not spinning and see if it works. thats essentially what you want.
if that doesnt work we can look further.

[budgieW]

You will need the cutting feed interlock M code, take a look in the manual, maybe M807/M808 If the spindle is not running it will not feed without his code

G140 Main spindle selection
M808 Cutting feed interlock release OFF
G91G94
G01Z50F500

blah blah

M807 Cutting feed interlock release ON
G90G95
M02

[fordav11]

here's a video showing the small C axis movement direction changing.
Basically it's.....

M15
Feed to C6.0 (the top edge of the hole)
M16
Feed tiny Z movements through numerous C angles to C-6.0 (the bottom edge of the hole at 180 degrees opposite)
M15
Feed tiny Z movements through numerous C angles back to C6.0
M16
G0 C0 (center cuttter)
X10.0 (get outta there)

that's really all there is to it. Just two M15's and two M16's.

https://www.youtube.com/watch?v=_hCf...58Pf-9lGMdrS8Q

[TommyCNCGuy]

I found out the problem. As budgieW said, I needed to put a M808 and M807 in there to allow the moves while the spindle was not turning. This solved the problem. As fordav11 also mentioned, I also added some directional codes (M15 and M16) to get the part to just turn in small increments. Thanks for the help, of course the Okuma manual doesn't mention the spindle interlock codes, you just to have to know that I suppose!!

Working code:

IF[ABS[V1]GT.003]N803
IF[ABS[V2]GT.003]N804
/IF[ABS[V3]GT.01]N805
TLID

M110
M146
G90G0X[0.+V1]T0101
M8
M15
C9.25(ORIENT TO ALLOW BROACH TO PASS THRU BROACHED SLOTS IN THREADS)
Z.5
M808 (CUTTING FEED INTERLOCK RELEASE ON)
G1G94Z.1F100.
()
V4=.035(STOCK AMOUNT TO BE REMOVED)
G1Z[-.905+.021+V4+V3]F100.


N101
G1Z[-.905+.021+V4+V3]F100.
IF[[V4]LT 0]N102
M16
C[V5]F3000.(ORIENT TO START CUTTING)
G4F.1
M15
G1C[[V5]+11.]Z[-.905-.051+V4+V3]F3000.
G4F.2
V4=V4-.00122
GOTO N101

N102
Z-.895F30
C9.25F3000.(ORIENT TO ALLOW BROACH TO RETRACT THRU BROACHED SLOTS IN THREADS)
G4F.2
G1Z1.F100.
V6=V6+1
G0X20.Z20.

N999
M9
M16
G0C250.
M109
M807(CUTTING FEED INTERLOCK RELEASE OFF)
()
GOTO N9999
(ERROR MESSAGES)
N803 M0(V1 IS GREATER THAN +-.003)
N804 M0(V1 IS GREATER THAN +-.003)
N805 M0(V3 GREATER THAN +/-.010)

N9999
M30

[fordav11]

the M code is listed in the manual but only in the big list of M codes at the back of the programming manual (LE33-013-R5). but unless you know what it's for and how to use it, that listing is not helpful because there's no info on what it does or how to use it and no program example. good one Okuma!

[troutman ae]

You can also try an M960 to avoid missing any M15/M16 codes. M960 is C-axis shortest path.