[Edster]

Our lathe was installed the other day, I was wondering if anyone would post a sample program so I can get a jump start. Training won't be scheduled untll sometime after the IMTS show, and I'd like to play with the machine a little so I have questions for the apps guy. Btw, it's a captain L370bbmw w/osp200p control. I just need something basic so I can see the start/end lines, tool call, etc., maybe something with a slot so I can see the live tool codes. Thanks in advance

[littlerob]

G90GOX50.Z50.T0202M3M8G97S500
GOX4.0Z.1(START POINT)
G96S800
G85N1OOD.1U.05W.005F.015(ROUGH BAR TURNING CYCLE)
N100G81(CALL START OF A FINISH PASS)
G0X-.064
G1 Z0.0F.005(THIS IS WHERE YOU CHANGE YOUR FEED RATE FOR FINISH, IF YOU ARE USING THE SAME TOOL).
X3.5
X3.5.Z-.25(.25 CHAMFER)
Z-2.5
X4.
G80(CANCEL CANNED CYCLE)
G87N100(END OF ROUGH SHAPE)
G0Z.1
X50.Z50.
M2




The thing to get used to is that the the codes have to be in the right order or the control doesn't like it. Especially if your fat fingering the code in just to see what happens. I.E. G87N100 as apposed to N100G87, just because they are in the same block does not necessarily mean they will be interpreted mnemonically, hope that helps, Robert.

[throttle_jockey]

G81 does not call a "finish pass", G81 calls "logitudinal shape design", yes it's the net profile of what you're after but it's certainly not a finish pass.

[throttle_jockey]

Not only that but why wouldn't you want to run cutter comp if this is a "finish pass", G41 or G42? Facing up or down, turning ID towards the spindle, or turining OD towards the spindle being the latter, where are you going, what are you trying to do?

[littlerob]

G81 does not call a "finish pass", G81 calls "logitudinal shape design", yes it's the net profile of what you're after but it's certainly not a finish pass.

That is absolutely correct, my bad, G80 calls the finish pass and G87n### cancels the rough cycle. Robert

[throttle_jockey]

"That is absolutely correct, my bad, G80 calls the finish pass and G87n### cancels the rough cycle." Robert


Mmm, no. G80 is "end of shape design", and you don't need a line number to end the shape, G80 can be on a line by itself, i.e.

G40
G80
G0

[slavetothemetal]

Isn't the G85 a rough cycle, and a G87 a finish cycle, with the N100 designating where the path definition begins?

[littlerob]

This guy (not an Okuma guy) is trying to get up and running, thats all, if you want to nit pick my control definitions do it with a P.M. If you can tell me the code I posted won't run the machine and make a part. than I am done arguing. By the way there is a little button in the bottom right side of my post that says "quote" so you can "quote" my post, instead of writing it out. Robert

[throttle_jockey]

This guy (not an Okuma guy) is trying to get up and running, thats all, if you want to nit pick my control definitions do it with a P.M. If you can tell me the code I posted won't run the machine and make a part. than I am done arguing. By the way there is a little button in the bottom right side of my post that says "quote" so you can "quote" my post, instead of writing it out. Robert

It's called copy and paste, but clearly you'll like this better.
Robert I'm sorry but you've obviously got little to no experience programming Okumas.
While I'm not trying to "own" you I am concerned with safe programming. Things like G50 (spindle max rpm), knowing when to use G97 instead of G96 (constant RPM vs. constant surface speed). Yes your code will make a part, will it make a good part? What cutter radius are you using? If you're not using cutter comp and you change your tool nose radius then what happens? Do you want to plunge rough the part, using G81 instead of G82, transverse or longitudinal shape design, remember this comes directly after the G85, G87 line? Or more plainly, do you want to turn an OD toward the chuck/away from the chuck, or face the material off in and X-/X+ move?
Like I said man, I'm not trying to wind you up, you're just upset because I pointed out your mistakes.

[throttle_jockey]

The lines that begin with *( I've added to littlerob's original post. This is strictly for educational purposes and in no way is inteneded to upset anyone.


G90GOX50.Z50.
*(G50 S????)(SPINDLE MAXIMUM RPM)
*(ALWAYS PUT YOUR ESCAPE MOVE ON A LINE BY ITSELF)
T0202M3M8G97S500
*(SIX DIGIT TOOL OFFSET IF YOU WANT TO USE CUTTER COMP i.e. T020202, DESIGNATING RADIUS, TOOL AND OFFSET)
GOX4.0Z.1(START POINT)
G96S800
*(WITH G96S800 AND NO G50 COMMAND THE MACHINE WILL HIT IT'S MAXIMUM MACHINE RPM BECAUSE YOU'RE GOING TO X-.064)
*(DANGEROUS)
G85N1OOD.1U.05W.005F.015(ROUGH BAR TURNING CYCLE)
*(D=depth of cut, diametral)
*(U=finish stock allowance in the X axis, no sign change for turning/boring)
*(W=finish stock allowance in the Z axis, no sign change for back turning/ forward turning)
*(F=roughing feedrate, can be change in the middle of the turning cycle by using $G84 XA=, ZA=, DA=, FA=, XA being the diameter at which to change cutting conditions, ZA, being the Z axis location to change cutting conditions, DA is the new depth of cut, FA is the new feed rate. These conditions can be changed twice in the rough bar turning cycle by adding $G84 XB, ZB, FB, DB. If any of the commands are omitted there are no change in cutting conditions for that specification, i.e. omit DA, no change in depth of cut, omit FA, no change in feed rate.)
N100G81(CALL START OF A FINISH PASS)
*(START OF LONGITUDINAL SHAPE DESIGN)
G0X-.064
G1 Z0.0F.005(THIS IS WHERE YOU CHANGE YOUR FEED RATE FOR FINISH, IF YOU ARE USING THE SAME TOOL).
X3.5
X3.5.Z-.25(.25 CHAMFER)
*(GOING FROM A 3.5" DIAMETER TO A 3.5" DIAMETER WILL NOT MAKE A CHAMFER)
*(YOU COULD HAVE SAID "G75 X3.5 L-.25")
*(G75 AUTOMATIC CHAMFER G76 AUTOMATIC RADIUS)
*(ONLY WORKS TO 2 TANGENT FEATURES, BUT DO NOT HAVE TO BE 90 DEGREES TO EACH OTHER)
Z-2.5
X4.
G80(CANCEL CANNED CYCLE)
*(END OF SHAPE DESIGN)
G87N100(END OF ROUGH SHAPE)
*(G87 CALL OF FINISH TURNING CYCLE)
*(YOU SHOULD ALSO HAVE YOUR X AXIS START POINT ON THE G0 LINE BELOW)
*(G0X4.Z.1G97S???)
Note: most Okuma turning centers will return to cutting cycle start point after the G80 line but it is parametrically drive. That is to say that if you turn off that parameter or it's off when you get the machine it will go where you tell it directly from the last cut in the G85/G87 cycle.
G0Z.1
X50.Z50.
M2


Don't take it the wrong way, learn from it.

[Edster]

Thanks to the both of you for the sample programs :cheers:

Sorry it took so long to reply, we were at the IMTS show fri, and sat. Sat I visited the okuma booth and the tech guy told me our training was scheduled on monday and tues. I guess I missed the email friday Anyway my head has been spinning the last week with everything that was going on.

I know how to program a lathe, but I've never used an okuma, or a lathe with live tooling or a sub before. There are definatly some programming differences with the okuma.

Anyway does okuma use u and w for an incremental move? I'm have a feeling they don't, especially since the sub spindle axis is w. It's probably not that big a deal to use g90/91 but I've gotten used to the u/w.

It's also strange that the machine coordinates are listed in the 900" range. The parameters have the stroke limits for z as 980-960 or something like that. It seems more cornfusing than it should be.

[AppsMan]

Okuma lathes use G90/G91 instead if U and W for incremental move. For the Z offset most machine tool manufacturers reset their encoders back to zero on full retract, Okuma does not. I am not sure why, but its been this way forever. Okuma's can be changed so you can read a zero, but have your machine tool distributor do it for safety reasons. If you look at your systems parameters page you will see a Z- machine limit and Z+ machine limit. This tells you the starting and finishing (stroke) postions of the turret. The new Okuma technically do not have a home position, just system stroke limits. Many of the Fanuc and Okuma codes are the the same but the biggest exception is the Lap or Canned cycles. Fanuc canned cycles tend to use radial dimensions for depths of cut and finish allowances and Okuma tend to use diametrical values. A friend of mine runs an Okuma site that has information that may be helpful as well. http://www.theinventionzone.com/