LB-15II question...Lengthy, I know...

[gene rhodes]

Ok here's my question.... we have recently began to venture into a new realm of existance in our company....live tooling. Until now, the only use they got out of this feature was a single vetical drill thru on a cylindrical part.
We have since purchased featurecam in our shop and I have been able to prove to be able to radially locate holes in a pattern...after initializing a new post for the machine... it sat for over 4 years w/o power and lost all its memory...
now I'm stuck. My question is, if I'm able to drill, index, drill, index, etc., then should I not be able to do these operations simultaneously?? Like, say , mill a flat on the OD of a tube?? My co-workers seem to think I'm crazy here and I'm dead set on proving them wrong. As I have said, so far I have been successful in producing a usable prototype involving your basic turn lathe ops ( turn, bore, thread, etc.) and put a 10 hole drill pattern on the face.
Now I want to see if it will interpolate, circular or horizontal it doesn't matter, by using turret motion in conjunction with spindle movement.
Featurecam outputs this idea w/o errors but the machine doesn't like the G101,102, or 103 codes saying that they're invalid. I can only guess that this is a parameter issue but who knows, I've been wrong before!
Any advice, contacts, anything... would be greatly appreciated. This feature in our shop is a cost savings waiting to happen!......
Almost forgot....the machine is a LB15II with an OSP7000 control....

[underthetire]

You can mill a flat, for sure. You can interpolate the C axis with X or Z, like cutting a slot across a face, milling a thread, etc. You can not "rotate" the turret and mill at the same time. That type of machine would have a magazine full of tools and cost about 300K more.

[littlerob]

Yes you can absolutely use movement in the X axis and Z axis at the same time you use the C axis, I guess you need to be more specific about what you are trying to accomplish.

Wrench flats?, Hex?, Contoured pockets on the face of the part? On the OD? That is what G101, G102 and G103 are going to help with, to compensate for not having a Y axis.

But no one else uses those G-codes to accomplish it, ie Fanuc, Yas, Haas. Haas and Fanuc use a "Cartesian" coordinate system, it's different.

So maybe the post needs to be modified.

But it isn't a parameter issue it's a code issue, Okumas (love em) are a little finicky about where one M-code is in order with another, especially with the live tools.

I'm not sure what you mean when you say "drill, index, drill, index" sorry.

[gene rhodes]

thanks guys, this is what I want to here! The scenario is I'm trying to make a 3/4" square in the middle of 6" piece of bar stock, billet, that is 1" thick...this will be used for a 3/4" socket ( it's a fixture we need for our assy. process) I am predrilling this hole and want no more than a .125" radius in the corners thus the question.
This is more or less a functionality test in our supervisions eyes... the real usefulness will be mill flats on the OD surface of tubes
Let me add one more piece to the equation I forgot to tell you about... the spindle drive went out about 2 months ago and we replaced it with an upgraded version of the same drive by scavenging from another machine (Okuma rep. did this, and there still crying about how much this cost us). This machine, however, did NOT have live tooling! Okuma rep. said it should not be a factor but have not been able to get the interpolation codes to work since. Ironic? who knows...I'll leave it up to the experts...you guys!

[littlerob]

Yes you can absolutely use movement in the X axis and Z axis at the same time you use the C axis, I guess you need to be more specific about what you are trying to accomplish.

Wrench flats?, Hex?, Contoured pockets on the face of the part? On the OD? That is what G101, G102 and G103 are going to help with, to compensate for not having a Y axis.

Sorry, I think I kind of came off sounding like a prick.

The G101 feature is pretty cool, but if you have feature cam you can still post C-axis moves without that, for flats or hex or "squares". The difference is it will be in tiny increments determined by the parameters in your software. And if you need a really good finish it might not work, if your inspecting with a profilometer for example.

I would suggest using the software as opposed to getting G101 dialed in, as it is much more simple.

[broby]

Does your machine have IGF with the Live Tooling programming option?
If so, try programming a simple shape through that to see what codes are output.
If the generated program does not work then there something else wrong on the machine, maybe the spindle drive unit that you changed??
Brian.

[OkumaWiz]

You know, it could just be your programming format.

Try this sample code to see if it works. You will most likely have to put in the cutter comp value in your tool data to run it. We use this to put a square on the front of our part. The square flares out to a larger diameter, thus the 9mm ball end mill. It will work with any end mill.

(OPERATION B6 - CONTOUR
TOOL 9- .3543 DIA. BALL ENDMILL
9MM BALL FINISH END MILL
FINISH FRONT SQUARE )
M110
NT9 G17 G90 T090909 SB=3056
N190 G137
N192 G0 X.4274 Y.4453 Z.0854 M15 M8
N194 M13
N196 Z.1
N198 VLMON[09]=16+3
N200 G1 Z-.802 F.002
N202 G41 G101 X.2493 Y.4453
N204 G101 X.2493 Y-.2493
N206 G101 X-.2493 Y-.2492
N208 G101 X-.2492 Y.2493
N210 G101 X.4453 Y.2493
N212 G40 G101 X.4453 Y.4274
N214 G0 Z.1
N216 VLMON[09]=0
N218 Z.0854
N220 G136
N222 G0 X20. Z5. M12
N224 M109

Best regards,

P.S.> If you get any alarms , post them by # and description, so we can tell if you possibly have a spec code issue.

[cncboy1]

Hello

On our LB15II with OSP7000L we can not use G101 G102 and G102 also not M19. (spindledrive unit? diff.).

[underthetire]

Std machine does not have orientation. Only M machines with live tooling or special order.

[gene rhodes]

...going on the assumption that what I have is a spindle drive issue (still won't take
G101-103 or G17-G19), does anyone have a affordable fix to this problem? Is this something that we can do in-house ( i.e. flip a switch on the drive) to activate this?
I have been in touch with our tech support (Featurecam) and they have givin me a baseline post that uses incremental programming and does not require the codes..... problem is the programs are WAY to long to store many in the memory.

[Algirdas]

..going on the assumption that what I have is a spindle drive issue (still won't take G101-103 or G17-G19)
Have You tried the part program, provided by OkumaWiz? Error messages? diagnostic messages?
I can't believe about incompetence of Your official Okuma representative there

[underthetire]

Just because it won't take a G code has nothing to do with a spindle drive. You would have a drive fault when you try to run the spindle, period. You have either a programming error, or a software option you don't have.