Okuma lathes M63 and other questions

[UWP_Wes]

I'm new to Okuma and have some questions.

Machines in question are 10 years old or newer with U10, U100, or U500 controls I think.

There is a code, M63 I believe, that will let the tool move while the spindle is accelerating. On other machines I have used, the tool can make rapid moves while the spindle is accelerating, but will wait for the spindle before it makes a feed move. Do I have to use the M63 every time? Or, can I change a setting to make the lathes work like other machines I have used?

Does anyone know if you can thread mill with the live tools? The manual states that you cannot move Z during G102 or G103. I wondered if there was a work around.

Thanks for any help.

P.S. I like the Okuma lathes so far. The code is a bit odd, but manageable. I'm not a huge fan of the mill control. It seems far behind our Mori with the MAAPS/mitsubishi control.

[budgieW]

There is a parameter for M63 that sets Cycle time reduciton for 1 block or by program. Why do you want to use G102 With Z why not use G1 CZ? or C360 QA=20 for 20 revs

[UWP_Wes]

There is a parameter for M63 that sets Cycle time reduciton for 1 block or by program. Why do you want to use G102 With Z why not use G1 CZ? or C360 QA=20 for 20 revs

I will look into that parameter. Before I change it, is there a reason you would not want it active all the time?

I could use the G1 CZ, but I am thread milling a pipe thread and I need to do a spiral helix move. To make it even worse, the threaded hole is not on the spindle center-line. I don't think what I want to do is possible.

[budgieW]

I see no reason to have M63 active for the whole program. You will need to use G101 XYZ or G1 XZC

[OkumaWiz]

You typically use M63 by one block to make sure that when you switch from rapid to feed (G00 to G01) your cutting speed is correct for the tool's desired surface footage. This code is part of Cycle time reduction function (option) along with M62, M64, M65, M66. These codes can save a ton of cycle time by letting you do combined operations such as rapid while the spindle is accelerating, index on the fly, or index anywhere. Needless to say you'd better be careful when using these since they can potentially be hazardous. As already mentioned, you can make it modal by setting parameter, but I typically don't. I also rarely use the other M-codes since you can reach the X or Z limit by the time the turret can unclamp, so you save little if any time based on my experience.

Another time saver for machines with servo drive turret index is to combine XZ moves with the T command. This allows it to clamp the turret as it rapids to the part. Use an M203 along with your G00 X20 Z20 command and it will unclamp the turret during your rapid move. By doing these 2 things, you will save close to 3 seconds per index.

Circular interpolation during Z feed is also an option, but if you have a cad system, you can have it program XZC moves in G01 and you can thread mill on any Okuma M-machine. Much more code, but works fine whether on or off centerline.

Best regards,

[littlerob]

Circular interpolation during Z feed is also an option, but if you have a cad system, you can have it program XZC moves in G01 and you can thread mill on any Okuma M-machine. Much more code, but works fine whether on or off centerline.

Yup.

@ Budgie, what would you use G101 for while thread milling? centerline or not?

Robert