Breakdown of Okuma Lathe Tool Call

[magilla85]

I am looking for some clarification regarding Okuma lathe tool calls.

I have noticed that Okuma lathes use two formats. T0101 just like Fanuc and T010101.

In the first case, I understand the tool call may be broken down as follows:

Taabb where ‘aa’ = tool number and ‘bb’ = tool offset.

I have two questions …

1. Can someone break down the Taabbcc tool call for me?
2. Can someone give me a rule of thumb to determine which form to use with any given Okuma lathe?

[underthetire]

The Txxyyzz is for calling a tool radius offset, shouldn't matter unless your using a different offset number. Been 15+ years though......

[Technical Ted]

There's a PDF from the manual in the following thread:
Will this program work?

[OkumaWiz]

They work like this:

T010101 = RTO (Radius#, Tool#, Offset#)
T0101 = TO
T01 = O

They drop from front to back. If you always use the six characters, you will never go wrong since it will know where to "look" if you decide to turn on Radius comp using G41 or 42 and will just ignore it if you don't need it.

Typically you are fine if you use 4 characters and have your CAD/CAM system do the radius comp for you.

Just 2 characters are useful for changing offsets on the same tool while running such as a groove tool that may use left and right offsets to control an OD groove width.

Best regards,

PS> I never have understood why you would ever want a Radius comp register different from the tool#. Has anyone ever used a tool with 2 different radii?

[ad64075]

Actually, I have used a tool with 2 different radii during complex grooving with custom-made tools. However, that is the only time in my 15 years in the field I have ever done so. Agreed, it is a bit redundant it is a bit redundant.

[broby]

The reason you can use multiple offsets is that it comes in useful when programming wide grooves.
T060606 could be used for the LH side of the tool as in tool 6 offset 6 TNR offset 6
T160616 could be used for the RH side of the tool as in tool 6 offset 16 TNR offset 16
Using two groups of offsets allows you to gain accurate control over the width of the groove without having to tweak the program. i.e. you program true geometry positions for the edges of the grooves and then you tweak the position/width of the groove as your tool wear/position dictates.
Okuma IGF will usually output the second offset automatically.
Cheers
Brian.