[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:
http://www.cnczone.com/forums/okuma/...gram_work.html

[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.

[jjanu]

They work like this:

T

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?

we use one turret with 2 spindles. need 2 different offset call outs for using different tools on each side, example being tool 7 on main side is a boring bar with a .007" radius, tool 7 on the sub side is a boring bar with a .015" radius. main side program is called out T070707 and subside is called out T270727

[OkumaWiz]

we use one turret with 2 spindles. need 2 different offset call outs for using different tools on each side, example being tool 7 on main side is a boring bar with a .007" radius, tool 7 on the sub side is a boring bar with a .015" radius. main side program is called out T070707 and subside is called out T270727

I think I explained it poorly. 1 offset with 2 different radii.

Two tools, two offsets, two different radii, completely understandable...1 tool (groove) with 2 offsets..done it may times...but 1 tool offset with two different radii?? - never. Radius# and offset# have ALWAYS matched. It's redundantly redundant as ad64075 says!

Seems as though 4 digit tool offset would always be enough.

[deadlykitten]

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?

hy mr wizard in case it matters, i have used different radius on same tool, in order to run multiple finish operations ( if i remember, at least extra 2 ), on a precision conical surface, with full depth control for each pass; igf allows only XZsetting, and i don't know how that affect tapered surfaces; it was easier to use a tricky code, rather than testing how igf behaves

radius was initialized & changed from code, with system variables, and the tool was always using same T comand


another time when i messed the radius, was for a roughing cycle, where shape had a radius < tool radius, so i tricked it


before 2 spindle lathes, i started using T = LINK * 101 / 10101 for 1st offset, and T = LINK * 101 / 10101 + 200020 for 2nd offset, thus always using #1-12 for main, and #20-32 for 2nd; like this, difference between main and 2nd was always 20, and i only had to type 1 or 2 digits to initialize a T comand, rather than 6; back then, i called it progress

but that formula did no longer work for 2 spindle lathes, because offset number was limited to 32, so i had to forget that method, and use a new one, that would satisfy both single and dual spindle lathes : i started using T= LINK * 100 for a short while, thus no longer having the offset and radius sent to the machine through the T comand, but through shape; i only used that for short time, because it's simplicity required much more background work

all the best mr wizard

[lshingleton]

Fanuc or Okuma its just ISO standard
T010101
T01 Tool Number
T0101 Tool number with Offsett
T010101 Tool Number With offsett and then Radius compensation value

[OkumaWiz]

Fanuc or Okuma its just ISO standard
T010101
T01 Tool Number
T0101 Tool number with Offsett
T010101 Tool Number With offsett and then Radius compensation value

Not quire right... see post from above.

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

Best regards,

[lshingleton]

T01 is always the tool number as we used to have to right T0100 at the end of each to cancel before index
Try and Type in T0102 and see what gets picked up ?------------Tool one with offseet two which people used to do alot
Alot of large shops will not used T010101 as the raidus can become deleted or changed and scrap many parts so they program the tool nose into the program

[OkumaWiz]

T01 is always the tool number as we used to have to right T0100 at the end of each to cancel before index
Try and Type in T0102 and see what gets picked up ?------------Tool one with offseet two which people used to do alot
Alot of large shops will not used T010101 as the raidus can become deleted or changed and scrap many parts so they program the tool nose into the program

What you are saying you do is correct, but if you type in only T01 you will only get offset 01 and if you type T02, you will not get an index, but only offset 02 active. I use this al the time on Grooving tools to switch from offset T12 (left) to T22 (right) using only the 2 digit command. Tool T1200 will cancel the offset just like T00 will cancel the offset.

Commanding:
T01
T02
T03
M2

Will NOT index but will change only offsets.

Okuma drops them rather weird as I show above, but I assure you that's how it works.

Best regards,

[deadlykitten]

T01 is always the tool number as we used to have to right T0100 at the end of each to cancel before index

hy lshingleton
T01 is not the same as T0100 :
... equivalent syntax for T01 are : T1 or T001 or T0001 or T00001 or T000001 and nothing else
... same for T0100, equivalent calls are T100 or T00100 or T000100 and nothing else

please, there is a difference between trailing and leading zeros ...

there are also other methods to cancel before index, related to cycle time reduction

Alot of large shops will not used T010101 as the raidus can become deleted or changed and scrap many parts so they program the tool nose into the program

there are safety methods to prevent wrong radius declarations, like in program checks, etc

if you wish, check also attached image, for more infos / kindly

ps : mr wizard is always right

[OkumaWiz]

ps : mr wizard is always right

LOL! If only my wife thought that! :argue:

[Superman]

ps : mr wizard is always right

LOL! If only my wife thought that! :argue:

Anyone got a pin ?
( someone has a large head)

[OkumaWiz]

Hey I didn’t say it, deadlykitten did, but it made me laugh! ????

[deadlykitten]

if i may, it could have been much worse

it is not important to be right / wrong, it really does not matter; is much harder to be yourself, your true onest you

nowadays stress is no longer a question, but monetized to sell, inhibiting human nature ; this makes many to lose their mind, uncounciusly, unable to see root things clearly, satified with superficial versions of truth

there is no right/wrong, but presence or absence of heart in the end, those moments that we remember, are not about rigth/wrong, but something else

she changed me; for example, find attached an image that i liked before, and what i like now if it wasn't for her, my god, i could have gone in a terrible wrong way, low health included

realizing such things, i stoped working full time; way better then being filled with additional/extra hours; but, there is a cost to this : when you are no longer busy, the thoughts that have been ignored, will flash back to your head, and i wish to deal with them now, or else ...

okey, things will change a bit now ...

in case you did not know, these are old methods :
... keeping a mind busy is a strategy to avoid life ending acts for young military guys, during long patrol shifts, when they are lonely for hours, with a single bullet in the riffle
... is possible to save a few $$, buy delaying with a few months the sending of the 1st pension, because some persons can not survive ( for that long ) the transition from active life to retirement

2020 update ( more refined methods ) :
... keeping a mind busy is a way to sell
... is possible to save even more $$, by increasing retirement age, and other things hard to imagine by a normal person; it's all statistics

take care !

[lshingleton]

Oh God not another one !!!---------------I know all the safety stuff to i am blue in the face -----------Dont put in the Rad and program it into the machine ----We had over 10,000 CNC amd i was programming Okuma Cadets and Crowns when know one could turn them on and even them pieces of **** Mx40 in the first year with the new control then -----N Jump or NA Jump Statments who cares -----Okuma became to smart for thier own good and to far away from ISO programming to be useful anymore ----------Have a good evening and leave room for learning as most of mine was learnt not from books but how Burger flipper operators could managent to **** stuff up