[deadlykitten]

hello, please, i need an example for OD turning with double holders

Y axis changes between tools lb3oooex2 osp3oo

and how can i gauge those tools, since gauging with "Y on" fails ? kindly !

[deadlykitten]

turning works fine with G138 Y...

... but i can't measure tools ... i wish VBZOY was not readonly, or something

[tea hole]

Stop putting the machine in G138.
Leave it in G136 and instead command "G0 Y1" or whatever the Y distance is you're after.
in manual mode i believe you'll get an alarm D but you can still touch off your tools.
you can also give it a y axis offset instead and call up the tool and a position in X. It will bring the tool to Y0 by default since that's where the machine was without the y offset active.
Then just touch off like normal in manual mode.
I don't believe there's any such thing as VBZOY. I believe that is a parameter known as Y axis turning position or something.
On the P200s it was a read/write variable, and on machines we didn't have Y axis turning on we'd lie to the control, change that number and change it back when we were done.
On the P300s they took that away so you need the Y axis turning option.

also, in your programming you will not be in G138 for a Y axis tool either. You will command a Y axis in the program or have a Y axis offset value set for each Y axis tool.

[deadlykitten]

Stop putting the machine in G138. Leave it in G136 ...

hello again tea hole this code :
G136
T
Goo X0 Z2.5 Y9 > will not raise the Y, also there will be no errors

if i replace 6 with 8, than all will be ok works on my Y lathe

I don't believe there's any such thing as VBZOY

and when i remeber that it was you who showed me these VBZO* variables ; pls check attached image from the file shared in #1 : http://www.cnczone.com/forums/okuma/...able-list.html

VBZOY shares same content as the base_o_offset_for_y_axis from system_para : if the value is edited inside the parameters, than the axis shift and i can measure the tools, but this involves editing the parameters, and that is a danger zone for the operators

if VBZOY was not read-only, than i could develop a faster way to shift the axis, like defining a G/M macro code

On the P200s it was a read/write variable ...

please, can you dig for this and share an example ? thcs
... i have tested a lot of variables, but not all

in your programming you will not be in G138 for a Y axis tool either

i can not raise the Y without the G138 kindly !

[deadlykitten]

turning works fine with G138 Y...

... but i can't measure tools ... i wish VBZOY was not readonly, or something

yesteray i found a way to measure Y turning tools with 0.2 accuracy, but this involves some calculations

it does not take long, but is a bit longer than lowering the senzor and measuring the tools

this should be done once, at initial setup, because after that only inserts are changed, and only small corections take place ...

however, i am still looking for a normal way to do this, but i see this no longer as an obstacle; maybe my dealer will reply on that

now i am looking forward into merging this double Y holders with dynamic_indexing and offset_protection

[hacdlux]

the tool call for a double stack is the same as long as you call y0.
put the y offset in the y off set position.
you have to turn on the y axis to jog to centerline on the presetter, then turn it off to do your touch. it will give you the ya xis not in turning pos alarm but will do the touch.

all my tool calls have the y0 call because i sweep drills to y and adjust turning tools to no nip condition

as far as y measure offset goes , eyeball it to center place cutting edge under center, face, measure nip, dim/2, offsetaccordingly

i generally delete all g138's unless i am doing propper y milling(rare)

[deadlykitten]

you have to turn on the y axis to jog to centerline on the presetter

hy hacdlux

... Y offset <> 0
... Y axis ON
... T X Z Y0
... getting close to presetter
...... so far so good

then turn it off to do your touch. it will give you the ya xis not in turning pos alarm but will do the touch

if i turn off the Y axis / G136, than the turret will lower at Y0, and i won't be able do to the touch

if Y axis is ON, than i can't touch, because i receive the "Y on alarm"

i generally delete all g138's unless...

Y axis will not move without G138 / kindly !

[deadlykitten]

both of you : teahole & hacker_de_luxe told me to avoid G138

but i can not call the tool ( T X Y Z ) without G138

if you have the lb3000ex2 osp300, than maybe i am doing something wrong

if so, please, can you share a code example ? kindly !

[deadlykitten]

this is how i measure X_offset for y_excentic tools :

1) OD / X+ / senzor upper edge / P8
... reset
... raise / lower the turret at specific Y value
... feed by hand until tool is in contact with senzor ; beep beep beep sound
... go at X_offset :
...... CALL : will input actual X value
...... ADD : -97.5

97.5 represent a diameter, where a corection with X_offset=0 is aligned with the upper edge of the senzor

"diameter" is materialized by the "X_axis_value"
"X_offset=0" is materialized by a "default id holder"

in other words : 97.5 is the value on my lathe were the "center axis" of the "id holder" is aligned with the "upper edge of the senzor"

this is represented in the attached images

2) ID / X- / senzor lower edge / P6
... same as above, only ADD value changes : -67.5

67.5 = 97.5 - 2 * 15, where 15 is the senzor edge ( the distance between upper and lower senzor edge )

[deadlykitten]

this is how i measure Z_offset for y_excentic tools :

1) using a machined surface with known Z : if a knife machined a straight face ( Z=0 ), than call the tool and simply get close to that frontal;go in offset_menu, and press CALL inside Z offset + input 0 ( or the known Z value )

2) using a machine surface with known Z : the spindle frontal

3) using the senzor :
3.1) frontal / Z+ / senzor right edge / P7
... reset
... raise / lower the turret at specific Y value
... feed by hand until tool is in contact with senzor ; beep beep beep sound
... go at Z_offset :
...... CALL : will input actual Z value
...... ADD : VSZOZ - 212.870

212.87 is the distance between "spindle frontal" and "senzor right edge", as shown in attached image

3.2) reversed frontal / Z- / senzor left edge / P5
... same as above, only ADD value changes : VSZOZ - 197.870

197.870 = 212.870 - 15, where 15 is the distance between left and right edges of the senzor

---

... touch the senzor by feeding the wheel
... press CALL inside the offset_menu
... ADD a corection value
...... accuracy < 0.2

it may be an option to use the senzor while Y is active; i still wait for a response from my dealer

i insisted again today

[hacdlux]

okuma lb3000 myw osp 300 circa 2015

(SUB SPINDLE DRILL)
N5 G141
G00 X30. Y0. Z15. T1100
N5 T1131
N5

G97 S2109 M03
M08
G00 X0. Z.1 Y0
M101
G74 G95 X0. Z-.32 K0 D.42 F.012
G00 Z.1
M09
M102
G00 X30. Y0. Z15. T1100
M01

y offset is irrelevant to me because i put them in the tool table. if you want to do it the other way y0 in the tool table and put it in the program. the way this is it doesn't matter what holder their in because y is set in the offset not in the program.

[deadlykitten]

hy hacdlux thank you for that sample, but it does not work 4 me ( attached images )

what are M101 and M102 for ?

please, will you share the content of "Ospmngcd.cnc" from your lathe ( c:\osp-p ) ? i wish to check the differences between lathes options; kindly !

ps : those images are clear, because i cleaned the control screen yesterday with a bit of coolant ...

[hacdlux]

m101 and m102 are high pressure coolant codes

its interestin though my y axis displays all the time.

there is an option called "off center turning" you might be missing or its a parameter thing. you should talk to your dealers applications dept

[deadlykitten]

hy hacker i will discuss again with my dealer next week

it has been a while since i started this thread, and meanwhile, the guy from the technical departement of our Okuma dealer left the country for 2-3 weeks

other guys are not so sharp, and i am tired of pointless discusions

at least i know that there is an "option" ; thank you

[deadlykitten]

hello, please is it possible to use G33 with the turret raised on Y ?

... i bought tools with smaller shank ( square 20 )
... i bought Y holders + finish touches :
...... screws to have same length
...... screws to stick out of the holder more, and at same distance as my actual holders
...... some i_dont_know_the_word to dont clamp the tool shank directly
...... coolant pipes
... i have written the code for this double holders

but i can not put them on the machine, because there is a thread tool, and G33 is not workin with turret raised ... and dealer is frozen

please :
G97 S600 M3
G138
VTOFY[VETON] = -9
G00 X100 Z2.5 Y0
G33 X99 Z-50 F1

kindly !

[deadlykitten]

hy teahole, hy hacdlux, it took a while for my dealer to figure it out that the Y-turning option actually exists