[nodochau]

Hi Deadlykitten,

I have osp 200 and 300. Please edit it so that I can start to try it. It is very interested though.
Thanks

paste your G22 code, and specify your control generation : if osp200 or 300 i will quick edit it for you, so to get the Z zero

about explanations about those variables, let's postpone them : you may not need to use all those variables, so to make the G22 work so if i start explaining them, you won't move your cnc ...

this is a paragraph : it has no safe position, no T codes; can you handle it ?
M19
G00 Z+10
G29 PZ=25
G22 PZ=25 Z-10 F+100*5 G94 D+10*2
G28
G00 Z+2.5 M18 G91
G90
NOEX VSZOZ = VSZOZ + VSIOZ - 2.5

[nodochau]

Here is what I want to do on X axis.
For right now as I have observed how the operator set up the zero set on Z and X
1. They skim the material by master tool (tool 05) then cal zero for that on Z
2. index next tool to the part face to set zero on Z
3. Keep doing that for the rest of tools to finish Z axis
4. Index tool 07 (roughing OD) and skim material and cal x offset
5. Keep doing that for the rest of tools (for OD )
6. If we have ID turn then we have to do the same to set the offset on X.
So my thought is that if we are able to write a macro so that we can eliminate step# 1 to 4 then it would be a big time saving. I am very interested in the topic that you have posted. As you know that I am very new in CNC field but I like it a lot.
Thanks

hi nodo, it is possible to use G22 among X axis, but i really don't understand why isn't it enough for you only on Z axis ?

why do you need both of them ?


also, there may be a problem with load detection among X axis; sometimes there is a remanent load, that simply goes away after a few seconds

this means that X load value, sometimes, may be greater without an aparent reason

check attached image : machine cuts air from X100 to X65, but effort is not constant; it simply starts high, and gets lower ( normalized ) arround X80

i have no clue what causes it, or if it appears also during G22

to handle this, you should use an effort limit >30%, and it seems a bit much for me, especially for a repetitive task

the lower the limit, the better, but there are some problems with limits that are too low; so far i have used 20-25%, mostly on Z axis / kindly

[deadlykitten]

hello nodo

in this post, is a code that should work on osp300... but wait a bit

after reading your last post, i realized that you wish for an alternative, so to measure the tools faster

oookeeey

• you need a touch setter; i mean you have a cnc with osp300, without touch setter ? what's wrong with your okuma dealer ? or did you steal the machine from somewhere ? come on man

check video from this post; buy that option; that setter may be manual ( cheaper ) or automatic ( more expensive )

• until you buy a touch setter ( or if touch setter option is not available ), you may use a simple zero-gauge ( check attached ) , and the CALL function inside the offsets table

• also you may calibrate your machine, and in this way :
... z_offset = distance between tool tip and turret frontal
... x_offset = distance between tool tip and turret polygon ( multiplied by 2, and also zero will be at cca90mm from the turret polygon )

• about facing&zeroing on osp300, i have a real nice code in this thread; give it a try : https://www.cnczone.com/forums/okuma...-reloaded.html

• i can explain you this autoZ/X method, but it is there for other purposes; some load limits will be too small, and you won't be able to measure some tools; no ... you have a big chance to break all your tools it won't work how you expect

kindly

    G00 X500 Z250
    T010101 ( consider touching with a od tool shank, a rod, toolholder, etc )
    M19
    G00 X50 Z10
    G29 PZ=25
    G22 PZ=22 Z-10 F+100*5 G94 D+10*2
    G28
    G00 Z+2.5 M18 G91
    G90
    NOEX VSZOZ = VSZOZ + VSIOZ - 2.5
    G00 X500 Z250

https://www.youtube.com/watch?v=zgRWVm4cKC8

[nodochau]

We do have the touch setter. But some older ones don't. That is the reason why I am interested in the auto zero.
I like to have the macro to use on old machines. .
Even though, if we have the touch setter then we don't need to use it....
I can load the material into the chuck then hit the cycle start then walk away to do something else.. Does it make sense?

[nodochau]

You are using metric system, right?

hello nodo

in this post, is a code that should work on osp300... but wait a bit

after reading your last post, i realized that you wish for an alternative, so to measure the tools faster

oookeeey

point 1) you need a touch setter; i mean you have a cnc with osp300, without touch setter ? what's wrong with your okuma dealer ? or did you steal the machine from somewhere ? come on man

check video from this post; buy that option; that setter may be manual ( cheaper ) or automatic ( more expensive )

point 2) until you buy a touch setter, you may use a simple thing like the one attached, and the CALL function inside the offsets table

point 3) also you may calibrate your machine, and in this way :
... z_offset = distance between tool tip and turret frontal
... x_offset = distance between tool tip and turret polygon ( multiplied by 2, and also zero will be at cca90mm from the turret polygon )

point 4) about facing&zeroing on osp300, i have a real nice code in this thread; give it a try : https://www.cnczone.com/forums/okuma...-reloaded.html

point 5)

i can explain you this autoZ and autoX method, but it is there for other purposes

some load limits will be too small, and you won't be able to measure some tools; no ... you have a big chance to break all your tools it won't work how you expect

kindly

    G00 X500 Z250
    T010101 ( consider touching with a od tool shank, a rod, toolholder, etc )
    M19
    G00 X50 Z10
    G29 PZ=25
    G22 PZ=22 Z-10 F+100*5 G94 D+10*2
    G28
    G00 Z+2.5 M18 G91
    G90
    NOEX VSZOZ = VSZOZ + VSIOZ - 2.5
    G00 X500 Z250

https://www.youtube.com/watch?v=zgRWVm4cKC8

- - - Updated - - -

You are using metric system, right?

[deadlykitten]

metric, yup

pls be sure that you read my previous reply; when you answered, i was still editing it

for your lathes without a touch setter, i would recomand a zero-gauge, but i am not sure if it will work on older ops; i will share the method for osp 300 :
... cut face and put program zero
... put zero-gauge on material face
... bring tool in contact with zero gauge
... zero gauge dial indicator should be at 0, etc
... go in offsets table, z offset, CALL + 50 ( considering 50 to be zero gauge zero position ) + enter
... for X, put the zero gauge on the tailstock, etc ... use your imagination

ps : please stop quoting my entire posts ! makes me go crazy

[deadlykitten]

Even though, if we have the touch setter then we don't need to use it ....
I can load the material into the chuck then hit the cycle start then walk away to do something else.. Does it make sense?

you can't use torque skip ( G22 ) to measure your tools

however, let's say that this won't break your tools ok ? you can't simply load the material and go ... no, it won't work

you will need to define for each turret post if gauging should be executed; but let's just say that you select all of them

for each turret post, you will still need to define which axis and which direction to use during G22; for example :
... x-z- for od tool P3
... x-z? for od tool P4
... x+z- for id tool P2
... z- for drill paralel to Z axis
... x- for drill paralel to X axis
*and so on; you can't skip this ! it is time consuming; if you would measure the tools at the touch setter, you would do the same : you would manually select which axis and which direction to move the turret



what may be possible to do, is to have an automatic touch setter, and a measuring program, and declare all tools in CAS ( or a soubroutine ), link all these togheter, and your turret will start measuring itsself ... however, if something is not ok, you may hit the chuck or the senzor

if i would have an automatic senzor, and if there would be system variables so to control the gauging procedure, i can write a program that would measure all tools from a turret; but i don't believe that it's worth it

maybe to detect broken tools ? beside this, i don't know any other use for the automatic sensor / kindly

[nodochau]

Thanks for your info. Just review your face off and z zero program and it is very great. I will try it someday. I have question about placing the tool above the bar. Above the bar and how far from the bar face? X>OD and Z?? I meant.
Regarding the tool broken detection, how do we detect the broken center drill? Can we use torque skip (G22) to check it? Saying, after finishing the center drill then I feed the center drill back into the hole to check the torque. If tool is broken, something will happen I think.??? Or using the tailstock to check...
For now, the program stops (M00) the machine. Operator opens the door to check tool to ensure center drill is good before go to the next cut.
Any idea?
Thanks

[deadlykitten]

hello

I will try it someday

it is fast & easy ... i will add a reply in that thread, so to guide you

i will also open a thread about fast offseting on lathe with the zero-gauge; only for you i will test it and share it soon

Can we use torque skip (G22) to check it?

my god, i have allready said 2 times that you can't use G22 to measure cutting edge offset :
... pls read blue lines in post 63
... pls read first line in post 67

and here you are, asking again look, to convince you that is not possible, maybe you should try and see what happens

take the code from post 63 and experiment with it

pls look at the movie shared at post 41 : the contact is done with the tool shank, not with the cutting edge of the tool

if you use the cutting edge of an od knife, or a drill, it will get broken, crashed, bye bye ...

G22 uses a torque limit to sense that the contact ocurs, and this torque limit, even if it is low, is powerfull enough to damage the tools

pls read post 6, from mr Wizard : "This feature was designed to transfer parts between spindles" ; thus it uses some amount of torque

Regarding the tool broken detection, how do we detect the broken center drill?

1) use no-load detection function ( load monitor 2 = LM2 ) :
... run the program in air, don't cut in material, but look at Z effort : let's say it is 15%
... now cut, and check effort : let's say it is 22%
... set in LM2 the limit of 18% : if Z effort during cutting is not greater then this limit declared in LM2, then the cnc will stop

you can't use this technique if there is no load difference between " cutting air" and " cutting into the material " : thus you can't use it on small tools, that do not require extra torque from the servos

2) whenever possible, use good quality tools, good specs, and change the tools often, thus don't push them until they get broked

3) someone was tapping a lot, 3-4 machines was running lights out, and he worried about taps that would fail : in the end, someguys installed a camera inside the cnc, and it would recognize ( with custom software ) if the tool was broken; however, if there were chips, or if the tap had light damage, this system would fail ... so it works as long as you can keep the tool clean

4) i guess it is possible to use an automatic tool setter to check tool offset before begining cutting

5) if the drill is big enough, for example if it is diameter 20, after it cut, index to a rod ( diameter 18 ) and use G22 to feed it inside the hole

6) raise coolant concentration; cutting edge will be more happy / kindly

[deadlykitten]

hello nodochau, i just opened a thread about measuring tools on a lathe without touch setter

if you wish, go check it out; i hope you will find it usefull

---

about those steps from previous post, that should help detecting if a tool is broked, are also downsides :

about step 1 ) LM2 will fail if there is a clearance too big; it also works paired with the VLMON function, that has no problem about a repositiong movement done in feed, but LM2 will have, and it will stop your machine; to handle this, it may be needed to remap the VLMON's across the code

about step 2 ) on short-runs, few parts, monitoring is not used, and a random tool may break inside the 1st part ( for example, some drills, may get a wear that is not visible : in other words it's cutting edge is not damaged, but dulled )

about step 3 ) is not always possible to keep the chips away from the tool, and if only the cutting edge is broked, but the tool is still there, then this won't work

about step 4 ) again, it won't work if tool is not clean

about step 5 ) G22 is time consuming

about step 6 ) it only delays the moment of a failure



there is a technique, which is based on signal-comparison method; it is not available for detecting sudden failures, but it is there :
... the mop function : the cnc can detect when load has decreased or increased with eq5%, and adjust feed, so to achieve cutting at a constant load as long as possible
... the dynamic load control : adjusting feed for individual inserts, that are mounted on same holder https://www.okuma.eu/technologies/premium-solutions/dynamic-tool-load-control

this capability is inside the controller; if some of it's parameters would be editable, it would be possible to detect an unusual load behaviour

well, it is easy to say, but not impossible / kindly

[nodochau]

Thank you very much.
Just read the book about the Load monitor. A little bit confusing of LM1 and LM2.
You said if there is no cut (cut air) look at the effort on Z and if it is 15% then we will set LM1=15%? and LM2=18% if the cut is 20%. So if the center drill is broken then there is a big clearance then the effort will be less than 18%. Yes, I understand that. How about the LM1? What does it mean? Let say if tool is not broken then the effort on Z will be greater than LM2 and LM1. If it is broken then the effort on Z will be less than LM2 and LM1??? Or less than LM2 or less than LM1?? or less than LM2 and greater than LM1??
Thanks

[deadlykitten]

hello, there are some functions that are based on load: load monitor, G22, G23, torque limiter, dtlc, mop, etc

about load monitor, on lathes, there are 3 types :
... load monitor 1 : will stop the cnc if the load is > a predefined limit ( for example a drill insert gets wasted during cutting; effort will increase, and cnc will stop )
...... for example, if a new drill is cutting inside the material at 22%, simply use an upper limit of 26-30%; if load will be bigger then this limit, it means that something happens, and if you continue cutting at this high load, then the drill may break
... load monitor 2 : will stop the cnc if the load is < a predefined limit; aka no-load detection : thus it is there to be sure that a tool is cutting
...... for example, if that drill is cutting air at 15%, and it is cutting inside material at 22%, then it makes sense to declare a limit of 18%; if the machine load won't go over 18%, it means that it is not cutting
... load monitor 3 : it uses a ratio of loads, so to determine if the part is about to fly-out from the spindle; i never used it

look inside your parameters : there are pages LOAD MONITOR 1 2 3, or at least LOAD MONITOR 1

check also the attachements from post 13 in here : https://www.cnczone.com/forums/okuma...r-stuff-2.html

didn't you received a full training about load monitor ? i said this, because it is easier to understand this if someone is near you; maybe is a good idea to request suport from your okuma dealer / kindly

[nodochau]

Thanks for your info. I got no training cause I just started to work on CNC programming. Actually focusing on macro variable stuff...cause I am CMM programmer. My boss wanted me to do that and I really like it. All I learn from books, google, you and this forum.
So there are a lot of term, words here are new to me. But I am getting it. I have a ADMAC software from OKUMA to play around to get more ideas and I learned it from books only .
FYI. I tried the auto face and set zero program yesterday and it worked great. I used X[VSIOX] NOT VSIOX-VTOFX. Thanks for that code. And now I am thinking about to do it on X-Axis. Will see. Don't know yet

[deadlykitten]

hello again, is not ok to leave a novice only with some books, a software, and this forum

at this moment you are no longer a novice, but your learning curve will be too long, and i am afraid that you can not see this ...

try requesting a basic instruction course from your Okuma dealer, so to check another point of view about the things that you allready know, but also it is an oportunity for you to learn some new stuff

---

is not ok to remove VTOF* from that code ; try this : run the code with and without VTOF, in step - by - step, and write the coordinates down, on a piece of paper compare the coordinates, and also compare the Z origin that is declared at the end

also, pls be aware, even if those coordinates may be identical, the toolpaths won't overlap; thus program "looks" the same, but real toolpaths are executed in different places / kindly

[nodochau]

I did that. Let say I move the tool above the material about 0.25 inch. the VSIOX is 7.25" the zero offset of the tool on Z always equal 0 so that is ok. But if i used VSIOX-VTOFX then the tool will move down to 5" if the tool offset is 2.25 on X axis.
I edited your code and run good on the machine. Here is my code.
V1 = 500(SPINDLE SPEED)
V2 = 0.03 (F - feed)
V3 = 0.005 (Z STEP)
TOF = 5(tool 5)
()
G00 X[VSIOX+.25] Z[VSIOZ - VTOFZ [TOF]]
Z[VSIOZ-V3]
G97 S[V1] M42 M03 M08 T[TOF*101]
V4 = VSIOX
V5 = VNSRX [TOF]
G01 X[-.0787*V5] F[V2] G95
G91 Z 0.012+V3
G90 X[V4] F100 G94 M05 M09
VZOFZ = VZOFZ + VSIOZ -.012
M02

[deadlykitten]

hi, i looked over your modifications, they are ok, thus the code will deliver, but that initial code is intended to work without such modifications

idea is to eliminate the need for such modifications, so to achieve face cut & zero pretty fast

before G97, you have 2 rapid codes, that will lead to real axis movements; such movements = time loss machine must begin cutting from where it is, thus 1st movement should be towards X-

this code of yours " -.0787*V5 " : here the insert must cut the full face, and stop at a negative diameter, equal with -2*radius; why did you used 0.0787 ?

here "G90 X[V4] F100 G94 M05 M09" F100 is too low, and you deleted M63; you lose time, because "linear movemement" and "spindle deceleration till full stop" no longer occur simulatenously

why did you replaced vszoz with vzofz ? you are editing the encoder origin; you may lose CAS calibration; did you tried the code on osp300 ?

[nodochau]

I have to change to vzofz and get rid of M63 cause I tested the code on the older machine which does not support vszoz and M63. And I am using inch not mm though.

[deadlykitten]

ok ... be carefull, even if that code can be edited so to deliver on older machines, it is important not to create downtime, thus is good to check if it's better to avoid using it, and facing&zeroing in the classical manner

it may be possible to update the code, so to make it behave faster on older machines, maybe as fast as i originally intended, but i only have acces to osp300

i am repeating my self, but pls be carefull because editing vzofz may change the CAS, more precisely, the solid models will be translated : for example, as a result, in virtual model, turret position won't reflect the reality; a consequence would be that the machine may stop suddenly ( even if all looks fine ), or a crash may occur ( even if it would normally be prevented ) / kindly