[xal3r]

Maybe anyone knows how to tap with this machine? I wrote simple program with Mastercam , but the pots processor is for Fanuc Ocuma controller and our is OSP-5000. But i usually write programs like this, just get the code and then i correct it by my self. Now
i have to tap a hole and the mastercam gives me the G77 code but the program doesn't work i get error. Maybe there is a simple way to tap a hole with floating holder just with M3 and M4? Thanks for any suggestions.

I tried code like this :
$T.MIN%
N100 G50 S1000
G00 X500 Z150
N110 T0505
N120 G95 S150 M03 M41
N130 G0 X0. Z5. M08
N140 Z2.
N150 G77 Z-10. F1.50
N160 G0 Z5.
N170 G0 X500 Z150
N180 M05
N190 M30
%


In this line : N130 G0 X0. Z5. M08 my ocuma lb 15 machine gave me an error that x is over travel, than i changed to G00 and then the program continued but than i got an error at G77 code.

[kurmay]

G77 Tapping cycle: Forward thread
[Command format]
G77 X_ Z_ K_ F_
X: X-axis coordinates of tapping cycle start point
Z: Z-axis coordinates of target point for tapping cycle
K: Shift distance from cycle start point to feed start point
at rapid feedrate
F: Cutting feed distance
[Note]
1. Feed override is fixed to 100% during tapping cycle.
2. Temporary stop and single block are invalid during tapping
cycle.
3. The spindle remains stopping during tapping cycle.
To resume the machining, instruct the spindle run command
again.

[kurmay]

G178 Synchronized tapping cycle (CW)
Use this code for tapping machining using the rigid tapper.
[Command format]
G178 X_ Y_ Z_ C_ K_(I_) F_ D_ J_ Q_
(R_ )
X: Cycle starting X coordinates for end face machining
X-axis cutting target point for side machining
Y: Y-axis cutting target point (Y-axis control specification)
Z: Z-axis cutting target point for end face machining
Cycle starting Z-axis coordinates for side machining
R: Cut depth (Designate cutting direction by a sign.)
Do not instruct any cutting target point when using
the R instruction.
C: C-axis indexing angle
I: G00 approaching distance at side machining
K: G00 approaching distance at end face machining
F: Cutting feedrate
D: M-tool tapping start position
J: Number of threads
Q: Number of uniform distance holes of the repeat function
[Applicable specification] Compound machine

[OkumaWiz]

Kurmay's format example appears correct. I think you are getting the error since you have no X coordinate. Your Mastercam post is probably deleting the redundant X value even though the okuma requires it.

Best regards.

[deadlykitten]

Maybe there is a simple way to tap a hole with floating holder just with M3 and M4?

hy there are codes for syncro, but, onestly, i don't like them

you said that you have a floating holder does it go "length compensation" ?
... if no, than maybe it is an ER type, so use it with the collet from image 2 + "kurmay examples"
... if yes, than how much ? if is "short", than "kurmay examples" ; if is long, than "M3/M4"

if is "short", than you can craft a special sleeve, to make it go with "M3/M4", so to make it advance when spindle is breaking thus, you eliminate syncro codes and pay less on the neccesary equipement; are you in ? if you don't have time for such, than i would suggest simple M3/4, with a holder with this capabilities ( image 1 ) :
... self centering ( = X compensation for 1..2 mm )
... length compensation ( = Z compensation -10 .. +20 )
... safety clutch

also, if you wish to go faster, go self-reversing kindly !

[deadlykitten]

actually, i avoid tapping on lathe ; for the nature of our parts, a " mosquito " is better

[Superman]

actually, i avoid tapping on lathe ; for the nature of our parts, a " mosquito " is better ( he's not doing your parts )


hy there are codes for syncro, but, onestly, i don't like them

you said that you have a floating holder does it go "length compensation" ? ( er.....how else does a "floating holder" work ? ...... )
... if no, than maybe it is an ER type, so use it with the collet from image 2 + "kurmay examples" ( ? ER...... you can get an ER floating holder...... if it don't float...it's called "Solid tapping"..... (for solid tapping, everything has to be spot-on...tool HAS to be on centreline )
... if yes, than how much ? if is "short", than "kurmay examples" ; if is long, than "M3/M4"

Maybe there is a simple way to tap a hole with floating holder just with M3 and M4? Thanks for any suggestions.

Don't go this way, unless you have experienced operators..... keep it to being a canned cycle
- if feedhold or single block is activated during the operation....... goodbye tool and/or holder, possibly the part also....your tapping axis would stop moving,... BUT the spindle will continue to turn
- plus the override controls will be functional.... if not at 100%, stuffing up the required pitch for the thread

If you don't have "solid tapping"
- a floating holder would assist in lowering the stop & reversing shock to the tap at the bottom of the hole ( when it tends to break the chip, is when a tap would jam up & snap )
When programming a floating holder, the idea is to set the feed at 90-100% of the pitch
....so the holder is slowly drawn out
.....the slide will instantaneously stop while the spindle stops & reverses
...... at the end of cycle, it would return to the same point as at the start.

[deadlykitten]

When programming a floating holder, the idea is to set the feed at 90-95% of the pitch

depends on thread length ; not needed if holder has compensation to "traction & compresion "

by the way, nice trick : it works like a charm on pitch:2

does it go "length compensation" ? how else does a "floating holder" work ?

holder may contain none, or at least 1 of these atributes :
... radial comensation = float ( static/hand adjusting to reduce radial play, or dynaminc/while moving )
... length compensation ( short/for syncro machining - long )
... angular compensation
... and others

"float or solid" are also used for the machine parameters, so to syncro at it's best or not

some producers reffer to "length compensation" as "float" or "syncro tapping" ... from this point of view, is same thing

[Superman]

depends on thread length ; not needed if holder has compensation to "traction & compresion " (the term used is.....Extension & Compression)

by the way, nice trick : it works like a charm on pitch:2



holder may contain none, or at least 1 of these atributes : ( has to have at least one )
... radial comensation = float ( static/hand adjusting to reduce radial play, or dynaminc/while moving )
... length compensation ( short/for syncro machining - long )
... angular compensation ( nah, not this one..... who'd want to tap a crooked hole )
... and others ( there are no others)

"float or solid" are more used for the machine parameters, so to syncro at it's best or not

ps : some producers reffer to "length compensation" as "float" or "syncro tapping" ... from this point if view, is same thing

Your "ps" is incorrect
"length compensation" as well as "radial movement" all refer to the ability to "float".... this is a function of the holder
......syncro tapping is a machine function ( feeding axis is synchronised to the spindle), .... not a tool...so they are very different
......solid tapping is another machine function, and requires a more accurately set machine

[deadlykitten]

... try blue instead of red
... "traction" because tap is pulled, and so, elastic component is "extended" ; some producers also use "deflection"
... some holders are simple ; just clamp the tool
... some extrafunctions are : hard start, clutch (adjustable or simple), neutral/ front release, harder elastic elements, depth control, self reverse, etc

[Superman]

[QUOTE=deadlykitten;1931248]... try blue instead of red Red to correct your "misinformation"
... "traction" because tap is pulled, and so, elastic component is "extended" ; some producers also use "deflection" "traction" is what a 4X4 would have.....never heard of a spring that has "traction"
... some holders are simple ; just clamp the tool what is called.... "solid tapping"
... some extrafunctions are : hard start, clutch (adjustable or simple), neutral/ front release, harder elastic elements, depth control, self reverse, etc
... review your 90..95% feed override, because a M14 will break a holder with 0.5 extension after 10 mm ???? 2mm pitch @95% is F1.90 .... it would need to tap 100mm deep to get to the 10mm extension
... review my post ....I'd corrected that long before you posted your reply...duh (chair)

[deadlykitten]

about traction, deflection, do you really wish to post some catalogues, so to see ? .... called it whatever, just get the job done

and about angular behaviour : this is an issue ; on classical machine :
... lathes : is enough to extend the live center, or how is it called in english the place where drills are clamped
... mills : is enough to drop down the head/spindle, and tools will be able to oscilate

so this fenomen appears "naturally" on classic ; cnc's are more rigid, and some time you need a floating chuck to achieve same behaviour long tools, taps going after a hole that is not turned by knife, but drilled by M, they would go angular, and still deliver ... if is not possibile for them to go so, than internal tension appears

ps : i think you fly all day / how do you know of 4x4 ?

[deadlykitten]

:wave:

[Superman]

if max extension is 0.5, than after 5 turns = 10mm, you may need a new holder

a link to typical ER.. T & C holders..... nothing anywhere for a 0.5mm max extension..... these show 5mm compression & 8mm max extension, means if I set feed at 95%, ....I could tap a 80mm deep thread

[deadlykitten]

there are holders with mini-compensation, for high accuracy syncro cnc's ... ( mapal & tapmatic )

[deadlykitten]

Tapping with ocuma lb15 osp 5000

hey, is somehow your Okuma "made in China" ? just kidding

[deadlykitten]

compression/extension is to protect the tool :
... during cutting
... at spindle breaking and axial rewind moment

if syncronization is low, than more elastic behaviour is required, thus longer travels ; when syncro is better, length can be reduced

overiding the feed with a smaller value, leads to leaking, and so, there will be less elasticity available when tap must rewind even on a high syncro machine, you can not know what will happen

[xal3r]

Thanks for advice guys but can someone just give me example of m3/ m4 code. For example i need to tap M6 in a blind hole let it be z - 10 deep. I will use floating holder.
I am just starter programming on ocuma. I work with milling machine and the feed rate and spindle speed is different from ocuma lb 15. When i need to tap m6 hole with my milling machine i use F 150 S150, but for ocuma i found some information that people writes feed rate 0.*** so someone just give me an example of the code with m3 m4 and feed rate and spindle speed . And if someone are not lazy i would be a good to look at the synchronized tapping cycle code to.

Sorry for my bad english i just need to solve this problem our parts that we are making are very simple so i just need a simple code and i will try it in the air first of all and later i will try to tap holes in the parts.

Thank you for any information.

[OkumaWiz]

$T.MIN%
N100 G50 S1000
G00 X500 Z150
N110 T0505
N120 G95 S150 M03 M41
N130 G0 X0. Z5. M08
N140 Z2.
N150 G1 Z-10. F1.50*.95
N160 M5
N165 M4 M63 F1.5 Z5
N170 G0 X500 Z150
N180 M05
N190 M30
%

This will "stretch out" your holder as it feeds in by using feed rate *.95.
Then stop with M5
Then reverse with correct feed to retract and will ignore spindle RPM arrival signal with the M63. (M63 is an option as part of cycle time reduction function)

If you don't have the M63, you can usually get away with changing the .95 to something smaller to "max" out your floating holder's travel so that when the spindle reverses, it can take the reversal error without breaking the tap or bottoming out.

I have not had much luck with the G77, but it will work if the same reduced feed is used with a floating holder and a slow RPM (100-300)

I wouldn't suggest doing over 500 unless you are on a newer machine. I've witnessed them synchro-tap without software or floating holder at 500 RPM since the drives react so much faster.

Best regards,

[deadlykitten]

hy xaler, about M3 / M4 tapping inside a blind hole

holder should allow tap to rotate, so to avoid tool breaking when Z reached end point and spindle breaks ; there may be machine lags
be sure that there is enough length compensation ( + & - ) :
.... to avoid breaking the tool near hole end ( caution this may happen )
.... to use slow feed overide ( not necessary )

M6 x 10 means little hole, so be carefull at chips direction, and not the tool to get stuck at hole bottom ... you may consider tapping a bit, than retract & clean, and continue futher; thus, it means entering the hole more times : in this case M3/M4 may not work at 2nd tool enter

in my opinion, if you wish to use M3/M4, you must be sure that you control all this aspects ; if you are not sure, than :
... please uplod a photo with your holder
... please go syncro
... consider testing it before on a clasical machine ( so to stop faster if something happens ) :
..... put gears into metric=6 state
..... rotate the chuck in manual mode until Z-10+2....3...4 ( depends on cnc lag & holder length compensation )
..... disengage gear and allow free rotate of the spindle
..... rotate the chuck, so for the tap to reach the botom of the hole, and than reverse
..... for multiple attacks : tap out, rotate it's position, enter gear mode and see if it enters the hole
..... if it works, all is ok, than move setup to cnc

code from Mr. Wizard is ok, just be carefull with the feed :
... M6 has normal pitch = 1
... carefull with low feed overide

ps : one more thing : if you can not beat a classical machine on this tapping operation, than try to leave this operation for classics