Rigid Tapping with okuma MC series vertical machining center

Discussion:

(too old to reply)

Tero Kaarlela

2006-10-13 06:41:50 UTC

Hi,

We have Okuma MC-40VB VMC controller is OSP 5020M(spindle controller is
Okuma VAC II). Machine has rigid tapping option but machine tends to
break taps very much. we use following line to command rigid tapping(tap
is M12 pitch is 1,75mm/r):

M03 S200
g84 x-108. z-24. R5 F350

Any ideas if we are doing something wrong or something wrong with machine?

Tero Kaarlela
Eka-Sorvaus OY
Nivala, Finland

C***@HOTMAIL.COM

2006-10-13 16:18:10 UTC

Permalink

Tero,

Has this operation been performing acceptably on another VMC with the
same coolant?

The reason I ask is that the condition and lubricity of the coolant has
had a major impact on our rigid tapping reliability.

Carl

Post by Tero Kaarlela
Hi,
We have Okuma MC-40VB VMC controller is OSP 5020M(spindle controller is
Okuma VAC II). Machine has rigid tapping option but machine tends to
break taps very much. we use following line to command rigid tapping(tap
M03 S200
g84 x-108. z-24. R5 F350
Any ideas if we are doing something wrong or something wrong with machine?
Tero Kaarlela
Eka-Sorvaus OY
Nivala, Finland

brewertr

2006-10-13 16:40:08 UTC

Permalink

Tero,

I haven't programmed an Okuma in years and none had rigid tapping.

G84 is a Tapping Cycle but I don't see anything in your sample code
that kicks in "Rigid" Tapping.

On other machines and controllers there is an "M" code that kicks in
rigid tapping usually M29. Check your operators manual.

Tom

Copied from http://www.mchysales.com Support & Services Page

Bridgeport VMC with 21i control
Handout 6-2 Tapping Cycles

G84 or G74= Tension/Compression Tapping; Feed in-Reverse spindle & Feed
out
G84R_X_Y_Z_F_ for right hand tapping
G74R_X_Y_Z_F_ for left hand tapping

Usually used for moderate numbers of holes, or holes to large for
available self-reversing tap heads. Faster than Solid tapping and
easier to set up than

Self reversing heads.
If G94; F=.98 * RPM / Threads per Inch
If G95; F=.98 * 1/ Threads per Inch.

The .98 may be increased towards 1 as the hole gets deeper.

G84 with M29= Solid Tapping; Stop Spindle, Accelerate spindle & feed
in, Stop spindle & feed, Accelerate spindle & feed out, Stop spindle.
M29
G84(G74)R_X_Y_Z_F_
X_Y_

Usually used for short runs, extreme thread tolerances or bottom
tapping. Easiest to set up but, also the slowest.
If G94; F=RPM / Threads per Inch
If G95; F=1/ Threads per Inch.
Adjust the Spindle speed to match an exact feedrate.

G85= Self-reversing Tap Head; Feed in, Feed out
G85R_X_Y_Z_F_
Usually used for production runs, especially of small holes. Takes the
most time to set up but taps many times faster than other methods.
If G94; F=.95 * RPM / Threads per Inch
If G95; F=.95 * 1/ Threads per Inch.
The .95 may vary by hole depth and Tap head type.

BottleBob

2006-10-14 01:20:02 UTC

Permalink

Post by Tero Kaarlela
Hi,
M03 S200
g84 x-108. z-24. R5 F350
Machine has rigid tapping option but machine tends to
break taps very much.
Any ideas if we are doing something wrong or something wrong with machine?

Tero:

I don't easily think in metric, but a 1.75mm pitch equals an inch pitch
of .068897 And a feed of F350 mm/min. equals an IPM feed of 13.7795
Since the RPM times the pitch should equal the feedrate on rigid tapping
we've got .068897 X 200 = 13.7795 So your feedrate should be OK. There
might be a problem in your rigid tapping callout. Are you sure your
machine HAS rigid tapping?

One way to check if your rigid tapping cycle is progressing at the same
lead as your programmed thread pitch, is to chuck up a large thread in a
tool holder and put an indicator on the flank of the thread and watch
the indicator as the machine goes through it's rigid tapping cycle.
(I'd use an expendable indicator in case things aren't set up just right
- maybe first hold a scale against your vise and the thread to check for
a really gross error)

If all else fails, you can always try a compression/extension tap
holder. They will accommodate a lot of minor pitch errors.

I was rigid tapping some 1-72 holes in titanium last week, and broke a
couple of taps. So I added an M00 to halt the program to brush some
"MicroFinish" on the tap. That solved the tap breakage problem.
As ***@HOTMAIL.COM suggested, the material you are tapping might
need a more lubricious (is that a word? <g>), coolant.

--
BottleBob
http://home.earthlink.net/~bottlbob

rlewisa1

2006-10-14 02:02:53 UTC

Permalink

Post by Tero Kaarlela
M03 S200
g84 x-108. z-24. R5 F350

lots of good info snipped

on our TREE to invoke rigid tapping

G84.1

THIS could be the problem as well

CNC Solutions

2006-10-14 11:46:54 UTC

Permalink

Post by Tero Kaarlela
Hi,
We have Okuma MC-40VB VMC controller is OSP 5020M(spindle controller is
Okuma VAC II). Machine has rigid tapping option but machine tends to break
taps very much. we use following line to command rigid tapping(tap is M12
M03 S200
g84 x-108. z-24. R5 F350
Any ideas if we are doing something wrong or something wrong with machine?
Tero Kaarlela
Eka-Sorvaus OY
Nivala, Finland

I do not have the info in front of me but Okuma has a parameter that
switches between "Floating/Synchronous tapping". I had a LU-45 that was set
on floating and would break taps on the way into the hole because the
machine automatically increased the feed for a floating tool. After
switching to "Synchronous tapping" it was fine. If you can't find it post
again and I will dig up the parameter for you.
Darcy

Tero Kaarlela

2006-10-14 15:32:44 UTC

Permalink

Once again thanks to all who helped me. Here are commands for OSP5020M
tapping:

G84 "normal" tapping
G284 "rigid" tapping

Tero Kaarlela
Eka-Sorvaus OY
Nival,Finland

brewertr

2006-10-14 17:59:54 UTC

Permalink

Tero,

Have you made the program change (from G84 to G284)?
Did it resolve your tap breakage issue?
Let us know your results.

Tom

Post by Tero Kaarlela
Once again thanks to all who helped me. Here are commands for OSP5020M
G84 "normal" tapping
G284 "rigid" tapping
Tero Kaarlela
Eka-Sorvaus OY
Nival,Finland

Tero Kaarlela

2006-10-14 21:36:43 UTC

Permalink

Yes I have and yes it helps.

Tero

Post by brewertr
Tero,
Have you made the program change (from G84 to G284)?
Did it resolve your tap breakage issue?
Let us know your results.
Tom

Post by Tero Kaarlela
Once again thanks to all who helped me. Here are commands for OSP5020M
G84 "normal" tapping
G284 "rigid" tapping
Tero Kaarlela
Eka-Sorvaus OY
Nival,Finland

t***@centurytel.net

2006-10-14 19:02:09 UTC

Permalink

IIRC, we shifted the machine into feed per revolution for rigid tapping
on a OSP5020 control.
ie:
S200M3
G95 (feed per revoloution)
G84 X-108. Z-24. R5 F1.75 (feed 1.75mm per spindle revoloution)
G94 (switch back to feed per inch/mm)
Then clearance moves etc...
Hope this helps, my OKUMA time is 6+ years out of date but this
worked great on 6VA, 500H (OSP5020) and MX60 with the OSP7000.
Tom

Tero Kaarlela

2006-10-14 21:36:25 UTC

Permalink

Thanks for this info :)

Tero

Post by t***@centurytel.net

IIRC, we shifted the machine into feed per revolution for rigid tapping
on a OSP5020 control.
S200M3
G95 (feed per revoloution)
G84 X-108. Z-24. R5 F1.75 (feed 1.75mm per spindle revoloution)
G94 (switch back to feed per inch/mm)
Then clearance moves etc...
Hope this helps, my OKUMA time is 6+ years out of date but this
worked great on 6VA, 500H (OSP5020) and MX60 with the OSP7000.
Tom