[brettcnc]

We get poor tap life when rigid tapping on our 2008 MB56 VMC.

Taps under M16, M4-M12, work very well as long as we use a tap holder with some float. (Annway TER-32 "Rigid Floater").Without the floating holder these were hopeless too.

We program in IGF which outputs a G284 cycle. OSP P200M control.
Always drill oversize holes. Have tried cutting compounds.

M16, M20 & M24 taps fail unpredictably and I am determined to get to the bottom of this! Failure usually starts with chipped cutting edges and eventual breakage. Tried every brand and geometry spiral flute tap under the sun-Dormer,Stock,Hahnrieter,Sutton etc.

Have just changed parameters "Synchronised Tapping" as per Okuma's recommendations:
TAP MODE G84/G74 = FLOAT TAP. (WAS SYNC. TAP)
RETRACT 100%. (WAS 200%)

They have also got me shopping for a Nikken Micro-Float tap holder or similar.

I asked if they can measure the spindle/Z axis synchronisation - said they haven't done this before.
Daewoo did one of our C axis lathes which had a rigid tapping problem and ended up tuning servos to fix it...

Any comments/ideas before I put my 4th $200 M24 tap in for this job?

What kind of tap holder are people using for larger taps?

[slavetothemetal]

When I have to tap holes that size in 4140, I just copy the canned cycle, change the Z, and voila! you have a peck tapping cycle! We only use rigid tapping here though.

[Algirdas]

check your Z axis accuracy. Maybe you need to set pitch error compensation? What is load on Z axis while tapping? What RPM?
In my practice, no need for floating tap holder for Okuma. It is recommended, of course.

[brettcnc]

Spindle load is around 30%-40% with a new M24 Tap. 80 RPM (6m/min)

Z axis P Pitch Error Comp = 461.000
z axis N Pitch error Comp = -1

I have no idea how to measure the error.

[littlerob]

If you lose the floating holder and change the G284 to a G84 you will at least minimize your possible errors, that machine ias perfectly capable of rigid tap (am I agreeing with a$$ hat?) anyway.

I have a question, why would you be spending that much on a tap when you could spend 3/4 of that on a thread mill that will do a range of threaded holes?

Robert

[WGJ]

Unless it is an extremely deep thread, that's a great question...although the single point threadmill which is good for multiple pitches is much slower than tapping. But dedicated pitch carbide (insert or solid) threadmills which give you in many cases depths of 2 x diameter with a single interpolation are pretty much as fast, and last a long time.

[littlerob]

Your right Greg I was mixing thoughts (single point-threadmill), still doesn't change the question though. Either way he is going to save money. Threadmill is great!!

Robert

[brettcnc]

We are tapping 60mm deep.
Had about 1000 holes to tap/thread.

Thread milling is slow, Mill should be able to tap M24.

[budgieW]

That really depends of what MAX spindle speed you have.

[littlerob]

We are tapping 60mm deep.
Had about 1000 holes to tap/thread.

Thread milling is slow, Mill should be able to tap M24.

Threadmills are NOT slow, even if you only have 5000 RPM it's faster than breaking $200 taps. 2 or 3 passes at 5000 RPM is not slow, in fact it's fast, and nore consistent. The point is your breaking taps and this is an alternative, in fact no one is tapping that big with cnc, for this reason.