Small Taps Breaking

[ALLtra Mach]

We have constant problems with breaking taps 1/4" and smaller.
Machine is a new Mori NV5000 VMC.
We are running low RPM, Ridgid tap cycles w/floating holders.
Have changed coolant.
The parts we are on now, we ran 50 of last run went fine, this run so far we are 4 of 6 scrap so far?
Material is CRMS bar.
Any body Ideasa on this.
Any one have luck in Steel with small taps?

[Geof]

Why are you using a floating holder with Rigid tapping? This is not needed and I have found it can be a detriment. In addition you cannot repeat rigid tap (peck tap) with a floating holder.

Keep your coolant richer than most manufacturers recommend; we use up to 15% and can expect problems when it gets below 10%.

How low is low rpm? I have found that sometimes the rpm can be too low, the chips seem to flow better at 1000 rpm than, for instance, 500rpm. On taps smaller than 1/4" go above 1000rpm and if necessary use a largish R for acceleration space.

If possible tweak the thread percentage; are you allowed to go down to 65% as opposed to 75%? This can help immensely.

Use the correct tap; machine taps, spiral flute for blind holes, spiral point for through holes.

Repeat rigid tap, aka Peck Tap, especially when going deeper than about 1-1/2 x dia.

Consider form taps, I don't use them so someone else will have to comment on this.

[djr76]

http://www.osgtool.com/index.asp


osg has real good technical data on tapping : application guide, troubleshooting, calcs ect.

[ALLtra Mach]

Why Can't I peck tap with a floating holder?
1000 RPM!?! l have to try that, was at 500 and slowed down to try to fix this.
Most of your other suggestions I have tried, helped some but the floating holders had seemed to have fixed the problem until recently it is back.

I follow mfg's parameters pretty closely most of the time, but all have failed me so far.

I have tried different styles, coatings & brands. Nothing seems to really work.

The only thing we can really get good results with is over sizing the holes.

[billystein]

Hi,

I have found that tapping fluid is 10 times better than my coolant.
even in aluminum the taps last much longer. just put m00 and squirt some on your tap.
I also have setup a tapmatic 50x head on a drill press and have my operators tap while the cnc is running.
billy

[ALLtra Mach]

I have done this also, but hate the oil in my machine.
And if you like Tap magic, try Castrols Moly Dee, hands down best tapping fluid on the Market.

Before I'd stop the machine to apply fluid, I would rather tap offline.

Ohh and why floating holders? Because thats what all the tap Manufactures suggested for tap breakage solution.

Appreciate all the input guys..lol..I will get to the bottom of this!

[Geof]

Originally Posted by ALLtra Mach Why Can't I peck tap with a floating holder?..

Because you need precise correlation between the position of the thread on the tap and the Z axis position. Rigid tapping users a marker pulse from the spindle to orient the tap so it will re-enter the thread when peck tapping, a floating holder may not return to exactly the same position so it throws the thread position off and when the machine enters the second times things do not line up.

[keebler303]

Geof

I would agree that its not best practices to use a floating tap holder while rigid tapping but if the machine is running a rigid tap cycle, it should be synced up so the floating holder doesn't move at all. Should be close enough that it will find the threads on the way back down.

Matt

[Geof]

Originally Posted by keebler303 Geof I would agree that its not best practices to use a floating tap holder while rigid tapping but if the machine is running a rigid tap cycle, it should be synced up so the floating holder doesn't move at all. Should be close enough that it will find the threads on the way back down. Matt

You have found a flaw in my logic, but I did use a floating holder once and it didn't give good threads; so I didn't think any deeper.

My holder must have had enough slop in it that it simply shook out of alignment. Of course the slop wouldn't matter for normal tapping going in only once. Bit difficult to check, I don't have it any more because I switched to using rigid holders, collets actually.

[ALLtra Mach]

BTW, did I mention depths of these holes are 4X Dia or moe?

And all of our floating holders are pretty tight, I have ran back through lots of holes with them.
I have been in the "Rigid tapping debate" for years & haven't decided what side I'm on.
I wasn't trying to argue, just figured you might have known something I didn't. Not to sound arrogant, but I have been doing this awhile and I think I pretty much know what I am doing. But I never quit listening to the advice of others. Which is why I love these forums, We only have two really well trained CNC guys in our shop. I run the shop & then my programmer. Good part is, I get things my way, which is always nice, bad part is I am expected to have all the answers all the time. So If I caan't figure it out, and the company reps can't figure it out...You guys are my "Last line of experts".
So, as you can guess, by the time I get on here with a problem, there has already been alot of time spent trying to fix it.

[HuFlungDung]

I don't know what kind of a test one could devise to check the 'tracking' of the tool. Do the successfully tapped holes seem to be on spec so far as an overcut condition is concerned? If there is some kind of lag error, I am thinking that the tap could cut the threads oversize, not in diameter but in thread thickness.

Even if that were the case, then one would have to come up with a theory about how that could happen. Perhaps a loose encoder coupling could cause the spindle to drift out of phase by a small amount. Also check the actual rpm against the commanded rpm in case there is some kind of bias in the spindle drive (parameters).

Is there any kind of repeatable characteristic as to when the tap fails? On the way down, stopping, on the way up? Is the down feed and up feed symmetric or is this one of those fast retract cycles?

[ALLtra Mach]

Always breaks on the down
Feeds same down & up

When the taps dont break, threads are always good. So if it is an encoder problem, it is not conistent.

Also, as long as we oversize the hole by a few thousanths, it does fine. And after my last post I have talked with operator again,. and most of our problems seem to be on holes deeper than 2X dia. So I am now thinking were just over powering a stalled cut.
Pecking may be the only option, or roll forming.