Breaking taps need help!

Hello all, fairly new to CNC lathe work after years of manual machine work. I have often searched the forum for answers with good success.
But I do have a problem with tapping M4 thread into stainless. I have just purchased a floating tapping head for the job which is 200 threads. Just broken my 4th carbide tap. My machine is an Okuma LB15.Need help don’t want to tap by hand.
I have also checked the alignment(within a couple of thou) and used recommended speed.
This is part of my program for the job:
T0808 G97 S350 M42 M03 M08
G00 X0.0
Z5
G01 Z-6 F0.7
M04 M63 Z5

Can anyone tell me what I am doing wrong?
The tapping head certainly seemed loaded up (pushed in) when the tap broke.
Regards
Will

Lets start with first things first. I noticed you said that you checked the alignments and they were within a couple of thousandths. Start there. This is way out of Okuma spec. I am assuming you are talking about the Incline and Parallel adjustment of the turret. The Okuma spec is 20 microns which is less than a thousandth. This is for both checks. The first thing that needs to happen is get the turret properly aligned. You will need a good coaxial indicator to sweep in the turret for the X alignment and zero set. Check the Parallelism first. If this is out then you need to adjust this first as it will change the Incline if you do the Incline first. It may also be that the Headstock is out of alignment. This also must be checked. I would recommend starting with these alignments first as this is what a service engineer will check first if he were to come out. Again the tolerances are 20 microns but you should be able to get them pretty close to zero which i would recommend when drilling or tapping. Most times these adjustments are the culprit when breaking drills or taps. It certinly could be something else but you need to start with these adjustments first.

yes, CNCZILLA is absolutelly right. Mechanical adjustments first.
and next.
You better use tapping cycle in part program, since feederate is not synchronized with spindle revolutions at regular G01.

First off, I would not recommend using carbide taps in stainless for the smaller size threads like M4. I am tapping 15-5 stainless @ 35 RC with a 3/8-24 tap @ 240 rpm & 10 ipm with a G84 cycle on a Okuma horizontal mill with a floating tap driver and Hangstefers heavy cut oil. I am using a Emuge HSS Rekord 1D-TI TICN Spiral flute tap. When using a small diameter tap like an M4, you are dealing with such a small diameter that by using a carbide tap, unless absolutely everything is perfect, carbide is going to be much more likely to break off since it is so brittle. I would recommend trying out Emuge catalog # B383, EDP# B0456001 spiral flute tap with a 3,30 minor diameter drilled hole. Also I would advise for you to try cutting your rpm & feedrate in half, when tapping with such small taps. Make sure the floating driver you are using is soft enough for the small tap size you are using. When I say soft, I mean when you push down on the driver it should collapse with just even pressure. You do not want it too soft for then it will be harder to get the tap to start but if it is too hard then it will act like a solid extension. Within the range of the depth you are tapping you want the tap cycle to be able to work within the rage of your tap driver. It should collapse slightly when you enter the hole and then slightly expand coming back out of the hole. I hope this will help out some. I do not use metric taps. The smallest I am tapping in 15-5 right now is a 10-24 STI thread that I run at 240 rpm @ 10 ipm. One of the 15-5 parts we are running has 4-40, 5-40 & 6-32 threads in them that we were hobbing but could never get them consistantly to size at full depth. We knew if we tried to tap these on the machines that we would just end up breaking some taps along thw way. Our machines are old enough that they cannot do syncronized tapping. We do all of our small taps manually by using a small air powered tapping arm. We first use a plug tap then chase that with a bottom tap. The end result is, no broken taps, threads are to full depth and it is faster. Good Luck!

The guys are right, alignment and center are critical. HSS and form tap help as well. From a code standpoint, you are leaving no "margin for error" with your floating head to allow for non-syncronous tapping. I've had good luck by reducing the feed on the way in so that your tapping head pulls out some by the time it reaches the bottom. Then when you reverse, feed out at actual feed when reversing. STM codes always are answered first before feed rate becomes active, and your M63 helps, but you have no float in your head at the point of reversal.

Try this: (I'm assuming your tapping head will extend but not compress)

T0808 G97 S350 M42 M03 M08
G00 X0.0
Z5
G01 Z-6 F0.7*.9 (=90 PERCENT FEED ON WAY IN)
M5 (OPTIONAL, BUT MAY HELP TO CONTROL DEPTH)
M04 M63 Z5 F.7 (ACTUAL FEED ON WAY OUT)

You will never reach the speed to justify the carbide, so I'd suggest going to the less expensive HSS.

Best regards,

PS>Synchronous tapping using the main spindle is an option on the newer machines....

Agree 100% with alignments, and not using the carbide tap. Also collet chuck or chuck? Feed a little slower, let the holder do some work, and coolant and small taps never works well in stainless. Get a hamster bottle with some tapping fluid and attach it to the firewall. Bump it with the tap to oil then do the tap.

I didn't see anyone mention the hole condition. The thread engagement needed for sst vs alum is lower, hence you can use a bigger hole.

Good point, it also needs to be deep enough to allow for the tip of the tap, but I'm thinking that as obvious as hole depth and diameter are that you wouldn't have been posting if it were that simple...right?

Underthetire - I liked the hamster bottle idea! LOL ;-)

Quote:

---

Originally Posted by underthetire

Get a hamster bottle with some tapping fluid and attach it to the firewall. Bump it with the tap to oil then do the tap.

---

That is good huggin' idea. But I feel bad just thinking about the production part you fought to come up with it:D

Also remember that stainless is really very soft, depending on your tolerances, using the chart for what hole size to drill can usually be exagerated pretty far with 304, as a cut tap will reduce drill hole diameter quite a bit. Almost like a form tap. Like Matt said drill it out big.

Also agreed on dumping the carbide, it holds up better but there is alot more forgiveness with HSS

Back in the game, Robert

Many thanks for all the input you guys have given me.
Things really were't stacking up for me at all yesterday and I have taken all your advice onboard.
This is I am switching to HSS taps.
Reducing the feed rate to suck the tapping head out on the infeed.

As I said I am fairly new to the CNC lathe world and am always going to be up against it as I am pretty much teaching myself.
Anyway I have found a fundamental mistake that only a first yaer apprentice would make.
This is the tool I called for the tap I usually carry a boring bar in and guess what, still had tool nose compensation on of 0.4mm.
Feel a bit ao a dill and probaly need a kick in the head.
But again many thanks and will keep you all posted on my progress after my new taps arrive.
Regards
Will

Quote:

---

Originally Posted by OkumaWiz

Good point, it also needs to be deep enough to allow for the tip of the tap, but I'm thinking that as obvious as hole depth and diameter are that you wouldn't have been posting if it were that simple...right?

---

You never know... :)

G'day mate

Try a squirt of rocol instead of coolant...

all of our tapping is done with rocol,It'll help you taps last a bit longer

http://www.rocol.com.au/index.php?op...=67&Itemid=150

I just happen to reading okuma posts and I saw your post.
I saw in your comand line that you were using a M42 at S350.
I seem to remember that when a M42 is listed, the machine will
lock your lowest rpm at about 750 rpm. You may need to switch to a
M41 (low range) to get your correct rpm. Also I would try a tin or ticn (hss)
coated roll-tap. If you have a minor dia. that is going o/s because of to big
of a drill, you may have to use a reamer for a more exacting thead. Also switch to a canned (G84) tapping cycle.

Good luck, Roundieland