ridgid tapping

rcavalieri · Jul 7, 2014

here at our shop we have a new cnc genos m460 mill and my operator has 7 + years running cnc mills but he is having a hard time with tapping on it, he is trying to run a m2 x 0.4 tap he is running it ridgid in 13-8 mtl. and only .135 deep in a thru hole but he keeps breaking the taps he is running at 480 rpm so we called the manufacturer of the taps and they say run it at 1700 rpm ? we have not do this yet not sure whats going on any suggestions.

shane123 · Jul 7, 2014

i always try to form tap on small holes. makes life easier.... that does seem high for rpm....

Dave K · Jul 7, 2014

That don't sound high to me for an rpm. Because that tap is so small. However, you should have no problems running slower, and I'm not exactly familiar with that material. I will share with you a story, not sure if this will help or not. I had a tap made by a company (it was an odd size), and it tore threads on me unless I tapped by hand and used cutting oil. The told me I was running it too slow,and wasn't getting a good "shearing" action at the cutting edges. So, reluctantly, I bumped up the rpm, and what do you know? It worked nice.
So, I'd give it a try. 1700 rpm is not too fast for that small of a tap.

SwarfsUp! · Jul 7, 2014

Suggestions:

Make sure the thread pitch is programmed correctly.

Try a spiral point tap that sends the chips out ahead of the tap.

Try using a cutting fluid instead of the machine's coolant.

Cheat a bit on thread depth vis a larger tap drill.

Peck tap?

I love forming taps but I've never done one smaller than M3. I especially like them for blind holes.

reedeprintice · Jul 7, 2014

sounds like a pain

Bobw · Jul 7, 2014

Its 13-8... Making holes in 13-8 just generally sucks. Tapping those holes is worse...

What kind of tap are you using?? 13-8 "annealed" technically solution treated... is going to be mid to high 30's on the C-scale,
and its a bitchy material.

I'd rather drill and tap Ti all day long...

Brandon Dixon · Jul 7, 2014

Any chance that this control requires the M29 and the previous controls did not?

tay2daizzo8 · Jul 7, 2014

Make sure your in ipr not Ipm my okuma and mycenters are completely opposite. . G94 starts one but it cancels on the other machine

AlumiMan · Jul 7, 2014

When does the tap break?

Dave K · Jul 7, 2014

AlumiMan said:
When does the tap break?

When he tries to tap the hole............ I just had to. :leaving:

Edster · Jul 7, 2014

You said it was a new Genos mill. Have you rigid tapped before on this machine? All my Okumas came with rigid tapping but were set to floating in the parameters. I don't remember the screen off hand, but it should be pretty easy to find. Set it to synchronous if it's not already.

Jashley73 · Jul 7, 2014

Another vote for cheat in the tap drill... Use a larger drill, if only by a few thou...

BobM3 · Jul 7, 2014

Is this a type of stainless that work hardens easy? If so, then the slow speed might be the problem.

TeachMePlease · Jul 8, 2014

Wasn't there a recent thread where someone specified that even during rigid tapping, some MTB/control automatically retracts at 1.10x the programmed feedrate? If you're tapping through holes, and going too deep, I could see the back of the tap colliding with the material and snapping the tap.

I have no experience with this just a shot in the dark.

upnorth5axis · Jul 8, 2014

Are your taps running out in your solid holder? are they breaking going in or on the way out? maybe try around 1000 rpm with cutting fluid

digger62 · Jul 8, 2014

I've had issues tapping 17-4 in the past. Make sure you have a quality tap rated for the hardness of material. Using Moly-Dee instead of coolant can make all the difference as well.

Edster · Jul 8, 2014

TeachMePlease said:
Wasn't there a recent thread where someone specified that even during rigid tapping, some MTB/control automatically retracts at 1.10x the programmed feedrate? If you're tapping through holes, and going too deep, I could see the back of the tap colliding with the material and snapping the tap.

I have no experience with this just a shot in the dark.

On some machines you can increase the spindle speed upon retracting the tap in rigid tapping mode, but the feed is also increased to match the retract speed.

What your saying is typically done when using floating tapping mode. Sometimes floating holders will only float in one direction so you have to make sure any error goes the direction the holder is able to float. For example your holder will only float out. You need to feed in slightly slower than you should so the tool will float out and retract slightly faster.

Don't forget on Okumas during rigid tapping you can hit the slide hold button while the tap is engaged. The machine will then reverse out of the hole and wait. Press cycle start to continue tapping the hole. A quick and dirty way to peck tap.

Metalcutter · Jul 8, 2014

Lay a 6" scale horizontal on the vise, sticking out in the air about an inch. Bring the Tap close to the scale end and run the tap cycle. While looking at the scale end, as a reference, let your mind concentrate on the tap threads. Thread movement should appear to be dead still, during the cycle.

If you find the air being tapped correctly, maybe the metal will also be happy.

Just had to say this.

Regards,

Stan-

rcavalieri · Jul 9, 2014

thank everyone we wound up running the spindle speed at 840 up from the original speed and not the 1700 that was told from the tap manufacture and the material is annealed, also we called the okuma rep and found out he peek cycle was going .050 at a time and we were able to reduce it to .030 and with all that it is working.

ridgid tapping

Plastic

Aluminum

Diamond

Aluminum

Stainless

Diamond

Aluminum

Hot Rolled

Plastic

Diamond

Diamond

Titanium

Cast Iron

Diamond

Hot Rolled

Aluminum

Diamond

Titanium

Plastic

Similar threads