need help tapping holes

Have you tried a roll form tap?

No, 1/2 inch thick part, 1/4-20 thread, will this cause any distortion in the sides of the workpeice? Is there some rule as to how thin or how close you can get to a side wall?

I was thinking with my coolant in the machine I would be better off cutting rather than forming. Am I wrong? Thank You, Randy

Remove 333 from email address to reply.

Randy, I've used the OSG 295 series taps. They are 2 flute spiral point. I'm thinking that the three flute tap is more for steel and there's not enough room for the chips.

I'm also curious why people don't use the G95, feed per revolutin, command more when tapping. I know the math is the same. I guess I feel like I'm locking in the spindle and the feed. Not sure control wise if this is any better than matching spindle speed to an inches per minute feed rate. Maybe someone with control knowledge can weigh in?

Best, Steve

snipped>

Check your thread depth, it is best to run a few holes shallow, and check the depth, then adjust the depth accordingly, with that floating holder, you may be "drifting" deeper that the .600 that you have programmed, therefore the tap is bumping the bottom of the hole, causing the breakage, you can stay with the spiral flute, it is the best tap for the blind hole, assuming you cannot use a roll tap.

Hope this helps Darrell Reid

Sorry Randy, you're getting outside of my expertise. I rarely tap on the machine. In the few times that I have, I've found that roll form taps don't create chips in the bottom of the holes. It seems that the chips are what broke my taps the most.

No, we do some fairly thin walls. As long as the part is held well into the pocket, you should be okay. Plus, you can grind a teeny bit off the front of the form tap to get closer to the bottom.

Naw. Although I'm going to tell you this before Dobedave jumps on you: oill will owrk better for tapping. On critical holes, we stop the machine, blow out the hole and put a dab of oil on the tap with a brush. I've also had a small container of oil bolted to the table - just before you tap move the X & Y to the corner of the table, dunk the tap, and return to the part.

I've also had a

That's a cool idea!

BTW, I like WD-40 for tapping aluminum.

Suggest a plenty rich mix of water soluble oil--better yet, brush a 'whipped up mix' ( 80% soluble oil / 20% water ) directly onto the tap...

Randy wrote in news: snipped-for-privacy@4ax.com:

What's the concentration of your coolant?

Randy wrote in news: snipped-for-privacy@4ax.com:

Also, retrieve one of the broken tap ends, look at it carefully. See if you can see why it broke. (build-up, and where)

If your machine has rigid tapping then M29S800 must be on a block immediately before the G84 block. This is for the Fanuc 0i-MC. Also a parameter has to be set correctly for this to work.

Also you may want to move the R value up to .5 in order to give the machine time to sync.

As someone else suggested try going shallow in order to see exactly how deep the thread is going compared to what you have programmed.

Make sure spring loaded floating tap holder does not have any endplay before springs compress. Make sure springs are stiff enough for the size tap and/or not too stiff.

If there is a mismatch between programmed RPM and FEED tapping won't work so well. Make sure spindle is actually doing the exact RPM that is programmed. The same should be checked with the FEED. Some machines can get a little out of calibration. Watching the tap holder while tapping notice if the holder is compressing or extending as the tap goes deeper. This would indicate the wrong RPM or FEED for that thread pitch.

Don't know if any of this will help.

Rocky

That brings up a good point: it's possible that your compression holder is not catching the tap in the same spot on the part each time, so when you set your offset to go a bit deeper, perhaps another part, catching half a thread sooner, is too deep causing you to break the tap.

Admittedly this sounds more likely to happen in stainless or with little bitty taps, but it might be something to look at. We stopped using compression tap holders on our Fadals because the rigid tap was so accurate. In fact, we don't even use compression holders on the lathes, only the back-floating kind. You want to know that the tap is going to start the at the same location in each part.

Randy:

Was that a spiral FLUTED tap, or spiral POINTED tap? A spiral pointed tap (Gun tap), pushes the chips ahead of the tap. A spiral fluted tap pulls the chips out of the hole while you're tapping without having a wad of chips ending up in the bottom of the hole to possibly create havoc and extra time to remove them with some sort of paperclip with a hook on the end. As Dave Lyon suggested, a form tap (roll tap), might be what you need since you can tap much closer to the bottom of a blind hole.

Another little tid-bit to be aware of: spiral fluted taps are usually weaker than gun taps since they have so much material ground away to let the chips flow out, and gun taps are weaker than form taps since form taps don't have "flutes" in the normal sense of the term.

Check the Z axis thrust bearing. You will be breaking taps unexpectedly and somewhat randomly if you have a bum bearing.

Even with a floating holder ?

If the drive/axis sync isn't real good and the thrust bearing is shock loading the tap, yes. The F-0 does "Rigid", and not "synchronous" tapping so Z axis trouble is compounded. I just went through this last week and am pleased, and lucky, to be able to report 300 4-40 tapped holes on a 50 HP, 50 taper, gear head machine at

The MTB changed out the thrust bearing, I tuned the drive timing constants and the machines taps like a dream now and I'm back to an ER 16 holder. Just like the OP, I had hoped a floater would do the job but it really didn't.

I also switched to an AlTiN coated tap that looks like a hogging end mill. Pulls the chips right out of the hole and the threads are noticeably "cleaner" than form tapped threads. I'm going back in a couple hours to load another eight hours of code and I'll get the brand and style. We are using A-9 for the tapping operation.

Valcool VNT-700 at 6%, recomended is 4-7%

Thank You, Randy

Remove 333 from email address to reply.

Thanks to all, I did get it to work, I backed off the thread depth .05" went up to a #5 drill, and slowed it down to S600 F30. and it finished the first group of parts. I will order some roll form taps and try some scrap to see how they work.

On the CRT I do see the spindle speed vary +/-2 or 3 RPM and the Feed bounces around alittle too. But I've done smaller threads with no problem. It's just these blind 1/4-20's that are messin' with me. I used to use a spiral point (SP) tap and go shallow, clean the chips out and then finish tap by hand. But as I slowly get used to this CNC thing I'm trying to get the machine do more and me less. I used to do lots of one or two of a kind parts so it was no big deal. This job is

Rocky, I was using the following M29S800 G84 X...Y.... Z-.6 R.2 F40. G80

I could try a bigger R value, but I see no movement in my T/C tap holder. I have held a tap in an ER32 collet on this machine before.

Maybe I'll call OSG too and see what they reccomend. I did the first

OH, I did get to see it break one, and it broke on the way in, just short of z-.6

Thank You, Randy

Remove 333 from email address to reply.

=================== Thanks for sharing your experiences.

Unka George (George McDuffee)

...and at the end of the fight is a tombstone white with the name of the late deceased, and the epitaph drear: ?A Fool lies here, who tried to hustle the East.?

Rudyard Kipling The Naulahka, ch. 5, heading (1892).