[CNCMike]

I am tapping 6-32 blind holes in our CNC VMC for the first time and I am having some trouble with it. The material is 6061 aluminum, drilled 0.75" deep with a #36 drill. I am tapping the hole 0.5" deep with a 3 flute plug tap, in a floating tap head, using a G84 cycle. I have tried multiple feed rates along with different coolants. No luck, just broken taps.

Should I be using a high performance tap, or a thread forming tap? Use a larger # drill?

Thanks for the help, Mike

[scadvice]

... a polished (no coating) 2 flute gun drill style. Use a good brand but you do not need a high performance.

Other things:

Check your hole size.

Check your coolant concentration.

Using Cooltool or some other tapping fluids can crash your coolant, not recommended and makes the boss real unhappy.(nuts)

If you want to not pack the chips in the hole, use a spiral flute tap that is for that purpose. Chip up and out instead down into the bottom of the hole.

One last thing, check the program for accuracy...

But I'm sure your problem is the tap your using.

Steve

[CNCMike]

Thanks Steve, I will look into your suggestions and give it another shot.

Mike

[HuFlungDung]

6-32 is one of those 'weak' tap sizes. I'd probably step tap the hole.

JFK (just for kicks) drill a hole and tap it with the type of tap you were using. Start it perpendicularly. Get a feel for how the tap begins to bind up after a few turns, even with the best oil on it.

Then try a spiral flute tap (blind hole) or a spiral point tap (through hole) with the hand tap and lube that will be used. You should be able to detect quite readily how many turns it is safe to go in one cycle.

[gsrmmeza]

I would use a thread forming tap for the .500 depth but if you really want to use a cut tap I would go with the high performance tap made by Greenfield. The only problem with that is they cost $16.74 each. I am using this style tap at work right now but metric on 2 different machines. Both taps have done over 1600 holes and they look as good now as when I started. The taps I use are the Greenfield EM-AL high performance for aluminum with the 45 degree helix. Here's a link to them at MSC:

http://www1.mscdirect.com/CGI/NNPDFF...8440&PMCTLG=00

[Caprirs]

On small holes (under 1/4"), I always use form taps. No chips and the tap is much stronger since there are no flutes to reduce the cross section.

1. Spot drill so you have some chamfer at the top of the hole after the threads are formed. With a 90* 3/16 spot drill, I would drill .08" deep.

2. Peck drill with a .128" drill 6000rpm .08" pecks F10. If you want .500" of thread, you'll need to drill sufficiently deeper for the lead of the tap, so maybe .650" with a tap that has 3 thread lead. Check the hole size after drilling and before tapping for the first part.

3. Rigid tap at 1000rpm.


Make sure the tap is running true. If there is more than about +/-.001" runout, the tap may be flexing too much as it gets deeper in the hole.

Try tapping in "air" at 100rpm and put a dwell at the bottom of the hole. Mark the spindle and count the revolutions to check the accuracy of the spindle/Z synchronization. So run G84 Z-.500 R0. E32 S100 P2. At the bottom, the spindle should have turned precisely 16 revs. If it isn't exact, that obviously can cause issues.

[Kevin Taylor]

First make sure that the floating tap holder does infact float both directions I had this experince early on with my CNC and found that the holder would compress but it would not strech and make sure that the feed is spot on I was instructed to program a slightly slower feed rate so the holder get's longer on the way in and shortens up as the spindle slows to reverse that fine of thread and the material I wouldent be in a hurry unless you have a lot of holes per part If you have room drill deeper than needed and make sure the chip's are out of the hole . Shorten the tip of the tap to make room for the chips and try WD40 or a stronger mix of coolint spirel tap's that small look like there wating to break Good luck Kevin

[scadvice]

...good suggestions. Two other points about forming taps, is that the thread form is tied very closely to the hole size, in other words, check the hole size of your drill to make sure you get a completely formed thread and check the machinist handbook for the drill size, as they are different than the cutting taps. The last comment is the formed thread, made using the correct sized hole, is about 25% stronger than a cut thread.
Steve

[Mitsui Seiki]

Use a spiral tap.Much better for blind holes.
Gun nose taps push the chips in to the hole and spiral taps pull it out.
S400 F12.5

[CNCMike]

Thanks again for the suggestions. I ended up using a 6-32 form tap with a 0.125" drill from memory. No special tapping fluids or WD-40 were required.

This specific application didn't require tight tolerences, so I would still like to try a few tap brands/drill size's before I am confident in repeating accuratly. This was my first time form tapping.

Mike