[pmurdock]

I've read and read all the posts on here about rigid tapping and it's supposed to be so easy. I don't see why i have such problems. Here's the scenario:

- 2008 Haas VF-2 w/ Rigid Tapping Option
-Tension Compression Tap Holder ("Command" mfg C4T4-0001 model #)
- Using Spiral Fluted 6-32 Bottoming Taps
- Tap Drill #36 per tap drill charts (maybe I need to go bigger?)
- Blaser 4000 coolant @ 8% on the Brix scale
- Depth of #36 Hole 0.6", Depth of Tap 0.2" - yes that's 0.4" of spacing for the bottoming tap to have PLENTY of room before it hits bottom!
- Material 6061-T6 Aluminum 3/8" thick Plate
- RPM is 1000, Feed is 31.25 for the rigid tapping (mastercam X2 MR2 SP1)


I break a tap about every 4 holes..:drowning:

Tell me I'm crazy but this should be working every time right?

Before I drill the #36 tap drill hole should I be using a center drill to start the hole out right for the #36? Maybe the #36 drill is wandering and causes the 6-32 to bend too much?

Is the tension compression tap holder hurting me here or should I just get a rigid tap holder?

Should I just forget the cutting taps and do a forming tap? will that solve all my woes?

Should I be doing any countersinking on the hole before tapping?

any ideas?

cheers,
Paul

[Eurisko]

First, throw the tension-compression holder away. They're useless. Use one of these with a dull tap, and you'll have hundreds of holes with shallow threads to hand tap later.

Since you're not breaking drills, I assume that the coolant isn't a problem, that the aluminum isn't gumming up on the tools. Make sure that the coolant is nice and slippery, though.

Spot the holes before drilling, leave a small chamfer for the threads.

Try a rigid tapholder, don't change the speed or feed. Use an uncoated tap.

If you still have problems, try a tension only holder (no compression).
Feed in at 95% of the actual pitch. This allows the tap to act as its own leadscrew, and will compensate for any minor spindle synchronization problems.

[dcoupar]

Are you tapping in low or high gear? I always had better luck with high gear on small taps.

[Geof]

You do have RIGID TAPPING turned on???? Sometimes this gets overlooked.

You can also turn on REPT RIGID TAP and then do two pecks for the tapping.

[pmurdock]

hehe.. the rigid tapping was the first thing I checked.. Parameter is set..

I have a rigid tapping head coming so I'll send an update regarding what the results are with the rigid tap holder.

Should I just go for the form taps and be done with it? any below 6-32 should be form taps - is that how one would approach it?

cheers,
Palu

[WayneHill]

I second the use of form taps for smaller tapped holes. They use a larger tap drill size. Check with the manufacturer for specifics.

[Geof]

hehe.. the rigid tapping was the first thing I checked.. Parameter is set.. ....cheers,
Palu

Also the SETTING? There are still both a Parameter and a Setting that have to be on? Yes? I know I was fooled for a while having only one turned on and breaking taps. That was on an older machine.

[chmillman]

Well I don't tap US threads, but I tap small metrics like 3mm fairly often...

First, you say that you are tapping in 6061 3/8" plate, but your hole depth is 0.6"? that's through the plate and far out the back side last I checked..

Second, you need 0.2" actual thread depth? And you have enough room to drill an additional 0.4" below that? Get a tap specifically designed for aluminum and for blind holes, the ones that actually pull the chip up out of the hole like a drill instead of pushing it ahead. Like this:

http://www.dcswiss.ch/EN/Products/ThreadTaps.htm

You can run your tap pretty close to the bottom of the hole with these, I usually leave 1-2mm or so, the rigid tap does stop the depth pretty close to programmed. I have pretty good results with these taps. --ch

[pmurdock]

Thanks for the suggestions again. You're right about going past the 3/8" plate but there is a sacrificial plate underneath so it looks like a blind hole..

the setting is also set for repeat rigid tapping..

these spiral fluted taps are just the type for removing chips out the top. Greenfield bottom taps.

I've been reading a few more posts and I'm beginning to wonder about my tap drill and whether it has dulled and is wandering upon drilling. I'm going to try using a center drill to center the hole and get a new tap drill and see how that does as well.


cheers!
Paul

[Donkey Hotey]

Time for the nOOb to help the nOOb. Relax. I just crossed this bridge myself...with 8-32 and 1/4-20 and I learned a bunch of things.

First: if in doubt about the taps or drill sizes, try tapping one manually using a drill press to keep everything square. Turn the chuck by hand or use it with a tap guide just to keep it vertical. I was shocked to learn how little force it was actually taking to push the 8-32 forming tap through aluminum. Most self locking nuts take more torque. You can get away with using collets. Trust me: a 6-32 shouldn't need much torque.

Second: the hole depth. You've covered it but it's worth repeating because that was part of my problem. :withstupi

Third: the drill size. There is no shame in going to a slightly larger drill. There are lots of drills available. Adding 0.004" to the hole diameter is only 0.002" per side. At 32 pitch, the threads are 0.016" deep. Blowing the hole out to a #35 will reduce the thread to 0.014". If the thread were that critical, you wouldn't be threading into the aluminum anyway. That chip clearance can make a small tap much happier.

Fourth: spot drill. It's been mentioned but the 'why' wasn't talked about. Small drills walk. I was doing 1/4-20 holes in brass and I scrapped about 5 parts before I figured out that it wasn't my work offset or dimensions. The drill was walking over. It was so far off center that you could see the problem. I don't know how far but I'd guess 0.020". The tap never broke. I have no idea how or why but it survived. I went back and spotted the drill location with a stubby engraving bit (I already had it in the machine and it was touched off). Problem solved. The rest tracked straight and true. I don't know if your 6-32 with the big spiral can survive being offset like I did it. Make sure it's going in straight.

Fifth: give the forming taps a try. No chips means no binding. Man, did they work nicely. I don't think I'm ever going to use another 'cutting tap' in aluminum.

So: I'd spot the hole to leave a small chamfer when you're done, go just a tad oversize on the holes, keep the bottom clearance generous and trust a forming tap to not bind the hole up with chips.

[fourperf]

I tap quite a lot of 6-32 holes on my vf2 rigid tapping er 16 or 32 collet. Spiral flute gun tap in 6061. 200 rpm .300 deep.

I might be able to go higher rpm but with such a small tap I am scared to.

mark

I am sure you probably know this but your feed has to be correct with your rpm. 1/pitchXrpm

1/32(tpi)X200(rpm)=6.25 feed rate

[Geof]

Go to 1000 rpm, easier to do the feed calculation .

I tap from 4-40 to 9/16" NC in steel or aluminum at 1000 rpm. Tried 3/8"NPT once and stalled everything.

[WayneHill]

I tap quite a lot of 6-32 holes on my vf2 rigid tapping er 16 or 32 collet.

(nuts) Use form taps on small threads. They last forever.

Check drill wandering like in the post above.

[fourperf]

scary but I will give it a try

[Geof]

scary but I will give it a try

Move your tool offset up a couple of inches and tap air.

[fourperf]

I put my clearance plane at .400

[Geof]

I put my clearance plane at .400

Actually I meant do some 'dry runs' without touching metal. Until you get comfortable with the speed at which it jumps around.

Regarding clearance plane there was a question in another thread: When you have Rigid Tapping why do you need a clearance plane raised above the work? The conventional reason is to allow for acceleration and for the machine to synchronize the spindle and feed before the tap enters. But with Rigid Tapping it is synchronized all the time...it has to be otherwise how does it stop at the bottom of the hole and then reverse out.

Yet I still use a clearance plane of around .2 to .4 just from habit.

[Vern Smith]

I had the same problems with 6-32 spiral flute taps, went to spiral point taps and all was well. Form taps are the easiest but I'm not really sold on cold forming aluminum.

Vern

[Caprirs]

I don't have a Haas, but am running a job currently with 6-32 threads in 1/4" thick 6061. Centerdrill .085" deep with a 90 degree spot drill, peck drill with 1/8" .390 deep, followed with a form tap in a drill chuck at 1000 rpm .35 deep. Flood coolant obviously. I start the tap at .025" above material.

[pmurdock]

I had the same problems with 6-32 spiral flute taps, went to spiral point taps and all was well. Form taps are the easiest but I'm not really sold on cold forming aluminum.

Vern

Vern,

are you using a #36 tap drill or do you upsize it a bit?

cheers,
Paul