[mike sr1]

I have a question on tapping aluminum, I have been tapping using the coolant for lubrication, I dont think this is sufficient after breaking a tap. Is it common practice to shut off the coolant and use tap magic or something similar for each hole?

The holes are tapped 5 mm x .8, drill size is correct for 75 percent thread they are .375, .5, .625 deep thru holes. rpm is 300, 10 ipm feedrate.

Thanks for any help with this.

[SCzEngrgGroup]

I would bet that depends a WHOLE lot on what coolant you're using. Some, like KoolMist, provide almost no luibricity. Others, like soluble oils, can be pretty good.

Regards,
Ray L.

[takewhatyoulike]

I have tapped 10s of thousands of blind holes in 6061-t6 aluminum using a Balax form tap with virtually no tap breakage. I use Relton A9 instead of flood coolant when tapping. Amazon.com: Relton PNT-A9 Aluminum Cutting Fluid Pint: Home Improvement

Don Clement

[mike sr1]

I would bet that depends a WHOLE lot on what coolant you're using. Some, like KoolMist, provide almost no luibricity. Others, like soluble oils, can be pretty good.

Regards,
Ray L.

I use soluble oil om my machine.
I also went to a 2 flute tap, I am having good luck with tapping half the depth, then repeating the operation at full depth, this is working fine so far on the deeper holes. It could have been the tap was getting dulll as well.

[SomeWhatLost]

I am using whatever coolant tormach sells, and it doesn't work at all for tapping aluminum...
Tap Magic on the other hand works great, BUT it does not mix well with any coolant that may still be on the part/table/etc... turns into some super gooey rusty staining type mess if not cleaned up right away...

[fizzissist]

Man, I can't imagine what kind of crap coolant you guys are using... but I have tapped thousands and thousands of holes in alum. with both cutting and forming taps with never a problem that wasn't related to improper tap drill hole size, chips in the hole, or a dull tap. ..... Using regular 'ole 10% water soluble ... E206 is the usual coolant, but I've used others with good success.
I've used a lot of WD-40 and Koolmist on alum too, and never had problems that were coolant related.

I'm inclined to think that there's a lot of cheap taps in use here, and you're payin' the price on the back end.

[BAMCNC.COM]

I've used KoolMist mixed 10% with no issues.

[mike sr1]

Thanks for the tip on the Relton A9, i will get some.
Thanks

[Just Me]

I would first kick up your RPM 300 is way too slow...you need a higher RPM to have the toque to break the chip (use low gear)...I tap 5MM holes 1/2 deep 800 RPM in 6061 using flood coolant (Rustlick areo)...I also tap 17-4 SS 1/2 deep 5mm holes at 500 RPM and use Moly D tapping fuild...
When did the tap break...going in, when change of spindle direct or on exit...did the tap over travel and bottom out...
Also why do you need 75% thread...I never drill to 75% unless called out on the print use 70% and I bet you will not break half as many taps...
what type of 2 flute tap did you use...

[jeffery926]

It's been my experience that you get what you pay for, so you need the best quality when tapping. I would recommend a OSG brand spiral flute tap designed for tapping aluminum and just use a 10% Koolmist & water for coolant. The spiral flute will raise the chips out of the hole like a drill does. I even use them for through holes. Quality does matter.

OSG Tap & Die, Inc.

[mike sr1]

Thanks for the suggestions guys....
I just need to get the hang of machine tapping, after all this is 6061 not 304 stainless. There is no "feel" when I tap on the machine, it either taps correctly or its broken ha! I probably had 250 holes on that tap, it was a spiral flute as well. The new ones are spiral point.

Thanks again

[jeffery926]

That OSG link I posted is for tapping aluminum, not 304 stainless. Under Recommend, there are 2 circles next to the 6061, 7075 and cast aluminum. Below, best is marked. On that page there are also links to recommendations for speed/feed and tap drill sizes. No tap will last forever, so you just need to figure out how many holes you can tap before it will fail and break from getting dull and change it before that hole count.

[takewhatyoulike]

Mike,

With aluminum 6061-T6 you can use a Balax forming tap instead of a cutting tap. http://www.balax.com/catalog/thredfl...ing-vs-cutting The main advantage for me in tapping blind holes is there are no chips produced with the forming tap. I also use a Procunier reversing tap head on my Tormach which stops within 1/3 rev. The Procunier tap head allows me to tap 4-40 blind holes at about the maximum feed my series I Tormach can go @1200rpm: 30 IPM down feed and retract at 60 IPM no dwell. Also because the tap is not cutting, there is no cutting edge to dull and the Balax forming tap appears to last a lot longer in my experience than with cutting taps in aluminum 6061-T6. YMMV

Don Clement

[BAMCNC.COM]

Just a FYI for form taps, the hole will not be the same size as you would have for a normal tap.

[jeffery926]

Also, if you don't chamfer the hole first when using a forming tap, it will raise a burr up above the surfaces. Formed threads are stronger then cut threads are.

[takewhatyoulike]

Also, if you don't chamfer the hole first when using a forming tap, it will raise a burr up above the surfaces. Formed threads are stronger then cut threads are.

I use a spot drill before drilling the hole for the forming tap. The the spot drill allows not only for better centering when drilling but allowance is made for the chamfer so no burr is formed when using a form tap. Here is the Balax chart drill size for forming taps. http://www.balax.com/catalog/thredfl...ole-size-chart

Don Clement

[jeffery926]

I use a spot drill before drilling the hole for the forming tap. The the spot drill allows not only for better centering when drilling but allowance is made for the chamfer so no burr is formed when using a form tap. Here is the Balax chart drill size for forming taps. ANSI Thredfloer Hole Size Chart | Balax | Forming Taps, Cutting Taps, Thread Gages

Don Clement

I never use spot or center drills in a CNC program, just peck start the hole with a split point tap drill size. It saves on one operation that is not necessary.

[mike sr1]

Thanks for the info Don, I have never tried a form tap, I do have a few of them, I will give them a try on some scrap and see how it goes.

[fizzissist]

I never use spot or center drills in a CNC program, just peck start the hole with a split point tap drill size. It saves on one operation that is not necessary.

I always use a 90deg spot drill in my CNC programs... Z- to a dia just larger than the major, so the drill has a comfortable place to start and I don't need to chamfer or deburr after the part is machined, saving an operation.

[jeffery926]

I always use a 90deg spot drill in my CNC programs... Z- to a dia just larger than the major, so the drill has a comfortable place to start and I don't need to chamfer or deburr after the part is machined, saving an operation.

I don't need to chamfer or deburr the part afterwards either. It really depends on what kind of parts/jobs each of us are making. I'm glad I have jobs I don't need to do all the extra operations that you do.

I'm sure Mike will do it his own way and I think we are getting a little sidetracked here.