What's new
What's new

Help with tapping a 0-80 UNF in 6061-t6 Aluminum on a Haas VF2

JHunt

Plastic
Joined
Mar 26, 2020
So I have roughly 5000 holes to tap on small parts made out of 6061-T6. My callout is a 0-80 UNF tap .224 down in a blind hole thats .287 deep. What I have gathered so far is the following:

-Use a # 54 Carbide Circuit Board drill (not sure why) @ 6000 RMM & 10 IPM
-Use a roll form tap @ 1200 RPM with normal coolant

Is this info good? also, can I expect 1 tap to get thru all 5000 pcs? Thanks for the help guys!
 

eaglemike

Stainless
Joined
Apr 25, 2014
Location
san diego
I'd suggest the 229 series drills from MA Ford. They are made for performance in aluminum. What ever the maximum rpm of your machine, and use the feed per rev they suggest. The are carbide, 3 flute, and work very very well.
Agree for the form tap. I don't know which VF-2 you have. It might make a difference, as in how much distance to allow for accel/decel/reverse. If you machine can hold tolerance, I'd suggest 1500 rpm. That's what I was using without issue on an older VF-2, as well as some newer machines (through 2012). Your speed will be limited by the machines' ability. If the machine is capable, you could run 6K - but I'm pretty sure the VF-2 can't do that. If you have spare taps and material, try tapping at 2K, 2.5K, etc. Use a bright finish tap, or check with a tap mfr and make sure you are using the correct coating for aluminum. The wrong coating will ruin your day.
Might need to have your R plane higher above the part than the drill cycle, again depending on machine performance.
Suggest rigid tapping if you machine is in good shape, don't use a spring loaded tool.
Double check to be sure feed per revolution is correct, DAMHIK.
Good luck!
 

Mtndew

Diamond
Joined
Jun 7, 2012
Location
Michigan
That tap should last a lot longer than 5k holes. But we all now how things work in this line of work lol.
If you're not familiar with form taps, the drilled hole size is crucial.
 

Finegrain

Diamond
Joined
Sep 6, 2007
Location
Seattle, Washington
0-80 form tap gets a .055" hole, so I would be drilling a lot faster than 6,000 RPM. Yes, I would use a carbide drill. I like MA Ford "Twister Drill". This is currently what I get when I order "Quick-Change Carbide Drill Bits" from McMaster-Carr, and they have worked a treat for me.

Make sure you get and use a teeny tiny spotting drill -- normal-sized spotting drills have a web that is likely wider than .055", so you wont get a localizing cone.

Make sure your drilled hole stays very close to .055". Just a little bit over that and your minor diameter will be too big. Hole size too small, minor diameter will be too small, and you're much more likely to break the tap.

For the tapping, I would again go a lot faster -- 80 TPI takes quite a while at only 1,200 RPM.

Regards.

Mike
 

Delw

Stainless
Joined
Jan 8, 2019
Keo center drills work better than spot drills and last a 100 times longer. I run them in #0 and #1 size for small holes. both 45 and 30 degree.
 








 
Top