What's new
What's new

M2 Form Tapping

cpreston

Plastic
Joined
Oct 9, 2019
Location
Michigan, USA
Long time Forum reader, first time poster.

Need help tapping M2 x .4, M2.5 x .45, and M3 x .5 holes in aluminum with 75% thread percentage. Taps snap with correct tap drill. Trying a drill the next size up drops the thread percentage causing ripped threads at assembly. Form taps and thread percentage is mandated by our customer. Torque specs for the assembly screws are mandated by our customer's customer.

6061 T6511 aluminum
2015 Haas VF-4SS. Tapping retract is set at 4, but we've tried both slower and faster
Spotting with a 1/4" x 120° NC spot drill
Using appropriate size solid carbide drills - 118° drill tip
Formula for determining appropriate drill size for 75% metric threads: Tap O.D. - ( desired thread% x pitch ) / 147.06
Example: (M2x.4) 2 - ( 75 x .4 ) / 147.06 = 1.796mm (.0707"), we're using a 1.8mm drill (.0709")
Rigid tapping. We do not have any floating tap heads. We have tried multiple brands of taps. Emuge. Guhring. OSG. Union Butterfield. Balax. Probably another 5 or 6 brands that I can't remember. All coated for aluminum. TiN or similar. We have purchased new tapping collets. We have purchased an Emuge Softsynchro high performance tap holder.
The coolant we use is a local brand I think, AFT (Advanced Fluid Technology) 619M2. The coolant concentration is nominal. I'm not a fan of the coolant, but there's no getting away from it. Coolant flow is great.
We've tried Tap Magic for aluminum - comes in a red/white spray can and is supposed to be cinnamon scented. We've tried Moly-dee. And some other off-brand, thick as molasses, tapping compound.

Maybe there's something simple that I just haven't thought of. Maybe there's something I just don't know about. Any help or advise would be appreciated, Thanks





Thanks everyone! A lot of great stuff here!
 
Last edited:
Are you measuring the hole your drill gives you?

You can drill a bit under and ream to size. This also allows you to make up for tight/loose % engagement by tenths if needed.

I would not use TiN coated taps, AFAIK TiN is kinda sticky when it comes to aluminum (not as bad as AlTiN but worse than shiny bright taps). I would think bright should be okay.
 
Hole size is critical.
Do you NEED 75% thread?
As for form taps, which style are you getting? 1 vent flute? Multiple vent flutes? Myself I prefer OSG form taps, we form tap C110 copper quite often and the tap has done thousands of holes.
Normally we buy Guhring taps, but for forming I think OSG has the upper hand.
 
Are you measuring the hole your drill gives you?

You can drill a bit under and ream to size. This also allows you to make up for tight/loose % engagement by tenths if needed.

I would not use TiN coated taps, AFAIK TiN is kinda sticky when it comes to aluminum (not as bad as AlTiN but worse than shiny bright taps). I would think bright should be okay.

Yes-yes... all of the above. Just 2nd-ing these suggestions. And 3rd-ing the fist suggestion that you must accurately measure hole size. Otherwise it's a crap shoot.

Dave
 
I like Balax for form taps, but we (fortunately!!!!) do not need to gage our holes as the work is our product. M2 = (approx) .08" so a bit larger than a 0-80 of which we do tons and tons of...

I ran into this problem years ago, have you checked coolant for concentration, as well as fines? Fines could actually be coming thru your coolant line and adding swarf to the coolant at the tap drill (yes total PITA and hard to control)...

As others mentioned, gage pre tap hole size as it is critical to form tapping, can also try different fits of taps, ie - H3-H2-H5.. whatever gets you to customer spec..
 
How deep?

1.8 is the right hole size for 75% M2x.4

I like to put my retract at .5 so the spindle isn't ramping up inside the hole...
 
Can you form tap larger, like M3 and M4, on this machine?
Can you post a code snippet?

Regards.

Mike



M2, M2.5, and M3 are the only 3 form taps we are struggling with for this customer. There are no other tapped hole sizes. We are new to form tapping. Mostly we cut tap or thread mill on parts for other customers. As the taps increase in size, the tap breakage is less often. So the breakage is likely related to the tap diameter.

This is a package of parts that gets assembled by our customer. The parts come in many shapes and sizes. Some have may six M3 holes, some may have fifty eight M2 holes and eighteen M2.5 holes. These parts run in multiple locations throughout the shop. Additionally, most of the parts have M3 STI holes in them that we cut tap. We have form tap breakage throughout. So it is not just that individual mill that can't tap.

Here is some of the code:

T9 M06 ( M2.5 X .45 FORM TAP )
G00 G90 G54 X-2.7523 Y1.4857 S300 M03
G43 H09 Z0.1 M08
G98 G84 Z-0.482 R-0.032 F5.315
X-1.905 Y1.3999
X-1.0373 Y1.4857
X-0.175 Y1.3999
X0.6902 Y1.4857
X1.555 Y1.3999
X2.4176 Y1.4857
X3.124 Y1.2583
X2.2789 Y-0.0001 Z-0.5214 R-0.0714
X0.6902 Z-0.482 R-0.032
X-0.175 Y0.5999 Z-0.5214 R-0.0714
Y-0.6001
X-1.0373 Y-0.0001 Z-0.482 R-0.032
X-2.6289 Z-0.5214 R-0.0714
X-2.9626 Z-0.482 R-0.032
X0.6902 Y-1.486
X1.555 Y-1.4001
X2.4176 Y-1.486
X3.124 Y-1.2586
G80 M09

T10 M06 ( M2 FORM TAP )
G00 G90 G54 X2.0624 Y-1.0946 S300 M03
G43 H10 Z0.1 M08
G98 G84 Z-0.475 R-0.0714 F4.7244
Y-0.1419
Y0.1416
Y0.1416
Y-0.1419
Y-1.0946
G80 M09


The speeds and feeds in this code are generic. The recommended RPM for a Balax M2 is S3555. We have tried anything in between S3555 and S300, thinking that might help. Not so much
 
Hole size is critical.
Do you NEED 75% thread?
As for form taps, which style are you getting? 1 vent flute? Multiple vent flutes? Myself I prefer OSG form taps, we form tap C110 copper quite often and the tap has done thousands of holes.
Normally we buy Guhring taps, but for forming I think OSG has the upper hand.


Hole size IS critical. We can manufacture these parts with a 65% thread percentage, but the torque specs on the screws will tear out threads at 65%

Some have 1 vent flute, some have 2
 
I actually thought that my retract HAD to be a whole number. I thought 1 was as slow as I could back out

Most are not tapping more than .200, some are up to .350
 
Maybe I missed it, but when are the taps snapping? Do you have a little chamfer at the top of the hole for leadin? Have you validated the hole size after drilling?
I agree with 1.8mm drill being correct for the M2x.4, bright taps(I like Balax), make sure it's not running out, run coolant at a minimum of 10% concentration. I keep my retracts at x4.
 
just curious, why is your retract plane below the top of the part?

These holes are inside a pocket. I rapid down to that point to cut time off the cycle. I am not a fan of G99 which would keep the retract inside the part. The G98 returns the tool to it's original plane at Z.1 after each hole. Then it rapids over and back down to the reference plane before starting the tapping process again
 
I'd make your R .200 min above start I usually run .5 your rpm is slow but I run slow also on alum and run at 500rpm on small taps 0-80 to 2-56 4's and up I run at 500-1000 depending on length.
make sure you spot about .025 deep max with a good center drill Like a #1 keo. you must have a straight round hole on the drilled hole. I only use cut taps as out customer requires it. form taps do break in smaller holes more. indicate your drill and tap if they dont run true thats a problem.
also on the spot drill put a small dwell in there that way you will get a perfect spot. if your spot is not sharp and defined your drill will walk.
I also have a haas vf2ss my machine doesnt like anything under .2 from the top of threaded hole.
we thread 4-40s and under ever day all day in alum. we did few thousand 0-80's a few months ago and 1 cut tap did them all parts were .175 tall with a through hole.
 








 
Back
Top