What's new
What's new

Breaking taps in aluminum on a fresh Haas VF2SS

evidence_UA

New member
Hi, couple of weeks ago have faced a problem that our fresh Haas VF2SS(2019) breaks taps on "small" treads like metric M2 and M2.5 in aluminum (6061, 2024) (it's something like UNC 2-56). Does anyone else also have such issue? Honestly, do not where should i look to find the solution: the hole is straight (i mean has no deviation in direcction, not it's sexuality), no chip inside, feeds and speeds are OK and we cut using them for the last couple of years until the problem occured. Pecking also won't help. I thought that there is a problem in material properties (maybe it wasn't heat treated properly) and tried thread formers but they also break on these threads...
 

Milland

Active member
Make two test blocks from either material, roughly 50mm x 150mm x 12mm. Clamp them together in a vise such that you have a block 50 x 150 x 24. Now set up such that you can drill and tap on the centerline, and make a series of drilled and tapped holes (replacing taps as needed if they break). Note any changes to your process if you decide to experiment with different speeds/feeds or coolant method.

Then remove the blocks from the vise, carefully separate the two pieces, remove any broken taps as required. Observe the threads - how deep did the tap go, do any of the threads look deformed, etc. Ideally take some pictures and post them here.

This will help you determine if it's an actual threading problem, or some other reason for breaking. Threads that show deformation may be due to a mismatch of thread pitch to programmed feed, or perhaps there's a setting that's withdrawing the tap faster than entry speed? I presume you're rigid tapping...

If nothing is obvious, it might be worth buying some compression/extension tap holders, which give you some freedom if the machine is not feeding correctly but is only a little off.

And there's always thread milling...
 

beege

New member
I got a new VF2 a couple of years ago. It came with the setting for 4X spindle speed on the retract. Broke a couple of taps before I discovered it. Check the retract RPM, change it to 2 or 1 .Mine at 1 has been working.
 

Orange Vise

Active member
It's probably the material. Too gummy, bad heat treat (possibly still within spec, just sucks for the machinist).

To rule out the machine, tap the same material in a different machine.

And/or tap different material in the same machine.

And/or anything else you can think of, following a system process of elimination. Try to change only one variable at a time.
 

coyoinu

Member
couple of things -

for those metric threads, it's important that you use the correct drill size, esp when form tapping. The closest imperial drill doesn't always get you the correct thread percentage. seeing as you're in europe, hope that's not a problem.

also, if there's not much clearance at the bottom of the blind hole, i have seen the tap overshoot the target by ~.050" once in a while. we found that out the hard way. you can test this by setting a travel limit and tapping a grid pattern, if the machine overshoots it'll throw an alarm. it even happens if you tap up.
 
Last edited:

Lazyman

New member
I got a new VF2 a couple of years ago. It came with the setting for 4X spindle speed on the retract. Broke a couple of taps before I discovered it. Check the retract RPM, change it to 2 or 1 .Mine at 1 has been working.

Same situation here. Eliminating 4x retract RPM solved a lot of tap breakage issues for me.
 

Lynn R.

New member
Also, make sure setting 133 is to ON (rept rigid tap)

This was set to OFF from the factory on our new vf2ss. Turning it on made things better.
 








 
Top