snapped tap

[rrrhaas]

Hello everyone,
I am running wf3 on a Haas vf3ss. I am tapping 5/16 18 threads in 6061 alum. to a depth of 1.190 with a high speed steel, hi spiral flute, 52 degree semi bottoming tap. spindle speed -782 thread feed 18. I have 30 some holes to tap- the tap described above was just what I had at hand , it broke on the 7 th hole.
any suggestions would be appreciated.Is there a rule of thumb for cnc tap depth, ex. 3x diameter, in that case would the rest of the threads be done by hand later?

thanks, randy

can you peck a deep tap, can you set a torque limit for rigid tap?

come on guys, this ain't rocket science, I'd help you if I could..... and will repay in time.

thanks again,randy



Edited by: rrrhaas

 

[cncwhiz]

There are a few ways to do this hole. I m not sure about a Haas but a fanuc can do a "peck" tap cycle. That would reduce the chip buildup in the flutes of the tap. You could form tap the hole and you should be ok. What type of coolant are you using? If it is a soluble make sure the mix is correct and the tap is getting plenty of coolant flow to it. The material you are tapping makes a gummy chip and it is alomost for sure the root of the issue.

 

[rrrhaas]

thanks, coolant is soluble and correct. anyone know if a Haas vf3 ss can execute peck tap
randy

 

[harrisa]

The tap mighty be snapping because from torquing or twisting. You need to add a dwell of 1 sec. to allow the tap from torquing or twisting. I do this in steel and alum. The tap cycle on the Haas increases speeds and feeds when backing out. This happens really fast going into reverse.


This will allow the tap to relief stress in the shank. Breakage usually occurs at the last thread on the tap. You didn't say at what part of the tap was it breaking.


Also I thoought the Haas has sinc tapping so you can retap the same hole. All you need to do is give a second Z-axis move.


G84 R.25 Z-.750


z-1.250



IQUESTION YOUR SPEED AND FEED.Try540 RPMs and 30 IPM. Feed.


RPM's / Pitch = Feed. Your RPM's seems kinda fast to me. Unless your using a special coated tap.

 

[dbrainsky]

rrrhaas,


From the Haas Answer man.


<A id=title_blu>Threading and Tapping
</A><A id=bold_gry>Multiple Deep Rigid Tapping
</A>
<A id=_gry>Dear Applications:


One of our customers wanted to perform deep rigid tapping by changing the Z value (Z = 20 mm, then 26 mm, then 31 mm) using G84. However, each time the tap penetrated in a different position it destroyed the tap. Any suggestions?


Jacob Atlas





Dear Jacob:


You need to enable parameter 57, bit 7, REPT RIG TAP. Set this value to 1. This enables repeatable rigid tapping and will allow you to peck tap any hole.


Sincerely, Haas Applications


</A><A id=_gry>Dear Applications:


Is there a special G-code for doing rigid tapping on my Haas VF-2? If I hold a tap in a regular collet holder, and use rigid tapping, can I tap a deep hole in two steps (i.e., tap 3/8" deep, clear chips, and then tap 3/4" deep)? Will the spindle orient and pick up a thread in the same spot? If I

 

[rrrhaas]

[No message]

 

[cncwhiz]

A few other things to consider. Your speed can go alot faster for aluminum. I program much older machines and I run at least 1000 rpm. I also change from ipm to ipr. This allows you to play with the rpm of the tap and not have to redo the feed. The lower the rpm is the more prone to breakage it will be due to a lower surface feed than the material needs to see.

 

[rrrhaas]

[No message]

 

[rrrhaas]

thank you all,

I'm not alone, there are others out there like me