Rigid tapping aluminum 2-56 tap

[DaOne]

I am trying to tap about 20 holes in an aluminum part I am making out of 6061 T6. The hole is a through hole that is .25 deep. I am using a 95 Haas vf-2with ridged tapping. My problem is I am breaking taps on the first hole. I am using a spiral point 2-56 tap. It goes in about .2 and snaps off. I have never needed to tap something this small before. I have done tapping on this machine 1/4-20 and up just fine. Any suggestions?

[dertsap]

if drawing permissible then your best bet is to use a roll tap

[DaOne]

Any recomended speeds and feeds?

[dertsap]

500-1000 rpm

[DaOne]

My calculation in mastercam is...

3109 RPM
Feed 55.5233256

Can you tell me if this is right? I know my spindle never even come close to that speed.

[DaOne]

Looks like good ole mastercams calculation is the issue.. can somebody check this for me??

From what I have been told. For rigid tapping you figure feed by RPM X thread pitch.

It appears as if the tread pitch for a 2-56 thread is .0744. This would mean that if the RPM is set at 3109 then the feed should be 231.3096 and its set at 55.5233256 instead. So this is what I should be using....??

RPM 1000
Feed 74.4

Please if someone could check the thread pitch value is correct and the calculation that would really help me out to know if I am back on track before breaking another $20 tap in a $50 part on the last op.

[Delw]

From what I have been told. For rigid tapping you figure feed by RPM X thread pitch.

thats the correct way

a roll tap will do a thread better than a cut tap on small alum threads.
its very important to have the proper size drill for a roll tap and use good coolant.
also make sure your holders are running true.

[Delw]

here this will help
http://haascnc.com/training/MillProgram_PDF/xmwb.pdf

[gsrmmeza]

From what I have been told. For rigid tapping you figure feed by RPM X thread pitch.

This is correct.

It appears as if the tread pitch for a 2-56 thread is .0744. This would mean that if the RPM is set at 3109 then the feed should be 231.3096 and its set at 55.5233256 instead. So this is what I should be using....??

The pitch is 1 inch divided by the number of threads.
So 1 divided by 56 threads per inch equals .017857

RPM 1000
Feed 74.4

This should be 1000 RPM x .017857 = Feed 17.857

The tap drill size is a 5/64

[Haas_Apps]

Okay, I checked this two ways:
3109/56 and 3109*(1/56)

and my Windows calculator comes up with 55.51785 unless Microsoft is wrong again this would be the feed rate for 3109 rpm.

Looks like good ole mastercams calculation is the issue.. can somebody check this for me??

From what I have been told. For rigid tapping you figure feed by RPM X thread pitch.

It appears as if the tread pitch for a 2-56 thread is .0744. This would mean that if the RPM is set at 3109 then the feed should be 231.3096 and its set at 55.5233256 instead. So this is what I should be using....??

RPM 1000
Feed 74.4

Please if someone could check the thread pitch value is correct and the calculation that would really help me out to know if I am back on track before breaking another $20 tap in a $50 part on the last op.

[crabbass]

for TPI I use --- 1"/ tpi *RPM= Ipm feedrate. I see this is how some of you calculate it also.

The cam software I use (this may be an error with my postprocessor) will always generate a feed slightly faster than the above mentioned method.
When I tap holes (not verry often) it is rigid tapping, as I don't have floating tap holders-drivers etc.
The slightly faster speed I am talking about is verry slight, Like the post rounds to the .XX decimal when dividing the TPI. For example, I would have to tap a 1/4-20 like 10 inches deep to have the feed skip one lead.
Do the people using floating tapping heads program with this feed slightly increased to "load" the spring? Again, I have written this off on a post processor error, and when I forget to edit the feed to the exact pitch, I havn't noticed any problems, I don't usually tap deeper than .6" on a 1/4"-20