[Delw]

I dont rigid tap that much and frankly I dont want to screw up a brand new machine with a badcode.
I have job that requiers 9 1/4-20 threads .50 deep through holes.
we normally do this on the hand mill and a tapmatic however I have some time and was thinking of trying it on the vfs22.

in the book they have the example set up as this.(using a 3/8-16)

T3 M06
G90 G54 G00 X.5 Y3.0 S900 M03
G43 H3 Z0.2 M08
G84 Z-0.6 R0.2 F45.0 (changed to 1/4-20)
X1.2 Y-2.0
etc etc


I read there was an option for coming out faster and I need to make it normal? Also Peck tapping that sounds interesting due to the deep tapped holes.

Someone care to give the proper code for rigid tapping and rigid peck tapping?
Also do I need to worry about the coming out speed being faster?
How fast can you rigid tap? I know the fadal is 2000rpm max but saw nothign about the HAAS and there manuals kinda are vague.

Its a factory stock vf2ss with every option,

Edit, the book didnt show the g99 on the G84 line but I know to put this in at least I think with the haas it needs to go in

Delw

[behindpropeller]

I dont rigid tap that much and frankly I dont want to screw up a brand new machine with a badcode.
I have job that requiers 9 1/4-20 threads .50 deep through holes.
we normally do this on the hand mill and a tapmatic however I have some time and was thinking of trying it on the vfs22.

in the book they have the example set up as this.(using a 3/8-16)

T3 M06
G90 G54 G00 X.5 Y3.0 S900 M03
G43 H3 Z0.2 M08
G84 Z-0.6 R0.2 F45.0 (changed to 1/4-20)
X1.2 Y-2.0
etc etc


I read there was an option for coming out faster and I need to make it normal? Also Peck tapping that sounds interesting due to the deep tapped holes.

Someone care to give the proper code for rigid tapping and rigid peck tapping?
Also do I need to worry about the coming out speed being faster?
How fast can you rigid tap? I know the fadal is 2000rpm max but saw nothign about the HAAS and there manuals kinda are vague.

Its a factory stock vf2ss with every option,

Edit, the book didnt show the g99 on the G84 line but I know to put this in at least I think with the haas it needs to go in

Delw

Delw-

Pull up the programming handbook on HAAS's site. It will answer both of these questions.

http://haascnc.com/training/MillProgram_PDF/xmwb.pdf

Tim

[Delw]

Thats the one my wife handed me earlier she got it in class last week and said to read it. I didnt, I just told her to go out program it LMAO and she did. Gotta love sending her to school.
I didnt see the max rpm in there yet I will look a tad later for it, again thanks
I didnt try the peck tapping one yet.

[Mic6]

Unfortunately, the Haas will not peck tap within one line of code. You'll have to create another operation with your 2nd depth in it.
As for speeds, I tap 1/4 - 20 roll taps in aluminum ,75 deep blind holes at 1200 rpm, and back out at 3000. Set your reverse speed @ setting 130 HTH:cheers:

[Geof]

Yes to peck tap you need to write multiple G84 lines with the different Z depths; it is not really peck tapping it is Repeat Rigid Tapping and you have to make sure both Settings (or Parameters, I forget which) are turned on.

For rpm be lazy like me and use 1000rpm, it makes calculating the feed so much easier and if you want to come out fast put in the J value on the G84 line and leave the Setting at 1 (I think it is a Setting) so you have the choice in the code.

[Delw]

Unfortunately, the Haas will not peck tap within one line of code. You'll have to create another operation with your 2nd depth in it.
As for speeds, I tap 1/4 - 20 roll taps in aluminum ,75 deep blind holes at 1200 rpm, and back out at 3000. Set your reverse speed @ setting 130 HTH:cheers:

Yes to peck tap you need to write multiple G84 lines with the different Z depths; it is not really peck tapping it is Repeat Rigid Tapping and you have to make sure both Settings (or Parameters, I forget which) are turned on.

For rpm be lazy like me and use 1000rpm, it makes calculating the feed so much easier and if you want to come out fast put in the J value on the G84 line and leave the Setting at 1 (I think it is a Setting) so you have the choice in the code.

That explains why I couldnt find anything.
Geof I am lazy to I was just using the book as an example.

Thanks guys
Delw

[Superman]

For rpm be lazy like me and use 1000rpm, it makes calculating the feed so much easier .

Be even lazier , use G95 before the tapping code, Feedrate is the thread pitch

finish the cycle with G80 and G94

Then set any RPM and the pitch is still set

G95
G84 Z-0.3 R0.02 F0.05 G99
Z-0.4 (peck)
Z-0.5
Z-0.6
G80
G94

The G80 G94 should be standard code before all toolchanges