The Collected Wisdom
of the Haas Answer Man

Threading & Tapping

(Spring ’04
vol 8 # 29)

Dear Applications:

     We would like to use the rigid tapping function to tap a 1/4-20 left-hand thread. How do we do that? Thanks.

     Joel Frost

Dear Joel:

     The Haas control has a G-code command specifically for this purpose: G74, Reverse Tap Canned Cycle. Like the normal tapping canned cycle (G84), it uses the variables F, J, L, R, Z, and optional X and Y commands. G74 is also modal like G84. The difference is that it starts with the spindle rotating counterclockwise, so you don’t need to program a CCW spindle motion.
TIP: When you’re using rigid tapping with G74 (or G84), be sure that the ratio between the feedrate and the spindle speed is exactly the thread pitch you want to cut. That means rpm x thread pitch = feedrate, so, in your case (1/4-20): 500 rpm x 0.05" = 25 ipm.

     Sincerely,
     Haas Applications

(Winter ’04
vol 8 # 28)

Dear Applications:

    When I’m using a G76 threading cycle on my Haas lathe, how do I distinguish between OD and ID threading?

    Mike Barney

Dear Mike:

    The way to distinguish between internal or external threads is by verifying the direction in which the tool is going to travel in the X direction. For instance, if the start point position has a larger value than the final dimension on the G76 line, then you will be cutting an external thread. If the start point is smaller than the final dimension on the G76 line, then it is an internal thread.

    Sincerely,
    Haas Applications

(Fall ’03
vol 7 # 27)

Dear Applications:

I’m cutting threads on my SL-20 turning center and would like to improve them. Is there an option in the G76 (threading, multiple pass) cycle to repeat the finish pass?

            Gabriel Romero

Dear Gabriel:

There are a couple of ways to do this. You can change Setting 99, Thread Minimum Cut, to a smaller number so that the thread cycle will take spring passes. The factory setting is 0.001; try 0.0001 and see if that gets the results you’re looking for.

The other thing you could do is write the spring pass into the program, using either G76 for two passes or G92 for one pass:

G76 X Z K F D           (make the D value large so it only takes two passes)
G92 X Z F

            Sincerely,
            Haas Applications

(Winter ’02
vol 6 # 20)

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

(Spring ’03
vol 7 # 25)

Dear Applications:

Is it possible to cut multiple start threads on an SL-30? If so, how?
     Carter Marcy

Dear Carter:

Yes, you can cut multiple start threads on an SL-30 – and on every other Haas lathe. Just change the start point of each threading cycle. For example, to cut a two-start 1”-8 thread:

(Note:  0.250" lead ÷ 2 starts = 0.125" Z shift from original start point)

Here’s something else to think about: Watch your feedrate! (MMSonline.com says it so well, we’re quoting them almost verbatim.) While the machine’s maximum feedrate is more than adequate for most machining applications, occasionally it can be a limiting factor. When threading on a turning center, for example, it is possible to unwittingly exceed the maximum feedrate. Say a turning center has a max feedrate of 300 ipm (with 600 ipm rapids). If you’re machining fine threads in large diameters, you are not likely to exceed the max feedrate. A 3.0"-16 thread machined at 300 sfm, for example, would require a feedrate of 23.88 (3.82 x 300 [sfm] ÷ 3.0 [dia] x 0.0625 [pitch]). This relatively slow feedrate is allowable on all current CNC turning centers.

On the other hand, when machining coarse threads at high speeds, you do need to worry about maximum feedrate. And multiple-start threads present the most problems, since the lead of the thread (not the crest-to-crest pitch) determines the feedrate. Say you’re machining a four-start 1.25"-4 thread having a lead of 1" (0.25" crest to crest) at 600 sfm. Now, the required feedrate becomes 1,833.6 ipm (3.82 x 600 [sfm] ÷ 1.25 [diameter] x 1.0 [lead]). This exceeds the capabilities of even the fastest CNC turning centers.
     Sincerely,
     Haas Applications

• • •

(Winter ’02
vol 6 # 20)

Dear Applications:

What is the maximum speed that can be safely used in threading? I want to keep my cutting speed up, but I am concerned about running out of Z axis feedrate.

     Thank you,
     Jim Jarosik

Dear Jim:

You can safely work at 150 inches per minute. You can determine feed per minute by multiplying rpm times feed per revolution. Let’s say you want a 4-pitch thread, which would be 4 threads per inch or 0.25 per revolution. If the rpm is 200, then 200 x 0.25 = 50 inches per minute.

     Sincerely,
     Haas Applications

(Spring ’99)
vol 3 # 9)

Dear Readers,

A Haas distributor recently sent us this handy macro program, which can be used to thread mill just about any size thread with any size tool. We liked it, so we decided to pass it on to you. 

%
O0001
...
G00 G40 G54 X0 Y0
T1 M06 
S1000 M03
G90 G43 H01 Z0.5 M08
G65 P1234 D1.98 C0.5 E0.0556 Z-0.75 F15. M2
G65 P1234 D2.0 C0.5 E0.0556 Z-0.75 F15. M2 
G00 Z1.
M05
... 
M30

O01234
(MACRO - ID RIGHT HAND STRAIGHT)
(THREAD MILLING WITH MULTI-POINT) 
(TOOL) 
(C=#3 CUTTER DIA)
(D=#7 PASS DIA)
(E=#8 LEAD)
(Z=#26 Z DEPTH)
(M=#13 Z LEAD UP LOOPS) 
G103 P1 (HALT LOOK AHEAD)
(BLANK LINE)
(BLANK LINE) 
IF [#13 EQ #0] THEN #13=1 
G01 Z[#26]F20. (FEED TO BOTTOM) 
#32=[#7-#3]/2 (CALC CUTTER PATH) 
#9=[#9*[#32/[#7/2]]] (CALC FEED RATE CENTER OF CUTTER) 
G03 X#32 I[#32/2]J0 F#9 (APPROACH) 
WHILE [#30 LT #13] DO1
#30 = #30 + 1 
G03 I[-#32]J0 Z[#26+[#8 * #30]]
(THREAD MILL UP)
END1 
G03 X0 I[-#32/2]J0 (ESCAPE) 
G103 (RESUME LOOK AHEAD)
M99
%