Peck Tapping using Mastercam

[mike561h]

I am going 1/2 inch deep in 17-4 with a 3/8 16 tap. Blind hole flat bottom. Its working a little to hard. Other then programming 2 tap cycles 1 deeper then the other is there a way to tell MCX how to peck tap.

 

thanks,

[Guest]

yes there is, what does your machine NEED to see to achieve a peck tap. Then we can tell you how.

[Charlie Pierson]

You talking about a pecking cycle such as a G84 with a Q value ???

 

You can setup and use the custom cycles in the post.

[crazy^millman]

I added that to my drilling cycles and when I put it in I get my Q output. Is this what you are after???

[mike561h]

It is a Haas Mini mill. G83 is peck for drill

G84 is tap cycle. is this what you are talking about??

[mike561h]

I think you guys are saying to add a Q for peck on the G84 tap cycle. Is this correct?

[ToolMan184]

On a Fanuc that is true. On a HAAS Im not sure.

[Charlie Pierson]

Yes if your control supports it

 

You can modify custom drill misc 2 for example,

make it look like the tap cycle but add peck1$ to the output line, kinda like this:

 

pmisc2$ #Canned Misc #2 Cycle (User Option)(now peck tap)

pdrlcommonb

result = newfs(17, feed) # Set for tapping Feedrate format

pcan1, pbld, n$, *sgdrlref, *sgdrill, pxout, pyout, pfzout, pcout,

prdrlout, *peck1$, *feed, strcantext, e$

pcom_movea

 

Then I think you can edit the text in the control def so that it looks nice for the drill cycle dropdown.

[Guest CNC Apps Guy 1]

HAAS does not support peck tapping. FANUS's with rigid tappind do and all you need is a Q on the line.

[GoetzInd]

quote:

---

It is a Haas Mini mill.

---

Someone correct me if I'm wrong but I think your out of luck as far as just using G84 w/ Q. Haas does not support it. You have to do as you said, two different cycles at two different depths.

 

Mike

[Guest]

From the Haas website

 

Linky

 

quote:

---

G84 or G74 Tapping Back into a Hole – You can go back into a tapped hole to go deeper if you have the Rigid Tapping option and if you have not moved the tool or part. Parameter 57 bit 6, REPT RIG TAP, must be set to 1 (On). Edit the Z depth to go deeper, or offset down by the amount of one thread pitch to rerun a tapped hole. NOTE: If you move, offset, or change the starting position of the part or tap and it is not equal to one pitch of the thread, you will cross-thread the hole.

---

quote:

---

G84 or G74 Peck Tapping – You can also peck tap into a hole to go deeper (for tough/hard material) if Parameter 57 bit 6, REPT RIG TAP, is set to 1 (On). Then all you would need to do is repeat the tapping cycle at the same XY location, going deeper in the Z axis on each command line. See the following examples.

 

 

Example 1:

 

G90 G54 X1.5 Y-0.5

S450

G43 H01 Z1.0 M08

G84 G99 Z-0.25 R0.1 F22.5

G84 Z-0.5

G84 Z-0.75

G00 Z1. M09

Example 2:

 

G90 G54 X1.5 Y-0.5

S450

G43 H01 Z1.0 M08

G84 G99 Z-0.25 R0.1 F22.5

X1.5 Y-0.5 Z-0.5

X1.5 Y-0.5 Z-0.75

G00 Z1. M09

---

quote:

---

Note: On Mill software versions12.09 and above, REPT RIG TAP has been moved from the Parameters to Setting 133. This is now an On/Off setting that is much easier for the user to change.

---

[Troy Gossett Indepak Inc.]

How would you make Mastercam post out consecutive depths...on consecutive lines?

[Guest]

custom cycle like this

 

code:

---

fmt   4 count             # timing counter                         #Peck TAP CYCLE

fmt 4 peck_cnt #remaining no. of pecks #Peck TAP CYCLE

fmt 4 numpeck # No. of pecks #Peck TAP CYCLE

fmt 4 pass # pass counter use to calculate depths #Peck TAP CYCLE

fmt Z 2 sub_depth #subsequent depths #Peck TAP CYCLE

fmt Z 2 calc_depth # The total caculated cutting depth #Peck TAP CYCLE

fmt Z 2 calc_peck # the calculated peck amount #Peck TAP CYCLE

fmt Z 2 strt_depth # the first tap depth #Peck TAP CYCLE

fmt Z 2 initial_calc # calculate the initial depth cut #Peck TAP CYCLE

---

code:

---

if drillcyc$ = 13,

[

numpeck = peck2$

peck_cnt = numpeck

initial_calc = (depth$ - tosz$) / peck_cnt

strt_depth = (tosz$ + initial_calc)

calc_depth = (depth$ - tosz$)

calc_peck = calc_depth / numpeck

"(PECK TAPPING CYCLE)", e$

pcan1, pbld, n$, *sgdrlref, *sg84, pdrlxy, *strt_depth, pcout,

prdrlout, *feed, strcantext, e$

count = peck_cnt - 1

pass = 1

WHILE count > 1,

[

sub_depth = strt_depth + (calc_peck * pass)

pbld, n$, *sub_depth, e$

pass = pass + 1

count = count - 1

]

pbld, n$, sg98, pfzout, e$

pcom_movea

]

---

code:

---

[drill cycle 14]

1. "Peck Tap cycle"

2. ""

3. ""

4. ""

5. ""

6. ""

7. ""

8. "# of pecks"

9. ""

10. ""

11. ""

---

I thought this sounded familiar, came home did some checking and it sounded familiar because it was

 

[Bryan Johnson]

there is a haas post on the ftp that is setup to automaticly do the repetive tap cycle for peck tap.

 

MILLX_HAAS-VF.zip

ftp://mastercam:[email protected]/Ma...LLX_HAAS-VF.zip

[mig]

Is okuma has pecking cycle for the taping?

[prussell226]

Try G282 with Q for peck amount.

[S.Luong]

On 1/21/2008 at 1:02 AM, Bryan Johnson said:

there is a haas post on the ftp that is setup to automaticly do the repetive tap cycle for peck tap.

 

MILLX_HAAS-VF.zip

ftp://mastercam:[email protected]/Ma...LLX_HAAS-VF.zip

The link is dead, would you re upload?

 

Thanks.

[Glenn Bouman]

Newer Haas will do peck tapping

https://www.haascnc.com/video/tipoftheday/ybk1mn_q9j0.html

 

[cncappsjames]

Not sure I'd want to update a 2008 era post.

[crazy^millman]

On 10/17/2022 at 4:23 AM, Glenn Bouman said:

Newer Haas will do peck tapping

https://www.haascnc.com/video/tipoftheday/ybk1mn_q9j0.html

 

The other would be to turn on and off the setting using the Macro to get around having to turn that on and off when you are not using and using it. Then you have the best way to cheat the control to reduce the unneeded orientation of the spindle he was talking about, but still get the peck tapping done when needed by using a macro to turn it on when you needed it.

Tim was the guest who posted that up and he is missed.

[ikertx0]

 

Hello, I am using this postblock, but the depth is calculated by infinity. The variable "count" it is not defined, 
since I have copied the code from the post above.

force_dpts     : 0      #Force XY output on all drilling lines including cycle call?

#PARA PECK TAPPING
fmt     4 peck_cnt #remaining no. of pecks #Peck TAP CYCLE
fmt     4 numpeck # No. of pecks #Peck TAP CYCLE
fmt     4 pass # pass counter use to calculate depths #Peck TAP CYCLE
fmt "Z" 2 sub_depth #subsequent depths #Peck TAP CYCLE
fmt "Z" 2 calc_depth # The total caculated cutting depth #Peck TAP CYCLE
fmt "Z" 2 calc_peck # the calculated peck amount #Peck TAP CYCLE
fmt "Z" 2 strt_depth # the first tap depth #Peck TAP CYCLE
fmt "Z" 2 initial_calc # calculate the initial depth cut #Peck TAP CYCLE

p_pecktap
    [
    numpeck = peck2$
    peck_cnt = numpeck
    initial_calc = (depth$ - tosz$) / peck_cnt
    strt_depth = (tosz$ + initial_calc)
    calc_depth = (depth$ - tosz$)
    calc_peck = calc_depth / numpeck
    "(PECK TAPPING CYCLE)", e$
    pcan1, pbld, n$, *sgdrlref, *sg84, pdrlxy, *strt_depth, pcout,
    prdrlout, *feed, strcantext, e$
    count = peck_cnt - 1
    pass = 1
    WHILE count > 1,
    [
    sub_depth = strt_depth + (calc_peck * pass)
    pbld, n$, *sub_depth, e$
    pass = pass + 1
    count = count - 1
    ]
    pbld, n$, sg98, pfzout, e$
    pcom_movea
    ]

pdrlxy         #Drill XYZ coordinates
      if force_dpts, pfxout, pfyout, !zabs, !zinc
      else, pxout, pyout, !zabs, !zinc

 

Some help?