Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

peck tapping


Go Navy
 Share

Recommended Posts

For our Fanuc controls, we had to add *peck1$ and place it before the feed in the ptap canned cycle.

This outputs a Q0 by default which the fanuc control is ok with.

If (for example) you select a 4. in the mcam dialogue box, it then outputs a Q4. for the peck amount.

HTH

Link to comment
Share on other sites
Guest CNC Apps Guy 1

If I HAVE to tap, I ALWAYS peck tap. It may not be reccommended (which I've not heard btw) but I've not broken a tap since changing to this method.

 

But an answer te question, like was stated earlier, add *peck1$, to the ptap postblock, then search down near the bottom of the post and change the following;

code:

[tap]

1. "G84/G74 -Peck Tap"

3. ""

7. "Peck" <<<<<

8. ""

9. ""

10. ""

11. ""

 

[drill cycle descriptions]

1. "G81/G82 - Drill/Counterbore"

2. "G83 - Peck Drill"

3. "G73 - Chip Break"

4. "G84/G74 - Peck Rigid Tap" <<<<<<<

5. "G85/G89 - Bore (feed out)"

6. "G86 - Bore (stop, rapid out)"

7. "G76 - Fine Bore (shift)"

You may have several places to change [tap] but change them all.

 

[hijack] Threadmilling RULES! [/hijack] biggrin.gif

 

 

HTH

Link to comment
Share on other sites

For this to work on a Haas you need to specify a different depth on each line for each hole. For example (and I'm just winging this):

 

X1.0 Y1.0 Z-.2

Z-.4

Z-.6

Z-.8

X2.0 Y2.0 Z-.2

Z-.4

z-.6

Z-.8

 

I asked my reseller to modify my post to support this and it works great. If the "peck" value on the parameters page is 0 then there is no peck. If I put a .2 value then it will peck in .200" increments. Maybe talk to your reseller and see if they can modify your post also, or maybe they can ask In-House for the changes they made.

 

FWIW, I don't see why Haas couldn't have made this as easy as adding a "Q" value to the tapping line a la Fanuc.....I could rant, but I'll quit while I'm ahead!

Link to comment
Share on other sites

Here is John Paris' peck tapping (Thanks John!) with a slight modification for a Haas machine.

 

This will output "G84", "Z" and "R" on each line.

 

Sorry, I'm not at work so I can't post the output.

 

code:

#-------------------------------------------------------------------------

# ADDED FORMATS FOR PECK TAPPING CYCLE

fmt 4 count # timing counter

fmt 4 peck_cnt #remaining no. of pecks

fmt 4 numpeck # No. of pecks

fmt 4 pass # pass counter use to calculate depths

fmt Z 2 sub_depth #subsequent depths

fmt Z 2 calc_depth # The total caculated cutting depth

fmt Z 2 calc_peck # the calculated peck amount

fmt Z 2 strt_depth # the first tap depth

fmt Z 2 initial_calc # calculate the initial depth cut

fmt 3 stepeck #Inital step peck down increment from top of stock

 

#------------------------------------------------------------------------

pdrlcst$ #Custom drill cycles 8 - 19 (user option)

 

if drillcyc$ = 13,

[

numpeck = peck2$,

stepeck = peck1$,

if stepeck = 0,

[

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

]

else,

[

peck_cnt = numpeck

strt_depth = (tosz$ + stepeck)

calc_depth = (depth$ - (tosz$ + stepeck))

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

]

pass = 1

WHILE count > 1,

[

sub_depth = strt_depth + (calc_peck * pass)

pbld, n$, *sg84, *sub_depth, *refht_a, e$

pass = pass + 1

count = count - 1

]

pbld, n$, sg84, pfzout, *refht_a, e$

pcom_movea

]

 

 

pdrlcst_2$ #Custom drill cycles 8 - 19, additional points (user option)

 

if drillcyc$ = 13,

[

numpeck = peck2$,

stepeck = peck1$,

if stepeck = 0,

[

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$, *sgdrlref, *sg84, pdrlxy, pfxout, pfyout, pcout, *strt_depth, *prdrlout, *refht_a, *feed, strcantext, e$

count = peck_cnt - 1

]

else,

[

peck_cnt = numpeck

strt_depth = (tosz$ + stepeck)

calc_depth = (depth$ - (tosz$ + stepeck))

calc_peck = calc_depth / numpeck

"(PECK TAPPING CYCLE)", e$

pcan1, pbld, n$, *sgdrlref, *sg84, pdrlxy, pfxout, pfyout, pcout, *strt_depth, *prdrlout, *refht_a, *feed, strcantext, e$

count = peck_cnt

]

pass = 1

WHILE count > 1,

[

sub_depth = strt_depth + (calc_peck * pass)

pbld, n$, *sg84, *sub_depth, *refht_a, e$

pass = pass + 1

count = count - 1

]

pbld, n$, sg84, pfzout, *refht_a, e$

pcom_movea

]

 

#---------------------------------------------------------------------------------

[drill cycle 14]

1. "Peck Tap cycle"

2. ""

3. ""

4. ""

5. ""

6. ""

7. "INC. 1st Step from TOS"

8. "# of PECKS"

9. ""

10. ""

11. ""

#---------------------------------------------------------------------------------

 

[ 05-29-2009, 08:34 PM: Message edited by: mgsanchez ]

Link to comment
Share on other sites

Both my Emuge and Guhring reps state not to peck tap since it causes chips to jam and break the tap. Ever since I started listening to that statement, we have not broken taps in our shop unless a freak situation. The right cutting parameters and coolant play a big role.

 

For cut taps, find what works for you but we have had great results 3xD deep no peck in materials up to 45 RC.

 

Forming, no reason whatsoever to peck.

Link to comment
Share on other sites

Honestly..... If you are using the correct type of tap, lube, and cut parameters, you shouldn't need to peck tap. smile.gif

 

Maybe an M00 to use better lube - moly dee for most tough stuff.

 

As for the "jam up" this is true for blind holes if you are using a gun or plug tap, rather than a spiral tap.

 

I have used peck tapping in the past, for blind holes with a gun tap, but I added a retract and M00 to remove the chips between subsequent pecks.

 

For all of you who are thinking spiral taps are weak and most likely to break, think again, Hypro Exotaps rule.

 

No prob tapping Hast-X, Inconel, Invar, Nimonic...you name it 5x dia deep. smile.gif

 

BTW. Don't forget to put minor dia at max for tough materials like these.

 

.

 

.

 

JP - Great post work....I'll have to add that to my custom drill cycles.

cheers.gif

 

[ 05-29-2009, 09:43 PM: Message edited by: MastercamGuru ]

Link to comment
Share on other sites
Guest CNC Apps Guy 1

quote:

...it must cost alot of cash a year for peck tapping...

Depends on a lot of factors. You can't roll tap every material. How much does a scrapped part cost?

Link to comment
Share on other sites
Guest CNC Apps Guy 1

quote:

...James, face it, you don't know what you're talking about....

Actually I don't know $#!+ from shinola, I just stayed at a Holiday Inn Express every night for the last 17 years, oh, and saved a bundle on my car insurance while I was at it. rolleyes.gif

 

If y'all haven't figured it out by now, there are numerous ways to skin a cat and each of us have a method to our madness and reasons for doing what we do.

 

JM2C

Link to comment
Share on other sites

35K - Undercut (Neck) the shank or have Harvey do it for you.

 

Re: ??.390??

 

You did say .350 deep, right?

 

A 1/4" Diamond wheel + .125 LOC = .375 LOR (one plunge cut)

 

.390 leaves a little room for clearance and the lead of the threadmill.

 

To get .350 deep you usually have to go .350 + the pitch(.0179) to get full thread depth.

 

You could neck the single form threadmill as well. Either one will do the trick.

 

HTH

 

[ 06-04-2009, 02:15 PM: Message edited by: MastercamGuru ]

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...