Anyone doing this on a HAAS? I haven't tried it, yet, but getting ready to. Do you just call up 2 tap cycles with different depths?

TYIA :cheers:

'Rekd

Rekd,

Do this all the time. And yes just call up two cycles with different depths. Rigid tapping of course. Both form taps , (my preference) and regular taps.

Cool, thanks. I always use form unless the print says it's a no-no. :D

'Rekd teh Roll baby, roll!

I've 'heard' Fadals and Fanucs can do it with 1 line of code, anyone know if HAAS can??

'Rekd

its just one line of code on our okuma
g274 z-1. r.1 f(rpm divided by tpi)
great cycle but watch the blind holes i think a
floating tap holder and using just g74 would be
better for these.

rob2424,
What kind of okuma is that? Is that on a u100 controller

Scott
the controller i think is a u10 on a es 2040 vmc
nice machine
the rigid tapping cycles are
g274 for left hand tapping and g284 for right hand
kinda neat to watch it tap 1/4-20 holes at 500rpm at 25ipm
dont know what they would be for a haas probably
the same as fanuc.

We just purchased a MCVAII. It's 80x60x54, 50 taper, 30 hp, and has hi square nc it's very big and very fast for such a large machine. Has a big price tag with it too!

its got the u100 control on it?

Rekd,

I forgot to tell you that you need to Check parameter #57 "REPT RIG TAP" it should be set to 1 to peck tap. I think it is set to 1 as default.

You didn't come back on after trying to peck tap and cuss and scream that you were braking taps so I guess it was set to 1.

Sorry I neglected to state this earlier.:o

Peck tapping with a thread former? Why? Sounds silly to me!
Regards, Ray

Originally posted by RBrandes
Peck tapping with a thread former? Why? Sounds silly to me!
Regards, Ray

Ever done any machining? I have.

I've seen very little in my short career as a machinist that I would clasify as 'silly'. One of them being someone that obviously knows nothing about the current situation calling a technique silly.

Regards. :rolleyes:

Rekd, if you haven't observed plenty of "silly", lots of "stupid", and a good helping of "moronic" then your machining career has definitely been short. I'd call pecking with a thread former unusual though, as it's something I've never seen in over 20 years of running a shop. Can you enlighten us as to what situation does call for this approach?

I think you can set your Haas control up as a fanuc control. I have 2 haas HSRP1's and we use them as a fanuc controller.

Originally posted by metlmunchr
Rekd, if you haven't observed plenty of "silly", lots of "stupid", and a good helping of "moronic" then your machining career has definitely been short. I'd call pecking with a thread former unusual though, as it's something I've never seen in over 20 years of running a shop. Can you enlighten us as to what situation does call for this approach?

No, Cliff; I generally work with professionals. Have been since about '84.

"Silly" is not something that generally goes on where I work. Stupid and moronic I've seen my share of, but silly just doesn't have a place in a machine shop.

sil·ly
adj. sil·li·er, sil·li·est

1. Exhibiting a lack of wisdom or good sense; foolish. See Synonyms at foolish.
2. Lacking seriousness or responsibleness; frivolous: indulged in silly word play; silly pet names for each other.
3. Semiconscious; dazed: knocked silly by the impact.


Since you're an engineer and a lawyer, I'll let you try to come up with some scenerios where you might wish to peck tap with form threads.

If you can't figure it out, let me know and I'll throw some light your way. :rolleyes:

Hmmmmm.......Don't know quite what my education or work background has to do with the question, but since it's been asked twice now, once by me and once by Ray, can we assume your smart aleck remarks to both of us means you don't know? As before, I'd still like to know, and I have no problem admitting I can't figure out a place where you'd use it.

I can imagine a situation in tough or gummy materials where it may improve the threads if the cold forming tap gets an extra shot of lubricant applied before the second pass. It may assist it either going in easier, or coming out easier.

Mostly the latter, dung; coming out of gummy, and sometimes harder material depending on the setup, will tend to bind around the tap. Instead of paying a guy to stand there and give a hand lube to each part, I wanted to try peck tapping.

Running a .06-80 tap more than 10 or so dia's deep is a pita, and peck tapping freed the machinist for 3 minutes every 1/2 hr. Made cents to give it a shot, don't you think? ;)

Originally posted by metlmunchr
Hmmmmm.......Don't know quite what my education or work background has to do with the question, but since it's been asked twice now, once by me and once by Ray, can we assume your smart aleck remarks to both of us means you don't know? As before, I'd still like to know, and I have no problem admitting I can't figure out a place where you'd use it.

I meant no disrespect to you Cliff or Ray. I just figured after reading most of your posts, with your education and 20 years experience, (and the fact that you called it 'unusual' instead of 'silly'), that you might be able to come up with a scenario that might require peck tapping. So I challenged you. I'm sorry if it seemed rude or smart alecky. (And I meant to click the :cool: instead of the :rolleyes: , meh bad.)

I've had to do some pretty stupid things to get stuff to work, and to call a potential solution to a problem that has not been tried 'silly' seemed like a somewhat odd request for the application I was using. And wouldn't you assume that I actually had a specific application for this, considering I started the thread and asked the question?

That makes sense. Kinda trying to avoid that magic squeak that always happens right before the bang when one locks up. Never thought about that since I've never been brave enough to try a former that didn't have either lobes or grooves for the lube.

if u hear the squeek with a slight 'twang', it's usually too late. :eek:

Hey Rekd,

This came from my Haas applications manager about a year ago. This was to peck tap in an SL-30 but I am sure this will work in a mill.


You can peck tap on the SL30. All you have to do is make sure you are
running the same RPM, same Lead, and using the same starting Z reference
position and you can create as many G84 tapping cycles back to back as you
wish at the different depths. An example would be:

G00 G53 X-5. Z-15.0
T505 (5/8 - 11 tap)
G50 S1500
G97 S150 M03
G00 G54 X0 Z.1
G84 Z-.25 F.0909 R.1
G84 Z-.5 F.0909 R.1
G84 Z-.75 F.0909 R.1
G84 Z-1.0 F.0909 R.1
G84 Z-1.25 F.0909 R.1
G84 Z-1.5 F.0909 R.1
G84 Z-1.75 F.0909 R.1
G84 Z-2.0 F.0909 R.1
G00 Z.5
G00 G53 X-5. Z-15.0
M01

There is a parameter on the machine called "Repeat Rigid Tap" that would
normally have to be turned on for mills, but I don't think it needs to be
used on the lathes because your feedrate is based on distance per rev.
anyway.

I haven't tried it yet so run a sim or something before hitting 100% !

Good luck
James

Hey Matt.........no hard feelings here. I really had no idea where a person might have to do that, so it seemed an unusual thing to me. I think we all have to try some crazy stuff to get things done. I'm sure none of it is because we're constantly dealing with designs that are double and triple dimensioned and over-toleranced, or machine screw holes tapped 10X deep, or, in my case right now, a rocket scientist designer who expects me to hold +/- .020 on shapes he wants me to flame cut from 2.5" plate. Yeah, Right. Just hold on for a minute and I'll burn those boys while u wait :D Here's one I've yet to figure out, but it works.....I regularly saw large titanium rings into segments for one customer. It's 6-4. The section is roughly 1.2x1.8. Bi-metal matrix blade. Run the blade at the recommended speed (~30 fpm) and the blade is dead in ten cuts. Run it at 180fpm (not an idea, just a desperation trial) and I can make 100 plus cuts on a blade, and each cut takes a quarter of the time it takes at the 'proper" speed. Not friction cutting, but just a good steady stream of coolant and chips pouring out of the cut. Thought maybe it was some kind of unusually soft Ti, but checked the hardness and it's a consistent Rc37. Why doesn't that blade croak in 30 seconds like the mfgr tells me it should under those conditions? Blade manufacturer's answer: Are you sure the material isnt aluminum? Yep, pretty sure about that.

Just thought i'd ask:

Has anyone else used a peck tap cycle on a newer Cincinnati CNC machine with the Vickers control?

The cycle looks awsome!
The machine rotates and feeds into the material then at a programmable depth or number of intrerupts the rotation is reversed for 1/2 a turn along with the change in feed direction, then normal rotation again and down feed...

It's just like you'd tap a hole by hand, you know ever couple of rotations you'd reverse the tap just to clear the chips. I'm sure this really improves chip control which is sometimes the problem with tapping.
As for Roll tapping, It's been so long since I personally turned a handle I just don't know if it would help with friction to reverse dirrection, obviously there would be no chips to clear or break up.
But with tapping, friction is the number "one" cause for failure...
Number "two" would be chip packing, especially with small taps, thus the benefit of this cycle I'm talking about...

I wish more control builders did this kind of tapping cycle...

Sincerely,

Cliff, no worries, meng. I hear you on the bimetal blades. We use them too and they seem to run better at higher cutting speeds when doing steel. I haven't used them on titanium, but it's funny that the sales guy has prolly never cut even wood with those blades.

My boss, (long story, but an engineer I'm teaching to be a machinist, ;) ), changed blades last month and cut 2 big peices of alum and couldn't figure out why it was melting thru instead of cutting. I've showed him how to do it, and he's picked everything up with amazing speed, but for some reason he put the blade on upside down. I didn't have to look at the blade, just what he was cutting. He knew what the problem was when I started laughing. :eek:

Oh, the stories I could tell. :D

Scott, I really HATE tapping by hand. Prolly cuz I'm so bad at it. Especially in steel. :ack:

James, it's funny the guys I talked to here in SD weren't exactally sure how it would handle this, and didn't know about the setting. Go figure. I guess different areas get different training.

Hey scott bob

The cycle you are speaking of works as good as it sounds.


There are a host of awsome hole making cylces on the A2100 control that make life easy. Some of the peck drilling cyles with variable peck depth are great too.

I agree that other control makers could learn alot from the A2100. They are nice to program and one of the the fastest to set up. Not to mention great canned cycles and boat loads of memory.


Later

ARB

Hi Matt,

Take a look at Parameter 57 bit number 6 and change it to 1 for the repeatable rigid tapping.

James McInnes
San Diego, Ca.

P.S. Say hi to Jay, Kathy and Phong for me.

Will do, James, thanks!!

How the ef are you? :D

Sorry to get in on the end of this , But peck tapping works great if you have a deep hole in some hard material, We use roll form taps in almost all applications,
we code it as a
G84 X1.0 Y1.0 Z-.500 F.02 R.1
Z-.75
Z-.1
AND SO ON
sure beats breaking taps in those mighty expensive parts we make
some of which has run time of hours

Since this topic has been resurrected, I have a question for you Haas guys: have or do any of you use the "J" word in your G84 to double or triple the reverse speed of the tap coming out of the hole? I was just reading the manual (okay, I have no life :D) and noticed this was mentioned.

Since this topic has been resurrected, I have a question for you Haas guys: have or do any of you use the "J" word in your G84 to double or triple the reverse speed of the tap coming out of the hole? I was just reading the manual (okay, I have no life :D) and noticed this was mentioned.


YES :D

But Normally we just set the corresponding parameter to 2 or 3...then you don't have to worry about setting the J value..

Forgot to mention..the setting for fast retract is a "setting" not parameter.
It is setting #130 and is only available on software versions 10 and higher.

Putting a "J" value in older versions (version 9 and lower) has no effect. And there is no "setting #130 in older versions of software..



we code it as a
G84 X1.0 Y1.0 Z-.500 F.02 R.1
Z-.75
Z-.1
AND SO ON


I believe a Haas control requires a "X,Y" move to make the tap cycle (or any other cycle for that matter) repeat.

So as you have it shown here, (with Z move), it will not repeat, hence no peck tap.. ;)

Yes, and Setting 130 (Rigid-Tap Retract Mult) is an option as well. "X,Y" need not be specified in the canned cycle call (G81, G82, G83, etc.) if the tool is already in position.

G00 G90 G54 X10.5000 Y-12.4567 M03 S250
G43 Z1.00 H01 M08
G84 Z-1.0000 R0.250 F12.5 (Tap Cycle will occur at coordinates listed above unless L0 is used)
X9.0000 Y5.9034 (Tap next hole - and so on)
G80

OOPS

N5 T5 M06 (1/8-27 Npt Tap)
G00 G90 G54 X0.512 Y-0.585 S125 M03
G43 H05 Z1.
/ M08
G84 G98 Z-0.23 R0.5 F4.6296
X0.512 Z-0.335
X0.512 Z-0.35
G80
G00 Z1.
M09
G00 G91 G28 Z0. M19
G91 G28 Y0.
M30

Rekd,

I forgot to tell you that you need to Check parameter #57 "REPT RIG TAP" it should be set to 1 to peck tap. I think it is set to 1 as default.

You didn't come back on after trying to peck tap and cuss and scream that you were braking taps so I guess it was set to 1.

Sorry I neglected to state this earlier.:o

Yes, but this parameter was moved to setting 133 a couple of years ago.

How correct you are..got all bases covered.. ;) as this thread is a couple of years old to start with.. :D


Thanks for the update..glad to see you around.

yes but im not sure about the j address. i used a setting for this --- im not sure witch one it is(i am at home but will post it when i find it) but it allows you to reverse up to 9 times faster than the move in ---this setting is ony for the newer machine controls (they put it in on controls some time between 1996 and 2002)

I have a Yasnac I80, and I would like to peck tap.


Gitanes

I didn't know Haas made a machine with a Yasnak control.....
Jim

Hello PBMW,
You are correct this is not a Haas mill. I was drawn into this forum by the peck tapping discussion. I would also like to hear of different ways to lube tap.
thanks,
Gitanes

We have a Haas SL_30, found the rigid tapping cycle (G95) for axial and (G195) for lineal very fine. Have found one draw back however, being the need to drill larger than the nominal tapping drill size in order to avoid overloading the Y-Axis. Try using spiral flute tap for blind and gun for long through tapping. Sorry but haven't heard anything of peck tapping. Our lathe supports live rigid but I know nothing of peck tapping.

I run HAAS Mills and Lathes everyday. I have had to peck tap when cutting or forming deep threads. The HAAS control will read multiple tap cycles one right after the other, Just change the Z depth on each cycle.

Sorry guys! Next time I will try not to use the word "silly." No offensens intended.
I just wanted to know what the reason would be.

I do so little tapping in hard material that I do it all by hand. I have broken many a tap in the last 45 years and pretty much have a good feal for how to avoid it!
I always look for at least 2 diameters thread engagement.
I always try for 75% or less thread.
I use Tap Magic on all tapping that doesn't happen the the Haas.
Regards, Ray