Tapping holes on CNC mill: problems
Joel Lenoir
I'm posting a question for a friend. His company has a Miltronics
Partner 1 with the rigid tap capability option. They are trying to tap
1/8 NPT and 1/4 NPT holes into the side of a stainless 1" schedule 80
pipe. They seem to be having a problem with stripping the threads when
the tap bottoms out, or even with an "excessive number" of threads (his
quote).
Other questions:
What should be the turning speed of the tap?
Any general pointers on tapping?
You may respond to him by email at
mark_j...@spantech.glasgow-ky.com
or to me and I will forward. Postings to the newsgroup will also be
forwarded.
Thanks.
Joel Lenoir, P.E. joel....@wku.edu
Western Kentucky University
cybe...@aol.com
In article <34DF2B31...@wku.edu>,
Less coolant compatible and messier is Molly-dee tapping oil. It may be more
effective if he still has problems in stainless.
Also, a tapered reamer gives better tap life, cleaner threads.
Tapping speed accourding to my chart, 25/35 sfm.
Ken
-----== Posted via Deja News, The Leader in Internet Discussion ==-----
http://www.dejanews.com/ Now offering spam-free web-based newsreading
cybe...@aol.com
Tim Markoski
A general rule-of-thumb to start with is this:
RPM = 10*Pitch
FeedRate = 10 IPM
From your description of the problem it sounds as if the spindle rotation is
not syncronized with the Z axis drive. Time to call the service tech. You
can Tach it out yourself but most of the time it isn't worth the trouble.
Joel Lenoir wrote in message <34DF2B31...@wku.edu>...
homey
Joel,
Your friend has a tough row to hoe. Under the best of
conditions,it's a hard job.Here's a few tip's that I've learned over the
years:
1) Drill your tap drill 1/64" to 1/32 oversize or better yet, use a pipe
reamer first.
2) Use a high pressure lube, somthing you might use in a dead center or on
a steady rest.
3) 25 - 50 RPM should work.
4) Don't you dare use soluble oil
5) Pray real hard and look out for flying pipe taps.
Stainless is generally Very gummy material. If you look at it sideways, it
will gall and strip your threads right out.
That gives the appearance of an "excessive number " of threads. I have
allways been leary of ridgid tapping, becuase of the accelerating and
decelerating issue, but I won't argue the point. ( Don't ya have a nice
Tapmatic or a spring loaded holder ?)
Lotsa luck, Homey.
Mike
What about generating the thread? Wouldn't that solve the problem?
-Mike
Elliott
Joel Lenoir <joel....@wku.edu> wrote:
>
> I'm posting a question for a friend. His company has a Miltronics
> Partner 1 with the rigid tap capability option. They are trying to tap
> 1/8 NPT and 1/4 NPT holes into the side of a stainless 1" schedule 80
> pipe. They seem to be having a problem with stripping the threads when
> the tap bottoms out, or even with an "excessive number" of threads (his
> quote).
>
> Other questions:
> What should be the turning speed of the tap?
> Any general pointers on tapping?
>
> mark_j...@spantech.glasgow-ky.com
> or to me and I will forward. Postings to the newsgroup will also be
> forwarded.
>
> Thanks.
>
> Joel Lenoir, P.E. joel....@wku.edu
> Western Kentucky University
>
>
>
There is the chance that the encoder in the spindle is slipping or
the pitch selection is not balanced to the gear ratio in the spindle
head. Also watch the servo following error as you may be tapping faster than the servo
controller can follow the master slave calculations from thje spindle
encoder.
good luck
elliott
homey
That gets kinda tough when you're only talking 1/4 NPT, But I suppose
someone makes a tool.
Homey.
Michael Hubbard
1/4 npt and 1/8 npt are standard thread mills and are available from
Scientific Cutting Tools, advent and several others. If the control has the
capability thread milling will solve the problem. There was a long thread
here about 2 months ago on how to program NPT thread mills. Use Dejanews to
find it.
Michael
homey wrote in message <6brasu$j0r$1...@news1.teleport.com>...
Rick Lucchetti
You may want to try the rigid tapping cycle while using a sping loaded
holder. This solved a problem I had on NPTF threads. Next choice would be to
threadmill it.
aek...@mc.net
Tim Jenkins
We have a Lambda control on our new Hitachi VM 40III - fancy as it's
supposed to be, the techies in the NY orifice said I should use the P
parameter to put a dwell at the bottom of the z movement. I began to argue
that this negates the money I gave them for a ridged tap feature - but that
will be a conversation for my sales guy.
I put a .5 sec dwell at the bottom of a Z-.425 4-40 into 6061 and taps kept
snapping like sap in a fresh cut pine log in a hot fire. I had to kick it up
to a second and a quarter to get the breakage down to about one every day.
A floating holder in a less tight CNC from Hurco tapped the same job for
several days before it would break.
Ain't progress grand....
Elliott wrote in message ...
Steve
Tim Jenkins wrote in message <35018...@news.cyberzone.net>...
snip
> I put a .5 sec dwell at the bottom of a Z-.425 4-40 into 6061 and taps
kept
>snapping like sap in a fresh cut pine log in a hot fire. I had to kick it
up
>to a second and a quarter to get the breakage down to about one every day.
> A floating holder in a less tight CNC from Hurco tapped the same job for
>several days before it would break.
> Ain't progress grand....
I do a job with a similar thread - 4-40 x .5"deep in 6061 and I use a
rollform tap , I get several thousand holes out of a tap - with the rollform
there is no "stuff" to jam in the hole.
the machine I use is a Mighty Comet with Mitsubishi Meldas control , and
I've had no problems rigid tapping from 2-56 in 6161 to 3/4 pipe in brass
Steve C
A Better Mousetrap!
Burlingame CA
(650)344-5157
Sheri + Jamie
Your rigid tapping problems could be related to the code or the way you have
written your program i.e. some controls use G84 for normal tapping and G84.1
for rigid tapping, some require you to use feed per rev ( G94 G95 ) with
rigid tapping and feed per minute with normal tapping. I have not always
never ) found application engineers to be of much help, in fact I think I
taught the last one more than he taught me.
Good luck
J.B.
Tim Jenkins wrote in message <35018...@news.cyberzone.net>...
> We have a Lambda control on our new Hitachi VM 40III - fancy as it's
>supposed to be, the techies in the NY orifice said I should use the P
>parameter to put a dwell at the bottom of the z movement. I began to argue
>that this negates the money I gave them for a ridged tap feature - but that
>will be a conversation for my sales guy.
> I put a .5 sec dwell at the bottom of a Z-.425 4-40 into 6061 and taps
kept
>snapping like sap in a fresh cut pine log in a hot fire. I had to kick it
up
>to a second and a quarter to get the breakage down to about one every day.
> A floating holder in a less tight CNC from Hurco tapped the same job for
>several days before it would break.
> Ain't progress grand....
>
Wes
On Sun, 08 Mar 1998 19:27:27 GMT, Haw...@home.com (HawkEye) wrote:
Make it easy! Just divide the RPM by the threads per inch.
200/20 = 10
>I have rigid tapping on bridgeport Discovery 308, The calculation I
>use is ( 1.0 divided by number of threads per inch on tap being used,
>then multiply by RPM of spindle will give you your z axis feed rate.
>
> Example-> (1.0 / 20 tpi x 200rpm = 10.0 feed rate)
>
Steve
Wes wrote in message <350528bb...@news.inficad.com>...
>On Sun, 08 Mar 1998 19:27:27 GMT, Haw...@home.com (HawkEye) wrote:
>
>Make it easy! Just divide the RPM by the threads per inch.
>200/20 = 10
Make it even easier - go to http://www.microsystemsgeogia.com and get a
copy of my The Machinist's Mate , there is a function to do just this , sub
section of tapdrills , both inch and mm.
Steve C
A Better Mousetrap!
Burlingame CA
(650)344-5157
>
Dave
To make it even easier take number of threads per inch multiply by the feed
rate=rpm, this way you will always end up with a whole number for rpm and
feed rate which makes it easier for operators to check on the floor at a
quick glance.(I normally use feed of 10 IPM) good luck
Steve wrote in message <6e3jdh$i5a$1...@news.ncal.verio.com>...
Phrede
Rigid tapping should not require any dwell at all and should be able to
retract faster than cutting giving an overall time improvement.
It sounds to me more like incorrect gain settings in the parameters.
If you can try running in a higher gear range at the same speed/feed.
Phrede
HawkEye wrote in message <6durjj$9...@bgtnsc03.worldnet.att.net>...
>I have rigid tapping on bridgeport Discovery 308, The calculation I
>use is ( 1.0 divided by number of threads per inch on tap being used,
>then multiply by RPM of spindle will give you your z axis feed rate.
>
> Example-> (1.0 / 20 tpi x 200rpm = 10.0 feed rate)
>
>
>
>On Sat, 7 Mar 1998 16:29:32 -0800, "Steve" <sca...@aimnet.com> wrote:
>
>>
>>Tim Jenkins wrote in message <35018...@news.cyberzone.net>...
>> snip
>>> I put a .5 sec dwell at the bottom of a Z-.425 4-40 into 6061 and taps
>>kept
>>>snapping like sap in a fresh cut pine log in a hot fire. I had to kick it
>>up
>>>to a second and a quarter to get the breakage down to about one every
day.
>>> A floating holder in a less tight CNC from Hurco tapped the same job for
>>>several days before it would break.
>>> Ain't progress grand....
>>
>> I do a job with a similar thread - 4-40 x .5"deep in 6061 and I use a
>>rollform tap , I get several thousand holes out of a tap - with the
rollform
>>there is no "stuff" to jam in the hole.
>> the machine I use is a Mighty Comet with Mitsubishi Meldas control , and
>>I've had no problems rigid tapping from 2-56 in 6161 to 3/4 pipe in brass
>>
J. O'Brien Myer
Dave wrote:
>
> To make it even easier take number of threads per inch multiply by the feed
> rate=rpm, this way you will always end up with a whole number for rpm and
> feed rate which makes it easier for operators to check on the floor at a
> quick glance.(I normally use feed of 10 IPM) good luck
The feedrate calculator software supports
tapping in various materials. Address is: