What's new
What's new

NPT tapping

Deezle

Plastic
Joined
Sep 19, 2007
Location
Keene
When bringing a 3/8-18 NPT (pipe tap) to depth,
the spindle gets into the 130% range (not in the red, but close).
Does this effect the spindle over a longer period of time.

Trying to avoid hand tapping every part we make.

I have broken the tapping cycle into 3 different steps and it's still
spiking right at the end.

May have to work an NPT reamer into the tool list.
 
You should give a interupted flute tap a try.

0466302-11.jpg


These take quite a bit less torque to drive.

Thread milling would be your next bet too.

I really like thread milling NPT.

The reamer would also cut your torque requirements too.



I'm guessing you don't have a gearbox machine.;)
 
It is normal for tapping to bring the load real high. Tapping requires a lot of torque and most of the time you are taping in low rpms when you dont have a lot of torque available. As long as you dont actually stall the machine I wouldnt worry about it. Let the machine do the work.
 
Would love to.

I have mentioned it, but the company takes 3 years to implement
simple ideas.
How is it done? IPS? Canned cycle?
I don't even know where to begin.
 
I have mentioned it, but the company takes 3 years to implement
simple ideas.
How is it done? IPS? Canned cycle?
I don't even know where to begin.




Depends on the type of work you are doing. Our work is one off tooling. So we have thread mill programs that are generic for a specific thread & threadmill. Most threadmill companies provide software for writing the program, or many will write the program for you.
I am sure you could also do this with stored macro programs, although I am not very verse in Macro programming.
 
For thread milling

Get yourself one of these
threadmillNPT.6.gif


Write a little helical code starting at the bottom of your hole. Blend into the cut with an upwards helical move then do one complete upward helix then blend off the cut.

Rapid out

Done.
 
For thread milling

Get yourself one of these
threadmillNPT.6.gif


Write a little helical code starting at the bottom of your hole. Blend into the cut with an upwards helical move then do one complete upward helix then blend off the cut.

Rapid out

Done.


True, but with an NPT thread mill you have to increase the dia. as you helix out of the hole.
 
True, but with an NPT thread mill you have to increase the dia. as you helix out of the hole.

You will probably find conflicting information on this. As many people I am told do not compensate for the taper of the thread when doing pipe threads. I asked haas about it and the applications guy said it was not necessary to comp for the taper.

I however do comp for the taper when cutting NPT and BSPT threads.

I break the helix up in to 4 segiments or basically have 4 helix each at 90 deg of arc and 1/4 of the pitch.

I downloaded some software from Vardex
http://www.vargus.com/vardex/template/default.aspx?pCatId=9#TM GEN

or maybe it was kennametal

http://www.kennametal.com/en-US/cus...rking/software_download_reference_tools.jhtml
 
You will probably find conflicting information on this. As many people I am told do not compensate for the taper of the thread when doing pipe threads. I asked haas about it and the applications guy said it was not necessary to comp for the taper.

I however do comp for the taper when cutting NPT and BSPT threads.

I break the helix up in to 4 segiments or basically have 4 helix each at 90 deg of arc and 1/4 of the pitch.

I downloaded some software from Vardex
http://www.vargus.com/vardex/template/default.aspx?pCatId=9#TM GEN

or maybe it was kennametal

http://www.kennametal.com/en-US/cus...rking/software_download_reference_tools.jhtml


That is interesting. If you do not increas the dia. coming out of the hole, the thread mill will no longer be cutting to size, right?
 
That is interesting. If you do not increas the dia. coming out of the hole, the thread mill will no longer be cutting to size, right?

I know, I am not sure if it is true or not. Here is how I milled some BSPT. They were internal threads. It appears that it was broken up into 8 segments. You are correct that the diameter does get bigger at the top for internal threads, However the thread mill is tapered at the correct angle. So as you come up one thread pitch in "z" you only comp the diameter over that length. Not from the top to bottom change in diameter.

In this case it is only about .002".

Code:
G0 G90 G94 G40 G49 G80 G17
T5 M06
G90 G00 G54 X0. Y0.
G43 H5 Z2. M3 S2841
Z-0.0993
G01 G41 D5 X0.6948 Y-0.4584 F5.0
G03 X1.1532 Y0Z-0.0909I0J0.4584 F5.0
G03 X0.8157 Y0.8157 Z-0.0795 I-1.1534 J0.0004 F10.0
G03 X0.0000 Y1.1539 Z-0.0682 I-0.8161 J-0.8155
G03 X-0.8162 Y0.8162 Z-0.0568 I-0.0004 J-1.1541
G03 X-1.1546 Y0.0000 Z-0.0455 I0.8160 J-0.8166
G03 X-0.8167 Y-0.8167 Z-0.0341 I1.1548 J-0.0004
G03 X0.0000 Y-1.1553 Z-0.0227 I0.8171 J0.8165
G03 X0.8172 Y-0.8172 Z-0.0114 I0.0004 J1.1555
G03 X1.1560 Y0.0000 Z0.0000 I-0.8170 J0.8176
G03 X0.6977 Y0.4584 Z0.0084 I-0.4584 J0
G00 G40 X0. Y0.
 
When bringing a 3/8-18 NPT (pipe tap) to depth,
the spindle gets into the 130% range (not in the red, but close).
Does this effect the spindle over a longer period of time.

Trying to avoid hand tapping every part we make.

I have broken the tapping cycle into 3 different steps and it's still
spiking right at the end.

May have to work an NPT reamer into the tool list.


130% is not the end of the world.

Three cycles is great and all...but an NPT Tap is cutting over the entire area is is engaging so it takes a whole lot of torque to keep it moving and the further it moves into the workpiece the more torque it requires.

Reamer and staggered tooth will help a good deal.

Threadmill can be nice as well...although they can be pricey unless you have enough need for them. Programming a threadmill looks intimidating...but not theat bad...basically a circular interpolation with a Z move for your pitch.
 
NPT's

I will chime in with everyone and say threadmilling is the way to go. It eliminates problems and also use a tornado emill to cut the hole and a 45 deegree chamfer emill to give a nice touch. It is nice not to worry about any problems anymore with the NPT's.
 
I've threadmilled many NPT threads, mostly 1/8 and 1/4. I don't comp for the taper, figuring it it's only about .002 mismatch on the diameter, thread sealants take care of that. It really simplifies programming. Most of the threads i've done were for 100-120 psi air and didn't leak, I did some spray bars earlier this year that were around 2500 psi, they worked, too.
 
To properly threadmill any tapered thread you should allow for dia adjustment. We only use NPTF so we have to comp as these are dryseal threads.
As was sais above break it into 90 degree moves and adjust according to pitch.

27 tpi-.0003 per 90 deg arc
18 tpi-.0004
14 tpi-.0006
11.5tpi-.0007

Any threadmill manufacturer should have at least an Excel spreadsheet program they can supply you.
 
The above methods will eliminate the load spike, but I don't see a problem to begin with.

The Haas vector drive and spindle motor will handle 130% intermittent loads indefinitely with no adverse effects.
 








 
Back
Top