Need Help!- NPT Milling

[jybute]

I will machine a .5" 14NPT thread using a kennametal threadmill. I know the cutter diameter, but I find it is always a pain in the a** to know what to program for a cut diameter.


I am using gibbscam to create the code.

[extanker59]

You basically pick some dimensions (major and depth) and stick with them. My cheat sheet has .83 major and .66 depth. Those were the numbers I programmed with the insert style threadmill we had. I always used cutter comp so I could adjust it at the machine.

[gromit68]

I have asked all over, and could never find pipe thread charts in anything other than pitch diameter. Called two local mach'y dealers, and they both aid, yeah, that would be really nice, no, we don't have that.

[cadman@teluspla]

jybute
Just as extanker59 wrote, You basically pick some dimensions (major and depth) and stick with them.
Your handtight engagement,(if you don't have a gage) should be 0.320"
Your major dia. in your program will also depend on where on the thread mill the diameter was measured.(it should be at the biggest diameter)
hope this helps

[JWK42]

Here is a chart I use to milling NPT threads. The engagement depth in 'Z' is
very important to follow. When I use these numbers and I know the diameter of the thread mill I get really close on the first try, usually no more than a .01 tool diameter adjustment.

I developed this chart from the Machinery's Handbook.
Mine is the 20th addition.
Look for Basic Dimensions, American National Standard Taper Pipe threads , NPT

INTERNAL NPT PIPE THREAD ENGAGEMENT DEPTH CHART

1/16 - 27 TPI NPT = .389
1/8 - 27 TPI NPT = .392
1/4 - 18 TPI NPT = .594
3/8 - 18 TPI NPT = .600
1/2 - 14 TPI NPT = .781
3/4 - 14 TPI NPT = .793
1 - 11 1/2 TPI NPT = .984
1 1/4 - 11 1/2 TPI NPT = 1.008
1 1/2 - 11 1/2 TPI NPT = 1.025
2 - 11 1/2 TPI NPT = 1.058
2 - 8 TPI NPT = 1.571
3 - 8 TPI NPT = 1.633

USE ENGAGEMENT DEPTH TO CALCULATE BOTTOM OF THREAD IN 'Z' AXIS

INTERNAL NPT PIPE THREAD MAJOR DIAMETER CHART

1/16 - 27 TPI NPT = .312
1/8 - 27 TPI NPT = .405
1/4 - 18 TPI NPT = .540
3/8 - 18 TPI NPT = .675
1/2 - 14 TPI NPT = .840
3/4 - 14 TPI NPT = 1.050
1 - 11 1/2 TPI NPT = 1.315
1 1/4 - 11 1/2 TPI NPT = 1.660
1 1/2 - 11 1/2 TPI NPT = 1.900
2 - 11 1/2 TPI NPT = 2.375
2 - 8 TPI NPT = 2.875
3 - 8 TPI NPT = 3.500

[extanker59]

Great chart JWK42. I'm going to put it with my much shorter chart and try it out when I use non-insert type threadmills.
jybute will probably have to adjust his dimensions that he uses if he uses insert type threadmills. I used .66 depth for the 1/2" NPT because that's all the insert engagement I had. Still worked to the gage. A solid carbide threadmill almost always has more, of course.

[littlerobb]

hey guys, if I needed to fat finger that same thread in what would be the easiest way? Robert

[JWK42]

I don't think fat fingering thread milling for a Haas will be much fun.
You need to know the diameter of the thread mill and include it in your calculations. You need to set the tool dia. to zero in the tool table.
Below is the code as that I wrote with my home made program writer.
I circle in and circle out and follow the helix as I circle in and out.
The code is for a .5 dia 14 TPI NPT thread. It took me about a minute to answer the questions and write the code. I can't imagine doing all those calculations by hand.



%
O5555 (TEST 123)
N30 ( WRITTEN 08-14-2008 12:29:19 )
N40 (MODIFIED 08-14-2008 12:32:30)
N50 #101=1 (.5 DIA 14-TPI THREAD MILL )
N60 G17 G54 G90
N70 G40 G49 G80
N80 G53 G00 Z0.
N90 G53 G00 X-20.0 Y0.
( TOOL #1 IS A .5 DIA 14-TPI THREAD MILL )
N110 G53 G00 Z0.0 ( RESTART TOOL #1 HERE )
N120 G53 G00 X-20. Y0.
N130 T#101 M6
N140 S2000 M3
N150 G54 G00 G90 X0. Y0.
N160 G43 Z2. H#101 D#101 M8
( START .840 MAJOR DIA - 14 TPI THREAD HERE )
( PROGRAMMED WITH .5 DIAMETER END MILL )
( SET TOOL RADIUS OFFSET TO ZERO )
( USE MINUS RADIUS TO INCREASE SIZE )
N210 G00 X0. Y0.
N220 Z.25
N230 G01 Z-0.781 F50. M8
N240 G41 X.0127 Y0. F10.
N250 G03 X.1593 Z-0.7721 R.0733
N260 G03 I-.1593 Z-0.7007
N270 G03 X.0127 Z-0.6918 R.0733
N280 G40 G01 X0. Y0. F50.
N290 Z-0.781
N300 G41 X.0234 Y0. F10.
N310 G03 X.17 Z-0.7656 R.0733
N320 G03 I-.17 Z-0.6942
N330 G03 X.0234 Z-0.6788 R.0733
N340 G40 G01 X0. Y0. F50.
N350 G00 Z2.
N360 G53 G00 Z0. M9
(UNLOAD HERE)
N380 G53 G00 X-20. Y0.
N390 M30 (END OF MAIN PROGRAM)
%

[littlerobb]

hey guys, if I needed to fat finger that same thread in what would be the easiest way? Robert

[extanker59]

JWK42 is right. However, if you don't care about a small quadrant mark, you can just feed straight to the diameter from the center, helix around, and feed back to the center. It passed QC and the gages fit. I did that the first couple of months before I found the calculations in a threadmill catalog (a great resource BTW). I changed to the right way after I became more familiar with the process.

[HuFlungDung]

Originally Posted by extanker59 JWK42 is right. However, if you don't care about a small quadrant mark, you can just feed straight to the diameter from the center, helix around, and feed back to the center. It passed QC and the gages fit. I did that the first couple of months before I found the calculations in a threadmill catalog (a great resource BTW). I changed to the right way after I became more familiar with the process.

Its not just a 'quadrant mark', its actually a warning that "this thread is not round and leans to one side". The gauges don't tell the whole story. But, this technicality is for the purists amongst us

[littlerob]

Thanks guys, I think for what we are doing that will suffice. I have an employee that overthinks BEFORE he thinks, (not that most of us aren't guilty of over thinking I just believe it should be in order) so we just need to get through the parts. Thanks again. Robert