[JWK42]

Good morning,
We had quite a discussion on this topic on a different forum.


http://www.practicalmachinist.com/vb...=166346&page=3

Although we have been milling threads for over 20 years without radial movement, I now believe that in order to get a more perfect taper thread I need to make a radial helical move as I mill the thread.

I have written this Macro using the Example Chattaman posted on the other forum to radial mill NPT threads. I have only tested this on our Haas simulator. The read outs seem correct, but I have not made real chips yet. So use this with caution.

I would be interested in hearing your thoughts on this subject.


%
O5557 (TEST TAPER THREAD)
N10 ( WRITTEN 10-15-2008 08:12:59 )
N20 (RETURNED 10-15-2008 10:24:01)
N30 #101=1 ( NPT TAPER THREAD END MILL )
N40 G17 G54 G90
N50 G40 G49 G80
N60 ( TOOL #1 IS A NPT TAPER THREAD END MILL )
N70 G53 G00 Z0.0 ( RESTART TOOL #1 HERE )
N80 G53 G00 X-20. Y0.
N90 T#101 M6
N100 S2222 M3
N110 G54 G00 G90 X0. Y0.
N120 G43 Z2. H#101 D#101 M8
N130 ( START 1.050. MAJOR DIA - 14. TPI NPT THREAD HERE )
N140 ( SET TOOL RADIUS OFFSET TO RADIUS OF END MILL )
N150 ( X=X CNT Y=Y CNT Z=Z BOTTOM R=Z RETRACT D=MAJOR DIA K=TPI )
N160 ( V=TAPER PER IN U=PASS DEPTH C=PASSES F=FEED T=TOOL NO. )
N170 G65 P9013 X0. Y0. Z-.793 R.1 D1.050 K14. V.0625 U.01 C2. F10. T1.
N180 G00 Z2.
N190 G53 G00 Z0. M9
N200 (UNLOAD HERE)
N210 G53 G00 X-20. Y0.
N220 M30 (END OF MAIN PROGRAM)
O9013 (THREAD MILL NPT THREAD WITH TAPER END MILL)
N10 #124= #24 ( X CENTER )
N20 #125= #25 ( Y CENTER )
N30 #126= #26 ( Z BOTTOM OF THREAD )
N40 #118= #18 ( R or RETRACT PLANE IN Z AXIS )
N50 #107= #7 ( D or THREAD MAJOR DIAMETER )
N60 #120= #20 ( T or TOOL NUMBER )
N70 #106= #6 ( K or THREAD PER INCH )
N80 #109= #9 ( F or CUTTING FEEDRATE )
N90 #121= #21 ( U or DEPTH OF MILLING PASS PER SIDE )
N100 #122= #22 ( V or DIA TAPER PER INCH )
N110 #103= #3 ( C or NUMBER OF MILLING PASSES )
N120 ( END OF INPUTS )
N130 #129= [ 1 / #106 ]
N140 #107= [ #107 / 2 ] ( THREAD RADIUS )
N150 #170= #[ 2400 + #120 ] ( FIND TOOL RADIUS/DIAMETER )
N155 IF[ #6040 EQ 1 ] #170 = [#170 / 2 ] ( SET TOOL DIA TO RADIUS)
N160 #133= [ #103 - 1 ]
N170 #170= [ #170 + [ #121 * #133 ] ] ( CHANGE TOOL RADIUS FOR ROUGH PASS )
N180 #176= [ #107 - #170 ] ( RADIUS TO CUT )
N190 #175= [ #176 / 2 ]
N200 #152= [ #129 * 0.25 ] ( PITCH PER ARC )
N210 #174= [ #129 * [ #122 / 2 ] ] ( RADIAL TAPER PER THREAD )
N220 #173= [ #174 * 0.75 ]
N230 #172= [ #174 * 0.5 ]
N240 #171= [ #174 * 0.25 ]
N250 #128= [ [ #176 + #174 ] / 2 ] ( ROLL OFF RADIUS )
N260 #129= [ #126 + [ #152 / 2 ] ] ( Z POS AT ROLL ON )
N270 #130= [ #126 + [ #152 * 5 ] ] ( Z POS AT ROLL OFF )
N280 #142= [ #103 - 1 ]
N290 G90 G00 X#124 Y#125
N300 Z#118
N310 WHILE [ #103 GT 0 ] DO1
N320 G01 Z#126 F50. ( FEED TO BOTTOM )
N330 X [ #124 + #175 ] Y [ #125 - #175 ]
N340 G03 X [ #124 + #176 ] Y#125 Z#129 R#175 F#109
N350 G91 G03 X - #176 Y [ #176 + #171 ] Z#152 I - [ #176 + #171 ]
N360 X - [ #176 + #172 ] Y - [ #176 + #171 ] Z#152 I0. J - [ #176 + #172 ]
N370 X [ #176 + #172 ] Y - [ #176 + #173 ] Z#152 I [ #176 + #173 ]
N380 X [ #176 + #174 ] Y [ #176 + #173 ] Z#152 J [ #176 + #174 ]
N390 G90 G03 X [ #124 + #128 ] Y [ #125 + #128 ] Z#130 R#128
N400 G01 X#124 Y#125 F50.
N410 Z#118 F75.
N420 #170= [ #170 - #121 ]
N430 #176= [ #107 - #170 ]
N440 #103= [ #103 - 1 ]
N450 END1
N460 M99
%

[Geof]

I did a crude calculation for how much radial movement would be needed when only one circle is done with a tapered thread mill to generate a complete thread. For small threads it was less or very close to the resolution of my machine so I figured it was not necessary.

I would say any inaccuracies in the thread are squished out of existence or filled by the sealing goop during assembly of a tapered thread.

It could be a different matter with the super precise tapered threads that are used without sealing goop and seal by metal to metal contact throughout the entire thread profile.

[Vern Smith]

I'm not real familiar with pipe (tapered) threads but I would think the more pitch (smaller number) you were dealing with the more critical or necessary a radial movement would be.

[Geof]

Clicked on wrong thread

[Vern Smith]

Nice to hear from you anyhow.

[HuFlungDung]

I haven't done a lot of taper thread milling for a while, and when I do, I use a graphical method. AND, I use a thread mill

I drew a single turn spiral helix (back in OneCNC XP this was), added a radial lead in/lead out to each end of the path to create a smooth center start routine. I cut from the bottom up.

I kept a template toolpath which I imported into the drawing. The template was the simple wireframe geometry described above, drawn at the proper rate of taper increase of 3/4" per foot, and with a 1" diameter at the bottom. By means of independant scaling of all 3 axis, I could modify the template to match the desired pitch and diameter of any size thread + thread mill combo. I placed this properly scaled bit of geometry at the bottom of every hole to be milled on the model.

The spiralling path as drawn consists of 3 or 4 blended tangent arcs of gradually increasing radius. But this is interpolated into linear segments when the toolpath is posted. The arc fitting tolerance can be set in the post to whatever is desired.

Use 'cut chain variable Z' on each instance of the path to be machined. It is not really all that much code per hole.

I suppose if I were creative, I could figure a way to do this with a custom drill cycle (since the routine is center start) and a G52 at the front of a subroutine.

EDIT: I went and looked at XR3 just to be sure, and it will draw the exact path required without importing a template, including the lead in and lead out. The only thing that is uncertain, is what the diameter of the helix should be drawn at, due to the unknown of the thread mill tip diameter.

So the method I would use is to mill the first one in a piece of scrap to obtain some sort of reference by gauging the engagement of a plug in the trial cut. Then, redraw the spiral helix a second time with adjusted (corrected) radii, and it should be good to go henceforth.

[Vern Smith]

This looks like fun, guess I'll have to invest in a thread mill. After I make several dry runs with a junk em.