Thread milling question

[cuttergrinder]

I have never thread milled before we had some holes that have a shoulder down in the bottom of the hole so threading with a tap is not real convenient plus the mill I was using wont drive a 3/4-10 tap. So I found a thread milling code generator on the internet and tried threading the holes. My thread mill has a dia. of .495 so I set that as my diameter on my tool page and I programmed it using .750 as my major diameter of my thread. I just used 1 radial pass to cut the thread and it came out perfect but the thread mill didnt sound too happy. The thread size was fine. Then I programmed it with 2 radial passes and then the cutter sounded much happier but the thread was too tight. So I threaded a few more after changing the tool size .005 smaller each time but the thread is still to tight. Hre are the 2 programs.

%
;( Date Generated: May 18, 2020, 3:50 am PST )
;( TMU Code Engine Build Date: 041417 )
;( Input Units: inches )
;( Output Units: inches )
;( Thread Type: UN, internal thread, right hand thread, climb cut )
;( Tool Profile: Full )
;( Major Diameter: 0.750 )
;( Minor Diameter: 0.656 )
;( Number of Radial Passes: 1 )
;( Radial Pass 1: 100% )
;( Thread Depth: 0.748 )
;( Threads Per Inch: 10.0000 )
;( Number of Depth Passes: 1 )
;( Tool Number: 1 )
;( Number of Flutes: 5 )
;( Major Tool Diameter: 0.495 )
;( Surface Feet Per Minute: 400 )
;( Revolutions Per Minute: 3087 )
;( Inches Per Tooth: .001 )
;( Inches Per Minute: 15.44 )
;(------------------------------------------------------------------)
N2 G20
N4 G80 G40 G17
N6 T1 M6
N8 G90 G54 S3087 M3
N10 G00 X0. Y0. M8
N12 G43 Z0.1 H1
N14 G90 G00 Z-0.748
;()
N16 G91 G00 X0.0179 Y0.0019
N18 G01 G41 X0.0621 Y0.0066 F5.25 D1
N20 G03 X-0.0879 Y0.1187 Z0.025 I-0.1015 J0.0167
N22 G03 X0. Y0. Z0.1 I0.0079 J-0.1273
N24 G03 X-0.0726 Y-0.1287 Z0.025 I0.0261 J-0.0995
N26 G01 G40 X0.0625 Y0.0011
N28 G00 X0.018 Y0.0003
N30 G00 G90 Z0.1
N32 G91 G28 Z0.
N34 M30
%



%
;( Date Generated: May 18, 2020, 11:51 am PST )
;( TMU Code Engine Build Date: 041417 )
;( Input Units: inches )
;( Output Units: inches )
;( Thread Type: UN, internal thread, right hand thread, climb cut )
;( Tool Profile: Full )
;( Major Diameter: 0.750 )
;( Minor Diameter: 0.656 )
;( Number of Radial Passes: 2 )
;( Radial Pass 1: 65% )
;( Radial Pass 2: 35% )
;( Thread Depth: 0.748 )
;( Threads Per Inch: 10.0000 )
;( Number of Depth Passes: 1 )
;( Tool Number: 1 )
;( Number of Flutes: 5 )
;( Major Tool Diameter: 0.495 )
;( Surface Feet Per Minute: 400 )
;( Revolutions Per Minute: 3087 )
;( Inches Per Tooth: .001 )
;( Inches Per Minute: 15.44 )
;(------------------------------------------------------------------)
N2 G20
N4 G80 G40 G17
N6 T1 M6
N8 G90 G54 S3087 M3
N10 G00 X0. Y0. M8
N12 G43 Z0.1 H1
N14 G90 G00 Z-0.748
;()
N16 G91 G00 X0.018 Y0.0013
N18 G01 G41 X0.0623 Y0.0044 F4.78 D1
N20 G03 X-0.0857 Y0.1053 Z0.025 I-0.0947 J0.0104
N22 G03 X0. Y0. Z0.1 I0.0054 J-0.1109
N24 G03 X-0.0751 Y-0.1131 Z0.025 I0.0182 J-0.0936
N26 G01 G40 X0.0625 Y0.0017
N28 G00 X0.018 Y0.0005
N30 G90 G00 Z-0.748
N32 G91 G00 X0.0179 Y0.0017
N34 G01 G41 X0.0622 Y0.0058 F5.09 D1
N36 G03 X-0.0872 Y0.114 Z0.025 I-0.0992 J0.0145
N38 G03 X0. Y0. Z0.1 I0.007 J-0.1215
N40 G03 X-0.0735 Y-0.1233 Z0.025 I0.0234 J-0.0975
N42 G01 G40 X0.0625 Y0.0014
N44 G00 X0.018 Y0.0004
N46 G00 G90 Z0.1
N48 G91 G28 Z0.
N50 M30
%

 

[13engines]

Generally I use 2-3 passes for course threads and 1 or 1-2 for fine. I also like to use the same tool path for all passes and simply change the comp number and value for each pass. Can't remember off the top of my head but I think I set the first comp (say D31) so the fist pass is 65 -70% of full diameter and the 2nd comp (Say D1) is the tool radius plus or minus whatever you have to change to get the thread to gauge right.

Without actually back plotting it the code looks right, but again two different paths. Maybe something about that is throwing a wrench in it. Also maybe you already toasted the cutter a bit.

Dave

 

[White Lightning]

You may want to pin gauge the minor diameter before thread milling. This may be causing a problem.

Sent from my SM-G960U using Tapatalk

 

[cuttergrinder]

The minor diameter was right on size.

 

[Booze Daily]

That a pretty small arc you're interpolating. The feed rate seems pretty high to me.
I'd slow the feed down and probably slow RPM down too, to keep from burning up your insert.

 

[alphonso]

Nothing wrong with your speeds and feeds. I usually make 3 passes in steels and 2 passes in alum. You need to increase your major diameter to .755 -.758.

 

[litlerob1]

Just guessing based on your feedback for the first try. You might have wiped out the corners of your Threadmill. Scope it out.

R