I.D. Thread mill problem

[JerryH]

Anyone have trouble with the quick code thread mill generator? I am trying to generate a 1"-11.5 NPT thread, and the code that I get from the control does not work (2002 VF-2). The path is too large in diameter, even with the diameter offset setting at zero. Can someone post a code for this thread?

Thanks!

Similar Threads:

• Thread Mill Wizard - Slanted thread produced
• Need Help!- thread mill problem
• Thread mill external NPT thread
• Fanuc OT thread problem

[dylskee]

Here's one I have for a 1" 20 pitch thread.

(THREAD MILL 1"-20) 
N3 G00 G17 G20 G40 G49 G80 G90 G98 
G53 Z0 
T8 M06 
S5000 M03 
G110 X0.9975 Y0. 
G43 H08 Z1. M08 

Z-0.596 
G01 G41 Y0.5 D08 F10. 
G03 X0.4975 Y0. R0.5 (RADIUS APPROACH) 
G03 I-0.4975 J0 Z-0.546 
G03 X0.9975 Y-0.5 R0.5 (RADIUS EXIT) 
G01 G40 X0.9975 Y0. 

G00 G80 Z1. M09 
G49 G53 Z0 
G110 X0 Y9. T9 M06

All you have to do is change the Z movements to match the 11-1/2 pitch. I start the thread at the bottom and cut up one pitch.

[JWK42]

Here is the way I do it. You have to know the diameter of your thread mill and subtract it from your major thread diameter. Then setting the tool radius to zero should generate the correct size. I really don't like this way of doing it. I would rather program actual major diameter and then put the thread mill radius in the tool tables. We do a lot of NPT threads wilh thread mills and this works on all our Haas controls. I wrote this with my own Finger Cam program.



%
O5555 (TEST 11.5 1.O DIA THREAD)
N30 (WRITTEN 05-23-2007 12:28:50)
N40 (MODIFIED 05-23-2007 12:32:32)
N50 G17 G54 G90
N60 G40 G49 G80
N70 G53 G00 Z0.
(TOOL #01 IS A 11.5 TPI NPT END MILL)
N90 G53 G00 Z0.0 (RESTART TOOL #01 HERE)
N100 T01 M6
N110 S1000 M3
N120 G54 G00 G90 X0. Y0.
N130 G43 Z1. H01 D01 M8
(START 1.315 MAJOR DIA - 11.5 TPI THREAD HERE)
(PROGRAMMED WITH .75 DIAMETER END MILL)
(SET TOOL RADIUS OFFSET TO ZERO)
(USE MINUS RADIUS TO INCREASE SIZE)
N180 G00 X0. Y0.
N190 Z.2
N200 G01 Z-0.984 F50. M8
N210 G41 X.0195 Y0. F10.
N220 G03 X.2695 Z-0.9609 R.125
N230 G03 I-.2695 Z-0.8739
N240 G03 X.0195 Z-0.8508 R.125
N250 G40 G01 X0. Y0. F50.
N260 Z-0.984
N270 G41 X.0325 Y0. F10.
N280 G03 X.2825 Z-0.9455 R.125
N290 G03 I-.2825 Z-0.8586
N300 G03 X.0325 Z-0.8201 R.125
N310 G40 G01 X0. Y0. F50.
N320 G00 Z1.
N330 G53 G00 Z0. M9
(UNLOAD HERE)
N350 M30 (END OF MAIN PROGRAM)
%

[mikenaturalice]

you don't have any programming software? i know htis will be vague, but i used to work at a place where we got all of our thread milling programming online. we just input pitch, dia , etc, maybe do a search?

[Vince Wessels]

:mad
Anyone have trouble with the quick code thread mill generator? I am trying to generate a 1"-11.5 NPT thread, and the code that I get from the control does not work (2002 VF-3). The path is too large in diameter, even with the diameter offset setting at zero. Can someone post a code for this thread? I have also tried using thread mill creating programmes(Iscar),Mastercam,which help categories are not explicit enough,As well as consulting the Haas operating manual,also not explicit enough & Haas service consultants. I think i battle to understand the logic seeing as though all dimentions & literature are in inches,even though i've converted them into millimeters, I'm in S.A,& would be forever grateful to the kind person who could help. 1"-11.5 NPT,Drill size 29Dia,Major Dia 31.21,in millimetrs. I've been battling this whole week,wasting my companies money on my lunacy & still have not generated a first off,but many scrap...SAD

[JWK42]

Try subtracting the diameter of your thread mill in MM from your 29 MM Major diameter. This should give you a smaller diameter tool path, then your zero tool offset should work.
When I write this for myself I have to subtract the thread mill diameter from the major diameter to create my code as in the above post.
I have never used Quick Code so this is my best guess.

[Mic6]

Try Vardex.com. Even if you're not using Vardex tools, they have an aplication that you download that will spit out the proper code. You may have to tweak it for your machine, but the toolpath shoul dbe right. Give that a look

[rbest27]

first off you need to know the diameter of the threadmill you're using otherwise it'll always cut big. Take that number and put it in your tool offset. I'll bet the thread is basically the size of the tool bigger. Good luck.

[HuFlungDung]

I don't know about using quickcode, but if you are using radius compensation, then you should put the full tool diameter (or perhaps the radius) in the D register. This is the way to make the path smaller because the tool offsets to the inside of the path. Methinks you are confusing wear comp with radius compensation.

[omy005]

Try Vardex.com. Even if you're not using Vardex tools, they have an application that you download that will spit out the proper code. You may have to tweak it for your machine, but the toolpath should be right. Give that a look

Here is what the Vardex code generator output. Usually only requires minor tweaking.

%
O0001(TMINRH CLIMB MM CYCLES =1)
(Tool cutting diameter = 15.9 mm - Fanuc 11M Controller.)
(Taper=1/32.0 dAlfa=22.5 Second Loop Teeth=0)
G90 G00 G57 X0. Y0.
G43 H10 Z50. M3 S1201
Z-2.6258
G01 G41 D60 X4.7569 Y-11.7686 F28.
G03 X16.5255 Y0Z-2.2087I0J11.7686 F28.
G03 X11.6914 Y11.6914 Z-1.9326 I-16.5298 J0.0104 F94.
G03 X0.0000 Y16.5428 Z-1.6565 I-11.7018 J-11.6871
G03 X-11.7036 Y11.7036 Z-1.3804 I-0.0104 J-16.5471
G03 X-16.5600 Y0.0000 Z-1.1043 I11.6993 J-11.7140
G03 X-11.7158 Y-11.7158 Z-0.8283 I16.5643 J-0.0104
G03 X0.0000 Y-16.5773 Z-0.5522 I11.7262 J11.7115
G03 X11.7280 Y-11.7280 Z-0.2761 I0.0104 J16.5816
G03 X16.5945 Y0.0000 Z0.0000 I-11.7237 J11.7384
G03 X4.8260 Y11.7686 Z0.4171 I-11.7686 J0
G00 G40 X0. Y0.
G90 G00 Z200.0000
G49 M5
M30
%


Andrew.