Im sure i have been doing somthing wrong.... The posted code from threadmilling operations always output an undersized path. The guys on the floor always comp the tool out, but i thought i would ask so someone can show me the corect way.
Thread is 1.062 x 12 internal.
tool is a single point .500 dia threadmill.
I tried telling NX the tool Dia is Ø.470 and its close.
T24 M6 (TM-500 THREAD MILL) (THREAD_MILLING_1062-12_OP1_B90_C-90) T24 G53 Z2.5 G90 G10 L11 P#3026 R0. (ADJUST H VALUE) G90 G10 L13 P#3026 R0. (ADJUST D VALUE) S7639 M3 G17 G90 G54 G254 M11 M13 G0 B90. C90. M10 M12 G94 G90 X-1.825 Y0.0 G43 Z2. H#3026 Z.7707 G41 G1 X-2.0612 Y-.0213 D#3026 F34.4 G3 X-2.1068 Y-.0915 Z.775 I.0058 J-.0536 K.0024 X-2.1068 Y-.0915 Z.8583 I.2818 J.0915 K.0133 X-2.1068 Y-.0915 Z.9417 I.2818 J.0915 K.0133 X-2.1068 Y-.0915 Z1.025 I.2818 J.0915 K.0133 X-2.1068 Y-.0915 Z1.1083 I.2818 J.0915 K.0133 X-2.1068 Y-.0915 Z1.1917 I.2818 J.0915 K.0133 X-2.1068 Y-.0915 Z1.275 I.2818 J.0915 K.0133 X-2.1068 Y-.0915 Z1.3583 I.2818 J.0915 K.0133 X-1.825 Y-.2963 Z1.375 I.2818 J.0915 K.0133 X-1.7722 Y-.2312 Z1.3793 I0.0 J.0539 K.0024 G40 G1 X-1.825 Y0.0
With the tool being Ø.500 dia inside NX then the code is undersized like this.
T24 M6 (TM-500 THREAD MILL) (THREAD_MILLING_1062-12_OP1_B90_C-90) T24 G53 Z2.5 G90 G10 L11 P#3026 R0. (ADJUST H VALUE) G90 G10 L13 P#3026 R0. (ADJUST D VALUE) S7639 M3 G17 G90 G54 G254 M11 M13 G0 B90. C90. M10 M12 G94 G90 X-1.825 Y0.0 G43 Z2. H#3026 Z.7705 G41 G1 X-2.0465 Y-.017 D#3026 F34.4 G3 X-2.0925 Y-.0869 Z.775 I.005 J-.0534 K.0025 X-2.0925 Y-.0869 Z.8583 I.2675 J.0869 K.0133 X-2.0925 Y-.0869 Z.9417 I.2675 J.0869 K.0133 X-2.0925 Y-.0869 Z1.025 I.2675 J.0869 K.0133 X-2.0925 Y-.0869 Z1.1083 I.2675 J.0869 K.0133 X-2.0925 Y-.0869 Z1.1917 I.2675 J.0869 K.0133 X-2.0925 Y-.0869 Z1.275 I.2675 J.0869 K.0133 X-2.0925 Y-.0869 Z1.3583 I.2675 J.0869 K.0133 X-1.825 Y-.2813 Z1.375 I.2675 J.0869 K.0133 X-1.7727 Y-.2159 Z1.3795 I0.0 J.0536 K.0025 G40 G1 X-1.825 Y0.0 G40 G0
here is the dialog
Solved! Go to Solution.
You don't show how the tool or geometery is defined. In NX10, the hole creation in modeling does not have a 1-1/6 thread. The attached zip file has a samle part, and post. I just created a 1.062 diameter hole and thread milled it with a single point tool . Code looks good to me for a .500 diameter thread mill (1.062-.500)/2=.281
(MACHINE MORI MILL)
(HOLE_MILLING - 16-MAR-2019 09:31 AM - MANNINO)
G40 G17 G90 G70
(OPER - HOLE MILLING)
G91 G28 Z0.0
N0 (TOOL NO. 0 - THREAD_MILL)
G0 G90 X0.0 Y0.0 S0 M03
G43 Z.5 H00
G3 X.281 I.1405 J0.0 F10.
X.281 Y0.0 Z0.0 I-.281 J0.0 K-.0133
X.281 Y0.0 Z-.0833 I-.281 J0.0 K-.0133
X.281 Y0.0 Z-.1666 I-.281 J0.0 K-.0133
X.281 Y0.0 Z-.2499 I-.281 J0.0 K-.0133
X.281 Y.0021 Z-.25 I-.281 J0.0 K-.0133
X0.0 Y0.0 I-.1405 J-.0011
G91 G28 Z0.0
G28 X0.0 Y0.0
Just wonder what makes you think it is indersized?
With a tool diameter of 0.5 and a major diameter of 1.0625 I would expect a path radius of
In your program you have
X-2.0925 Y-.0869 Z1.1083 I.2675 J.0869 K.0133
SQRT(I^2 + J^2) delivers the path radius
In your case (0,2675^2+0,0869^2)^0,5 =0,28126 ....
you are corect. when the guys on the floor said they alway need to comp the tool in i took a look and was only focused on the K number. the code is corect.
Thread milling indeed does not output the correct size toolpath. The path for threaded holes is driven by the major diameter value in the hole_standards.xml file instead of a pitch diameter value. Currently, the best workaround I've come up with is using an excel calculator to give me a part stock value to enter in the operation which will generate the proper toolpath size.
I am also working on a comprehensive ER for submitting to GTAC on this issue. I'll make a thread copying the contents of the ER so others can share their thoughts and submit a "me too" request to GTAC if they like.
Threadmills have always come in undersized for me. I define them exactly as they are in the catalog. Comping them open is normal for me and not an issue. I'd rather have them come in a little small, and dial them in. Unless it is always the exact same manufacturer and treadmill, I don't try to hit it size without dialing it in. I also noticed that different machines handle cutting a helix at a high speed slightly different. If I run the same program, but post for and run on a different machine, I end up with a slightly different cutter comp value in some cases.
I have a test block with matching material for the jobs I am working on to dial in the threadmill before the job starts.
While on the topic, I found 2 finish passes (1 spring) keeps the size very consistent even though it takes a little longer, especially on titanium. I can run lights out all weekend and still sleep at night.
When using the major diameter of the thread and major diameter of the tool I have always added 0.250mm to the major diameter in the operation geometry. This may need fudged further for tool pressure if you have a long tool. If you use the pitch diameter for both the major and tool diameters you will get closer to the correct value. If I remember correctly "nominal" pitch diameter in the Handbook is actually low limit so watch for that.
For anyone interested, this is a calculator I made to get threads milled correctly the first time. I designed this for internal threads and did not consider external threads, so if you use this be sure to do your own due dilligence and modify for external if necessary.
This will aid in generating mathematically correct thread milling toolpath where the pitch diameter is the average of the min and max limits. I use this for metric and imperial threads, the calculator is unit neutral and intended for 60deg thread profile.
To use, simply enter your thread major and pitch values in their respective cells, then use the calculated value labeled "NX part stock value" in the thread milling operation's part stock field.
Pretty cool, and quite useful, thanks. I've replicated this and will be using it. If you have the knowledge and chance to get the eternal Fx done one day please post. Much appreciated.
Note you should be able to journal this ;-)
Journal should be able to handle ID/OD, UNJ, 55 degree, etc. cases
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled