Cancel
Showing results for 
Search instead for 
Did you mean: 

Thread milling output is undersized

Valued Contributor
Valued Contributor

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

threadmill.JPG

 

Damian Forsythe
Impact Manufacturing Group
NX 10.0.3.5
10 REPLIES 10

Re: Thread milling output is undersized

Siemens Phenom Siemens Phenom
Siemens Phenom

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

 

O1999 (TMILL)
(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)
(=======================)
T00 M06
G0 G90 X0.0 Y0.0 S0 M03
G43 Z.5 H00
Z.0833
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
G0 Z.5
G91 G28 Z0.0
G28 X0.0 Y0.0
G90
M30
%

Re: Thread milling output is undersized

Siemens Legend Siemens Legend
Siemens Legend

Hi IMG,

 

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 

(1.0625-.500)/2=.2813

 

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 ....

 

Thanks,

 

Toon

 

 

 

Re: Thread milling output is undersized

Valued Contributor
Valued Contributor

Toon,

 

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.

 

Thank you!

Damian Forsythe
Impact Manufacturing Group
NX 10.0.3.5

Re: Thread milling output is undersized

Valued Contributor
Valued Contributor

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.

NX 1855.2900 on Windows 10 v1809

Re: Thread milling output is undersized

Phenom
Phenom

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. 

Glenn Balon
Production: NX 12.0.2 MP10 Primarily CAM

Re: Thread milling output is undersized

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.

Re: Thread milling output is undersized

Valued Contributor
Valued Contributor

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.

 

thread_calc.png

NX 1855.2900 on Windows 10 v1809

Re: Thread milling output is undersized

Legend
Legend

@avantmfg

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.

Charles

 

tmcalc.jpg

Re: Thread milling output is undersized

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

Note you should be able to journal this ;-)

Journal should be able to handle ID/OD, UNJ, 55 degree, etc. cases

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled


Learn online





Solution Information