[october]

I am doubt to write a thread mill program for FANUC controller, this program using thread mill tool selected for 1/2-24 UNS -2B with 0.5" deep, what is the speed, feed and depth of cut to make a thread hole? What is the best hole to drill before thread milling?

What is the program different between using thread mill tool and single tip tool to make the thread milling on FANUC machine? Any example?

I look forward anyone to assist in this matter soon. Thanks.

Regards
October

[dpuch]

Here is some good info for the cnc code. mmsonline article 0407cnc and the full macro

Hole size for thread milling is the same as for a cutting tap. The thread mill Mfg. usually has some information on using their tool.

Single point vs full thread mill. Just how many full revolutions around the hole. 1 for the full mill, and 1 for each thread for the single point.

See:
http://www.emuge.com/news_events/a_time_to_tap.html
http://www.moldmakingtechnology.com/...es/100401.html
http://www.threading101.com/resources.php

The last has lots of good information from www.threadmillsusa.com

[Jay]

Kennametal has a program for this. Go to http://www.KennaMetal.com. It is under Support & Services, go to References, then Software.

[qinaide2]

i want to know below thread mill program is it suitable for fanuc machine (makino)~

N10 G54 G90 G00 X... Y... Z2 S3747 T1 M3 (X and Y is Starting point)
N20 G91 G00 Z-26
N30 G01 Y0.75 F2248 (Contour) F576 (Centre point)
N40 G41 G01 X7.25
N50 G03 X-7.25 Y7.25 Z0.375 I-7.25 J0
N60 G03 X0 Y0 Z1.5 I0 J-8
N70 G03 X-7.25 Y-7.25 Z0.375 I0 J-7.25
N80 G00 G40 X7.25 Y-0.75
N90 G90 Z2

Is it any problem for this program??my threadmill is D11.9mm Thread depth:24mm , pitch is 1.5
anyone could help me to solve this problem??thanks!!

[sinha_nsit]

N30 G01 Y0.75 F2248 (Contour) F576 (Centre point)

Two F-words in the same block is not written in Fanuc. The first word from left would simply be ignored.

[qinaide2]

Two F-words in the same block is not written in Fanuc. The first word from left would simply be ignored.

That's mean no need put F in program??i have using fanuc machining simulation software to test it step by step~from N40 G41 G01 X7.25 this step the thread mill already rapid move to right hand side 7.25mm~Anyone else can help me test whole program is it correct?i really confuse now coz the program actually i'm follow EMUGE catalogue one but i dont know why it not work on my MAKINO machine and make the tool break already....

[angelw]

i want to know below thread mill program is it suitable for fanuc machine (makino)~

N10 G54 G90 G00 X... Y... Z2 S3747 T1 M3 (X and Y is Starting point)
N20 G91 G00 Z-26
N30 G01 Y0.75 F2248 (Contour) F576 (Centre point)
N40 G41 G01 X7.25
N50 G03 X-7.25 Y7.25 Z0.375 I-7.25 J0
N60 G03 X0 Y0 Z1.5 I0 J-8
N70 G03 X-7.25 Y-7.25 Z0.375 I0 J-7.25
N80 G00 G40 X7.25 Y-0.75
N90 G90 Z2

Is it any problem for this program??my threadmill is D11.9mm Thread depth:24mm , pitch is 1.5
anyone could help me to solve this problem??thanks!!

Unless your Makino uses a Macro Program called via a "T" code for the tool change, or that the machine is a lathe with a Y axis, "N10 G54 G90 G00 X... Y... Z2 S3747 T1 M3" is not going to work well.

That's mean no need put F in program??

Sinha was referring to the fact that you have two Feed Rates specified in the one block "N30 G01 Y0.75 F2248 (Contour) F576 (Centre point)", not that you don't need to use a Feed Rate in the program.

At numerous places in your listed program, you have omitted the period (decimal point) when integer values have been specified. Unless your control has been set via parameter to use what Fanuc refer to as "Pocket Calculator Form", these values will be interpreted as the number of least incremental inputs.

For example:
N20 G91 G00 Z-26 will be interpreted as Z-0.026 and not Z-26.0

Again, unless your machine is a lathe with a Y axis, neither the Tool Length, nor the Tool Radius Offsets numbers have been specified.

Following is your program rewritten in more typical Machining Centre format

N1 G91 G28 Z0.0
G28 Y0.0
T01 M06
S3747 M03
G54 G90 G00 X... Y... (X and Y is Starting point)
G43 Z2.00 H01 M08 (APPLY THE TOOL LENGTH OFFSET)
G91 G00 Z-26.000
The above block is positioning the tool to the bottom of the hole to be threaded. Depending on the control set up, you may have more control over the tool in this move if a feed motion at a fast feed rate were used as follows:
G91 G01 Z-26.000 F3000
G41 G01 X7.25 Y0.75 D01 F576 (APPLY CUTTER RADIUS COMP USING "D" OFFSET NUMBER 01) The Offset Number will depend on the Offset System supplied and set with your control.
G03 X-7.25 Y7.25 Z0.375 I-7.25 J0
G03 X0 Y0 Z1.5 I0 J-8.000
G03 X-7.25 Y-7.25 Z0.375 I0 J-7.25
G00 G40 X7.25 Y-0.75
G90 Z2.000
G91 G28 Z0.0 M09
G28 Y0.0 M05
M01

Regards,

Bill

[qinaide2]

Thanks for your reply^^
another question i want to ask is the thread height is will affect the result of thread hole?Now my pitch is 1.5 so the thread height is 0.816 but after manufacturing the thread mill just have 0.78 thread height only.Is it need to do some adjustment on the program when do the thread milling process??

[javier1]

Unless your Makino uses a Macro Program called via a "T" code for the tool change, or that the machine is a lathe with a Y axis, "N10 G54 G90 G00 X... Y... Z2 S3747 T1 M3" is not going to work well.


Sinha was referring to the fact that you have two Feed Rates specified in the one block "N30 G01 Y0.75 F2248 (Contour) F576 (Centre point)", not that you don't need to use a Feed Rate in the program.

At numerous places in your listed program, you have omitted the period (decimal point) when integer values have been specified. Unless your control has been set via parameter to use what Fanuc refer to as "Pocket Calculator Form", these values will be interpreted as the number of least incremental inputs.

For example:
N20 G91 G00 Z-26 will be interpreted as Z-0.026 and not Z-26.0

Again, unless your machine is a lathe with a Y axis, neither the Tool Length, nor the Tool Radius Offsets numbers have been specified.

Following is your program rewritten in more typical Machining Centre format

N1 G91 G28 Z0.0
G28 Y0.0
T01 M06
S3747 M03
G54 G90 G00 X... Y... (X and Y is Starting point)
G43 Z2.00 H01 M08 (APPLY THE TOOL LENGTH OFFSET)
G91 G00 Z-26.000
The above block is positioning the tool to the bottom of the hole to be threaded. Depending on the control set up, you may have more control over the tool in this move if a feed motion at a fast feed rate were used as follows:
G91 G01 Z-26.000 F3000
G41 G01 X7.25 Y0.75 D01 F576 (APPLY CUTTER RADIUS COMP USING "D" OFFSET NUMBER 01) The Offset Number will depend on the Offset System supplied and set with your control.
G03 X-7.25 Y7.25 Z0.375 I-7.25 J0
G03 X0 Y0 Z1.5 I0 J-8.000
G03 X-7.25 Y-7.25 Z0.375 I0 J-7.25
G00 G40 X7.25 Y-0.75
G90 Z2.000
G91 G28 Z0.0 M09
G28 Y0.0 M05
M01

Regards,

Bill

Question on how to touch off the single thread mill & how to get the feed it is my first time that I am going to thread mill 2.625-16 UN-2B