Make your own CNC program easily

Make your own CNC program easily

Hello guy ! welcome back to cadcamx. We are once again glad to present another post on CNC manual programs,here in this post we are going to learn about which are common manual programs in CNC machining and how to make them easily.
Hope you enjoyed our last post which was on G-codes functions.If you wanna understand this article in a better way we strongly suggest you to read that article first. In that post we have described “G & M codes” in very simple style so that you can understand it quickly.
So without wasting time let’s begin to our topic hope you enjoy this post also. If you like it don’t forget to share it with others.

1.DRILLING

www.cadcamx.com
image courtesy_wikimedia
O0083 (main program name)
G0 G90 G54 (absolute mode-work coordinate 54)
G0 Z50 (z+50-rapid motion)
X0 Y0 (x,y job center)
S1000 M03 (RPM 1000 – spindle CW)
G90 G98 G83 R0.5 Q0.5 Z-10. F100 (drilling cycle) (absolute mode-ref point return-chip break-start from z+0.5-0.5 doc-go till -10mm-feed 100)
M97 P5001 L0 (local sub program number 5001 call x 1 time)
M97 P5002 L2 (local sub program number 5002 call x 2 time)
G0 G90 G54 (after program complete call work co ordinate)
G0 Z50 (go to z+50 from work coordinate 54)
M30 (program end & reset)
%
N5001 (Local sub program)
X10. Y20. (drilling point)
Y15. (drilling point)
Y10. (drilling point)
Y5. (drilling point)
M99 (return to main program)
%
N5002 (Local sub program)
X20. Y5. (drilling point)
Y10. (drilling point)
Y15. (drilling point)
Y20. (drilling point)
M99 (return to main program)
%

2.FACE MILLING ( AREA – 40 X 40, TOOL – 6 END )

www.cadcamx.com
image courtesy_pxhere
O0001 (main program name)
G0 G90 G54 (absolute mode-work coordinate 54)
G0 Z10 (Z+10-rapid motion)
X-30 Y-30 (entry point of tool)
G01 Z0. F200 (tool reach to job face in feed mode)
S1000 M03 (RPM 1000 – spindle CW)
M97 P6001 L5 (local sub program number 6001 call x 5 time)
G0 G90 G54 (after program complete call work co ordinate)
G0 Z50 (go to z+50 from work coordinate 54)
M30 (program end & reset)
%
N6001 (Local sub program)
G01 G91 Z-0.2 F200
M97 P6002 L4
M99
N6002 (Local sub program)
G01 G91 X5 F500
Y45
X5
Y-45
X5
M99
%

3.COUNTERING SHARP CORNER ( MAKING 20 X 20 Rectangle, TOOL – 10 END )

www.cadcamx.com
image courtesy_wikimedia
O0001 (main program name)
G0 G90 G54 (absolute mode-work coordinate 54)
G0 Z10 (Z+10-rapid motion)
S1000 M03 (RPM 1000 – spindle CW)
X0 Y-30 (entry point of tool)
G01 Z0. F200 (tool reach to job face in feed mode)
M97 P7001 L10 (local sub program number 7001 call x 10 time)
G0 G90 G54 (after program complete call work co ordinate)
G0 Z50 (go to z+50 from work coordinate 54)
G91 G00 Y0 G28 (homing Y-axes)
M30 (program end & reset)
%
N7001 (Local sub program)
G91 G01 G41 D01 Z-0.2 F1500 (taking DOC in incremental mode,cutter comp. left, D01-taking tool dia)
G90 G01 G54 F1500 (absolute mode-work coordinate 54)
Y-15. (moving in Y-axes)
X-15. (moving in X-axes)
Y15 (moving in Y-axes)
X15. (moving in X-axes)
Y-15. (moving in Y-axes)
X0. (moving in X-axes)
G90 G00 G40 X0. Y-20. (cutter compansation cancel & moving in XY-axes)
M99 (return to main program)
%

4.COUNTERING RADIUS CORNER ( MAKING 20 X 20 Rectangle with Corner 1R, TOOL – 10 END )

O0001 (main program name)
G0 G90 G54 (absolute mode-work coordinate 54)
G0 Z10 (Z+10-rapid motion)
S1000 M03 (RPM 1000 – spindle CW)
X0 Y-30 (entry point of tool)
G01 Z0. F200 (tool reach to job face in feed mode)
M97 P7000 L10 (local sub program number 7000 call x 10 time)
G0 G90 G54 (after program complete call work co ordinate)
G0 Z50 (go to z+50 from work coordinate 54)
G91 G00 Y0 G28 (homing Y-axes)
M30 (program end & reset)
%
N7000 (INCREMENTAL MODE PROGRAM)
G91 G01 G41 D01 Z-0.2 F500. (taking DOC in incremental mode,cutter comp. left, D01-taking tool dia)
G01 G90 G54 F1500. (absolute mode-work coordinate 54)
X0. Y-10. (moving into stock 1st time)
G91 G01 X-9. F1200. (moving in X-axes)(incremental mode started)
G91 G02 X-1. Y1. R1. F1200. (moving in XY-axes & making radius also)
G91 G01 Y18. (moving in X-axes)
G91 G02 X1 Y1. R1. (moving in XY-axes & making radius also)
G91 G01 X18. (moving in X-axes)
G91 G02 X1. Y-1. R1. (moving in XY-axes & making radius also)
G91 G01 Y-18. (moving in X-axes)
G91 G02 X-1. Y-1. R1. (moving in XY-axes & making radius also)
G91 G01 X-9. (moving in X-axes)
G90 G00 G40 X0. Y-25. (cutter compansation cancel & moving in XY-axes)
M99 (return to main program)
%
N7777 (ABSOLUTE MODE PROGRAM)
G01 G91 Z-0.1 F500. (taking DOC in incremental mode)
G90 G01 G41 D01 F1000. (cutter comp. left, D01-taking tool dia)
G01 Y-10. (moving into stock 1st time)
G01 X-9. (moving in X-axes)
G02 X-10.Y-9. R1. (moving in XY-axes & making radius also)
G01 Y9. (moving in Y-axes)
G02 X-9. Y10. R1. (moving in XY-axes & making radius also)
G01 X9. (moving in X-axes)
G02 X10. Y9. R1. (moving in XY-axes & making radius also)
G01 Y-9. (moving in Y-axes)
G02 X9. Y-10. R1. (moving in XY-axes & making radius also)
G01 X0. (moving in X-axes)
G90 G00 G40 X0 Y-20. (cutter compansation cancel & moving in XY-axes)
M99 (return to main program)
%

5.SLOTTING (CUTTING IN ONE DIRECTION ONLY)

www.cadcamx.com
image courtesy_pixabay
O0001 (main program name)
G0 G90 G54 (absolute mode-work coordinate 54)
G0 Z10 (Z+10-rapid motion)
S1000 M03 (RPM 1000 – spindle CW)
X0 Y0 (entry point of tool)
G01 Z0. F200 (tool reach to job face in feed mode)
M97 P500 L10 (local sub program number 500 call x 10 time)
G0 G90 G54 (after program complete call work co ordinate)
G0 Z50 (go to z+50 from work coordinate 54)
G91 G00 Y0 G28 (homing Y-axes)
M30; (program end & reset)
%
N500 (Local sub program)
G91 G01 Z-0.1 F500. (taking DOC in incremental mode)
G90 G01 X132. F600. (moving in X-axes,absolute mode)
G91 G01 Z-0.1 F500. (taking DOC in incremental mode)
G90 G01 X0 F600. (moving in X-axes,absolute mode)
M99 (return to main program)
%

6.HELICAL MILLING (SPIRAL COUNTERING)

www.cadcamx.com
image courtesy_flikr
O0001 (main program name)
G0 G90 G54 (absolute mode-work coordinate 54)
G0 Z10 (Z+10-rapid motion)
S2000 M03 (RPM 2000 – spindle CW)
X0 Y0 (entry point of tool)
M97 P700 (local sub program number 700 call )
G0 G90 G54 (after program complete call work co ordinate)
G0 Z50 (go to z+50 from work coordinate 54)
G91 G00 Y0 G28 (homing Y-axes)
M30 (program end & reset)
%
N700 (Local sub program)
G0 Z10 (Z+10-rapid motion)
G01 Z0. F500 (tool reach to job face in feed mode)
G91 G01 G41 D01 X2.5 F500. (incremental mode,cutter comp. left, D01-taking tool dia)
G91 G03 X0 I-2.5 Z-0.05 L70 F600. (taking DOC in incremental mode,circular countering CCW, making hole dia 5mm.,0.05 DOC x 70 times)
G91 G03 X0 I-2.5 F600. (circular countering CCW, final pass radius 5mm.)
G01 G40 X-2.5 F500. (cutter compansation cancel, tool coming out)
G90 G00 Z100. (return to Z+100.)
M99 (return to main program)
%

7.ENGRAVING (LETTER)

www.cadcamx.com
image courtesy_flikr
O0001 (main program name)
G0 G90 G54 (absolute mode-work coordinate 54)
G0 Z10 (Z+10-rapid motion)
S2000 M03 (RPM 2000 – spindle CW)
X0 Y0 (entry point of tool)
G01 Z0. F500 (tool reach to job face in feed mode)
G47 P0 X0 Y0 I90. J2.5 R0.5 Z-0.1 F400. E100. (TEXT HERE) (engraving code,start point xy0,engraving angle,letter height,ref. Point,letter deep,cutting feed,plunge feed)
G90 G00 Z50. (return to Z+50.)
M30 (program end & reset)
%

*** So these were some common manual program which you can try on your CNC machine. Don’t worry about anything these all are tested on the machine with FANUC control. Use given above test program to check your programming skill. Just give a try to your knowlegde you will experience making a manual CNC program is not so hard mate, you just have to remember common codes and place them properly on the CNC control, That’s it…… !!!

Note :- These all programs are tested on a ” HAAS MACHINE” with “FANUC” control.

*** don’t forget to read our next article which will really helpful to those who are fresher. And share the information with others. B’ause sharing is good though !!

If you like our post share it with your freinds and on social media also. If you have any questions and suggetions regarding the post above please feel free to put your thoughts in the comment box below.

You can share our blog directly from your phone or tablet to whatsapp, facebook or twitter.

And if you really like our article and wanna stay connected and informed about the upcoming articles which are interesting and full of knowledge.

please do subscribe to our newsletter and blog.

Thank you !!

2960total visits,1visits today

Mr. Sharma

He is very passionate about learning new things and teach them to others as well. He have experience in several software for installation and usage. He has started this blog to keep the world updated regarding new invention in CNC technology.

This Post Has 6 Comments

  1. Компания [url=http://mstore-nn.ru/]MachineStore[/url] обеспечивает производственные, строительные и торговые организации, а также домашних мастеров разнообразным инструментом, технологической оснасткой, сварочным оборудованием, бензомоторной техникой. Ассортимент предлагаемой нами продукции постоянно расширяется и на сегодняшний день составляет свыше 5000 наименований инструмента.
    Всегда в наличии:
    [url=http://mstore-nn.ru/elektroinstrument/pily-setevye/pily-torcovochnye/torcovochnaya-pila-metabo-ks-305-plus-0103050100.html]Торцовочная пила Metabo KS 305 PLUS 0103050100[/url]

  2. Pretty! This has been an incredibly wonderful
    post. Thank you for supplying these details.

Leave a Reply

Close Menu
%d bloggers like this: