milling circles

[CaptainVee]

Hi guys,

I have a bit of trouble writing g-code to mill circles. I guess I have a bit of trouble in understanding technical English.

I read about milling helical arcs, tool offsets and starting points.... I just get lost...

I want to mill a bunch of circles in two sizes, 6.1 mm and 30 mm (just 1) that untill now I've been drilling in a jig. I want to put the coordinates of the 6.1 mm in a list and use a subroutine to work each hole. Then do the 30 mm last.

I want to mill a 6.1 mm diameter hole with the centre at x=25 y=25, to a depth of 10 mm using a 4 mm router bit.

What should I write to program this correctly?

p.s. I would like to look in to translating emc in to Dutch as I don't think it is available yet. But finding how to get started on that is just as difficult.

[leggazoid]

The sub program could look like this.

%
:1234
G1 Z-10. F5.
G91 G3 X1.05 R.525
I-1.05
X-1.05 R.525
G90 G0 Z10.
M99
%

The main program could look like this.

%
:1233
T1
M6 (M6 NOT NEEDED IF NO AUTOMATIC TOOL CHANGER)
GO X25. Y25. G97 S8000 M3 M8 (G97 S8000 M3 M8 NOT NEEDED IF SPINDLE AND COOLANT NOT AUTOMATIC)
GO G43 H1 Z10.
G1 Z1. F5.
M98 P1234
G0 X50. Y50. (NEXT HOLE LOCATION)
G1 Z1. F5.
M98 P1234
G0 G28 G91 Z0
M30
%

Just check the program above the part, make sure I got my + and - directions right.

[leggazoid]

I normally use a macro to do this very thing...
I am not sure about EMC2 having a built in circle cutting cycle?

call macro from main program like this...

G65 P13 D2. I3.05 F8. (D=radius of cutter I=radius of hole)

%
O0013(CIRCLE MACRO)
#33=#4001
#1=#4003
#2=[#9*[#4-#7]/#4] (fancy feedrate calculation based on radius of cut)
IF[#4EQ#0]GOTO1(I)
IF[#7EQ#0]GOTO1(D)
IF[#9EQ#0]GOTO1(F)
IF[#7GE#4]GOTO99(TEST)
G91G3X[#4-#7]R[[#4-#7]/2]F#2
I-[#4-#7]
X-[#4-#7]R[[#4-#7]/2]
G[#1]G[#33]
GOTO100
N1#3000=0(COMMAND INCOMPLETE)
N99#3000=1(MILL TOO BIG)
N100M99
%

[jmelson]

Originally Posted by CaptainVee Hi guys, I have a bit of trouble writing g-code to mill circles. I guess I have a bit of trouble in understanding technical English.

I have some c programs I use to write the G-code to do these operations. One starts at the center and spirals out, finally making a circular pass at the desired diameter. This is the first program mentioned here :
http://jelinux.pico-systems.com/gcode.html

A second program makes one circular pass, dropping out the slug from the middle, then makes a finish pass for the desired diameter. That is the next to last one, called "make ring". Both of these programs can do the entire hole or pocket in one pass, or step down in Z depth as needed. The finish pass is done after stepping down to the full depth.

You can download DOS executables for these programs, or the C source code that should compile on either Microsoft or Linux c compilers.

Jon

[dpuch]

A quick search turned this link up. Should be pretty easy to understand, and has some simple examples. Perhaps it will help.
http://www.etec.wwu.edu/faculty/McKell/nccnc_prog3.pdf
http://www.etec.wwu.edu/faculty/McKell/ if you want to see a few other similar pdf's

Note, while G-codes are pretty standard, different machines, machine modes (G90,G91 ect.) and parameter settings can change their behavior. If you run into this, check the manual for your machine. In this case EMC and make sure what your doing matches the documentation.

[CaptainVee]

Thanks Guys!

This is exactly the kind of info I need. I'm a bit busy at the moment but will let you know how stuff goes!