Quick index program for Mach3

Mc2

Mc2

AzB Silver Member
Silver Member
Since I am the lazy sort, I created this quick and simple index program for Mach 3 to index a set number of times any inlay that I am cutting a pocket for. In Mach 3 all you need to do is copy your inlay program where this program indicates with comments. Then set the number of indexes that you want. Delete the original M02 or M30 in your program. Hit cycle start every time the program ends and the A axis will already be at the correct location.
Jim.

#500=12 (NUMBER OF INDEX POSITIONS)
#501=[360/#500] (BASIC MATH DO NOT CHANGE)

M98 P100
G0 G91 A#501
G90
M30

O100
(past program here)
M99
 
Here is an example of a .250 circle cut .050 deep and set for a 12 indexes. When I run this program the circle will be cut then the A axis will index 30 degrees. Then, I would hit cycle start to run again.

#500=12 (NUMBER OF INDEX POSITIONS)
#501=[360/#500] (BASIC MATH DO NOT CHANGE)

M98 P100
G0 G91 A#501
G90
M30



O100
(PROGRAM NUMBER)
(PROGRAM NAME - .25 CIRCLE.NC)
(POST - MACH 3 MILL)
(DATE - SUN. 03/15/2009)
(TIME - 08:41AM)

N01 G20 G40 G49 G80 G90

(JOB 1 POCKET)
(FEATURE POCKET)

N02 T1 M06
N03 S10 M03
N04 G00 G90 X0.1094 Y0.0000
N05 G43 H1 Z0.1000 M08
N06 G01 Z-0.0500 F10.0000
N07 G17 G02 X0.1094 Y0.0000 I-0.1094 J0.0000
N08 G01 X0.0938
N09 G02 X0.0938 Y0.0000 I-0.0938 J0.0000
N10 G01 X0.0781
N11 G02 X0.0781 Y0.0000 I-0.0781 J0.0000
N12 G01 X0.0625
N13 G02 X0.0625 Y0.0000 I-0.0625 J0.0000
N14 G01 X0.0469
N15 G02 X0.0469 Y0.0000 I-0.0469 J0.0000
N16 G01 X0.0313
N17 G02 X0.0313 Y0.0000 I-0.0313 J0.0000
N18 G01 X0.0156
N19 G02 X0.0156 Y0.0000 I-0.0156 J0.0000
N20 G00 Z0.1000
N21 M09
N22 M05
N23 Z.1
N24 X0. Y0.
N25 M99


%
 
Hey guys here is an updated one program indexer. It is very easy to use. Just set the number of indexes you want, the angle of the a axis you would like to start, and paste you simple G-code program in where it belongs. Then save this file under a different name. This keeps the original intact. For anyone running Bobcad 23 send me your e-mail and I will send you back a post that outputs raw g-code for Mach3. This post will only generate the bare min. that Mach3 will need. Use this post just for things like indexer programs. As an example your z axis will only go up to .1" for indexing. At the end of the indexer program I run z up to 1" then return x, y, and a to zero.
Jim
Copy and save past this point

(This program written by James Babcock @ Mc2)
(This is intended for his exclusive use and whom ever the hell he chooses)
(You will need to copy and paste your program into this program)

(When done save file as what ever new name you want and then load into Mach3!)



#500=4 (Number of total indexes for program)
#501=0 (Angle to start inlay indexes)




#510=[360/#500] (Indexing degrees)

G0 A#501

M98 P1000 L#500 (End of Program)

G0 Z 1.
G0 X0 Y0
G0 A0

M30


o1000
(Paste your G-code program under this line)







G91
G0 A#510
G90



M99
 
You must log in or register to reply here.
Back
Top