[jay_dizzle]

hello everyone,
i'm hoping some one can help me out with this.
my shop is currently producing many gears/spline profiles using our cnc mills.
since this is something we are going to be doing for a while i would like to simplify my programming so as to produce code quicker, in turn pruduce parts faster. currently i am producing programs that utilize tool radius comp and run multiple tools around a given profile. my problem is, every time i do a tool change the full list of code is output, so if the program has five tools, you will see five large blocks of code that are all identicle. there has to be a better way to do this? i hope i havn't confused you i'm having trouble explaining what exactly i am looking for. i'll try to make up an example...


how my program looks now (three tools, profile cutter, top rad. bot rad)


T1
X2.0 Y2.0
ECT
ECT
ECT
ECT
ECT
T2
X2.0 Y2.0
ECT
ECT
ECT
ECT
ECT
T3
X2.0 Y2.0
ECT
ECT
ECT
ECT

AND WHAT I WOULD LIKE TO SEE IS

T1
???
T2
???
T3
???
X2.0 Y2.0
ECT
ECT
ECT
ECT
ECT

i'm very new to this, i'm sure there is a very simple way to accomplish this i just can't seem to figure it out.

thanks in advance

[dcoupar]

You can use main and subprograms to accomplish this. Store both O1000 and O1001 in the memory.

O1000 (MAIN PROGRAM)
T1
M98 P1001 (CALL SUB 1001)
T2
M98 P1001
T3
M98 P1001
M30

O1001 (SUB PROGRAM)
X2.0 Y2.0
ECT
ECT
ECT
ECT
ECT
M99 (RETURN TO MAIN)

[christinandavid]

You could put your contour into a separate program and call it up after initializing each tool and moving it to the correct start point eg: -

o0001 (main pgm)
T1 M6
S? M3
G0 G90 G17 G40 X? Y?
G43 H1 D1 Z? M8
M98 P0002
G91 G28 Z0 M9
M5

T2 M6
S? M3
G0 G90 G17 G40 X? Y?
G43 H2 D2 Z? M8
M98 P0002
G91 G28 Z0 M9
M5

T3 M6
S? M3
G0 G90 G17 G40 X? Y?
G43 H3 D3 Z? M8
M98 P0002
G91 G28 Z0 M9
M5
M30

Separate Sub-Pgm: -

o0002 (sub)
G1 X? Y? F?
etc
etc
M99




If you have Macro B capability:-

You can use G65 rather than M98 and pass arguments for Offsets, Z position and Feedrate, to shorten your main program: -

G65 P0002 H? D? Z? F?

in sub program: -

G43 H#11 D#7 Z#26
G1 X? Y? F#9
etc
etc
M99

If you want to keep it all in a single program you need to have Macro B capability. Use GOTO and N sequence numbers, and specify the arguments/return point with #__ = ?.

It might look like this: -

o0001
N10 T1 M6
S? M3
G0 G90 G17 G40 X? Y?
G43 H1 D1 Z? M8
#9=500
#14=20
GOTO50

N20 T2 M6
S? M3
G0 G90 G17 G40 X? Y?
G43 H2 D2 Z? M8
#9=800
#14=30
GOTO50

N30 T3 M6
S? M3
G0 G90 G17 G40 X? Y?
G43 H3 D3 Z? M8
#9=800
#14=40
GOTO50

N40 M30

N50
G1 X? Y? F#9
etc
etc
G91 G28 Z0 M9
M5
M99 P#14

There are other combinations/variations of those techniques - choose the format that best suits the situation.

DP

[jay_dizzle]

thanks all! i will most likely just try ou the sub programs for now, maybe as i get a little more advanced i'll try some of the other suggestions.
thanks again!