MAHO-PHILIPS 432 M60 and G23 problem

[micktat]

Hi, I have a little problem....

I have a MAHO MAT 550 model milling machine with 2 pallet.

Whe I try to change the pallet I have:

N10002 (PROGAM NUM.)
..
..
N39 G0 Z200
N40 M60 (change)
N41 G23 N=10003 (jump to program)

and the other program finish with

N10003
..
..
N25 G0 Z200
N26 M60 (change)
N27 G23 N=10002 (jump to program)

but the CNC stop for an error because there are 2 G23.

I need help to jump between 2 program, one program in the pallet A, when finish change to pallet B that change to A and more....

The only system that I found since today is to finish the first program with M30 and after the finishing of the second program the machine STOP and I have to push the start button.... but it is a loss of time

MANY THANKS

[cncmm]

What you need to do here is load the programs that cut your parts into
(MM) macro memory.
In your main program memory (PM) you have a program that makes the pallet change and then calls the macro program to be executed. The macro call is done with a G22. Your programs in macro memory need to have the M30
as the last line. When the M30 is read the program control will then return to the main program. In the main program, make the pallet change to the second part and make a macro call G22 for the second part. You can loop the main program as many times as you like with a G14 N1=xxx N2=xxx J= xxx.

[micktat]

Hi... I try many way bu the only one soluction that I found is:


N3 E1=1
N4 G29 N=10001 (first program)
N5 M60 (palette change)
N6 G29 N=10002 (second program)
N7 M60
N8 G29 E1 N=4 (jump to line N4)
N9 M30

The only one problem is that the variable E1 is the utensil life...
In this moment I don't use this function.... but in the future....

The command G29 don't work if the utensile life is 0.

I don't wont to use the macro memory because the singol program (es. 10001) I can use it in a "stand alone" method

[cncmm]

Hi... I try many way bu the only one soluction that I found is:


N3 E1=1
N4 G29 N=10001 (first program)
N5 M60 (palette change)
N6 G29 N=10002 (second program)
N7 M60
N8 G29 E1 N=4 (jump to line N4)
N9 M30

The only one problem is that the variable E1 is the utensil life...
In this moment I don't use this function.... but in the future....

The command G29 don't work if the utensile life is 0.

I don't wont to use the macro memory because the singol program (es. 10001) I can use it in a "stand alone" method

Mick I have never used a G29 the way you are using it but if that works for you then .......
ADD TO LINE N8 "K0" .
The K0 tells the control to reduce the E word by 0 so the value of E1
remains 1. The skip is only done if the E value is > 0.
A reduction of 1 is the default if there is no K word on the G29 line.
G29 works like a FORTRAN IF statement:
IF the E word is > 0 the skip is carried out
IF the E word is < = 0 then no skip is carried out


N3 E1=1
N4 G29 N=10001 (first program)
N5 M60 (palette change)
N6 G29 N=10002 (second program)
N7 M60
N8 G29 E1 N=4 K0 (jump to line N4)
N9 M30

Hope this helps!

Mick,
Do you have a programing manual? If not I may be able to get you one.
take care and have fun

[micktat]

Hi, thanks...

But I read the instuction on the manual but I think that the K0 is not necessary.

The program works good, only I don't know what it make if I use the Tool life.

Thaks