Newbie- Fadal VMC 15

[guido5286]

I am very new at Fadal machines. I have been given the task of writing a new program for this machine, and I dont understand the programming. I do know how to program CNC machines but this is like no other CNC that I've worked with. I don't understand the "subroutine". The other 2 programs that Ihave in the machine have subroutines (L100) is that in the machine? if it is then how do I find it? also I wrote a new program today and it won't run. I'm getting a bad Z or R0 in can cycle statement when I go to "sum". Maybe you guys can catch my mistake. Thanks for any help!


N10G20
N20G17G40G80
N30G90G54G0X0.25Y-0.361S1000M03M8
N40G1.Z0.5F11.
N50M6T6(DRILL)
N60M3S1000
N70G81Z-0.85R1.1F11H6
N80X1.75
N90X3.25
N100X4.75
N110X6.25
N120X7.75
etc....

the machine says the error is in line 70, but I see nothing wrong.

[heilcnc]

hears your fix one thing your z start was below the r value and you forgot G43
and you can not have 2 m commands in 1 line like m3 and m8

N10G20
N20G17G40G80
N30G90G54G0X0.25Y-0.361S1000M03
N35G43X0.25Y-0.361Z1.75H6M8
N40G1Z01.5F11.
N50M6T6(DRILL)
N60M3S1000
N70G81Z-0.85R1.1F11
N80X1.75
N90X3.25
N100X4.75
N110X6.25
N120X7.75
etc....

[jbexplorer]

I don't see an H offset and the Z is at .5 but the R0 is at 1.1 The Z needs to be the same or higher then the R0 Change it to this.


N30G90G54G0X0.25Y-0.361S1000M03M8
N40G1.Z0.5F11.
N50M6T6(DRILL)
N60M3S1000
E1X0Y0
H6Z.1
N70G81Z-0.85R0+.1F11.M45
N80X1.75
N90X3.25
N100X4.75
N110X6.25
N120X7.75
etc....

[guido5286]

I noticed the Z is lower then the R0 and I changed that at the machine and it still didn't work. but I didn't think about the M43 or having 2 M codes in one line. Thanks alot guys! I'll try those suggestions tomorrow.

Still looking for a little help with the subroutines.

[little bubba]

First on a Fadal, you don't need a G43 when calling a height offset, it will take it, but its not necessary. Also M codes, no problem whatsoever with and M3 and an M8 on the same line.

I see several problems, besides the R being higher than than the Z.

N10G20
N20G17G40G80
N30G90G54G0X0.25Y-0.361S1000M03M8
N40G1.Z0.5F11. <--- go to Z .5
N50M6T6(DRILL) <--- change tool which brings you back to H0Z0
N60M3S1000
N70G81Z-0.85R1.1F11H6 <---- calling up a height offset in a canned cycle, not cool.
N80X1.75
N90X3.25
N100X4.75
N110X6.25
N120X7.75


JBexplorers code looks pretty happy to me, though I'm not sure what line 40 is for.

Guido, download the manuals, they are actually fairly easy to understand, also, type MU from the command line and I think it starts from page 29, but the syntax of all the canned cycles is actually in the control if you need a quick reference.

[SBC Cycle]

Originally Posted by guido5286 Still looking for a little help with the subroutines.

If you are familiar with sub programs, user subroutines will feel familiar. Instead of being a separate program, they are inside the program all the way at the top. In Format 2 (maybe 1 also??) they are separated from the main program by an M30. They have a special end of subroutine function denoted by M17

L100 ( FIRST SUBROUTINE )
G91
X0.5 Y0.866
G90
M17 ( END OF SUB 1 )
L200 ( SECOND SUBROUTINE )
G91
X-1
G90
M17 ( END OF SUB 2 )
L300 ( THIRD SUBROUTINE )
G91
X0.5 Y-.866
G90
M17 ( END OF SUB 3 )
M30 ( END OF ALL SUBROUTINES )
G20 ( FIRST LINE OF MAIN PROGRAM )
G0 G17 G40 G80 G90 (SAFE CODE, USE YOUR OWN! )
T1 M6 (TOOL CHANGE )
S1000 M3 (SET SPINDLE SPEED )
G90 E1 X0 Y0 ( RAPID TO FIXTURE 1, CAN USE G54 INSTEAD OF E1 )
G43 Z3.5 H1 (THE H AND THE G43 ARE TOTALLY REDUNTANT, USE H ALWAYS )
M8
Z0.25 D1
G1 Z-1. F25.
L101 ( RUN SUB 1 ONCE )
L201 ( RUN SUB 2 ONCE )
L301 ( RUN SUB 3 ONCE )
L102 ( RUN SUB 1 TWICE )
L202 ( RUN SUB 2 TWICE )
L302 (RUN SUB 3 TWICE )
G0 Z0.25
M5 M9
G53 Z0
Y8.5 E48
T1 M6
M30

[DareBee]

N40G1.Z0.5F11. < you need to remove the decimal point between the G1 and Z as well