Disclaimer: CNC Concepts, Inc. accepts no responsibility for the use
or misuse of techniques shown in this web page. We simply publish information
we feel will be of interest to CNC users. In all cases, the reader is totally
responsible for considering the implications, good and bad, of implementing one
or more of the techniques we show.
Why can't I load all programs from one file?
Hello Mike. We are trying to call up our programs from a PC-DNC in my office
to the control out in the shop. We are using a Fanuc 6M control on an older
(1981) Mazak V Micro-Center Mill. The problem is that when we call up the main
program O1614, only the sub-program O1615 comes up by itself. As you can see in
the following programs that they are combined in the same file in the PC. In
the past the operator would call up both programs one at a time and receive
both one at a time. Now when we do it, we call up the main program (O1614) and
only receive the sub-program (O1615). If we try to call up O1615 by itself, we
receive an alarm. We are using Suburban Machinery software in the DNC system.
Is there a way we can call up both programs, one at a time to the control
and receive both? Remember, both the sub and main program are in the same file
in the PC, but they have done this in the past without a hitch. I would
appreciate your help. Thank you, Robert Barker
File containing programs:
:1615 (SUB-PROGRAM FOR 80551614)
N005 G91 G00 X-.5
N010 G90 Z-.9
N015 G1 Z-1.215 F7.
N020 G00 Z-.9
N030 G1 Z-1.43
N035 G00 Z-.9
N045 G1 Z-1.645
N050 G00 Z-.9
N060 G1 Z-2.11
N065 G00 Z0
N005 G00 G92 X0.7399 Y9.5682 Z0
N010 G90 S1500 M03
N015 X-.25 Y.25
N020 G46 Z-.9 H1 M25
N025 G83 G99 X-.25 Y.25 Z-2.11 R-.9 Q.245 F7.
N030 G80 G00 Z0
N035 M98 P1615 L47
N040 G28 G91 X0 Y0 Z0 M09
N045 G90 M05
N060 G92 X0.7399 Y9.5682 Z0
N065 G00 G90 S500 M03
N070 X-2.25 Y.69
N075 G46 Z-.9 H2 M25
N080 G83 G99 X-2.25 Y.69 Z-2. R-.9 Q.245 F7.
N085 G80 G00 Z0 M09
N090 G28 G91 X0 Y0 Z0
N095 G90 M05
With all Fanuc controls, including the 6M , a parameter controls when the
control will stop reading a program coming in from your DNC device. By my 6M
documentation, it appears to be parameter number 306, bit number 3 (it's label
is NEOP - don't ask me what that stands for) for a 6M control. Please check
this in your own documentation to confirm. If bit 3 (the fourth from the right)
is set to a 0 (as I believe it is on your control), the control will stop
reading a program as soon as it sees the first M02, M30 or M99. Since your
subprogram ends with an M99, the control doesn't continue reading the main
program, even though it's part of the file being sent. If this bit is set to a
one, the control will continue reading all programs until it sees an end of
file character, which is a percent sign (%) for Fanuc controls.
I'd bet that this parameter was set correctly in the past, but somehow it
has been changed.
Note that this parameter/bit number will vary from one control model to
another. If you had this problem with a different Fanuc model, you'd have to
look up which parameter controls when the control will stop reading.