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

  • N025 Z-1.165

  • N030 G1 Z-1.43

  • N035 G00 Z-.9

  • N040 Z-1.38

  • N045 G1 Z-1.645

  • N050 G00 Z-.9

  • N055 Z-1.595

  • N060 G1 Z-2.11

  • N065 G00 Z0

  • N070 M99

  • :1614 (80551614)

  • (P3A31-08CD)

  • (FIRST OPERATION)

  • (-----1/4 DRILL-----)

  • 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

  • N050 M00

  • (-----11/32 DRILL-----)

  • 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

  • N100 M30

  • %

Response:

Robert,


With all Fanuc controls, 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.

7 views

Recent Posts

See All

How does G66 work?

G66 is one of the more misunderstood custom macro B commands. Fanuc calls it a modal custom macro call. It looks just like a G65 command. Consider these two commands: N045 G65 P1000 X3.0 Y3.0 Z0 A45.0

What are directional vectors?

Current model CNC controls make it easy to create circular commands. You simply specify the direction (G02: clockwise or G03: counter clockwise), the end point (usually X and Y), and the radius (with

cnc reverse logo.jpg
0

44 Little Cahill Road

Cary, IL  60013

Ph: 847-639-8847

  • Facebook Social Icon