[BJSwart]

Hi guys,

I am getting a 373 INVALID CODE IN DNC on three machine we moved from one shop to another. We are drip feeding these machines and using the same post between shops. The two other Haas mills we are running have never given us this alarm. It seems the the M30 at the end of the program is firing the alarm. When we take it out we do not get the alarm. Any thoughts as to what may be causing this alarm?

Thanks.

[dcoupar]

It seems to me that in the older machines, M30 wasn't allowed at the end of the program, so you had to use M02 instead. Also, I believe a % is required after then M02/M30. But I could be wrong... it's been a loooooooooong time.

[txcncman]

Post the code marked with the approximate point in the code where it stopped.

[Machineit]

It seems to me that in the older machines, M30 wasn't allowed at the end of the program, so you had to use M02 instead. Also, I believe a % is required after then M02/M30. But I could be wrong... it's been a loooooooooong time.

M30 is fine, used in my old 1991 when I had it.

Ya, post code.

Mike

[roofis27]

I too get an error for invalid code at the end of program at M30. As it's been at the end of program, one reset would clear the alarm and go back to waiting for DNC, but it's annoying. Running a 1993 VF-0. Yes, I'm sending a % at end of program. I'm going to watch this thread, hoping for a solution to the annoyance.
Cheers
Ken

[BJSwart]

Sorry for the delay guys, it been a crazy week. Here is a toolpath where we get the 373 alarm:

%
O0005
( NC File name : 35dp-fx1 Part Name : 35dp-2fx1 )
( Program Date : 2013.02.08 04:37.:52 )
( Winona Pattern & Mold)
( 1025 East King, Winona MN, USA 55987)
G90G80G40G17
( Tool Number :11 )
( Tool ID : 3/8 x 90deg Spotter )
( Tool type : DRILL )
T11M6
S1200M3
G0G54X-4.075Y-2.
G43Z1.H11
M8
X-4.075Y-2.
Z1.
G98G81X-4.075Y-2.Z-.1R.1F5.
Y2.
X4.925
Y-2.
G0G80
X7.925Y0
G98G81X7.925Y0Z-.1R.1F5.
X11.5
X-7.075
X-11.5
G0G80
X-4.075Y-2.
G49Z0M9
( Tool Number :17 )
( Tool ID : 17/32 Drill )
( Tool type : DRILL )
T17M6
G54G90S800M3
G43Z1.H17M8
X-4.075Y-2.
Z1.
G98G83X-4.075Y-2.Q.05Z-1.125R.1F5.
Y2.
X4.925
Y-2.
G0G80
X7.925Y0
G49Z0M9
( Tool Number :14 )
( Tool ID : 31/64 Drill )
( Tool type : DRILL )
T14M6
G54G90X-4.075Y-2.S700M3
G43Z1.H14M8
X7.925Y0
Z1.
G98G83X7.925Y0Q.05Z-1.125R.1F5.
X11.5
X-7.075
X-11.5
G0G80
X7.925
G49Z0M9
( Tool Number :15 )
( Tool ID : .490 Truem )
( Tool type : DRILL )
T15M6
G54G90X-4.075Y-2.S650M3
G43Z1.H15M8
X7.925Y0
Z1.
G98G81X7.925Y0Z-.5R.1F5.
X11.5
X-7.075
X-11.5
G0G80
X7.925
G49Z0M9
( Tool Number :16 )
( Tool ID : .501 Reamer )
( Tool type : DRILL )
T16M6
G54G90X-4.075Y-2.S400M3
G43Z1.H16M8
X7.925Y0
Z1.
G98G81X7.925Y0Z-1.125R.1F5.
X11.5
X-7.075
X-11.5
G0G80
M9
G0G49G90Z0M9
M5
M30
%

[mactec54]

G49 what are you using this for, this cancels tool offsets, not normal to have to do this

G54G90X-4.075Y-2.S700M3 I'm surprised that this runs, there is nothing to tell the X & Y what to do

G54 should be on it's own line as well

G0G80 G80G0Z3. Give the G0 something to do or it is not needed, the G80 cancels the canned cycle


G0G49G90Z0M9 Remove this line & see if it will help

It seems you have a lot of junk in your programing, & your post processor needs some work

[angelw]

G49 what are you using this for, this cancels tool offsets, not normal to have to do this

I agree that this could be a hazard, depending of the method used to set the tool length and Z Work Shift. I'd guess that the OP uses the air gap between the tool tip and Workpiece as the Tool Length Offset and with little or no Z Work Shift. Using G28 or G53 to return the Tool to the Z reference point is much more reliable and fool proof.

G54G90X-4.075Y-2.S700M3 I'm surprised that this runs, there is nothing to tell the X & Y what to do

G54 should be on it's own line as well

It seems you have a lot of junk in your programing, & your post processor needs some work

This would work in the OP's program because on every occasion the Modal G0 code has been set in conjunction with G80 prior to the next G54 G90 X_ Y_ command line. Its common to see G54 - G59 executed in the same block as move addresses. G0 will cancel a canned cycle, but it goes against convention, and relying on a code to be modal for the G54 G90 X_ Y_ command line is not good form.

It seems to me that in the older machines, M30 wasn't allowed at the end of the program, so you had to use M02 instead. Also, I believe a % is required after then M02/M30. But I could be wrong... it's been a loooooooooong time.

Hi Dave,

The kicker here is that the OP is executing a DNC application. M02 is End of Program, whilst M30 is End of Program and Rewind and has the same effect as M02; M99. It relates to the structure of the PLC interface, but in a DNC event there is no program to rewind when the end is reached. Accordingly, I believe that is the reason for the program running on other of the OP's machines and not the focus machine. Using M02 should fix the OP's issue, and is a far better option than just deleting the M30, as I assume the OP referred to in his first Post. M02 is normally linked to the Reset Rung of the PLC Ladder and therefore has the advantage of Resetting the control.

Regards,

Bill