What's new
What's new

Doosan DNM6700

watson13

Plastic
Joined
Nov 18, 2021
HI there can anyone help me, every time the machine changing tools X&Y always in to home position, I just want to know where to dis-able it, hope I can find answer here. cheers!!!
 

LockNut

Stainless
Joined
Jan 6, 2007
Location
Bergen County
Fanuc Oi-F control. Check which program runs when tool changes. The below program is from a Doosan. It will be O9001 or O9006. G30 X0 Y0 position depends on a parameter, #1241.

%
O9001(DVF5000 A1 M06 W0 TM 20180419)
IF[#1007EQ1]GOTO600(MACRO M CODE MST SKIP)
#14=#4114(REC SEQ NO)
#15=#4001(REC G1 G0)
#16=#4003(REC G90 G91)
G31
IF[#1000EQ1]GOTO500(HEAD=T)
IF[#3010EQ-1]GOTO500
G05.1Q0
N10G80G40
N30G91G30Z0.M19M222M233
M39
N40G91G30X0.Y0. (Change this line or comment it out. I wouldn't delete because it does come in handy)
N50M06
N60
M232M223
N500
N#14G#15G#16
G05.1Q1
N600
M99

%
 

angelw

Diamond
Joined
Sep 10, 2010
Location
Victoria Australia
I would change the program number of the following Tool Change Subprogram to any available number between and including O9020 and O9029, then register the numeral 6 in the corresponding parameters 6080 to 6089. This would have the following program called as a Macro Program and not a Subprogram and therefore, allow arguments to be passed to it by the Macro Call block. By doing so, the actual tool change position in X and Y could be specified via the Tool Change Command Block. To use this system, parameter 6071 would have to be set to Zero (it would currently have "6" registered) so that there is no conflict with regards to which program number will be called by M06.

The Block shown in Red in the following program would be changed to the following:

G53 X#24 Y#25

To specify a Tool Change location by the Tool Change Call Block, the syntax would be as follows:

M6 X_ _ Y_ _

Where:
X_ _ = the desired X Tool Change position in Machine Coordinate values

Y_ _ = the desired Y Tool Change position in Machine Coordinate System values

If either argument is omitted in the Call Block, the respective axis Tool Change Position will be the Reference Return position (Machine Coordinate System Zero)

Regards,

Bill

%
O9001(DVF5000 A1 M06 W0 TM 20180419)
IF[#1007EQ1]GOTO600(MACRO M CODE MST SKIP)
#14=#4114(REC SEQ NO)
#15=#4001(REC G1 G0)
#16=#4003(REC G90 G91)
G31
IF[#1000EQ1]GOTO500(HEAD=T)
IF[#3010EQ-1]GOTO500
G05.1Q0
N10G80G40
N30G91G30Z0.M19M222M233
M39
N40G91G30X0.Y0. (Change to G53 X#24 Y#25)
N50M06
N60
M232M223
N500
N#14G#15G#16
G05.1Q1
N600
M99

%
 

angelw

Diamond
Joined
Sep 10, 2010
Location
Victoria Australia
Hi Bill, Im using Fanuc Control I-series.
Look at parameters 6071 to 6079, these relate to program numbers O9001 to O9009 called as Subprograms and parameters 6080 to 6089, these relate to program numbers O9020 to O9029 called as Macro Programs. Whichever parameter has "6" registered, will point you to the program number of the Sub, or Macro program you need to modify.

Regards,

Bill
 

watson13

Plastic
Joined
Nov 18, 2021
Fanuc Oi-F control. Check which program runs when tool changes. The below program is from a Doosan. It will be O9001 or O9006. G30 X0 Y0 position depends on a parameter, #1241.

%
O9001(DVF5000 A1 M06 W0 TM 20180419)
IF[#1007EQ1]GOTO600(MACRO M CODE MST SKIP)
#14=#4114(REC SEQ NO)
#15=#4001(REC G1 G0)
#16=#4003(REC G90 G91)
G31
IF[#1000EQ1]GOTO500(HEAD=T)
IF[#3010EQ-1]GOTO500
G05.1Q0
N10G80G40
N30G91G30Z0.M19M222M233
M39
N40G91G30X0.Y0. (Change this line or comment it out. I wouldn't delete because it does come in handy)
N50M06
N60
M232M223
N500
N#14G#15G#16
G05.1Q1
N600
M99

%

Hi locknut, thanks mate highly appreciated, I will let you know the outcome.
 

watson13

Plastic
Joined
Nov 18, 2021
Look at parameters 6071 to 6079, these relate to program numbers O9001 to O9009 called as Subprograms and parameters 6080 to 6089, these relate to program numbers O9020 to O9029 called as Macro Programs. Whichever parameter has "6" registered, will point you to the program number of the Sub, or Macro program you need to modify.

Regards,

Bill

Hi Bill, you're awesome cant wait to go through the parameters at coz the moment I'm doing something else, I will let you know the out come, thank you Guys.
 

watson13

Plastic
Joined
Nov 18, 2021
Hi Guys, it worked so I just went to SYSTEM parameter #3202 and and change NE9 from 0 to 1 to enable edit the sub program, I just add open close parenthesis on the program ex.(G91 G28 X0), Cheers Guys.
 








 
Top