Need help fanuc OiD parametric program instead M98 Q33 L5

Hello everyone, I'm a mechanical engineer who faces the cnc programming . I plan about a week a work center with Fanuc Hartford OID equipped with hard drives seen as dataserver , I just managed to make a profile path with repetitions and increase with M98 Q loaded on the memory of the CNC , the same path if given in DNC mode directly from hard drive gives me error file not found, from what I deduced that M98 only works when loaded into memory , the path is as follows:

%
O001
G17 G54 G5.1Q1 R6
T07 M06
S4000 F8000 M03
G00 G91 G28 Z0 (Z DI SICUREZZA)
G90
M58
G43 H07 Z100
G00 X0 Y-66
G00 Z2
G01 Z0 F100
M98 Q33 L5
G00 G91 G28 Z0
G90
G00 G53 X-700 Y0 (SPOST TAVOLA FRONTE OPERAT)
G5.1Q0
M30

N33
G01 G91 Z-0.5 F100
G90
G01 X0 Y-46 G41 F8000 D07
G01 X-249
G02 X-255 Y-40 I0 J6
G01 Y40
G02 X-249 Y46 I6 J0
G01 X249
G02 X255 Y40 I0 J-6
G01 Y-40
G02 X249 Y-46 I-6 J0
G01 X0
G00 X0 Y-66 G40
M99
%

I ask you experts if I can create a path with the parameters that make me repeat the profile for XX times and increase Z . I hope I helped to load because a path on the memory without being able to create folders in fact I complicates things over to the production , manufacture progressive dies from 300 parts and then the career paths taken by cam, with some changes , I'd like you could to feed directly from HD DNC mode so that they are divided by folder and would not go into total confusion . I have a laptop on the machine from which I transfer the files to the dataserver and intake modifications to the paths . If you need more information do not hesitate to ask

i made it for -0.5 for each step on Z
the step of deep on Z you can easily set up on #101
%
O001
G17 G54 G5.1Q1 R6
T07 M06
S4000 F8000 M03
G00 G91 G28 Z0 (Z DI SICUREZZA)
G90
M58
G43 H07 Z100
G00 X0 Y-66
G00 Z2
G01 Z0 F100
#100=0
#101=-0.5(step of Z axis)
#102=-5(the finish depth of cut--you can set it as much as you want to go with Z )
N1
#100=#100+#101
G01 Z#100 F100
G01 X0 Y-46 G41 F8000 D07
G01 X-249
G02 X-255 Y-40 I0 J6
G01 Y40
G02 X-249 Y46 I6 J0
G01 X249
G02 X255 Y40 I0 J-6
G01 Y-40
G02 X249 Y-46 I-6 J0
G01 X0
G00 X0 Y-66 G40
G0Z0
IF[#100 LE #102]GOTO 2
GOTO 1
N2
G00 G91 G28 Z0
G90
G00 G53 X-700 Y0 (SPOST TAVOLA FRONTE OPERAT)
G5.1Q0
M30

this program will go over and over untill Z will be -5.5mm deep in the workpiece.this because i put in the condition LE-less or equal ,if you can increase or decrease with #102
good luck

minor problem.
if for example depth should be -5.6 the program wil create a overrun of 0.4 mm making a total depth op 6.0 mm.
same happens if incremental cutting depth doesnt ad up to eccactly the needed total depth.
Ones i programmed a macro with overrun protection.
tryed to implement in zavateandu's program but be carful when trying out and if #102 is a Z+ value it might not work

%
O001
G17 G54 G5.1Q1 R6
T07 M06
S4000 F8000 M03
G00 G91 G28 Z0 (Z DI SICUREZZA)
G90
M58
G43 H07 Z100
G00 X0 Y-66
G00 Z2
G01 Z0 F100 (IF Z0 SHOULD BE YOUR START POSITION)
#100=#5042 (start position Z axis)
#101=-0.5(step of Z axis)
#102=-5(the finish depth of cut--you can set it as much as you want to go with Z )
WHILE[#100GT#102]DO1
IF[[#100+#101]LT#102]THEN#101=#102-#100(PREVENT OVER-RUN)

#100=#100+#101
G01 Z#100 F100
G01 X0 Y-46 G41 F8000 D07
G01 X-249
G02 X-255 Y-40 I0 J6
G01 Y40
G02 X-249 Y46 I6 J0
G01 X249
G02 X255 Y40 I0 J-6
G01 Y-40
G02 X249 Y-46 I-6 J0
G01 X0
G00 X0 Y-66 G40
G0Z0
END1
N2
G00 G91 G28 Z0
G90
G00 G53 X-700 Y0 (SPOST TAVOLA FRONTE OPERAT)
G5.1Q0
M30

Quote:

---

Originally Posted by duivenhok

minor problem.
if for example depth should be -5.6 the program wil create a overrun of 0.4 mm making a total depth op 6.0 mm.
same happens if incremental cutting depth doesnt ad up to eccactly the needed total depth.
Ones i programmed a macro with overrun protection.
tryed to implement in zavateandu's program but be carful when trying out and if #102 is a Z+ value it might not work

%
O001
G17 G54 G5.1Q1 R6
T07 M06
S4000 F8000 M03
G00 G91 G28 Z0 (Z DI SICUREZZA)
G90
M58
G43 H07 Z100
G00 X0 Y-66
G00 Z2
G01 Z0 F100 (IF Z0 SHOULD BE YOUR START POSITION)
#100=#5042 (start position Z axis)
#101=-0.5(step of Z axis)
#102=-5(the finish depth of cut--you can set it as much as you want to go with Z )
WHILE[#100GT#102]DO1
IF[[#100+#101]LT#102]THEN#101=#102-#100(PREVENT OVER-RUN)

#100=#100+#101
G01 Z#100 F100
G01 X0 Y-46 G41 F8000 D07
G01 X-249
G02 X-255 Y-40 I0 J6
G01 Y40
G02 X-249 Y46 I6 J0
G01 X249
G02 X255 Y40 I0 J-6
G01 Y-40
G02 X249 Y-46 I-6 J0
G01 X0
G00 X0 Y-66 G40
G0Z0
END1
N2
G00 G91 G28 Z0
G90
G00 G53 X-700 Y0 (SPOST TAVOLA FRONTE OPERAT)
G5.1Q0
M30

---

The following is nearly the same, but with the Conditional Statement simplified. The logic will work with a + value for #102, #3 in my example. Your example and the following has a chance of working in a DNC session, but I don't believe the example in Post #2 does, because of the GOTO statements. The GOTO searches forward and if the target Sequence number is not found, the search continues from the top of the program.

Regards,

Bill

%
O001
G17 G54 G5.1Q1 R6
T07 M06
S4000 F8000 M03
G00 G91 G28 Z0 (Z DI SICUREZZA)
G90
M58
G43 H07 Z100
G00 X0 Y-66
G00 Z2
G01 Z0 F100 (IF Z0 SHOULD BE YOUR START POSITION)
(Local Variables will suffice as no other program is using the Variables)
#1 = #5043 (start position Z axis)
#2 = -0.5 (step of Z axis)
#3 = -5.0 (the finish depth of cut--you can set it as much as you want to go with Z )

WHILE [#1 GT #3]DO1
#1 = #1 + #2
IF[#1 LT #3] THEN #1 = #3 (PREVENT OVER-RUN)
G01 Z#1 F100
G01 X0 Y-46 G41 F8000 D07
G01 X-249
G02 X-255 Y-40 I0 J6
G01 Y40
G02 X-249 Y46 I6 J0
G01 X249
G02 X255 Y40 I0 J-6
G01 Y-40
G02 X249 Y-46 I-6 J0
G01 X0
G00 X0 Y-66 G40
G0Z0 (As the End X, Y Position in previous block is the same as the Start Position, this move to Z0 is not required.)
END1
G00 G91 G28 Z0
G90
G00 G53 X-700 Y0 (SPOST TAVOLA FRONTE OPERAT)
G5.1Q0
M30

hello and thanks to all but in DNC mode from dataserver the machine give the error: illegal mode if/ while/ do. Instead if i load it on cnc memory it works fine. how can i resolve? thanks for your great works

Quote:

---

Originally Posted by bigodinos

hello and thanks to all but in DNC mode from dataserver the machine give the error: illegal mode if/ while/ do. Instead if i load it on cnc memory it works fine. how can i resolve? thanks for your great works

---

I don't believe you will be able to. I knew the version using the GOTO branch wouldn't work, for the reason given in my previous Post, When supplying data to the control via DNC, the program code goes to God once its been executed by the control. Accordingly, branching to a previous block using GOTO wont work because that previous block no longer exists.

I thought the DO Loop method may have had a chance of success due to the amount of code that's buffered and the different process of the WHILE/DO Loop, but I've since found that a repeat instruction or branch instruction is not possible. If such an instruction is executed, P/S alarm No. 123 is raised. Also, when reserved words such as IF, WHILE, COS, and NE etc are used used with User Macro Code in DNC operation, a blank is inserted between adjacent characters.

Regards,

Bill

thanks but your give me bad news, i think that fanuc is an economic and simply control but it has limited functions, heidenhain is the best!!