[CNCturtle]

I'm pretty new to the Fanuc 10M controller and I recently had a "learning experience." I was trying to load a program using DNC software and I skillfully deleted all the O90XX programs in my program directory...OOps. I'm not looking for anything that I'm not entitled to or proprietary, but is there a way to recover those or a place to get them? I have a list of the ones that were installed.

Also, what are they? Were they the optional macros I hear about sometimes? Do they enable the use of more G-codes? When I run some programs I get alarms such as "improper G-code" or "illegal g-code" and I'm wondering if it could be related...

Any and all suggestions, recommendations, comments, insults, etc... are welcome.

Thank You!

[underthetire]

There is no standard list. Some are from machine builders, others are assigned macros to g or m codes someone wrote.

[angelw]

I'm pretty new to the Fanuc 10M controller and I recently had a "learning experience." I was trying to load a program using DNC software and I skillfully deleted all the O90XX programs in my program directory...OOps. I'm not looking for anything that I'm not entitled to or proprietary, but is there a way to recover those or a place to get them? I have a list of the ones that were installed.

Also, what are they? Were they the optional macros I hear about sometimes? Do they enable the use of more G-codes? When I run some programs I get alarms such as "improper G-code" or "illegal g-code" and I'm wondering if it could be related...

Any and all suggestions, recommendations, comments, insults, etc... are welcome.

Thank You!

Macro programs can be called via G65 and G66, or the program having Macro statements can be called as a Subprogram using M98. Macro programs can also be called using a G code by making reference to a particular G code. Subprograms can be called by M codes other than M98 by making reference to a particular M code. This is done by registering the number associated with the G or M code in a parameter that has an association with a O90XX program number; see the tables following:

G code registration to call a Macro Program
Parameter Num -------------- Associated Program Num
7050 ---------------------------- 9010
7051 ---------------------------- 9011
----------------
----------------
7059 ---------------------------- 9019

M code registration to call a Subprogram
Parameter Num -------------- Associated Program Num
7071 ---------------------------- 9001
7072 ---------------------------- 9002
----------------
----------------
7079 ---------------------------- 9009

You can see if any specific, or custom G and M codes were being used to call a O90XX by viewing the above parameters to check for the registration of a number other than Zero. However, deleting the O90XX programs won't result in an "improper G-Code" (PS/10 alarm). If a custom "G" code had been created by registering a number in the appropriate parameter, lets say 101 in parameter 7050, and the parameters of the machine were deleted, then this would result in a PS10 alarm when G101 is attempted to be executed. If the parameter 7050 still had 101 registered, but program O9010 was deleted, you would not get an "improper G-Code" alarm, but a "program not found" error.

For more help, post the G codes that you're getting the "improper G-Code" error with.

Regards,

Bill

[CNCturtle]

Thank You angelw and underthetire for the information. Those are good things to know. It sound like erasing those programs is probably not the problem. Now suspect #1 is my post processor. I got "PS010 improper G code" when the program came to a G70. I believe G70 is for finish contouring on a lathe and I'm milling. I'm not sure why my post processor put a G70 in there but I may have configured something wrong. I have a couple of things I need to try on that front, including some suggestions from the post processor support team. I will report back. Thanks Again!

[CNCturtle]

Okay, I'm reporting back. I have tried several more things and found that I get "PS011 Improper NC-Address" whenever my program calls drilling, reaming, and boring cycles (G73-G89). I haven't actually tried all of them but enough to see that I always get the same alarm. Is there a way to make my controller "understand" G73-G89 ?

Here is a super simple program that just reams four holes:

%PM5
N100 (0005)
N102 (main holes)
N104 (T2 D=0.368 CR=0 TAPER=118deg - ZMIN=-1.)
N106 G90
N108 G94
N110 G18
N112 G20
N114 (0.375 holes)
N116 M9
N118 S1000 M3
N120 M9
N122 G0 X-0.375 Z-0.375
N124 Y0.6
N126 G18
N128 G0
N130 Y0.2
N132 G85 Z-0.5356 Y0.1 B0.6 F5
N134 G79 X-0.375 Y-1.0356 Z-0.375
N136 G79 X-2.625 Y-1.0356 Z-0.375
N138 G79 X-2.625 Y-1.0356 Z-3.625
N140 G79 X-0.375 Y-1.0356 Z-3.625
N142 Y0.6
N144 M9
N146 M30

My Fanuc 10M controller just gets to the G85 and throws the alarm. I'm not sure why or how to fix it. Any help is appreciated.

Thanks!

[dcoupar]

Okay, I'm reporting back. I have tried several more things and found that I get "PS011 Improper NC-Address" whenever my program calls drilling, reaming, and boring cycles (G73-G89). I haven't actually tried all of them but enough to see that I always get the same alarm. Is there a way to make my controller "understand" G73-G89 ?

Here is a super simple program that just reams four holes:

%PM5
N100 (0005)
N102 (main holes)
N104 (T2 D=0.368 CR=0 TAPER=118deg - ZMIN=-1.)
N106 G90
N108 G94
N110 G18
N112 G20
N114 (0.375 holes)
N116 M9
N118 S1000 M3
N120 M9
N122 G0 X-0.375 Z-0.375
N124 Y0.6
N126 G18
N128 G0
N130 Y0.2
N132 G85 Z-0.5356 Y0.1 B0.6 F5
N134 G79 X-0.375 Y-1.0356 Z-0.375
N136 G79 X-2.625 Y-1.0356 Z-0.375
N138 G79 X-2.625 Y-1.0356 Z-3.625
N140 G79 X-0.375 Y-1.0356 Z-3.625
N142 Y0.6
N144 M9
N146 M30

My Fanuc 10M controller just gets to the G85 and throws the alarm. I'm not sure why or how to fix it. Any help is appreciated.

Thanks!

My 10M manual doesn't list G79. Also, what does the B in the G85 block represent? Usually that is a rotary (B-axis) command. I think that it should be R0.6, not B0.6

[CNCturtle]

Thank you dcoupar. I think you're totally right. I don't know why my post put that in there. Good catch! I missed it. When I change the "B" to "R" I don't get an alarm. I'm still not 100% sure it's doing what was intended but at least there's no alarm . I have never seen a G79 and I couldn't find it in any of my manuals. I was surprised that my post put it there. I'm guessing/hoping it's simply the wrong G-code. Maybe G99 to return to R-level? G89 is a boring cycle. That at least sounds closer. Maybe I'll try those....