Fanuc RoboDrill21Ti

[jorgehrr]

Today my operator press the "clear" soft key in my screen. I couldn't believed that he deleted all "H" offsets and G54...G59 ETC. ETC.

Is there a parameter that can be used to avoid this, It was not a problem to set all the "H" offsets back but now how can I find the PRZ (program zero) for all the fixtures, I have about 15 programs in there (I did not wrote them), and I do not know how to get those numbers back, the fixtures are old and they do not have any reference.

Any ideas????

Thank you.

[Mitsui Seiki]

Originally Posted by jorgehrr Today my operator press the "clear" soft key in my screen. I couldn't believed that he deleted all "H" offsets and G54...G59 ETC. ETC. Is there a parameter that can be used to avoid this, It was not a problem to set all the "H" offsets back but now how can I find the PRZ (program zero) for all the fixtures, I have about 15 programs in there (I did not wrote them), and I do not know how to get those numbers back, the fixtures are old and they do not have any reference. Any ideas???? Thank you.

Take a look in your programs.You must be able to determine where the "Zeros" are by looking at each program.

[jorgehrr]

Yes, you are right.

But it took me all afternoon. I set up a vise with a part already made and I use one of the holes as reference and little by little I was able to get drill inside the hole everything else was in place at that point I copy my X and Y.

I'm hopping there is a better way and faster was to do this.
What about a parameter to keep this key to delete all the offsets.

Thank you

Jorge

[Mitsui Seiki]

I'm sure there's a parameter for this, because it shouldn't be that easy to erase these things with the "clear" button.I can't help you with the parameter.I'm sorry.

[cnc-king]

Why don't you use G10 to load all work and height offset so this will not be a problem

[jorgehrr]

Originally Posted by cnc-king Why don't you use G10 to load all work and height offset so this will not be a problem

cnc-king

Show me how. I'm new with machine centers, I'll do some research about this G10 business.

But correct me if I am wrong. Sims like I can use the same G54 for different set ups as long as I have a G10 making the changes in my coordinates instead of using a G55...G59???? Is this how G10 works???

Thank you for the idea.


Jorge

[cnc-king]

G10 G90 L2 P1 X0.0000 Y0.0000 Z0.0000 Will Set Offsets G54 Thru G59 Where P1 Sets G54 And P6 Sets G59

G10 G90 L20 P1 X0.0000 Y0.0000 Z0.0000 Will Set Offsets G54.1 P1 Thru G54.1 P48 Where P1 Sets G54.1 P1 And P48 Sets G54.1 P48

Substituting G91 For G90 Will Add Or Subtract From The Offsets

This Is A Sample From A Fanuc With 99 Tool Geometry Offsets And No Wear Table

P001 Sets Tool #1 And R Denotes The Tool Lenght
The Same Holds Thru For G91 And G90 From Above

G10 G90 P001 R 5.1110
G10 G90 P002 R 5.8398
G10 G90 P003 R 5.5743
G10 G90 P004 R 4.5703
G10 G90 P005 R 5.0723
G10 G90 P006 R 4.8913
G10 G90 P007 R 7.1203
G10 G90 P008 R 5.1517
G10 G90 P009 R 4.5283
G10 G90 P010 R 7.9605
G10 G90 P011 R 4.9773
G10 G90 P012 R 5.3523
G10 G90 P013 R 4.0809
G10 G90 P014 R 4.7273
G10 G90 P015 R 4.4943
G10 G90 P016 R 6.4353
G10 G90 P017 R 5.2723
G10 G90 P018 R 5.4220
G10 G90 P019 R 4.6553
G10 G90 P020 R 3.9270
G10 G90 P021 R 4.2493
G10 G90 P022 R 3.2253
G10 G90 P023 R 3.4883
G10 G90 P024 R 0.0000
G10 G90 P025 R 5.9795
G10 G90 P026 R 0.0000
G10 G90 P027 R 0.0000
G10 G90 P028 R 0.0000
G10 G90 P029 R 2.9603
G10 G90 P030 R 0.0000
G10 G90 P031 R 0.0000
G10 G90 P032 R 0.0000
G10 G90 P033 R 0.0000
G10 G90 P034 R 0.0000
G10 G90 P035 R 0.0000
G10 G90 P036 R 0.0000
G10 G90 P037 R 0.0000
G10 G90 P038 R 0.0000
G10 G90 P039 R 0.0000
G10 G90 P040 R 0.0000
G10 G90 P041 R 0.0000
G10 G90 P042 R 0.0000
G10 G90 P043 R 0.0000
G10 G90 P044 R 0.0000
G10 G90 P045 R 0.0000
G10 G90 P046 R 0.0000
G10 G90 P047 R 0.0000
G10 G90 P048 R 0.0000
G10 G90 P049 R 0.0000
G10 G90 P050 R 0.0000
G10 G90 P051 R 0.0000
G10 G90 P052 R 0.0000
G10 G90 P053 R 0.0000
G10 G90 P054 R 0.0000
G10 G90 P055 R 0.0000
G10 G90 P056 R 0.0000
G10 G90 P057 R 0.0010
G10 G90 P058 R 0.0000
G10 G90 P059 R -0.0010
G10 G90 P060 R 0.0000
G10 G90 P061 R 0.0000
G10 G90 P062 R 0.0000
G10 G90 P063 R 0.0000
G10 G90 P064 R -0.0010
G10 G90 P065 R 0.0000
G10 G90 P066 R 0.0000
G10 G90 P067 R 0.0000
G10 G90 P068 R 0.0000
G10 G90 P069 R 0.0000
G10 G90 P070 R 0.0000
G10 G90 P071 R 0.0000
G10 G90 P072 R 0.0000
G10 G90 P073 R 0.0000
G10 G90 P074 R 0.0000
G10 G90 P075 R 0.0000
G10 G90 P076 R 0.0000
G10 G90 P077 R 0.0000
G10 G90 P078 R 0.0000
G10 G90 P079 R 0.0000
G10 G90 P080 R 0.0000
G10 G90 P081 R 0.0000
G10 G90 P082 R 0.0000
G10 G90 P083 R 0.0000
G10 G90 P084 R 0.0000
G10 G90 P085 R 0.0000
G10 G90 P086 R 0.0000
G10 G90 P087 R 0.0000
G10 G90 P088 R 0.0000
G10 G90 P089 R 0.0000
G10 G90 P090 R 0.0000
G10 G90 P091 R 0.0000
G10 G90 P092 R -0.0005
G10 G90 P093 R 0.0000
G10 G90 P094 R 0.0000
G10 G90 P095 R 0.0000
G10 G90 P096 R 0.0000
G10 G90 P097 R 0.0000
G10 G90 P098 R 0.0000
G10 G90 P099 R 0.0000
%

[jorgehrr]

GREAT!!!!!!
Amazing stuff.

I need to use this G10 to understand it better, When working with lathes I was told G10 is "evil" never got to know or use the code.

Well...that changes today.

Thank you for your help

Jorge
......................

I read can be used in a sub program as well: This way you keep coordinate system in you program Library.

Sample:

O6001 (Coordinate system number one SUB PROGRAM))
G90 G10 L2 P1 X-22.3837 Y-12.2827 Z-11.0387 (Assign fixture offset, this line will be edited whenever coordinate system number one is modified)
G54 (Invoke the offset just assigned)
M99 (End of sub-program)


O0001 (Main program)
N005 T01M06 (1/2 Drill)
N010 G90 S600 M03 T02
N015 M98 P6001 (Select coordinate system number one)
N018 G00 X1.0 Y1.0
N020 G43 H01 Z0.1 M08
N025 G81 R0.1 Z-0.3 F5.0
N030 G80 M09
N035 G91 G28 Z0 M19
N040 M01

[Mitsui Seiki]

Originally Posted by jorgehrr GREAT!!!!!! Amazing stuff. I need to use this G10 to understand it better, When working with lathes I was told G10 is "evil" never got to know or use the code. Well...that changes today. Thank you for your help Jorge ...................... I read can be used in a sub program as well: This way you keep coordinate system in you program Library. Sample: O6001 (Coordinate system number one SUB PROGRAM)) G90 G10 L2 P1 X-22.3837 Y-12.2827 Z-11.0387 (Assign fixture offset, this line will be edited whenever coordinate system number one is modified) G54 (Invoke the offset just assigned) M99 (End of sub-program) O0001 (Main program) N005 T01M06 (1/2 Drill) N010 G90 S600 M03 T02 N015 M98 P6001 (Select coordinate system number one) N018 G00 X1.0 Y1.0 N020 G43 H01 Z0.1 M08 N025 G81 R0.1 Z-0.3 F5.0 N030 G80 M09 N035 G91 G28 Z0 M19 N040 M01

Why complicate things?
You will still be able to keep it in your program Library.

O6001
G80 G40
T01M06 (1/2 Drill)
G0 G90 G10 L2 P1 X-22.3837 Y-12.2827 Z-11.0387 M3 T2
G43 H01 Z0.1 M08
G54.1 P1 X1.0 Y1.0
G81 R0.1 Z-0.3 F5.0
G0 G80 Z1.0 M9
G91 G28 Z0 M19
M30

[jorgehrr]

Man...this is good.
Let me get this

I am using my G54.1P1 but my G10 is replacing the values??? or setting the values if empty.
If I understand this well, I think I see an error in your sample, please correct me if I am wrong ( I am sure I am )

Your G54.1P1 Should be only G54P1...right????


I have to try this.

Thank you all.

Jorge

[Kool Parts]

Just call methods service dept. They will have you up and running in no time. There is nothing about that control they haven't seen before.

http://www.methodsmachine.com/

[Mitsui Seiki]

Originally Posted by jorgehrr Man...this is good. Let me get this I am using my G54.1P1 but my G10 is replacing the values??? or setting the values if empty. If I understand this well, I think I see an error in your sample, please correct me if I am wrong ( I am sure I am ) Your G54.1P1 Should be only G54P1...right???? I have to try this. Thank you all. Jorge

The G54.1 is not an error.You use G54.1 instead of G54 with G10.Maybe you can use only G54, I haven't tried that.