offsetting the B axis on an A55 with a Fanuc OMC

[Mike Whitten CAD/CAM Contractors]

Hello folks,

 

I am working with a client that has a 1991/1992 Makino A55 with a Fanuc OMC control and 1 degree indexer. We can not find a way to G10 the B axis as it seems to just ignore the entry on the G10 line. We also tried G92 without success. It will accept an offset typed in manually on the offset page but we need to be able to do it by program.

 

This is the format we tried:

-----

G90

G10 L2 P1 X0 Y0 Z0 B90.

-----

What will happen is that the XYZ data will be ignored and the machine will just move to B90. If you remove the B value, the XYZ data writes just fine.

 

If you input a G92 B90., it just moves to absolute B90. and ignores the G92 command.

 

My guess is that it must be input with a special format or by user macro. Does anyone have a clue as to how to make the G10 work?

 

Thank in advance for any help on this one.

Mike

[iowajim62]

Michael,

 

This worked on an A55 I ran back in the day.

 

1st side

G90G10L2P1X0Y0Z-21.076

G0G90B0.

 

2nd side

G90G10L2P2X0Y0Z-21.076

G0G90B90.

 

3rd side

G90G10L2P3X0Y0Z-21.076

G0G90B180.

 

4th side

G90G10L2P4X0Y0Z-21.076

G0G90B270.

 

Good Luck

[YoDoug®]

Can you just write the variable instead of using G10. You should be able to look in the Fanuc parameter book for the machine and see what variable number is the G54 B offset. Something like

 

#2022 = 90.

 

Then G10 the XYZ coordinates.

[Mike Whitten CAD/CAM Contractors]

Hello,

 

Jimmy,

-------

G90G10L2P2X0Y0Z-21.076

G0G90B90.

--------

Are you saying that the control will know this is a G10 B90 because it is on the line after the G10 line?

 

Doug,

This is what I am also thinking about but we do not have the book to find the variable #.

 

Thanks!

Mike

[iowajim62]

Michael,

Yeah that was the way it worked. I always thought that there was a parameter that needed changed. But those Makino controls are different from any other Fanuc control I've ever ran. If that doesn't work I would do like Doug said and use variables to get it in the control.

[Mike Whitten CAD/CAM Contractors]

Jim,

 

I will have them try it as soon as they can.

 

Thanks!

[iowajim62]

Your Welcome Sir

[Dave Ball]

#5224 #5244 #5264 #5284 #5304 #5324 should be the variables for B axis G54 - G59. Also check the common/shift offset to see that they are set to zero as this will affect the outcome regardless of how you set things.

 

HTH

[Mike Whitten CAD/CAM Contractors]

Hello ShefferCNC,

 

I appreciate the info. We will try it soon and post.

 

Thanks!,

Mike

[Mike Whitten CAD/CAM Contractors]

Hello,

 

Jim,

We tried the method as you wrote and the machine just moved to the B angle.

----

1st side

G90G10L2P1X0Y0Z-21.076

G0G90B0.

----

 

 

ShefferCNC,

The machine just alarmed out. It did not seem to recoginze the variable numbers.

 

 

I was able to get some different variable numbers from another source and it worked fine just as Doug wrote above. IE: #2801=90. will set G54 to B90.

 

#2801......G54 B value

#2802......G55 B value

#2803......G56 B value

#2804......G57 B value

#2805......G58 B value

#2806......G59 B value

 

Thanks again for the help!

Mike

[Dave Ball]

Michael,

 

Sorry for the mix up. The variables I gave you work fine on my machine. Glad you found your answer though.

[Mike Whitten CAD/CAM Contractors]

Hello ShefferCNC,

 

All is well. This one surprised everyone over here. I had never seen a machine where you could not G10 the B until now. Kind of wierd I think.

 

Thanks!