![]() | |
| Home Page | Mark Forums Read | Today's Posts | My Replies | Classifieds | Reviews | Photo Gallery | Web Links | Share Files | Advertise With Us | Ad List |
| |||||||
| CNC Machining Centers Discuss wood cutting CNC machining centers, and Point-to-Point machines here. |
| This forum is sponsored by: |
![]() |
| | LinkBack | Thread Tools | Search this Thread | Display Modes |
|
#1
| ||||
| ||||
All my fixture offsets are full (G54, G55.....) I know I can use G10 to input new offsets, my question is at the end of the program.... are the original numbers going to go back and what is the M/G code that does it. I just want to make sure if the original fixture offsets will remain after I use G10. Thank you in advance George |
|
#2
| ||||
| ||||
Yes the offsets should remain. Here is an example of what we use. G10L20P1X-9.9149Y-11.8528Z-22.419 G10L20P2X-1.9459Y-11.8528Z-29.771 G10L20P3X-17.8819Y-11.8528Z-29.771 G0G17G40G80 T5 M6 T6 G54.1P1 G0G90X0.Y1.375S1579M3 G43Z1.H5M8 G81G98X0.Y1.375Z-.1565R.1F9.47 Y-1.375 G0G80Z1. G91G28Z0. G54.1P2 G90G0X.75Y0. G43Z1.H5 G81G98X.75Y0.Z-.0985R.1F9.47 G0G80Z1. G91G28Z0. G54.1P3 G90G0X-.75Y0. G43Z1.H5 G81G98X-.75Y0.Z-.0985R.1F9.47 G0G80Z12. M9 G91G30X0Y0Z0M67 M1 |
|
#3
| ||||
| ||||
| Ohhh. Do you see anything wrong with mine???? 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 P1 X1.0 Y1.0 G81 R0.1 Z-0.3 F5.0 G0 G80 Z1.0 M9 G91 G28 Z0 M19 M30 Thank you in advance George |
|
#5
| |||
| |||
Based on the little bit you have written I think you should do some reading about G52. G52 gives you an offset shift and it does not change the G54, etc offset values. You can use many different G52 commands in a single program; in effect with G52 you have an unlimited number of offsets possible. Depending on your machine the G52 values may be zeroed by M30 or RESET but you can always zero them by using G52 X0. Y0. Z0.
__________________ An open mind is a virtue...so long as all the common sense has not leaked out. |
| Sponsored Links |
|
#7
| ||||
| ||||
| Well....... It changed mine. I was convince numbers will remain the same after the M99 code but Geof. is correct, the change stays. In my machine I can not use G54.1 P? (machine alarms out) It has to be only G54 P? May be that is the reason. Thank you guys. I'll find the way to get them back. Cheers George |
|
#8
| |||
| |||
|
Like I said above...read up on G52, it will do what you want.
__________________ An open mind is a virtue...so long as all the common sense has not leaked out. |
|
#9
| |||
| |||
| "my machine I can not use G54.1 P? (machine alarms out).." You do not have the Extended offset option so the G54.1 P? will generate an alarm, there is a cost if you need that many offsets. G54 G55, G56, etc. is standard on the controls, and it gives you six offests to play with. The extended offset option gives you those 6 plus 48 additional. |
|
#11
| |||
| |||
| Our machines run several different programs and we change the work offset many, many times within a given program. I guess my question would be: Why not use the G10 as much as needed. With good programing discipline you can change as much as need to accomplish the programming needs. |
|
#12
| |||
| |||
| These were production machines and machine operators did not adjust the offsets. That was process engineer function. We used a single G54 offset register but transfered in the offsets for specific table positions from the extended offset table. The B<value> selected the offsets to use automatically. Basically think of a dynamic offset that follows the table, but on a control that did not have the option. So we created a sub program that accomplished the task automatically. |
![]() |
| Currently Active Users Viewing This Thread: 1 (0 members and 1 guests) | |
| Thread Tools | Search this Thread |
| Display Modes | |
| |
Similar Threads | ||||
| Thread | Thread Starter | Forum | Replies | Last Post |
| G68 Coordinate Rotation System | ebigfoot2 | Fanuc | 2 | 08-13-2007 07:33 AM |
| coordinate system | kiethnt | G-Code Programing | 6 | 04-26-2007 07:46 AM |
| Coordinate system problems | R.thayer | LinuxCNC (formerly EMC2) | 0 | 11-19-2006 02:36 PM |
| coverting from Right-hand to left-hand coordinate system | eltonr | General CAM Discussion | 6 | 10-14-2004 08:40 PM |
| User coordinate system? | HuFlungDung | OneCNC | 5 | 04-18-2003 09:26 PM |