A sample tool change macro.

[gar]

050817-0729 EST USA

This morning I looked in the HAAS manual for their timed compensation.

There is no definition of the algorithm so it is maybe linear. See settings 109, 110, and 112.

Maximum time is 300 minutes, and maximum compensation is +/- 2/1000".

.

[Geof]

I had looked at that and I somehow came to the conclusion it needed the temperature sensor option. Reading too fast I guess. Next time we do the part we will try this and see if it helps.

Thanks

[gar]

050822-1305 EST USA

Warning --- For those unfamiliar with G10 L12 ...etc.

This instruction changes (overwrites) the content of the addressed location. This means for example if you are selecting the "diameter offset" ( diameter offset is what L12 specifies ) of D code ( logical address of the offset ), then you overwrite whatever is at that location with the value associated with R at the time of execution of the G10 instruction. You can change this diameter offset value many times to different values within a program.

This means if you were to manually set the "diameter offset" before running the program and that manually set value was different from what is in the program, then your manually set value would be destroyed, i.e., have no effect.

One execution of G10 affects one and only one location at a time. Thus, changing tool diameter has no effect on the "wear offset" for that tool.

.

[Geof]

Advice appreciated; unfortunately I learnt it the hard way. No machine damage just tool and me scratching my head for a short while.

[gar]

050822-1407 EST USA

Geof:

Does your last post mean you tried the tool change routine, or just the G10 command, or from past experience.

The real neat thing illustrated in my initial sample program is that you can create a subroutine for a part path for your finished path, and then simply using the G10 command keep changing the tool diameter and calling the path subroutine to do any number of rough passes and finally one or more finish passes with the same tool or different tools.

The G10 L12 has no effect on the value you manually or automatically put in the wear offset for the tool.

.

[Geof]

This happened a four or five years back when I was teaching myself G code programming. I was entering tool diameters manually for tool compensation and then finally figured out how to do it from the program with the G10 L12 so I finished up with some programs that needed it manually and some had it in G10. I forget the details but I think it was a case of using a different sized tool and changing the manual entry but the particular program was using G10. The part was in a fixture with not much room so the tool tried to create enough room when tool compensation did not offset it the correct amount. High helix two flute carbides don't last long machining cold rolled steel at a fast speed and feed.

I have not tried your tool change routine because in my shop we have standardized on a different format for clarity. I like your post though because it is a very lucid explanation which clarifies macro formats. Regarding your comment about changing the tool diameter and then going to a common subroutine for roughing and finishing I do this quite frequently. I have found that I can simulate the Haas G150 general purpose pocket milling function with a subroutine and multiple calls using different tool diameters entered from G10 lines preceding the M97 line(s). These take a bit longer to program but run faster than the Haas function for the same pocket shape so over a few hundred pieces it saves time.