Short workpieces must be machined on turning centers on a regular basis, but lot sizes may not justify the use of a bar feeder or puller. In these cases, it is often helpful to machine more than one workpiece from a single piece of raw material. (See the illustration below.)
With this technique, cycle time is minimized, there is a longer period of unattended operation and the remnant (scrap) can be averaged over several workpieces.
Programming for this application can be cumbersome, because the same series of commands must be repeated based upon the number of workpieces being machined from the bar. There is a technique that dramatically simplifies the programming of this application—if your turning center control uses geometry offsets and work shift (as most current model Fanuc and Fanuc-compatible controls do) and if you can program offset changes.
Here's how it works: You'll write the program for one of the workpieces in the normal manner, but end it as a subprogram (with M99 on Fanuc controls). The controlling program (the program the operator activates) will first set the work shift value to its initial setting (7.25 in our example). It will then command that the subprogram be activated to machine the first workpiece. The controlling program will then incrementally step the work shift value by the distance between the workpieces (1.0 in our case). We're simply shifting the program zero point to a new location. Then the subprogram will be activated again. This is simply repeated for the number of workpieces that must be machined.
Here is an example controlling program that assumes program number O1000 is the subprogram that machines one workpiece. Note that in the G10 commands, the P0 word is specifying that the work shift value is being set.
O0001 (Control program)
N005 G10 P0 Z7.25 (Work shift value to initial setting)
N010 M98 P1000 (Run first workpiece)
N015 G10 P0 W-1.0 (Incrementally step work shift value by –1.0)
N020 M98 P1000 (Run second workpiece)
N025 G10 P0 W-1.0 (Incrementally step work shift value by –1.0)
N030 M98 P1000 (Run third workpiece)
N035 G10 P0 W-1.0 (Incrementally step work shift value by –1.0)
N040 M98 P1000 (Run fourth workpiece)
N045 G10 P0 W-1.0 (Incrementally step work shift value by –1.0)
N050 M98 P1000 (Run fifth workpiece)
One limitation of this technique has to do with restarting. If a tool breaks, or if, for any other reason, you must stop the cycle in the middle of running one of the workpieces, it is nearly impossible to restart from where you left off. You'll have to run the entire program from the beginning, cutting air until you reach the point when the program was interrupted.blog comments powered by Disqus