In last month’s column I stated that one of the most common causes of wasted setup time is improper trial machining to make the first workpiece pass inspection. Trial machining involves taking each tool in the program and making it cut to size prior to going on to the next tool.
While it may not be possible to trial machine on sliding headstock or Swiss- type centers, it is possible to run a test workpiece. The test workpiece can be very simple, making it obvious as to which tool has machined a given surface. Measurements will be taken with standard measuring tools. If custom macro techniques are used, getting ready to run the test workpiece will take about a minute. Figure 1 shows the test workpiece in our example.
While we’ve shown a dimensioned workpiece, every dimension may change from job to job, so we’ll need an easy way of specifying the related sizes. Additionally, we’re setting up for five cutting tools (facing tool, turning tool, drill, boring bar and cutoff tool) but there may be times when internal tools are not required for the job. With a relatively simple main program, you can easily define the test workpiece and operations you want to perform. Here is an example:
O0001 (Main program)
N1 G65 P6000 D0.5 Z1.0 (define workpiece)
N2 G65 P6001 T1.0 S1.0 (facing tool)
N3 G65 P6001 T2.0 S2.0 D0.48 Z0.25 (turning tool)
N4 G65 P6001 T5.0 S7.0 Z.75 (0.25 drill)
N5 G65 P6001 T6.0 S8.0 D0.27 Z0.25 (boring bar)
N6 G65 P6001 T7.0 S3.0 D-0.01 (cut-off tool)
N7 M30 (end of program)
Notice that two custom macro programs will be required, O6000 (the part definition custom macro) and O6001 (the cutting operations custom macro). Here is what the variables mean in each:
D: Test part stock diameter
Z: Test part length
T: tool type
1: facing tool
2: turning tool
3: external threading tool
4: center drill (stop after this tool)
6: boring bar
7: cut-off tool
8: threading tool
9: internal threading tool
10: end mill (cross tool)
11: cross drill (cross tool)
S: Station number
Z: Z depth of machining for certain tools
D: diameter to machine
Program O0001 (the main program) will be modified for each job. Line N1 defines the part as 0.5 inch in diameter.
Line N2 is the facing operation. Notice the code number for tool type. Type 1 (in our example) is a facing tool. The S word specifies that it is in station one. No additional variables are required, because the previous command specifies the stock diameter, and this tool will always face to Z0 and to the center of the workpiece.
In line N3, the turning is being done. Additional variables include D for the diameter to turn (0.48 in our case) and Z for the length of the turned diameter (0.25 in our case).
In line N4, drilling is being done. The Z in this command is the drilling depth (not including drill point).
Line N5 does the boring with the same variables that were used for turning (D and Z).
Finally, line N6 does the cutoff. D specifies the diameter to which the cutoff tool will go.
One last point. If the machine has a sub-spindle (as most Swiss-type turning centers do), similar techniques can be used after the actual workpiece has been machined in the main spindle.blog comments powered by Disqus