Two popular applications for probing systems are: providing help when making setups and in-process gaging. Setup help applications include determining and entering program zero assignment values into fixture offset, aligning the angular position of the workpiece with the program (with axis rotation) and determining which of several workpieces is being machined at the current time. In-process gaging, of course, involves measuring workpiece attributes right on the CNC machining center.
The more accuracy that is required in your application, the more you might tend to worry about your probing system. With in-process gaging applications, you should use the same rules as those that apply to any measuring tool. Most tool engineers will agree that the accuracy required of your measuring device should be within 10 percent of the tolerance band you intend to measure. If you have an overall tolerance of 0.001 inch, for example, then your measuring device should be accurate to ±0.0005 inch.
Though many probe manufacturers claim extreme accuracy for their probes, accuracy is just one consideration. When you consider machine-related factors and how adequately overshoot and droop are handled by the probing system, the overall accuracy usually worsens.
Again, the more you require from your probe, the more likely you are to worry about your probe’s accuracy. All probing systems, of course, incorporate calibration procedures, but you may be questioning whether something has happened since calibration that affects probing accuracy. Or you may be questioning the accuracy of the calibration procedure itself.
The test I show assumes that you are using the probe for the purpose of assigning program zero (possibly among other applications). However, it shouldn’t be too difficult to modify this test based upon whatever probing application you have. Also, we’re only testing for XY accuracy.
This test involves placing a block with a round hole on the table. To make it quick and easy to test whenever you wish, I recommend permanently mounting the block, or at least providing a way to quickly mount the block, in exactly the same location (by keying it to the table). Manually measure the distance from the zero return position to the hole in each axis (using a dial indicator mounted in the spindle). Place the results in permanent common variables #521 and #522 respectively (as positive values).
Whenever you question the accuracy of your probing system (or its calibration), place the dial indicator in the spindle and run this program:
O1000 (Test program for probe accuracy)
G91 G28 Z0 (Be sure the Z axis is well away from obstructions)
G54 (Invoke the coordinate system measured by the probe)
#101 = #521 + #5221 (Determine distance from program zero to hole center in X)
#102 = #522 + #5221 (Determine distance from program zero to hole center in Y)
G90 G00 X-#101 Y-#102 (Move over hole)
M30 (End of program)
This program assumes the normal use of fixture offsets. That is, the X and Y values in fixture offset number one are the distances from the machine’s zero return position to program zero in X and Y. They will be large negative values entered by the probing system during program zero measurement. We’re also assuming that #5221 and #5222 are the system variables that contain the current values of fixture offset number one’s X and Y registers (respectively). You must reference your programming manual to confirm the correct system variables.
After running this program, the spindle’s center should be right above the center of the hole in the block—that is, if your probing system is working properly. You simply bring down the Z axis and indicate the hole to find out.