Probing is something a lot of programmers and manufacturing engineers never consider when trying to reduce cost and improve quality but probes can do both!
Here are some basic programs to get you started on probing. If you remember to use the Protected Positioning cycle when moving the probe around you have nothing to fear!
Calibrating a Renishaw Probe's Tool Length (12/23/97)
This program uses two variables, #537 and #538, to position the probe in X and Y and then calibrates the probe's tool length. An approximate tool length Offset must be entered for the probe before running this program. Using variables to position the probe makes the program very flexible. Simply move the machine to the point where you want to touch the stylus and look at the position display. Enter these values for #537, #538 and run the program. You will need to edit T60 to match the tool number of your probe.
%
O9102
(SET PROBE TOOL LENGTH)
(#537=X POSITION TO TOUCH)
(#538=Y POSITION TO TOUCH)
G0G91G30Z0
G0G91G30Y0
T60T0M6
#5203=0(CLEAR COMMON Z)
G0G90G54X#537Y#538
G65P9810Z2.0F200.0
G65P9801Z0T24
G65P9810Z2.0F200.0
G0G91G30Z0
G0G91G30Y0
M30
%
Calibrating a Renishaw Probe on a Machining Center (11/28/97)
A spindle mounted probe can be one of the best tools you'll ever buy for increasing productivity but keeping it calibrated or calibrating after breaking a stylus (a rare event of course) can be a pain. Using the program and fixture in this tip makes calibrating a simple task that can be done in a few minutes. This example calibrates the probe's stylus offset and diameter. The probe's tool length offset must be calibrated before using this example.
The first step is to purchase a 1.000 ring gage that can be dedicated to the fixture. Next, decide how the fixture can be mounted to the machine quickly and easily. The fixture in the figure is held in a three jaw chuck on one mill, bolts to a sub-plate on another mill and bolts to a two axis tilting table on another. The key feature is that it can be mounted quickly and without major problems.
In the figure, the ring gage is held down on the left side of the fixture and a replaceable aluminum plate is held on by two cap screws in the center. To calibrate the probe a boring bar is used to bore a hole in the plate at X0Y0. This establishes an exact center to set the stylus's X, Y offset. When the bore gets too large simply throw the plate away and make another one.
To calibrate the probe, a G54 coordinate system is established and then the top of the plate is probed to set an exact Z0, and the bore is probed to set an approximate X0, Y0. Next, the boring bar opens the bore up to establish the exact X0, Y0 of the plate. Make sure that the bore was completely cleaned up by the boring bar.
The probe is then positioned over the plate and the bore is probed using the standard Renishaw 9802 cycle. Next the ring gage is probed using 9804 Vector calibration. The whole cycle should only take a few minutes and when finished the probe is calibrated for stylus offset and stylus diameter.
In this example, G54 X, Y, Z are preset in the program using the code
#5221=-9.1607
#5222=-6.8235
#5223=-21.7230
The code #5203=0(CLEAR COMMON Z) is an important safety feature that you should include in all probe programs. If the operator had put an offset in the Z axis common work shift and then runs the probe, the offset is added to the coordinate system and the probe will error. However, if the operator notices the offset, presses Slide Hold, clears the offset and then presses Cycle Start the machine will rapid the amount of the offset and wont be in protect position mode. In any event, this one line of code will prevent wasted time.
You will have to use values that fit the location of your fixture. Presetting the coordinate system like this removes the operator from the setup and eliminates the risk of a crash and the lost time indicating the fixture. The probe is tool 19 in this machine. You'll have to edit the tool change to fit your particular machine.
Here's the program:
%
O0621
(CALIBRATE PROBE STYLUS)
(BORING HEAD IS USED)
(TO ESTABLISH AN EXACT)
(X0Y0 BEFORE CALIBRATING)
G91G30Z0
G91G30Y0
T19T0M06
#5221=-9.1607(SET G54 X0)
#5222=-6.8235(SET G54 Y0)
#5223=-21.7230(SET G54 Z0)
#5203=0(CLEAR COMMON Z)
G0G90G54X1.4Y0
G65P9810Z1.F100.
G65P9811Z0S1(UPDATE G54 Z0)
G54
G65P9810X0Y0
G65P9810Z-.25
G65P9814D1.5S1
G91G30Z0
G91G30Y0
M01
N2(BORING HEAD)
G91G30Z0
G91G30Y0
T1T19M06
S1500M04
G0G90G54G95X0Y0
G0Z1.0M08
G89Z-.6R.1F.004
G91G30Z0M9
G91G30Y0
M00
(BLOW OFF CHIPS)
N3(PROBE)
G91G30Z0
G91G30Y0
T30T0M06
G0G90G54G94X0Y0
G65P9810Z-.25F100.0
G65P9802D1.5
G65P9810Z2.F100.
G65P9810X-2.775Y0F200.0
G65P9810Z-.55F100.0
G65P9804D1.0000
G65P9814D1.000
G65P9810Z2.F200.0
G91G30Z0
G91G30Y0
T01T0M06
M30
%
Clearing Common Work Shift Offsets before Probing (11/28/97)
Have you ever been called to the shop to troubleshoot a probe routine only to find out the operator had put an offset in the Z axis Common Work Shift when he proofed the machining program and forgot to remove it? You can add one line of code in your probe programs to prevent this problem.
The code #5203=0(CLEAR COMMON Z) is an important safety feature that you should include in all probe programs. If the operator had put an offset in the Z axis Common Work Shift and then runs the probe, the offset is added to the coordinate system and the probe will probably error because it will miss the part.
However, if the operator notices the offset, presses Slide Hold, clears the offset and then presses Cycle Start the machine will rapid the amount of the offset and wont be in protected positioning mode. In any event, this one line of code will prevent wasted time.
To use this tip insert #5203=0(CLEAR COMMON Z) before calling G54 and positioning the probe to the part. Also, don't put this code in the machining program. If the operator expects the tool to position above the part and you have cancelled his Z axis Common Offset a crash can occur.
Using a probe to verify that a tilting table is at 90 degrees (12/23/97)
If you have a CNC tilting table on your mill you have probably overloaded it and caused it to move off location. This macro uses your spindle mounted probe to verify/set the table to 90 degrees. This macro verifies that the current G55 X, Y and Z values are appropriate before probing. This is done to prevent damage to the probe if the coordinate system is set wrong. You will need to modify the values in the macro to fit your machine's configuration but the effort is worth it if it prevents one crash of the probe.
For example:
IF[ABS[#5241+32.984]GT.2]GOTO997 checks to see if G55 X is within .2 of 32.984 which is the X center of the tilting table. If the coordinate system has been changed by more than .2, the macro will jump to an error message. Change 32.984 to match the table on your machine. T30 is the tool number of the probe, modify it to fit your application.
This table has a rotary and a tilt axis and the tilt axis is programmed as the B or 5th axis. The macro uses #5245=#5245-.5 to force a .5 degree error in the table's tilting axis. This is so that I'm not doing trig on very small values. Most machine control's recommend against using trig functions on very small values. In this example, Z zero is the center of rotation of the table and the probe uses Z values that are 2" apart. This program typically sets the table to within a couple tenths in 2 inches.
%
O606
(THIS PROGRAM CHECKS ROTARY AT 90 DEG.)
G90 G40 G80 G17 G95
G91 G30 Z0.
G30 X0. Y0.
G90 G00 G55 B0.0
G90T30T0M6
IF[ABS[#5241+32.984]GT.2]GOTO997
IF[ABS[#5242+8.760]GT.2]GOTO998
IF[ABS[#5243+21.4967]GT.2]GOTO999
(FORCE .5 DEGREE OF ERROR IN B)
#5245=#5245-.5
#5201=0(CLEAR COMMON X)
#5202=0(CLEAR COMMON Y)
#5203=0(CLEAR COMMON Z)
(X4.332 IS FACE OF ROTARY)
G0G90G94G55X6.432A0B90.
G0Y0
G65P9810Z7.630F200.
G65P9810X4.582F200.
G65P9811X4.332Q.25
#100=#135
G65P9810Z5.630F100.
G65P9811X4.332Q.25
#101=ATAN[[#100-#135]/2]
(#101 IS THE ERROR VALUE IN B)
#5245=#5245-#101
G91G30Z0
G91G30X0Y0
GOTO1000
N997#3000=1(G55 X SET WRONG)
N998#3000=1(G55 Y SET WRONG)
N999#3000=1(G55 Z SET WRONG)
N1000M30
%