Calls on the set_h.cnc and O8851.cnc macros to measure the height offset for the specified tool, or for the current tool if no tool is specified.
An approximate diameter should be entered in the tool's diameter offset before calling M51. If that diameter is less than 0.400", then length will be measured on centerline, with the spindle stopped. If the preset diameter is 0.400" or more, then length will be measured off-center by the tool radius, and with the spindle turning CCW.
For large drills or ball end mills, the diameter should be preset to zero so that measurement will take place on centerline.
Calls on the set_hd.cnc, O8851.cnc and O8852.cnc macros to measure the height offset and diameter offset for the specified tool, or for the current tool if no tool is specified.
An approximate diameter should be entered in the tool's diameter offset before calling M52. It is used for length measurement as described under the M51 code.
The control also uses the preset diameter in diameter offset measurement: it will add the nominal tool radius when calculating how far to move the Y axis in front and in back of the tool detector, in order to clear before moving in to measure diameter.
For drills and ball end mills larger than about 1/2" (13mm) you will need to call the set_hd.cnc or O8852 macro directly, in order to override the side clearance and Z depth for diameter measurement.
Calls on the chk_brk.cnc macro to check a previously measured tool for breakage.
This routine will rapid up and over the detector; move quickly down to within 1mm of the detector; then move down until the tool touches the detector or reaches a position 0.2mm below the expected contact point. If the tool reaches that position without contact, then it is presumed broken and the CNC program cycle is canceled.
If the tool is okay, then this routine rapids back up, over, and down to the previous location. Most G code modal conditions (coordinate system, feedrate, movement mode, spindle speed) are restored. However, spindle rotation is not restarted, and canned cycles (e.g. drilling, boring, tapping) are not restored. The CNC program will have to repeat the M3 code and, if needed, canned cycle code after calling M53.
Called from M51; see M51 description for details.
If set_h.cnc is to be called directly from a CNC program, it will
need to be called by its full path name. E.g.
G65 "c:\cnc10\set_h.cnc" T10
Called from M52; see M52 description for details.
If set_hd.cnc is to be called directly from a CNC program, it
will need to be called by its full path name. E.g.
G65 "c:\cnc10\set_hd.cnc" T10
SET_HD accepts an optional Z position, to override the default diameter measuring depth; and an optional R distance, to override the default radial clearance when positioning the tool in front and in back of the detector, prior to measuring diameter. These values are needed when measuring larger drills and ball mills.
For example, if you are measuring height and diameter for a 1"
ball end mill, you will want to preset the diameter offset to
zero so that length measurement is done on centerline. But you
would then need to tell SET_HD that it needs at least a half inch
extra clearance to get the tool in front or back of the detector
(remember, SET_HD would otherwise think your 1" diameter tool has
zero diameter). You would also need to tell SET_HD to go down at
least a half inch to get a valid diameter measurement. E.g.
G10 D12 R0 ; preset tool 12 diameter to zero G65 "c:\cnc10\set_hd.cnc" T12 R0.6 Z-0.6 ; measure height and diameter
If you do not override R, then the default radial clearance is 4mm plus half of the tool's preset diameter (leaving approximately 4mm clearance).
If you do not override Z, then the default Z depth for measuring tool diameter is with the tool tip 4mm below the top of the tool detector stylus (i.e. about half way down the side of the stylus).
Called from M53; see M53 description for details.
If chk_brk.cnc is to be called directly from a CNC program, it
will need to be called by its full path name. E.g.
G65 "c:\cnc10\chk_brk.cnc" T10
Called through SET_H and SET_HD macros; may also be called directly with G65.
Called through SET_HD macro; may also be called directly with G65.
Called from other routines, in order to set the following variables
#29 = multiplier to convert millimeters to user units (user units per millimeter)
#31 = multiplier to convert inches to user units (user units per inch)
#33 = multiplier to convert default machine units to user units
If a routine wants to execute a move with a distance or feedrate
known in millimeters, it should multiply by #29. E.g. to move X
incrementally 2mm at 4mm/min:
G1 G91 X[2.0*#29] F[4.0*#29]
If a routine wants to execute a move with a distance or feedrate
known in inches, it should multiply by #31. E.g. to move X
incrementally by the amount stored in variable #152 (which is
always in inches) at 10 in/min:
G1 G91 X[#152*#31] F[10.0*#31]
All the macro files for these services are located in the
/cncroot/c/cnc10 directory, which is displayed in
the Centroid software as c:\cnc10. Files are:
cnc10.m51 cnc10.m52 cnc10.m53 set_h.cnc set_hd.cnc chk_brk.cnc O8799.cnc O8851.cnc O8852.cnc
Diameter measurement depends on a calibrated stylus diameter, stored in static user variable #152. This variable value is saved on the hard drive in the file cnc10m.job, along with other job setup information (current WCS, name of current job, part count, whether machine home is set, etc.). In the unlikely event cnc10m.job is corrupted or deleted, the control will display a warning on startup (e.g. "Error loading job information, using defaults"). In that case all static variables, including #152, will be reset to zero.
You can set #152 using the MDI prompt. To set it to a known
value, enter a simple assignment. E.g.
#152 = 0.5
To change it by some amount, without necessarily knowing its
value, enter an assignment with addition or subtraction. E.g.
#152 = #152 - 0.0015
To display the current value stored in #152, you have to open a
command prompt and use the cnc10conv utility to display the
contents of the cnc10m.job file. When done, use the exit
command to close the command prompt E.g.
Alt-F6 /cncroot/c/cnc10> cnc10conv -dj cnc10conv v. 2.70 - Centroid configuration file utility cnc10 v. 2.70 job info file Last job file: c:\cnc10\ncfiles\test.cnc Part count: 0 Edge Finder Diameter: 0.1239 [...] Saved user variable values: #150 = 0.0000 #151 = 0.0000 #152 = 0.4990 #153 = 0.0000 #154 = 0.0000 [...]/cncroot/c/cnc10> exit
The stylus diameter you store in #152 should always be in inches, even when the control has been changed over to run in millimeters.
To determine the necessary value or adjustment for #152, simply
use M52 or set_hd.cnc to measure the height and diameter of a
tool with a precise known diameter (e.g. a length of drill rod,
which you have confirmed has zero runout in the tool holder).
Compare the resulting diameter stored in the offset library with
the known tool diameter. If the measured diameter is less
than the actual diameter, you need to make #152 smaller by
the amount of the error. If the measured diameter is more
than the actual diameter, you need to make #152 larger by
the amount of the error.