CNC Services Northwest

Centroid CNC control sales, service, training and support

Setting Parameter 2 for CAD/CAM Compatibility

If you are using a typical Fanuc postprocessor, you may need to configure the Centroid control so that its canned drilling cycles will drill a hole any time Z is given, even if X and Y are omitted.

To do so, set Centroid Machine Parameter #2 to a value of 2.0.

This feature works with any version of Centroid's CNC10 Linux-based control software, and with version 7.06 or higher of Centroid's CNC7 DOS-based control software.

To set Parameter 2:

Press F1/Setup
Press F3/Config
Enter the configuration password ("137")
Press F3/Param
Arrow down to Parameter 2
Enter the desired value (e.g. 2.0)
Press F10/Save
Press ESC twice to return to the main screen

Note that Parameter 2 is a bit-mapped parameter which also controls some additional G code interpretation options. To determine the correct value for Parameter 2, you add up the values for the options you want, and enter the sum. The options are as follows:

Flag Value Meaning (include value if:)

Absolute arc centers 1.0000 You want I/J/K arc centers to be absolute instead of incremental, when in G90 mode

Drill with Z alone 2.0000 You want canned drilling cycles to drill in the current X/Y location when only Z is specified

Dwell times in milliseconds 4.0000 You want to specify dwell times (G4, G82, G84 etc.) in milliseconds instead of seconds

Slave rotary feedrate to linear movement 8.0000 You want the rotary axis or axes to move as fast as necessary to keep up with linear feedrates (in/min)

Scale/rotation center at current position 16.0000 You want the default center point for G51 scaling and G68 rotation to be the present position, instead of X0 Y0 Z0

Flag	Value	Meaning (include value if:)
Absolute arc centers	1.0000	You want I/J/K arc centers to be absolute instead of incremental, when in G90 mode
Drill with Z alone	2.0000	You want canned drilling cycles to drill in the current X/Y location when only Z is specified
Dwell times in milliseconds	4.0000	You want to specify dwell times (G4, G82, G84 etc.) in milliseconds instead of seconds
Slave rotary feedrate to linear movement	8.0000	You want the rotary axis or axes to move as fast as necessary to keep up with linear feedrates (in/min)
Scale/rotation center at current position	16.0000	You want the default center point for G51 scaling and G68 rotation to be the present position, instead of X0 Y0 Z0

See the M-Series Operator's Manual Chapter 14 (Configuration) for additional information on this parameter and its options.

See M-Series Operator's Manual Chapter 12 (G Codes) for additional information on drilling cycles, arc centers, dwell times, scaling and rotation.

CNC Services Northwest Home