Centroid CNC control sales, service, training and support
Centroid controls use Fanuc-style G codes. They are quite permissive regarding formatting details. In general, a Fanuc 0T post processor with basic functions will work fine.
There is no difference among the different model numbers of the Centroid T-Series controls. The same post processor will work for a T15, T39, T400, or any other control in the series.
There have been minor differences with increasing software versions over the years. In general these changes have been to make the G code interpreter more permissive.
In the information which follows, "optional" means just that: permitted, but not required. Therefore if you are modifying an existing post processor, don't waste time and effort adding or removing such features.
See the Manual for syntax details. CNC program codes are covered in Chapters 10 - 13.
Canned drilling, tapping and boring cycles (G83 - G85) are available.
Stock removal cycles (G70 - G72) are available, but do not conform to Fanuc standards. You will be better off posting long-hand codes for repetitive stock removal.
Single closed-circuit turning, threading and facing cycles (G90, G92, G94) are available.
Multi-pass threading with single-edge cutting and constant chip load (G76) is available.
Arcs may be specified either by center (I and K values) or by radius (R value). Radius values are preferred if you will be using tool nose radius compensation (G41/G42) as they are not affected by roundoff errors as much as center values are.
The I value, for an X axis arc center, is a Diameter amount.
I and K values for the arc center are always incremental from the arc start point.
R values, specifying arc radius, are signed. A positive R will yield an arc less than or equal to 180° (the short way). A negative R will yield at arc greater than or equal to 180° (the long way). On a lathe, there is no need for arcs exceeding 180°, so R should always be positive.
In general, program storage capacity and memory space are not an issue on Centroid controls, so it is better to post out CNC programs long-hand rather than to use subprograms.
If you wish to include G code subprograms and calls in the program file, you must number the subprograms in the range 9100 - 9999, and you must include the subprogram definition (O9xxx through M99) prior to any call to that subprogram.
O9123 G1 F.005 X1.0 X0.8 W-0.1 G2 W-0.2 R0.1414 G1 X1.0 W-0.1 G0 X1.1 M99 T0101 G97 M3 S1200 M8 G0 X1.1 Z.1 G96 S350 G0 Z-0.5 M98 P9123 G0 Z-1.0 M98 P9123 G0 Z-1.5 M98 P9123 G0 Z0.1 M5 M9 G28
In general, Centroid controls do not require the traditional "safety block" at the beginning of a program. The following modes are automatically reset at the beginning of every program cycle:
The following codes do remain active (modal) between cycles:
Even so, these codes generally do not need to be reset in a safety block at the beginning of a program; just set to new values when needed.
There should be no coordinate-setting codes (i.e. G50 X_ Z_) in the CNC program. The operator will set the work coordinate system (fixture offsets) using the control's Part Setup screen before he starts the job running.
The comment found on the first line of programs posted from Intercon, which specifies "ICN_PATH = somefilepath.LTH" is intended for Intercon, to help locate the conversational program file from which the G codes were generated. That comment need not, and should not, be duplicated in CAD/CAM post processors.
You can move both axes to a safe position (home or tool change position) using G28. G28 will move both axes to whatever position is specified for Return Point #1 (G28), referenced in Machine Coordinates on the WCS Tables under Part Setup.
G30 may be used to move to additional reference points. However, a postprocessor should generally assume that G28 is the desired position for tool changes and end-of-job clearance.
Tool nose radius compensation (G41/G42) must be cancelled (with G40) before using G28 or G30.
It is not necessary to cancel tool length compensation (e.g. change from T0101 to T0100) before moving to home.
No special M code or other character is required to mark the end of a CNC program. When the control reaches the end of the file, the program cycle ends.
You may optionally include an M30 code. Most controls are configured to simply ignore M30 (it is a valid code which does nothing). Some users will install a custom M30 which performs some housekeeping tasks.
M2 and M102 request automatic restart of the program cycle, and so should be avoided unless such continuous looping is specifically required.
No post processor changes are strictly necessary in order to support machines with automatic tool changers. Just change the T code to change tools, as always.
On a machine with manual tool changing, the control will display a prompt ("Insert tool and press Cycle Start"), and wait for the Cycle Start key.
On a machine with automatic tool changing, the control will do whatever is required by the tool changer, as directed by its PLC and macro programming.
CNC Services Northwest Home
Copyright © 2010 Marc Leonard
Last updated 16-Jun-2010 MBL