Table of Contents

Enum NcFlag

Namespace
HiUniNc.Numerical
Assembly
HiUniNc.dll

NC Flag.

public enum NcFlag
Extension Methods

Fields

[NcLifeCycle(NcLifeCycleMode.Modal)] Cooling = 66

Cooling enabled.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup01))] G00 = 0

Group01. Rapid move.

Although fanuc document says that G00 is an one shot command, (I think it may send warning if use G0 as modal.) set it to modal may fit other CNC controller and is much conservative from collision.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup01))] G01 = 1

Group01. Move by feedrate.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup01))] G02 = 2

Group01. Move in CW arc.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup01))] G03 = 3

Group01. Move in CCW arc.

[NcLifeCycle(NcLifeCycleMode.OneShot)] [NcGroup(typeof(NcGroup00))] G04 = 6

Group00. Dwell.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup21))] [NcName("G12.1")] G12p1 = 7

Group21. Polar coordinate interpolation mode ON. Use G13p1 to turn off polar coordinate interpolation mode.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup21))] [NcName("G13.1")] G13p1 = 8

Group21. Polar coordinate interpolation mode OFF. Use G12p1 to turn on polar coordinate interpolation mode.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup02))] G17 = 9

Group02. XY plane selection.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup02))] G18 = 10

Group02. ZX plane selection.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup02))] G19 = 11

Group02. YZ plane selection.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup06))] G21 = 12

Group06. Input in mm. For Fanuc specification. RS274D specification is G71.

[NcLifeCycle(NcLifeCycleMode.OneShot)] [NcGroup(typeof(NcGroup01))] G28 = 13

Group01. Automatic reference position return.

Positioning to the intermediate or reference positions are performed at the rapid traverse rate of each axis. Therefore, for safety, the compensation functions, such as the tool radius compensation and tool length compensation, should be cancelled before executing this command. The coordinates for the intermediate position are stored in the CNC for the axes for which a value is specified in a G28 block. For the other axes, the previously specified coordinates are used.

G28 Fanuc parameters Nos. 1240 to 1243.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup07))] G40 = 14

Group07. Cancel radius compensation. See G41 and G42 for left and right compensation.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup07))] G41 = 15

Group07. Tool radius/tool nose radius compensation. Left compensation: the updated tool tip location is at +y direction compensation from tool running direction. See G40 to cancel compensation and G42 for right compensation.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup07))] G42 = 16

Group07. Tool radius/tool nose radius compensation. Right compensation: the updated tool tip location is at -y direction compensation from tool running direction. See G40 to cancel compensation and G41 for left compensation.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup08))] G43 = 17

Group08 Positive height compensation.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup08))] [NcName("G43.4")] G43p4 = 18

Group08 G43.4: start RTCP (Rotational Tool Center Point).

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup08))] G44 = 19

Group08 Negative height compensation.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup08))] G49 = 20

Group08. Cancel height compensation.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup00))] G52 = 25

Group00. Local coordinate system setting. It can be cancelled by G52X0Y0Z0 or M30.

[NcLifeCycle(NcLifeCycleMode.OneShot)] [NcGroup(typeof(NcGroup00))] G53 = 26

Group00. Machine coordinate system setting.

When an incremental command is specified, the G53 command is ignored.

[NcLifeCycle(NcLifeCycleMode.OneShot)] [NcName("G53P1")] G53WithP1Flag = 27

Enables the high-speed G53 function. P1 flag accompanies with G53.

[NcLifeCycle(NcLifeCycleMode.OneShot)] [NcGroup(typeof(NcGroup00))] [NcName("G53.1")] G53p1 = 29

Group00. Tool axis direction control.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup14))] G54Series = 30

Group14. Coordinate settings.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup16))] G68 = 35

Group16. 3-dimensional coordinate system conversion. run a pattern of operations in a rotated angle.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup16))] [NcName("G68.2")] G68p2 = 36

Group16. Tilted working plane command.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup16))] G69 = 37

Group16. Coordinate system rotation cancel or 3-dimensional coordinate conversion mode off

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup06))] G71 = 39

Group06. Input in mm. For RS274D specification. Fanuc specification is G21.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup09))] G80 = 40

Group09. Canned cycle cancel. Electronic gear box : synchronization cancellation. See G81, G82, G83, G85, G86 for available canned cycles.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup09))] G81 = 41

Group09. Drilling cycle or spot boring cycle. Electronic gear box : synchronization start. The same parsing behavior group: G81,G85,G86.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup09))] G82 = 42

Group09. Drilling cycle or spot boring cycle with bottom staying time.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup09))] G83 = 43

Group09. Drilling cycle or spot boring cycle. drilling cycle in form of pecking.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup09))] G85 = 44

Group09. Drilling cycle or spot boring cycle. Electronic gear box : synchronization start. The same parsing behavior group: G81,G85,G86.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup09))] G86 = 45

Group09. Drilling cycle or spot boring cycle. Electronic gear box : synchronization start. The same parsing behavior group: G81,G85,G86.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup03))] G90 = 46

Group03. Absolute coordinate system.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup03))] G91 = 47

Group03. Relative coordinate system.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup05))] G94 = 48

Group05. Use F as mm/min.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup10))] G98 = 49

Group10. Canned cycle : return to initial level. See G99 for R point level return.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup10))] G99 = 50

Group10. Canned cycle : return to R point level. See G98 for initial level return.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup14))] [NcName("DATUM")] HeidenhainDatum = 34

Group14. Heidenhain flag. Coordinate settings for CYCL DEF 7 and CYCL DEF 247.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcName("FMAX")] HeidenhainFMax = 51

Heidenhain flag. Flag Name 'FMAX'.

[NcLifeCycle(NcLifeCycleMode.OneShot)] [NcGroup(typeof(NcGroup01))] [NcName("L")] HeidenhainL = 4

Group01. Heidenhain flag. Straight linear motion.

[NcLifeCycle(NcLifeCycleMode.OneShot)] [NcGroup(typeof(NcGroup01))] [NcName("LN")] HeidenhainLN = 5

Group01. Heidenhain flag. Nonlinear motion.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroupHeidenhainM107M108))] [NcName("M107")] HeidenhainM107 = 73

Heidenhain flag. Enable Suppress error message for replacement tools with oversize.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroupHeidenhainM107M108))] [NcName("M108")] HeidenhainM108 = 74

Heidenhain flag. Reset M107. disable Suppress error message for replacement tools with oversize.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroupHeidenhainShortestRotaryPath))] [NcName("M126")] HeidenhainM126 = 75

NcGroup.HeidenhainShortestRotaryPath. Heidenhain flag. Shortest rotation for commands of ABC axise. The M126 will be canceled automatically at the end of the program. For Heidenhain.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroupHeidenhainShortestRotaryPath))] [NcName("M127")] HeidenhainM127 = 76

NcGroup.HeidenhainShortestRotaryPath. Heidenhain flag. Cancel HeidenhainM126, i.e. disable shortest rotation for ABC axises. For Heidenhain.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup08))] [NcName("M128")] HeidenhainM128 = 23

Group08. Heidenhain flag. M128: start RTCP (Rotational Tool Center Point).

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup08))] [NcName("M129")] HeidenhainM129 = 24

Group08. Heidenhain flag. M129: cancel RTCP (Rotational Tool Center Point).

[NcLifeCycle(NcLifeCycleMode.OneShot)] [NcName("M140")] HeidenhainM140 = 77

From TNC640 documentation: Retraction from the contour in the tool-axis direction: M140. If you do not enter a feed rate, the TNC moves the tool along the entered path at rapid traverse. M140 is also effective if the tilted-working-plane function is active. On machines with swivel heads, the TNC then moves the tool in the tilted coordinate system. With M140 MB MAX you can only retract in the positive direction. Always define a TOOL CALL with a tool axis before entering M140, otherwise the direction of traverse is not defined.

[NcLifeCycle(NcLifeCycleMode.OneShot)] [NcName("M140")] HeidenhainM140InitiativeF = 78

Feedrate on HeidenhainM140. The TNC640 documentation does not show that the Feedrate on M140 is one shot or modal. HiNC assumes Feedrate on M140 is one shot feedrate with M140 command.

[NcLifeCycle(NcLifeCycleMode.OneShot)] [NcName("M91")] HeidenhainM91 = 72

Heidenhain flag. If you want the coordinates in a positioning block to be referenced to the machine datum, end the block with M91.

[NcLifeCycle(NcLifeCycleMode.OneShot)] [NcName("MOVE")] HeidenhainMove = 71
[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroupHeidenhainPlane))] [NcName("PLANE RESET")] HeidenhainPlaneReset = 67

Heidenhain Plane command is exclusive

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroupHeidenhainPlane))] [NcName("PLANE SPATIAL")] HeidenhainPlaneSpatial = 68

Heidenhain Plane command is exclusive

[NcLifeCycle(NcLifeCycleMode.OneShot)] [NcName("STAY")] HeidenhainStay = 69
[NcLifeCycle(NcLifeCycleMode.OneShot)] [NcName("TOOL CALL")] HeidenhainToolCall = 56

Heidenhain flag. Tool call. Flag Name 'TOOL CALL'.

[NcLifeCycle(NcLifeCycleMode.OneShot)] [NcName("TOOL DEF")] HeidenhainToolDef = 57

Heidenhain flag. tool definition. Flag Name 'TOOL DEF'.

[NcLifeCycle(NcLifeCycleMode.OneShot)] [NcName("TURN")] HeidenhainTurn = 70
[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup14))] [NcName("CYCL DEF 247")] Heidenhain_CYCL_DEF_247 = 32

Group14. Heidenhain flag. With the DATUM SETTING cycle you can activate as the new datum a preset defined in a preset table. After a DATUM SETTING cycle definition, all of the coordinate inputs and datum shifts(absolute and incremental) are referenced to the new preset.

When activating a datum from the preset table, the TNC resets the datum shift, mirroring, rotation, scaling factor and axis-specific scaling factor. If you activate preset number 0 (line 0), then you activate the datum that you last set in the Manual Operation or El. Handwheel operating mode.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup14))] [NcName("CYCL DEF 7")] Heidenhain_CYCL_DEF_7 = 31

Group14. Heidenhain flag. For shifting contours directly within the program or from datum tables.

[NcLifeCycle(NcLifeCycleMode.OneShot)] M03 = 52

Activate spindle rotation in CW.

[NcLifeCycle(NcLifeCycleMode.OneShot)] M04 = 53

Activate spindle rotation in CCW.

[NcLifeCycle(NcLifeCycleMode.OneShot)] M05 = 54

deactivate spindle rotation.

[NcLifeCycle(NcLifeCycleMode.OneShot)] M06 = 55

Tool changed.

[NcLifeCycle(NcLifeCycleMode.OneShot)] M08 = 58

Start cooling.

[NcLifeCycle(NcLifeCycleMode.OneShot)] M09 = 59

Stop cooling.

[NcLifeCycle(NcLifeCycleMode.OneShot)] M13 = 60
[NcLifeCycle(NcLifeCycleMode.OneShot)] M14 = 61
[NcLifeCycle(NcLifeCycleMode.Modal)] M30 = 62

Program end.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup16))] [NcName("CYCLE800")] SiemensCycle800 = 38

Group16. Siemens flag. Tilted working plane command.

CYCLE800() cancels the previous transformation.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup14))] [NcName("G500")] SiemensG500 = 33

Group14. Siemens command. Deactivation of the current settable zero offset. G500指令在没有赋值的时候为机床坐标系，可以把机床从工件坐标系转换到机床坐标系

[NcLifeCycle(NcLifeCycleMode.OneShot)] [NcName("SUPA")] SiemensSupa = 28

Group00. Siemens command. G53: G53 suppresses the settable zero offset and the programmable zero offset non-modally. G153: G153 has the same effect as G53 and also suppresses the entire basic frame. SUPA: SUPA has the same effect as G153 and also suppresses: Handwheel offsets (DRF) Overlaid movements External zero offset PRESET offset

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup08))] [NcName("TRAFOOF")] SiemensTrafoof = 21

Group08. Siemens flag. Disable RTCP (Rotational Tool Center Point) (=Tool Center Point Management, TCPM).

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroup08))] [NcName("TRAORI")] SiemensTraori = 22

Group08. Siemens flag. Enable RTCP (Rotational Tool Center Point) (=Tool Center Point Management, TCPM).

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroupSpindleRotation))] SpindleCcw = 65

NcGroupSpindleRotation. Rotate spindle counter-clockwise (CCW). See SpindleStop to stop rotation and SpindleCw for clockwise rotation.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroupSpindleRotation))] SpindleCw = 64

NcGroupSpindleRotation. Rotate spindle clockwise (CW). See SpindleStop to stop rotation and SpindleCcw for counter-clockwise rotation.

[NcLifeCycle(NcLifeCycleMode.Modal)] [NcGroup(typeof(NcGroupSpindleRotation))] SpindleStop = 63

NcGroupSpindleRotation. Stop spindle rotation. See SpindleCw and SpindleCcw for clockwise and counter-clockwise rotation.