Forming of the toolpath in geometric axes

SetSystemUnits

The method sets the units of measurement of the project.

Input parameter: Units ( TNCSystemMeasure )

smMetrics - metric;
smImperial - inch.

To interpret commands similar to G20, G21 in ISO codes.

SetFeedrateUnits

The method sets the units of measure for the feed.

Input parameter: Units ( TNCFeedrateMeasure )

fmMMPerMinute - mm per minute;
fmInchPerMinute - inches per minute.

To interpret commands similar to the G700, G710 for the Heidenhain rack.

GetSystemUnits

The function returns project units of measurement (TNCSystemMeasure)

GetFeedrateUnits

The function returns the current feed units (TNCFeedrateMeasure)

OutStandardFeed

The method adds to the toolpath the command to change the feed to the standard one.

Input parameter: Feed (TNCFeedType) - feed type:

ff Working - working;ffRapid - rapid;
ffFirst - first;
ffEngage - engage;
ffRetract - retract;
ffPlunge - plunge;
ffFinish - finish;
ffNext - next;
ffReturn - return;
ffApproach - approach.

The feed value for each type is specified in the 'Feed' tab of the operation in CAM system.

To interpret commands similar to G00 (Rapid) / G01 (Working) in ISO codes.

OutFeed

The method adds a feed change command with the specified type and value to the tool path.

Input parameters: Feed (TNCFeedType) - feed type (see OutStandardFeed), Value (number) - feed value, MPM (boolean) - sign of feed units:

True - mm per min. False- mm per turn.

To interpret commands similar to F in ISO codes.

SetCurrentPlane

The method adds a command to change the current plane to the specified one in the tool path.

Input parameter: Plane (TNCPlaneType) - plane type:

ptXY - plane XY;
ptYZ - plane YZ;
ptZX - plane ZX.

To interpret commands similar to G17-G19 in ISO codes.

AddSpindleSpeedOnRPM

The method adds a command to enable the active spindle with a given frequency in revolutions per minute to the tool path. If the spindle is already on, the spindle speed changes to the specified one.

Input parameters: RPM (number) - spindle rotation speed in revolutions per minute; Range (integer) - the number of the spindle's rotation range, Direction (boolean) - the direction of the rotation (True - clockwise CW, False - counterclockwise CCW).

To interpret commands similar to S in ISO codes.

AddSpindleSpeedOnCSS

The method adds a command to enable the active spindle with a constant cutting speed to the tool path. If the spindle is already on, the mode and speed changes to the specified one.

Input parameters: CSS (number) - the value of the constant cutting speed; MaxRPM (number) - the maximum spindle speed; Range(integer) - the number of the spindle's rotation range, Direction (logical) - the direction of the rotation (True - clockwise CW, False - counterclockwise CCW).

To interpret commands similar to the G96 for the Sinumerik rack

AddSpindleOff

The method adds a command to turn off the active spindle to the tool movement path.

There are no input and output parameters.

To interpret commands similar to M05 in ISO codes.

AddSpindleOrient

The method adds to the toolpath the command of the oriented active spindle stop.

Input Parameter: OrientationAngle (number) - the angle of rotation of the spindle.

AddOpStop

The method adds an optional command to the execution of the G-code to the tool path. When an optional stop block is reached, the execution of the program is interrupted only if the corresponding mode is activated in the NC rack. When you turn off this mode, the execution of the program is not interrupted.

There are no input and output parameters.

To interpret commands similar to M01 in ISO codes.

AddCoolant

The method adds a command to enable or disable machine cooling systems to the tool movement path.

Input parameters: OnOff (logical) - True - enable, False - disable; PipeNumber (integer) - The number of the cooling pipe to be turned on (1 - liquid, 2 - fog, 3 - tool).

To interpret commands similar to M08 / M09 in ISO codes.

AddDelay

The method adds to the toolpath the command to pause the program for a specified time.

Input Parameter: Value (number) —During time in seconds.

To interpret commands similar to G04 in ISO codes.

AddLengthCompensation

The method adds a tool length compensation command to the tool path with the specified parameters.

Input parameters: Mode (TNCLengthCompensationMode) - mode:

lcOff - turn off the compensation for the tool length; lcOn - enable positive compensation for the tool length;

lcOnNegative - enable negative compensation for tool length.
OffsetNumber (number) - The number of the length offset.

To interpret commands similar to G43, G44, G49, H in ISO codes.

AddLengthCompensationValue

The method adds a tool length compensation command to the tool path with the specified parameters.

Input parameters: Mode, OffsetNumber (see AddLengthCompensation);

Value (number) is the tool length offset value.

Attention! In the current version, the function works in the same way as AddLengthCompensation, without the possibility of setting a value.

AddLengthCompensationWithSpecifiedAxis

The method adds a tool length compensation command to the tool path with the specified parameters.

Input parameters: Mode, OffsetNumber (see AddLengthCompensation);

SpecifiedAxis (integer) - the number of the axis along which compensation is made for the length.

Attention! In the current version, the function works in the same way as AddLengthCompensation, without the possibility of selecting an axis.

To interpret commands similar to G43 (together with G17-G19) in ISO codes.

AddRadiusCompensation

The method adds a tool radius compensation command to the tool path with the specified parameters.

Input parameters: Mode (TNCRadiusCompensationMode) - mode:

rcOff - turn off tool radius compensation;

rcLeft - enable tool radius compensation to the left;

rcRight - enable tool radius compensation to the right.

OffsetNumber (number) - The number of the length offset.

To interpret commands similar to G41, G42, D in ISO codes.

AddRadiusCompensationValue

The method adds a tool radius compensation command to the tool path with the specified parameters.

Input parameters: Mode, OffsetNumber (see AddRadiusCompensation);

Value (number) is the tool radius compensation value.

Attention! In the current version, the function works in the same way as AddRadiusCompensation, without the possibility of setting a value.

CutTo3d

The method adds a linear tool movement command to the specified point in the tool path.

Input parameter: P (TNC3DPoint) - coordinates of a specified point.

To interpret commands similar to G00/G01 X Y Z A B C in ISO codes .

CutTo5d

The method adds a command of linear movement of the tool to the specified point with the specified direction of tool position in the tool motion path.

Input parameters: P (TNC3DPoint) - coordinates of a specified point. N (TNC3DPoint) - tool normal vector in part coordinate system.

ArcTo2d

The method adds to the tool path of the tool the command to move the tool along the arc of a circle with the specified parameters.

Input parameters: Pe (TNC3DPoint) - the end point of the arc (X, Y, Z); Pc(TNC3DPoint) - coordinate of the arc center (X, Y, Z); Plane ( TNCPlaneType , see SetCurrentPlane ) - arc plane; R (number) is the radius of the arc (the radius is greater than zero, if the rotation is counterclockwise, and the radius is less than zero, if the rotation is clockwise); CanBeFull (boolean) - can be closed.

To interpret commands similar to G02 / G03 X Y Z I J K R in ISO codes.

ArcTo3d

The method adds to the tool path of the tool the command to move the tool along the arc of a circle with the specified parameters.

Input parameters: Pe (TNC3DPoint) - the end point of the arc (X, Y, Z); Pc(TNC3DPoint) - coordinate of the arc center (X, Y, Z); Nc ( TNC3DPoint ) - the normal vector of the plane in which the arc lies; R (number) is the radius of the arc (the radius is greater than zero, if the rotation is counterclockwise, and the radius is less than zero, if the rotation is clockwise); CanBeFull (boolean) - can be closed.

ArcTo5d

The method adds to the tool path of the tool the command to move the tool along the arc of a circle with the specified parameters.

Input parameters: Pe (TNC3DPoint) - the end point of the arc (X, Y, Z); Ne ( TNC3DPoint ) - t ool normal vector in part coordinate system at the end point ; Pc (TNC3DPoint) - coordinate of the arc center (X, Y, Z); Nc ( TNC3DPoint ) - the normal vector of the plane in which the arc lies ; R (number) is the radius of the arc (the radius is greater than zero, if the rotation is counterclockwise, and the radius is less than zero, if the rotation is clockwise); CanBeFull (boolean) - can be closed.

GetLastPosition

The function returns the coordinate of the current tool position the tool normal vector relative to the part coordinate system.

The function is used to get the current position of the tool.

WasAxisMovement

The function returns whether the first move. True - the first move has already been effected, the current position of the tool can be obtained using GetLastPosition . False - movements have not been made yet.

See GetLastPosition

CreateLinearMotionFormer

The function returns the interface of the linear motion generator ( INCT_GeomLinearMotionFormer ). Using the driver in the interpreter simplifies the construction of a linear tool path. Working with the driver is described in the article Linear movements.

No input parameters.

To interpret commands similar to G00/G01 X Y Z A B C in ISO codes.

CreateCircularMotionFormer

The function returns the arc path maker interface ( INCT_CircularMotionFormer ). Using the driver in the interpreter simplifies the construction of the tool path along the arc. Work with the shaper is described in the article Circular movements.

No input parameters.

To interpret commands similar to G02/G03 X Y Z I J K R in ISO codes.

CreateDrillingCycleFormer

Depending on the set parameter, the function returns the interface of the trajectory driver of one of the drilling cycles. Working with shapers is described in the articles Drilling cycle, Drilling cycle with shift, Drilling cycle with chip breaking.

Input parameter: CycleType (TNCDrillingCycleType) - type of cycle.

dctSimple is a simple drilling cycle, in this case the driver that is returned by the function supports only one interface: INCT_DrillingCycleFormer .
dctWithShift - the offset drilling cycle returned by the function, the driver supports two interfaces: INCT_DrillingCycleFormer, INCT_DrillingCycleWithShiftFormer.
dctPeck - drilling cycle with chip breaking, the function returned by the driver: two interfaces: INCT_DrillingCycleFormer, INCT_PeckDrillingCycleFormer.

To interpret commands similar to G73, G74, G76, G80-89 for a Fanuc rack.

CreateLatheCycleFormer

Depending on the set parameter, the function returns the interface of the trajectory driver of one of the turning cycles. Working with formers is described in the articles Turning cycle grooving, Turning cycle threading, Turning machining cycle.

Input parameter: CycleType (TNCLatheCycleType) - type of cycle.

lctGrooving - the turning cycle of grooving, in this case the shaper returned by the function supports one interface: INCT_LatheGroovingCycleFormer .
lctThreadCutting - turning the threading cycle, in this case the shaper returned by the function supports one interface: INCT_LatheThreadCuttingCycleFormer .
lctStockRemoval - turning cycle of rough and finishing contour turning, in this case the shaper returned by the function supports one interface: INCT_LatheStockRemovalCycleFormer .

To interpret commands similar to CYCLE93, CYCLE95, CYCLE97 for the Sinumerik rack.