Path functions
Straight line
Cartesian coordinates
With the G00 and G01 NC functions, you program a straight movement in rapid traverse or with a machining feed rate in any desired direction.
N110 G00 Z+100 M3 | ; Straight line at rapid traverse |
N120 G01 X+20 Y-15 F200 | ; Straight line at machining feed rate |
If the feed rate was programmed using a numerical value, it is active only up to the NC block in which a new feed rate is programmed. G00 is active only for the NC block in which it was programmed. When the NC block programmed with G00 has been executed, the feed rate programmed most recently with a numerical value becomes active again.
Make sure to program rapid traverse movements exclusively with the G00 NC function instead of very high numerical values. This is the only way to ensure that rapid traverse is active on a block-by-block basis and that you can control rapid traverse independently of the machining feed rate.
G00 and G01 correspond to the L Klartext syntax with FMAX and F.
Polar coordinates
With the G10 and G11 NC functions, you program a straight movement in rapid traverse or with a machining feed rate in any desired direction.
N110 I+0 J+0 | ; Pole |
N120 G10 R+10 H+10 | ; Straight line at rapid traverse |
N130 G11 R+50 H+50 F200 | ; Straight line at machining feed rate |
The polar coordinate radius R corresponds to the PR Klartext syntax.
The polar coordinate angle H corresponds to the PA Klartext syntax.
G10 and G11 correspond to the LP Klartext syntax with FMAX and F.
Chamfer
With the G24 NC function, you can insert a chamfer between two straight lines. The chamfer size references the point of intersection you are programming using the straight line.
N110 G01 X+40 Y+5 | ; Straight line at machining feed rate |
N120 G24 R12 | ; Chamfer at machining feed rate |
N130 G01 X+5 Y+0 | ; Straight line at machining feed rate |
The value following the R syntax element corresponds to the chamfer size.
G24 corresponds to the CHF Klartext syntax.
Rounding arc
With the G25 NC function, you can insert a rounding arc between two straight lines. The rounding arc references the point of intersection you are programming using the straight line.
N110 G01 X+40 Y+25 | ; Straight line at machining feed rate |
N120 G25 R5 | ; Rounding arc at machining feed rate |
N130 G01 X+10 Y+5 | ; Straight line at machining feed rate |
G25 corresponds to the RND Klartext syntax.
The value following the R syntax element corresponds to the radius of the rounding arc.
Circle center
Cartesian coordinates
With the I, J, and K or G29 NC functions, you define the circle center.
N110 I+25 J+25 | ; Circle center in the XY plane |
N110 G00 X+25 Y+25 | ; Pre-positioning on a straight line |
N120 G29 | ; Circle center at the last position |
- I, J, and K
The circle center is defined in this NC block.
- G29
The control assumes the most recently programmed position as the circle center.
I, J, and K or G29 correspond to the CC Klartext syntax with or without axis values.
With I and J, you define the circle center in the X and Y axes. In order to define the Z axis, program K.
Polar coordinates
With the I, J, and K or G29 NC functions, you define a pole. All polar coordinates reference the pole.
N110 I+25 J+25 | ; Pole |
- I, J, and K
The pole is defined in this NC block.
- G29
The control takes over the most recently programmed position as the pole.
I, J, and K or G29 correspond to the CC Klartext syntax with or without axis values.
Circular arc with center
Cartesian coordinates
With the G02, G03, and G05 NC functions, you program a circular path around a circle center.
N110 I+25 J+25 | ; Circle center |
N120 G03 X+45 Y+25 | ; Circular path around circle center |
- G02
Circular path in clockwise direction, corresponds to the C Klartext syntax with DR–.
- G03
Circular path in counterclockwise direction, corresponds to the C Klartext syntax with DR+.
- G05
Circular path without direction of rotation, corresponds to the C Klartext syntax without DR.
The control uses the most recently programmed direction of rotation.
When you program a radius R, there is no need to define a circle center.
Polar coordinates
With the G12, G13, and G15 NC functions, you program a circular path around a defined pole.
N110 I+25 J+25 | ; Pole |
N120 G13 H+180 | ; Circular path around pole |
- G12
Circular path in clockwise direction, corresponds to the CP Klartext syntax with DR–.
- G13
Circular path in counterclockwise direction, corresponds to the CP Klartext syntax with DR+.
- G15
Circular path without direction of rotation; corresponds to the CP Klartext syntax without DR.
The control uses the most recently programmed direction of rotation.
The polar coordinate angle H corresponds to the PA Klartext syntax.
Circular path with a defined radius
Cartesian coordinates
With the G02, G03, and G05 NC functions, you program a circular path with a defined radius. If you are programming a radius, no circle center is required.
N110 G03 X+70 Y+40 R+20 | ; Circular path with a defined radius |
- G02
Circular path in clockwise direction, corresponds to the CR Klartext syntax with DR–.
- G03
Circular path in counterclockwise direction, corresponds to the CR Klartext syntax with DR+.
- G05
Circular path without direction of rotation; corresponds to the CR Klartext syntax without DR.
The control uses the most recently programmed direction of rotation.
Circular arc with a tangential transition
Cartesian coordinates
Polar coordinates
With the G16 NC function, you program a circular path with a tangential transition to the previous path function.
N110 G01 G42 X+0 Y+35 F300 | ; Straight line |
N120 I+40 J+35 | ; Pole |
N130 G16 R+25 H+120 | ; Circular path with tangential transition |
The polar coordinate radius R corresponds to the PR Klartext syntax.
The polar coordinate angle H corresponds to the PA Klartext syntax.
G16 corresponds to the CTP Klartext syntax.
Contour approach and departure
With the G26 and G27 NC functions, you can approach or depart the contour smoothly using a circle segment.
N110 G01 G40 G90 X-30 Y+50 | ; Starting point |
N120 G01 G41 X+0 Y+50 F350 | ; First contour point |
N130 G26 R5 | ; Tangential approach |
* - ... | |
N210 G27 R5 | ; Tangential exit |
N220 G00 G40 X-30 Y+50 | ; End point |
HEIDENHAIN recommends the use of the more powerful APPR and DEP NC functions. In some cases, these NC functions combine multiple NC blocks for approaching and departing the contour.
G41 and G42 correspond to the RL and RR Klartext syntax.
Approach and departure functions with Cartesian coordinates
You can also use polar coordinates when programming the APPR and DEP NC functions.