6.5 Path Contours—Polar
Coordinates
Overview of path functions with polar coordinates
With polar coordinates you can define a position in terms of its angle H and its distance R relative to a previously defined pole I, J (see
“Definition of pole and angle reference axis,” page 66).
Polar coordinates are useful with:
nPositions on circular arcs
nWorkpiece drawing dimensions in degrees, e.g. bolt hole circles
Zero point for polar coordinates: pole I, J
You can set the pole I, J at any point in the machining program, before indicating points in polar coordinates. Set the pole in the same way as you would program the circle center.
Programming
U U U
UEnter Cartesian coordinates for the pole, or if you want to use the last programmed position, enter G29. Before programming polar coordinates, define the pole. You can only define the pole in Cartesian coordinates. The pole remains in effect until you define a new pole.
Tool movement Function Required input
Straight line at feed rate Straight line at rapid traverse
G10 G11
Polar radius, polar angle of the straight-line end point Circular path in clockwise direction
Circular path in counterclockwise direction
G12 G13
Polar angle of the circle end point
Circular path corresponding to active direction of rotation
G15 Polar angle of the circle end point Circular arc with tangential connection to the
preceding contour element
G16 Polar radius, polar angle of the arc end point
Y
Y=J
6.5 P a th Cont ours—P olar Coor dinat e s Straight line at rapid traverse G10 Straight line with feed rate G11 F . . .
The tool moves in a straight line from its current position to the straight-line end point. The starting point is the end point of the preceding block.
Programming
UU
UUPolar coordinates radius R: Enter distance from the straight line end point to the pole I, J
UU
UUPolar-coordinates angle H: Angular position of the straight-line end point between -360° and +360°
The sign of H depends on the angle reference axis:
nAngle from angle reference axis to R is counterclockwise: H >0 nAngle from angle reference axis to R is clockwise: H <0 Example NC blocks
Circular path G12/G13/G15 around pole I, J
The polar coordinate radius R is also the radius of the arc. It is defined by the distance from the starting point to the pole I, J. The last programmed tool position before the G12, G13 or G15 block is the starting point of the arc.
Direction
nIn clockwise direction: G12 nIn counterclockwise direction: G13
nWithout programmed direction: G15. The TNC traverses the circular arc with the last programmed direction of rotation.
Programming
U U U
UPolar-coordinates angle H: Angular position of the arc end point between -5400° and +5400°
Example NC blocks
6.5 P a th Cont ours—P olar Coor dinat e s
Circular arc with tangential connection
The tool moves on a circular path, starting tangentially from a preceding contour element.
Programming
UU
UUPolar coordinates radius R: Distance from the arc end point to the pole I, J
UU
UUPolar coordinates angle H: Angular position of the arc end point
Example NC blocks
Helical interpolation
A helix is a combination of a circular movement in a main plane and a linear movement perpendicular to this plane.
A helix is programmed only in polar coordinates.
Application
nLarge-diameter internal and external threads nLubrication grooves
Calculating the helix
To program a helix, you must enter the total angle through which the tool is to move on the helix in incremental dimensions, and the total height of the helix.
For calculating a helix that is to be cut in an upward direction, you need N120 I+40 J+35 *
N130 G01 G42 X+0 Y+35 F250 M3 * N140 G11 R+25 H+120 *
N150 G16 R+30 H+30 * N160 G01 Y+0 *
The pole is not the center of the contour arc!
X
6.5 P a th Cont ours—P olar Coor dinat e s
Shape of the helixThe table below illustrates in which way the shape of the helix is determined by the work direction, direction of rotation and radius compensation.
Programming a helix
UU
UUPolar coordinates angle H: Enter the total angle of tool traverse along the helix in incremental dimensions.
After entering the angle, specify the tool axis with an axis selection key.
UU
UUEnter the coordinate for the height of the helix in incremental dimensions.
UU
UUEnter the radius compensation G41/G42 according to the table above.
Example NC blocks: Thread M6 x 1 mm with 5 revolutions Internal thread Work
direction Direction Radius comp.
Always enter the same algebraic sign for the direction of rotation and the incremental total angle G91 H. The tool may otherwise move in a wrong path and damage the contour.
For the total angle G91 H, you can enter a value from –5400° to +5400°. If the thread has more than 15 revolutions, program the helix in a program section repeat (see “Program Section Repeats,” page 374)
N120 I+40 J+25 *
6.5 P a th Cont ours—P olar Coor dinat e s
Example: Linear movement with polar coordinates
%LINEARPO G71 *
N10 G30 G17 X+0 Y+0 Z-20 * Define the workpiece blank N20 G31 G90 X+100 Y+100 Z+0 *
N30 G99 T1 L+0 R+7.5 * Define the tool
N40 T1 G17 S4000 * Tool call
N50 G00 G40 G90 Z+250 * Define the datum for polar coordinates
N60 I+50 J+50 * Retract the tool
N70 G10 R+60 H+180 * Pre-position the tool
N80 G01 Z-5 F1000 M3 * Move to working depth
N90 G11 G41 R+45 H+180 F250 * Approach the contour at point 1
N110 G26 R5 * Approach the contour at point 1
N120 H+120 * Move to point 2
X Y
50 100
50 I,J
5 100
R45 60°
5 1 1
21 31
1 4
51 1
6
6.5 P a th Cont ours—P olar Coor dinat e s
Example: Helix
%HELIX G71 *
N10 G30 G17 X+0 Y+0 Z-20 * Define the workpiece blank N20 G31 G90 X+100 Y+100 Z+0 *
N30 G99 T1 L+0 R+5 * Define the tool
N40 T1 G17 S1400 * Tool call
N50 G00 G40 G90 Z+250 * Retract the tool
N60 X+50 Y+50 * Pre-position the tool
N70 G29 * Transfer the last programmed position as the pole
N80 G01 Z-12.75 F1000 M3 * Move to working depth N90 G11 G41 R+32 H+180 F250 * Approach first contour point
N100 G26 R2 * connection
N110 G13 G91 H+3240 Z+13.5 F200 * Helical interpolation
N120 G27 R2 F500 * Tangential departure
N170 G01 G40 G90 X+50 Y+50 F1000 * Retract in the tool axis, end program N180 G00 Z+250 M2 *
X Y
50
50 I,J
100 100
M64 x 1,5
6.5 P a th Cont ours—P olar Coor dinat e s
N110 G98 L1 * Identify beginning of program section repeat N120 G13 G91 H+360 Z+1.5 F200 * Enter pitch directly as incremental Z value
N130 L1.24 * Program the number of repeats (thread revolutions) N999999 %HELIX G71 *