Siemens CNC Milling | G110-G111-G112 | Polar Coordinates

In this article, we describe how to use polar coordinate function in Siemens CNC controlled milling (machine centre) machines with all details and examples. 

0
716

Polar Coordinate Introduction

In addition to the common specification in Cartesian coordinates (X, Y, Z), the points of a workpiece can be specified using the polar coordinates in Siemens CNC controller.

Polar coordinates are also helpful if a workpiece or a part of it is dimensioned from a central point (pole) with specification of the radius and the angle.

Plane

The polar coordinates refer to the plane activated with G17 to G19. In addition, the third axis standing vertically on this plane can be specified. When doing so, spatial specifications can be programmed as cylinder coordinates.

Polar radius RP=…

The polar radius specifies the distance of the point to the pole. It is stored and must only be written in blocks in which it changes, after changing the pole or when switching the plane.

Polar angle AP=…

The angle is always referred to the horizontal axis (abscissa) of the plane (for example, with G17: X axis). Positive or negative angle specifications are possible.

The polar angle remains stored and must only be written in blocks in which it changes, after changing the pole or when switching the plane.

See the following illustration for polar radius and polar angle with definition of the positive direction in different planes:

You may be interested also:
“Siemens CNC | Inch – Metric Conversation”

G110 – G111 and G112 Code Format

G110 : Pole specification relative to the set point position last programmed (in the plane, e.g. with G17: X/Y)
G111 : Pole specification relative to the origin of the current workpiece coordinate system (in the plane, e.g. with G17: X/Y)
G112 : Pole specification, relative to the last valid pole; preserve plane

Pole Specifications

  • Pole definitions can also be performed using polar coordinates. This makes sense if a pole already exists.
  • If no pole is defined, the origin of the current workpiece coordinate system will act as the pole.

Polar Coordinate Examples

Siemens CNC Polar Coordinate Example – 1

N10 G17 ; X/Y plane
N20 G0 X0 Y0
N30 G111 X20 Y10 ; Pole coordinates in the current workpiece coordinate system
N40 G1 RP=50 AP=30 F1000
N50 G110 X-10 Y20
N60 G1 RP=30 AP=45 F1000
N70 G112 X40 Y20 ; New pole, relative to the last pole as a polar coordinate
N80 G1 RP=30 AP=135 ; Polar coordinate
M30

Traversing with Polar Coordinates

The positions programmed using polar coordinates can also be traversed as positions specified with Cartesian coordinates as follows:

G00 – Linear interpolation with rapid traverse
G01 – Linear interpolation with feedrate
G02 – Circular interpolation CW
G03 – Circular interpolation CCW

 


Need to More?

Our volunteers have worked together and carefully prepared the articles published here in their native language without using machine translation. You can search the entire site for more information on the subject. You can start a discussion on CNCarea.com forums and join us to get support, ask questions, improve a published article or give your opinion.


Previous articleSiemens CNC | G70 and G71 Codes | Inch – Metric Conversation
Next articleSiemens CNC Milling | TRANS and ATRANS | Programmable Work Offset