Linear Interpolation (G01) - Siemens SINUMERIK 808D Programming And Operating Manual

Note
As in positioning with G00, the axes traverse independently of each other (not interpolated), each axis reaches its end point
at a different time. Hence, one must be very careful in positioning with several axes, so that a tool does not collide with a
workpiece of the tool during the positioning.
Linear interpolation (G00)
Linear interpolation with G00 is defined by setting the machine data 20732 $MC_EXTERN_GO_LINEAR_MODE. Here, all
programmed axes traverse in rapid traverse with linear interpolation and reach their target positions simultaneously.
4.2.1.3

Linear interpolation (G01)

With G01 the tool travels on paraxial, inclined or straight lines arbitrarily positioned in space. Linear interpolation permits
machining of 3D surfaces, grooves, etc.
Format
G01 X... Y... Z... F... ;
In G01, the linear interpolation is executed with the path feed. The axes that are not specified in the block with G01 are not
traversed. The linear interpolation is programmed as in the example given above.
Feed F for path axes
The feedrate is specified under the address F. Depending on the default setting in the machine data, the units of
measurement specified with the G commands (G93, G94, G95) are either in mm or inch.
One F value can be programmed per NC block. The unit of feedrate is defined over one of the mentioned G commands. The
feed F acts only on path axes and remains active until a new feed value is programmed. Separators are permitted after
address F.
Note
An alarm is triggered while executing a G01 block if no feed was programmed in a block with G01 or in the previous blocks.
The end point can be specified either as absolute or as incremental. For more information, refer to Section
"Absolute/incremental dimensioning (G90, G91) (Page 106)".
Linear interpolation:
Programming and Operating Manual (ISO Turning/Milling)
93
01/2017