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

Programming example:
Linear interpolation (G00)
Linear interpolation with G00 is set by setting the machine data 20732 $MC_EXTERN_GO_LINEAR_MODE. Hence all
programmed axes traverse in rapid traverse with linear interpolation and reach their target position simultaneously.
3.2.1.2

Linear interpolation (G01)

With G01 the tool travels on axially parallel, inclined or straight lines arbitrarily positioned in the space. Linear interpolation
permits machining of 3D surfaces, grooves, etc.
Format
G01 X... Z... F... ;
In case of G01 the linear interpolation is executed with the path feed. The axes not specified in the block with G01 are also
not traversed. The linear interpolation is programmed as given in the example 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 (G98, G99) are either in mm or inch.
One F value can be programmed per NC block. The unit of the feedrate is defined via one of the G commands mentioned.
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
If no feed Fxx is programmed in a block with G01 or in the previous blocks, an alarm is given off when a G01 block is
executed.
The end point can be specified either as absolute or incremental. For details see Section "Absolute/incremental
dimensioning (G90, G91) (Page 106)".
Programming and Operating Manual (ISO Turning/Milling)
22
01/2017