Preprocessing

G-Code: G40, G41, G42, G43, G50, G51, G52, G60, G61, G70, G71

Function: The commands activate preprocessing modules, such as SMC_SmoothPath, SMC_RoundPath, SMC_AvoidLoop, SMC_ToolCorr, SMC_ToolLengthCorr, and SMC_ToolRadiusCorr.

Tip

If the Show preprocessed path option is selected, then the edited path is visible in the graphical editor.

Syntax

G40
G41 D
G42 D
G50
G51 D
G52 D
G60
G61

G Code Word	Description
`D`	Tool radius or overlay radius for `G51/G52`.

Note

For versions before 4.18.0.0: The angle rounding/smoothing (G51/G52) and tool radius correction (G41/G42) can influence each other because both preprocesses interpret each D word in the G code. For example, if a tool radius correction with radius=1 is active when an angle rounding starts with D=5, then as a result the tool radius correction also uses a radius of 5.

For version 4.18.0.0 and higher: Angle rounding/smoothing (G51/G52) and tool radius correction (G41/G42) can be used simultaneously without affecting each other. The following behavior applies for this.

For tool radius correction (G41/G42): By default, the 'Tool' radius used by SMC_ToolRadiusCorr is 0. If a D word is specified after the G words G41/G42, then the 'Tool' radius is adjusted and taken into account by the function blocks. When no value is specified, the currently set 'Tool' radius is used.
For angle rounding/smoothing (G51/G52): By default, the 'Smooth' radius used by SMC_Round/SmoothPath is 0. If a D word is specified after any G word (except G36/G37/G40/G41/G42) or on its own (for example, N00 D5), then this affects the current 'Smooth' radius and is taken into account by the SMC_Round/SmoothPath function blocks.

Table 47. Commands for tool correction

G Code	Description
`G40`	End of tool radius correction
`G41`	Start of tool radius correction to the left of the workpiece
`G42`	Start of tool radius correction to the right of the workpiece
`G43`	Starts the tool length correction The tool offset to be corrected is specified with the `I, J, K` parameters (for `X, Y, Z`). The tool length correction is deactivated by setting the parameters to zero. After activation or deactivation, ramping in or out is performed. For more details, see: `SMC_ToolLengthCorr` Note: The length of the tool must not change during an active tool radius correction because a jump in the path can result. The tool length correction (G43) works in the online decoder only (not in the CNC editor).

Table 48. Commands for angle rounding and angle smoothing

G Code	Description
`G50`	End of angle rounding and smoothing
`G51`	Start of angle smoothing by means of `SMC_SmoothPath`
`G52`	Start of angle rounding by means of `SMC_RoundPath`
`G70`	End of smoothing of additional axes by means of `SMC_SmoothAddAxes`
`G71`	Start of smoothing of additional axes by means of `SMC_SmoothAddAxes`

Table 49. Commands for loop suppression

G Code	Description
`G60`	End of function for loop suppression
`G61`	Start of function for loop suppression by means of `SMC_AvoidLoop`

Example 39. Example: Angle smoothing

N0 G51 D10 F100
N10 G01 X$g_x$ Y0 F50 E30 E-30
N20 G01 X0 Y$g_y$
N30 G01 X0 Y0
N40 G50