Programming manual.
CNC 8070
20.
HSC. HIGH SPEED MACHINING.
HSC SURFACE mode. Optimization of surface finish.
·368·
(REF: 1709)
Maximum chordal error allowed.
The E command sets the maximum contouring error allowed between the programmed path
and the resulting path (mm or inches). This command is applied to the first three linear axes
of the channel. Programming it is optional; if not programmed, the CNC assumes as
maximum contouring error the value set in machine parameter HSCROUND.
Maximum angle for square corner.
The CORNER command sets the maximum angle between two paths (between 0º and 180º),
under which the CNC machines in square corner mode. Programming it is optional; if not
programed, the CNC assumes the angle set in machine parameter CORNER.
Maximum error on rotary axes.
The RE command defines the error in all the rotary axes and linear axes (except the first
three axes of the channel). Programming it is optional; if not programmed, the CNC assumes
as maximum error the highest value between machine parameter MAXERROR and the E
command.
Path filter frequency for linear slope.
The SF command allows applying different filters to those set in the machine parameters.
Lower the value of this command to obtain a smoother movement and slightly slower without
losing accuracy.
Programming the SF command is optional; if not programmed, the CNC assumes as
frequency of the filter the one defined in machine parameter SOFTFREQ.
Axis filter frequency in HSC mode.
The AXF command allows applying different filters to those set in the machine parameters.
Lower the value of this command to obtain a smoother path and faster but with lower
accuracy.
Programming the AXF command is optional; if not programmed, the CNC assumes as
frequency of the filter the one defined in machine parameter SURFFILTFREQ.
Orientation smoothing of the rotary axes working with RTCP.
The OS command may be used to smooth the orientation of the rotary axes, without tool tip
error, when working with RTCP in HSC SURFACE mode. Increase the value of this command
to obtain smoother RTCP movements.
Programming the OS command is optional; if not programmed, the CNC assumes the value
set in machine parameter ORISMOOTH.
Considerations.
Commands E and CORNER.
The CNC maintains the value of the commands programmed until a different one is
programmed, the HSC mode is canceled, a reset is done or the program ends.
When switching HSC modes, the CNC keeps the values programmed in the previous mode
for the commands that are not programmed (for example, the contouring error). If no HSC
mode has been programmed earlier, the CNC takes the default values for the commands
that are not programmed.
Commands RE, SF and AXF.
The CNC maintains the value of the commands programmed until a different one is
programmed, the HSC mode is changed or canceled, a reset is done or the program ends.
Example 1.
#HSC ON [CONTERROR, E0.050]
·
#HSC ON [SURFACE]
(Chordal error = 0,050)
To Next Page
Loading...
