HEIDENHAIN TNC 426B (280 472) ISO programming - Manual (Page 224)

8 Programming: Cycles 208
CYLINDER SURFACE (Cycle G127)
The TNC and the machine tool must be specially
prepared by the machine tool builder for the use of Cycle
G127.
This cycle enables you to program a contour in two dimensions and
then roll it onto a cylindrical surface for 3-D machining. The
programmed contour is traversed with G40 or with G41/G42.
The contour is described in a subprogram identified in Cycle G37
CONTOUR GEOMETRY.
The subprogram contains coordinates in a rotary axis and in its
parallel axis. The rotary axis C, for example, is parallel to the Z axis.
The available path functions are G1, G11, G24, G25 and
G2/G3/G12/G13 with R.
The dimensions in the rotary axis can be entered as desired either
in degrees or in mm (or inches). You can select the desired
dimension type in the cycle definition.
1 The TNC positions the tool over the cutter infeed point, taking the
allowance for side into account.
2 At the first plunging depth, the tool mills along the programmed
contour at the milling feed rate Q12.
3 At the end of the contour, the TNC returns the tool to the setup
clearance and returns to the point of penetration;
4 Steps 1 to 3 are repeated until the programmed milling depth Q1
is reached.
5 Then the tool moves to the setup clearance.
Before programming, note the following:
The memory capacity for programming an SL cycle is
limited. For example, you can program up to 128 straight-
line blocks in one SL cycle.
The algebraic sign for the depth parameter determines
the working direction.
This cycle requires a center-cut end mill (ISO 1641).
The cylinder must be set up centered on the rotary table.
The tool axis must be perpendicular to the rotary table. If
this is not the case, the TNC will generate an error
message.
This cycle can also be used in a tilted working plane.
The TNC checks whether the compensated and non-
compensated tool paths lie within the display range of
the rotary axis, which is defined in Machine Parameter
810.x. If the error message „Contour programming
error“ is output, set MP 810.x = 0.
C
Z
8.7 SL Cy
cles
Gr
oup II (not in
TNC 41
0)
Kkap8.pm6 29.06.2006, 08:06 208