The TNC offers two cycles for machining surfaces with the following characteristics:
■Flat, rectangular surfaces
■Flat, oblique-angled surfaces
■Surfaces that are inclined in any way
■Twisted surfaces
Cycle Soft key
230 MULTIPASS MILLING For flat rectangular surfaces 231 RULED SURFACE
For oblique, inclined or twisted surfaces
MULTIPASS MILLING (Cycle 230)
1From the current position, the TNC positions the tool in rapid traverse in the working plane to the starting position. During this movement, the TNC also offsets the tool by its radius to the left and upward.
2The tool then moves in FMAX in the tool axis to set-up clearance.
From there it approaches the programmed starting position in the tool axis at the feed rate for plunging.
3The tool subsequently advances to the stopping point 2 at the feed rate for milling. The stopping point is calculated from the programmed starting point, the programmed length and the tool radius.
4The TNC offsets the tool to the starting point in the next pass at the stepover feed rate. The offset is calculated from the programmed width and the number of cuts.
5The tool then returns in the negative X direction
6Multipass milling is repeated until the programmed surface has been completed.
7At the end of the cycle, the tool is retracted in FMAX to set-up clearance.
8.5 Cycles for Multipass Milling
133 HEIDENHAIN TNC 310
Before programming, note the following:
From the current position, the TNC positions the tool at the starting point 1, first in the working plane and then in the tool axis.
Pre-position the tool in such a way that no collision between tool and clamping devices can occur.
úStarting point in 1st axis Q225 (absolute value):
Min. point coordinate of the surface to be multipass-milled in the main axis of the working plane
úStarting point in 2nd axis Q226 (absolute value):
Min. point coordinate of the surface to be multipass-milled in the secondary axis of the working plane
úStarting point in 3rd axis Q227 (absolute value):
Height in the spindle axis at which multipass-milling is carried out.
úFirst side length Q218 (incremental value): Length of the surface to be multipass-milled in the main axis of the working plane, referenced to the starting point in 1st axis
úSecond side length Q219 (incremental value):
Length of the surface to be multipass-milled in the secondary axis of the working plane, referenced to the starting point in 2nd axis
úNumber of cuts Q240: Number of passes to be made over the width
úFeed rate for plunging Q206: Traversing speed of the tool in mm/min when moving from set-up clearance to the milling depth
úFeed rate for milling Q207: Traversing speed of the tool in mm/min while milling.
úStepover feed rate Q209: Traversing speed of the tool in mm/min when moving to the next pass. If you are moving the tool transversely in the
material, enter Q209 to be smaller than Q207 If you are moving it transversely in the open, Q209 may be greater than Q207.
úSet-up clearance Q200 (incremental value):
Distance between tool tip and milling depth for positioning at the start and end of the cycle.
8.5 Cycles for Multipass Milling
X
8 Programming: Cycles 134
RULED SURFACE (Cycle 231)
1From the current position, the TNC positions the tool in a linear 3-D movement to the starting point .
2The tool subsequently advances to the stopping point at the feed rate for milling.
3From this point, the tool moves in rapid traverse FMAX by the tool diameter in the positive tool axis direction, and then back to starting point .
4At the starting position the TNC moves the tool back to the the last traversed Z value.
5Then the TNC moves the tool in all three axes from point in the direction of point to the next line.
6From this point, the tool moves to the stopping point on this pass. The TNC calculates the stopping point using point and an offset in the direction of point
7Multipass milling is repeated until the programmed surface has been completed.
8At the end of the cycle, the tool is positioned above the highest programmed point in the tool axis, offset by the tool diameter.
Cutting motion
You can freely choose the starting point and thus the milling direction since the TNC always performs the individual cuts from point to point and the process sequence is executed from point / to point / . You can position point in any corner of the surface to be machined.
If you are using an end mill for the machining operation, you can optimize the surface finish in the following ways
■a shaping cut (tool axis coordinate of point greater than tool axis coordinate of point ) for slightly inclined surfaces.
■a drawing cut (tool axis coordinate of point less than tool axis coordinate of point ) for steep surfaces
■When milling twisted surfaces, program the main cutting direction (from point to point ) parallel to the direction of the steeper inclination. See figure at center right.
If you are using a spherical cutter for the machining operation, you can optimize the surface finish in the following way
■When milling twisted surfaces, program the main cutting direction (from point to point ) perpendicular to the direction of the steeper inclination. See figure at lower right.
8.5 Cycles for Multipass Milling
X
135 HEIDENHAIN TNC 310
Before programming, note the following:
From the current position, the TNC positions the tool in a linear 3-D movement to the starting point 1. . Pre-position the tool in such a way that no collision between tool and clamping devices can occur.
The TNC moves the tool with radius compensation R0 to the programmed positions.
If required, use a center-cut end mill (ISO 1641).
úStarting point in 1st axis Q225 (absolute value):
Starting point coordinate of the surface to be multipass-milled in the main axis of the working plane
úStarting point in 2nd axis Q226 (absolute value):
Starting point coordinate of the surface to be
multipass-milled in the secondary axis of the working plane
úStarting point in 3rd axis Q227 (absolute value):
Starting point coordinate of the surface to be multipass-milled in the tool axis
ú2nd point in 1st axis Q228 (absolute value): Stopping point coordinate of the surface to be multipass milled in the main axis of the working plane
ú2nd point in 2nd axis Q229 (absolute value): Stopping point coordinate of the surface to be multipass milled in the secondary axis of the working plane ú2nd point in 3rd axis Q230 (absolute value): Stopping
point coordinate of the surface to be multipass milled in the tool axis
ú3rd point in 1st axis Q231 (absolute value):
Coordinate of point in the main axis of the working plane
ú3rd point in 2nd axis Q232 (absolute value):
Coordinate of point in the subordinate axis of the working plane
ú3rd point in 3rd axis Q233 (absolute value):
Coordinate of point in the tool axis ú4th point in 1st axis Q234 (absolute value):
Coordinate of point in the main axis of the working plane
ú4th point in 2nd axis Q235 (absolute value):
Coordinate of point in the subordinate axis of the working plane
ú4th point in 3rd axis Q236 (absolute value):
Coordinate of point in the tool axis
úNumber of cuts Q240: Number of passes to be made between points and , and between points
and
8.5 Cycles for Multipass Milling
X
Q228 Q231 Q234 Q225
úFeed rate for milling Q207:
Traversing speed of the tool in mm/
min when milling the first pass. The TNC calculates the feed rate for all subsequent passes dependent of the stepover factor of the tool (offset less than tool radius = higher feed rate, high stepover factor = lower feed rate)
8 Programming: Cycles 136
Example: Multipass milling
Define the workpiece blank Define the tool
Tool call Retract the tool
Cycle definition: MULTIPASS MILLING Starting point for X axis
Starting point for Y axis Starting point for Z axis 1st side length 2nd side length Number of cuts Feed rate for plunging Feed rate for milling Feed rate for cross pecking Setup clearance
Pre-position near the starting point Call the cycle
Retract in the tool axis, end program 0 BEGIN PGM 230 MM
6 CYCL DEF 230 MULTIPASS MILLNG Q225=+0 ;STARTNG PNT 1ST AXIS
8.5 Cycles for Multipass Milling
X
137 HEIDENHAIN TNC 310