Siemens SINUMERIK 840D, Operating Manual

Page: 351 / 610

Programming technological functions (cycles)
8.3 Contour milling
Milling
Operating Manual, 03/2010, 6FC5398-7CP20-1BA0
351
8.3.12 Milling contour spigot (CYCLE63)
Function
You can mill any spigot using the "Mill spigot" cycle.
Before you mill the spigot, you must first enter a blank contour and then one or more spigot
contours. The blank contour defines the area, outside of which there is no material, i.e. the
tool moves with rapid traverse there. Material is then removed between the blank contour
and spigot contour.
Machining type
You can select the machining mode (roughing, base finishing, edge finishing, chamfer) for
milling. If you want to rough and then finish, you have to call the machining cycle twice
(Block 1 = roughing, Block 2 = finishing). The programmed parameters are retained when
the cycle is called for the second time.
Approach/retraction
1. The tool approaches the starting point in rapid traverse at the height of the retraction
plane and goes to the safety clearance. The cycle calculates the starting point.
2. The tool first infeeds to the machining depth and then approaches the spigot contour from
the side in a quadrant at machining feedrate.
3. The spigot is machined in parallel with the contours from the outside in. The direction is
determined by the machining direction (climbing or conventional).
4. When the first plane of the spigot has been machined, the tool retracts from the contour
in a quadrant and then infeeds to the next machining depth.
5. The spigot is again approached in a quadrant and machine in parallel with the contours
from outside in.
6. Steps 4 and 5 are repeated until the programmed spigot depth is reached.
7. The tool moves back to the safety clearance in rapid traverse.
Procedure
1. The part program or ShopMill program to be processed has been
created and you are in the editor.
2. Press the "Contour milling" and "Spigot" softkeys.
The "Mill spigot" input window opens.
3. Select the "Roughing" machining type.