Milling Contour Spigot (Cycle63) - Siemens sinumerik 840D sl Operating Manual

Programming technology functions (cycles)
8.5 Contour milling
Parameter Description
Maximum depth infeed
DZ or - (only for G code and ShopTurn, machining surface, face C/Y/B) or
DX - (only for ShopTurn, machining surface, peripheral surface C/Y)
Lift mode Lift mode before new infeed
If the machining operation requires several points of insertion, the retraction height can
be programmed:
to RP

Z0 + safety clearance - (only for G code and ShopTurn, machining surface, face

C/Y/B) or
X0 + safety clearance - (only for ShopTurn, machining surface, peripheral surface

C/Y)
On making the transition to the next insertion point, the tool returns to this height. If
there are no elements larger than Z0 (X0) in the pocket area, then Z0 (X0) + safety
clearance can be programmed as the lift mode.
8.5.12

Milling contour spigot (CYCLE63)

Function
You can use the "Mill spigot" function to mill any spigots on the face or peripheral surface.
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. there,
the tool moves with rapid traverse. Material is then removed between the blank contour and
spigot contour.
Machining type
You can select the machining type (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 at rapid traverse at the height of the retraction
2. The tool first infeeds to the machining depth and then approaches the spigot contour from
3. The spigot is machined in parallel with the contours from the outside in. The direction is
4. When the first plane of the spigot has been machined, the tool retracts from the contour
406
plane and is fed in to the safety clearance. The cycle calculates the starting point.
the side in a quadrant at machining feedrate.
determined by the machining direction (climb/conventional) (see "Changing program
settings").
in a quadrant and then infeeds to the next machining depth.
Operating Manual, 07/2010, 6FC5398-8CP40-0BA0
Unit
mm
mm
mm
Turning