Siemens SINUMERIK 840D sl Operating Manual

Also see for SINUMERIK 828D Turning: Diagnostic manual Function manual Equipment manual Programming manual Operating manual

Approach/retraction1. The tool approaches the starting point at rapid traverse at the height of the retraction planeand is fed in to the safety clearance. The starting point is always on the positive X axis.2. The tool approaches the spigot contour sideways in a semicircle at machining feedrate.The tool first executes infeed at machining depth and then moves in the plane. The circularspigot is machined depending on the programmed machining direction (up-cut/down-cut)in a clockwise or counterclockwise direction.3. When the circular spigot has been traversed once, the tool retracts from the contour in asemicircle and then infeed to the next machining depth is performed.4. The circular spigot is approached again in a semicircle and traversed once. This processis repeated until the programmed spigot depth is reached.5. The tool moves back to the safety clearance at rapid traverse.Machining typeYou can select the machining mode for milling the circular spigot as follows:● RoughingRoughing involves moving round the circular spigot until the programmed finishingallowance has been reached.● FinishingIf you have programmed a finishing allowance, the circular spigot is moved around untildepth Z1 is reached.● ChamferingChamfering involves edge breaking at the upper edge of the circular spigot.Procedure1. The part program or ShopTurn program to be processed has been cre‐ated and you are in the editor.2. Press the "Milling" softkey.3. Press the "Multi-edge spigot" and "Circular spigot" softkeys.The "Circular Spigot" input window opens.Programming technology functions (cycles)10.4 MillingTurningOperating Manual, 05/2017, A5E40868721 455