Kyocera - Основной каталог 2011-2012 ENG

                                  для заказа - kyocera@kyocera-tools.ru

          MagicDrill® DRW

                                                           Q&A

                                  [High rate + Small feed]
                                  This setting makes the chips thinner and uses centrifugal force to cut them off.
                                  E.g. Vc=200m/min f=0.07 0.09mm/rev
                                  [Step machining at entrance]
                                  E.g. Entrance to 10 mm deep: 1 mm step machining
                                  E.g. 10 mm deep or more: Vc = 150 m/min, f = 0.15 mm/rev (Continuous machining)

          Q-4                     Tool markings are made on the finished surface. Is there any countermeasure?

          A-4                     During processing, force of deflection is applied to the     Tool marking
                                  center of the drill.
                                  If the drill is just pulled out from the position where
                                  processing is finished, tool markings will be made.
                                  To prevent tool markings, perform offset before pulling out
                                  the drill.

          How to prevent tool markings                                                                                                         Example of tool marking

                  Drill the hole. (The spindle revolves.)                          Turn back approximately 0.5 mm.
                                                                                   (The spindle revolves.)

K                                 Inner edge side                                                               Chips are adhering to the bottom
                                                                                                                when drilling stops.
                 Outer edge side

Drilling  Stop revolution and perform offset.                                      Without turning back, chips remains adhering to the bottom.
          (The spindle stops.)
                                                                                   If offset is performed without turning back, the bottom of drill
                                                      Avoid contact.
                                                                                   contacts with the inner surface of hole.

                                                                                   Turning back is necessary for blind holes but not for through holes.

                                                                                    Pull out the drill.

                                                                                                                     Example of drilling program

                                                                                                                G90G54G0G43X0Y0Z100.0H10

                                                                                                                S477M03

                                                                                                                Z2.5M8

                                                                                                                G01Z-80.0F48

                                                                                                                Z-79.5M19     The spindle stops at

                                                                                                                X0.2Y0.2      the specified position.

                                                                                                                Z100.0M9

          Outer edge side         Inner edge side                                                               * The M code and X and Y moving
                                                                                                                  directions are unique to the equipmen

          Make a clearance to prevent the tool from contacting                     Tool markings are not made (or are only slight even if made).
          when pulling out.
          (Approximately 0.1 to 0.2 mm)

          Q-5                     Chattering occurs. Is there any countermeasure?

          A-5                     Chattering usually occurs during chamfering and when the feed rate per revolution is not high enough.
                                  Try changing the drilling conditions as follows.

                                    Increase the feed rate if it is small.
                                    If the feed rate is f = 0.06 mm/rev, for example, increase it to f = 0.08 to 0.12 mm/rev.
                                    Increasing the feed rate will improve chamfering and thus prevent chattering.

                                    If the cutting speed is too high, lower it to Vc = 100 to 150 m/min.

                                    If the chamfering point and pass-through point are not plain, or if the workpiece clamping rigidity is low, lower the
                                    feed rate to f = 0.07 ~ 0.08 mm/rev.

                                    If chattering occurs on the full contact surface (e.g. during step machining), make adjustments by increasing the
                                    feed rate during chamfering or lowering the cutting speed.
                                   Once chattering occurs during chamfering, it will continue throughout the drilling.

K58                               для заказа - kyocera@kyocera-tools.ru www.kyocera-tools.ru