Fundamentals of thread milling
Requirements
- Your machine tool features internal spindle cooling (cooling lubricant at least 30 bar, compressed air supply at least 6 bar)
- Thread milling usually leads to distortions of the thread profile. To correct this effect, you need tool-specific compensation values which are given in the tool catalog or are available from the tool manufacturer (you can set the compensation in TOOL CALL using the DR delta radius).
- If you are using a left-cutting tool (M4), the type of milling in Q351 is reversed.
- The working direction is determined by the following input parameters: Algebraic sign Q239 (+ = right-hand thread / – = left-hand thread) and milling method Q351 (+1 = climb / –1 = up-cut).
The table below illustrates the interrelation between the individual input parameters for rightward rotating tools.
Internal thread | Pitch | Climb/Up-cut | Work direction |
---|---|---|---|
Right-handed | + | +1(RL) | Z+ |
Left-handed | – | –1(RR) | Z+ |
Right-handed | + | –1(RR) | Z– |
Left-handed | – | +1(RL) | Z– |
External thread | Pitch | Climb/Up-cut | Work direction |
---|---|---|---|
Right-handed | + | +1(RL) | Z– |
Left-handed | – | –1(RR) | Z– |
Right-handed | + | –1(RR) | Z+ |
Left-handed | – | +1(RL) | Z+ |
Notice
Danger of collision!
If you program the plunging depth values with different algebraic signs a collision may occur.
- Make sure to program all depth values with the same algebraic sign. Example: If you program the Q356 COUNTERSINKING DEPTH parameter with a negative sign, then Q201 DEPTH OF THREAD must also have a negative sign
- If you want to repeat just the counterbore procedure in a cycle, you can enter 0 for DEPTH OF THREAD. In this case, the machining direction is determined by the programmed COUNTERSINKING DEPTH
Notice
Danger of collision!
A collision may occur if, upon tool breakage, you retract the tool from the hole in the direction of the tool axis only.
- Stop the program run if the tool breaks
- Switch to the Manual operation operating mode in the MDI application
- First move the tool in a linear movement towards the hole center
- Retract the tool in the tool axis direction
Tip
Programming and operating notes:
- The machining direction of the thread changes if you execute a thread milling cycle in connection with Cycle 8 MIRRORING in only one axis.
- The programmed feed rate for thread milling references the cutting edge of the tool. However, since the control always displays the feed rate relative to the center path of the tool tip, the displayed value does not match the programmed value.
- When using the thread cycles, CYLINDER SURFACE cylinder kinematics must not be active.