Instead of using programming techniques that are limited to “slicing off” material at a constant Z-value, it is highly advantageous to use contouring tool paths in combination with down-milling. The results include:
+ A considerably shorter machining time+ Better machine and tool utilization+ Improved geometrical quality of the machined shape+ Less time-consuming finishing and manual polishing work+ Cutting speed control - ve+ Enabling HSM+ High feed rates+ Long insert life+ Security
The initial programming work is more difficult and will take somewhat longer; however, this is quickly recouped as the machine cost per hour is normally triple that of a workstation. It is preferable to use a machine with software that has look-ahead functions, to avoid tool path deviations.
- Use a contouring type of tool path, such as “Waterline milling”, as the best method to ensure down milling
- Contouring with the periphery of the milling cutter often results in higher productivity, as more teeth are effectively in the cut on a larger tool diameter
- If the spindle speed is limited in the machine, contouring will help maintain and control the cutting speed
- Contouring also creates fewer quick changes in the work load and direction. In high-speed and feed milling, and in hardened materials, this is of specific importance, as the cutting edge and the process are more vulnerable to any changes that can create differences in deflection or create vibration
- For good tool life, stay in the cut continuously, and for as long as possible
Note! Avoid cutting with the center of the tool when cutting speed is zero.
Tool path strategy
Z – constant contouring, two axes. Roughing to finishing
Waterline milling Z – constant contouring
- Common when CAM-controlled maximum scallop function is available
- Smooth engagement and retraction
- Easy programming
- Wide tool choice
Helical contouring, three to five axes. Finishing
Contouring in a ramping tool path
- Smooth changes of direction
- Good form accuracy and surface finish
- Controlled scallop height
- Constant engagement
- Short programs
- Short tool
Generation of sculptured surfaces
Down milling with a cutter tilted approx. 10° in two directions ensures a good surface finish and reliable performance. A ball nose cutter or a radius-shaped cutting edge will form a surface with a certain cusp height, h, depending on:
- Width, ae, of cut
- Feed per tooth, fz
Other important factors are the depth of cut, ap, which influences the cutting forces and the tool indicator reading of the run-out – TIR. For best results:
- Use high-precision hydraulic chuck with Coromant Capto®
- Minimize tool overhang
Roughing and semi-roughing
If the feed per tooth is much smaller than the width and depth of cut, the surface generated will have a much smaller cusp height in the feed direction.
Finishing and super-finishing
It is beneficial to achieve a smooth, symmetrical surface texture in all directions, which can be easily polished afterwards, regardless of the polishing method selected.
This is obtained when fz ≈ ae.
Always use a tilted, two-tooth cutter in super-finishing to achieve the best surface texture.
Semi-roughing with fz much smaller than ae
Super-finishing with a tilted cutter and fz equal to ae