| Q1: |
It’s easy to cut "free cutting steel," but when using cermet or a solid carbide tool, its tool life is short and the finished surface is not very good either. Why is this? Are there any good ways to cope with it? |
|
 |
|
|
| A1: |
The name "free cutting steel" gives us the impression of easy cutting, but additives such as sulfur and lead are included in the material compound in order to improve the machinability.
The tool life of cermet tools becomes shorter when machining materials containing such additives. Solid carbide has a natural chemical reaction with steel, resulting in the adhesion of material to the cutting edge.
For "free cutting steel" machining, we recommend using PVD coated tools, since they do not react to the additives in the material and help prevent material from adhering to the cutting edge.
(Kyocera offers many PVD coated tools in its product lineup.) |
|
 |
| Q2: |
What ways are there to improve chip control during turning operation? |
|
|
|
|
| A2: |
There are several options, including changing the chipbreaker or insert geometry and cutting conditions. Please see the comparison table below. Increasing the feedrate, selecting a smaller corner radius, reducing the cutting speed, and switching to a smaller lead angle are all suitable options to improve chip control.
 |
|
|
| Q3: |
I am working with forged steel of SCM435 (AISI 4135), diameter 60 mm with an interrupted cut part. Though both the depth-of-cut (DOC) and the feed-rate are not so high (DOC 1.5mm, feed-rate 0.25mm/rev.), even coated carbide inserts crack. Why is this? Are there any good ways to cope with it? |
|
|
|
|
| A3: |
Actually, both the DOC and the feed-rate seem low but forged steel has a layer of hardened scale at the surface, and there is also an interrupted cut in the workpiece. This situation can create the potential for microscopic chipping at the cutting edge, which can lead to insert fracture.
For this kind of application, a tough coated carbide with a chipbreaker possessing a strong edge is recommended.
(For example, Kyocera’s grade CA5525 with GT-chipbreaker is recommended.) |
|
|
| Q4: |
During aluminum turning, is there any effective way to obtain a shiny finished surface? |
|
|
|
|
| A4: |
Use a diamond tool to obtain a shiny finished surface in aluminum.
There are two types of diamond tools; mono-crystal and multi-crystal.
If you prefer a polished surface resembling a mirror, use the mono-crystal type.
In the case of the multi-crystal type, the cutting edge is composed of fine grains, thus each grain form is microscopically reflected on the finished surface. This can result in a rainbow-colored appearance in the finished surface. |
|
|
| Q5: |
What are the best cutting conditions for turning Titanium? |
|
|
|
|
| A5: |
Titanium is a heat resistant material, with a thermal conductivity of 1/5 to 1/6 that of normal steel. The heat generated during the cut tends to remain at the contact point between the cutting edge and the workpiece. If the cutting speed increases, more heat will be generated at the cutting edge and the insert will break down quickly. Moreover, if it is machined in a dry condition, chips from the Titanium may spontaneously combust. The cutting speed should be set up at a low range. Carbide inserts (K-grade classification) or diamond tools are recommended for this application. Cermet tools will wear too quickly.
The cutting speed should be set around 50 m/min when roughing with K-grade carbide, and it should be around 100 m/min when finishing with a diamond tool.
The depth-of-cut and the feed-rate can be similar to those of steel.
Please remember to use coolant for both the roughing and finishing processes to prevent unusual wear from occurring at the cutting edge.
(Kyocera offers our KPD series of diamond tools and our KW10 as our recommended K-grade carbide tool.) |
|
|
| Q6: |
How do I decide between the toolholder option "with offset" and "without offset" mentioned in the catalog? |
|
|
|
|
| A6: |
If you use the toolholder option "with offset" on a machine such as a Swiss automatic lathe, the toolholder may interfere with the chuck. (Please see the drawing of "with offset" toolholder in the catalog.) For Swiss automatic lathes, straight shank or “without offset” tooling is preferred. |
|
|
| Q7: |
I'm experiencing chattering and vibration when face milling with a multi-tooth cutter (diameter 160mm, 12 teeth). Why is this? |
|
|
|
|
| A7: |
Muli-tooth milling cutters offer the advantage of higher table feedrates, but they may cause chattering or vibration. This is because a large number of inserts are engaged in the cut at the same time, resulting in increased cutting forces and workpiece deflection. As a result, the quality of the finished surface may suffer.
To reduce chatter and vibration, remove every other insert from the cutter. This will allow the cutter to stay balanced while also reducing the number of inserts engaged in the cut. The end result will be an overall reduction of cutting forces. |
|
|
| Q8: |
Are there any good ways to improve the tool life for difficult-to-machine material applications such as rough turning of stainless steel? |
|
|
|
|
| A8: |
One recommendation is to use the “ramping” approach to the workpiece.
For example, when machining with 2 passes at 2mm DOC/pass, consider changing the DOC as follows:
| 1st Pass: |
|
Create a “ramp” on the work surface by starting with a 3mm DOC at the beginning and gradually tapering up to a 1 mm DOC at the end. |
| 2nd Pass: |
|
Begin with a 1mm DOC at the beginning and finish at 3mm DOC |
(In the 2nd pass, simply traversing across the work surface will remove the ramp created during the first pass, and will create the same effect.)
By “ramping” across the work surface, the DOC is constantly changing. This changes the point at which the cutting edge receives the cutting load, and thus the tool life will increase due to less notch wear. |
|
|
| Q9: |
Are there any tips for machining resins or plastics? |
|
|
|
|
| A9: |
A diamond tool is recommended for the machining of resins or plastics.
Cutting speed can vary between 200 - 800 m/min. However, please be aware that at high speed machining of plastics, softened chips produced by the cutting heat may adhere to the finished surface. Uncoated carbide grades are also an option, but it is recommended to use an insert with a rake angle as large as possible in order to prevent chip adhesion. When using uncoated carbides, the cutting speed should be under 200 m/min. |
|
|
| Q10: |
Are there any tips for milling stainless steel? |
|
|
|
|
| A10: |
Stainless steel is a so-called difficult-to-machine material. Here are a few tips for milling stainless steel:
| 1) |
|
Restrain the cutting resistance |
| 2) |
|
Lighten cutting load at the cutting edge |
| 3) |
|
Do not set up DOC and feed-rate too small |
| 4) |
|
Milling at down-cut |
Therefore,
| 1) |
|
A milling cutter with a high rake angle combined with high rake inserts are recommended to reduce the cutting resistance. |
| 2) |
|
A milling cutter with a large corner angle is recommended so as to lighten the cutting load at the cutting edge. |
| 3) |
|
Be cautious about choosing a DOC or feedrate that is too light. Ideally, the DOC should be at least 2mm, and feedrate between 0.1 to 0.2mm/t so as to reduce work hardening. A cutting speed of 200m/min is also recommended. |
| 4) |
|
Climb milling is preferred. |
|
|
Japan
Frequently Asked Questions
