| Q1: |
It is easy to cut "free cutting steel", but when using cermet or solid carbide tool, its tool life is short and the finished surface is not good either.
Why ? Are there any good ways to cope with it ? |
|
 |
|
|
| A1: |
The name of "free cutting steel" gives us the impression of easy cutting, but the additives such as Sulfur and Lead are included in the material in order to increase the machinability.
The tool life of cermet tools becomes shorter to the material containing such components' additives. Also, the solid carbide has the adhesive characteristic originally.
Therefore, it may cause such inconveniences mentioned in the question when cutting "free cutting steel" by cermet or solid carbide tool.
For the "free cutting steel" machining, it is recommended to use the PVD coated tool, since it does not react to the additives in the material nor cause the adhesion.
(Kyocera CERATIP has such PVD coated tools in its product line.) |
|
 |
| Q2: |
What kind of ways are there to improve chip control at the turning operation ? |
|
|
|
|
| A2: |
There are several ways such as changing chipbreaker geometry and cutting conditions. The actual chip's comparison table is attached hereunder. Higher feed-rate, smaller corner-R, lower cutting speed, and smaller approach angle are suitable to cut chips short.
|
|
|
| Q3: |
The work is the forged steel of SCM435 (AISI 4135), diameter 60 mm with an interrupted cut part. Though both the depth-of-cut (d.o.c.) and the feed-rate are not so large (d.o.c. 1.5mm, feed-rate 0.25mm/rev.), even coated carbide insert cracks. Why ? Are there any good ways to cope with it ? |
|
|
|
|
| A3: |
Actually, both the d.o.c. and the feed-rate seem small but the scale part of a forged steel is hardened and this machining includes the interrupted cutting too. So, the minute chippings might have happened to the cutting edge and turned into a fracture.
For this kind of machining, tough grade of coated carbide insert, and with the chipbreaker of a strong edge are recommended.
(E.G. Kyocera CERATIP's insert of grade CA5025 with GT-chipbreaker is recommended.) |
|
|
| Q4: |
At Aluminum turning, is there any effective way to obtain the shiny finished surface ? |
|
|
|
|
| A4: |
Use a diamond tool to obtain the shiny finished surface of Aluminum.
In diamond tools, there are two types, mono-crystal and multi-crystal types.
If the polished surface is preferred as a mirror, use the mono-crystal type.
In case of multi-crystal type, the cutting edge is composed of fine grains and each grain's form is reflected on the finished surface micrographically. So, the finished surface becomes the rainbow-colored one. |
|
|
| Q5: |
What are the cutting conditions for Titan turning ? |
|
|
|
|
| A5: |
Titan's thermal conductivity is extremely bad, which is 1/5 to 1/6 of that of normal steel. So, the cutting heat tends to remain at the contact point between the cutting edge and the work. If the cutting speed increases, the wear at the edge will become quite fast. Moreover, if it is machined in dry condition, chips from Titan may cause spontaneous combustion. So, the cutting speed should be set up at low range. Inserts of K-grade solid carbide or diamond tool are recommended to this application. Cermet or coated carbide tool will wear soon.
The cutting speed should be around 50 m/min at roughing by K-grade carbide, and it should be around 100 m/min at finishing by 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 roughing and finishing, or unusual wear will happen to the cutting edge.
(Kyocera CERATIP has KPD lines for diamond tools and KW10 for K-grade carbide tool.) |
|
|
| Q6: |
How do we choose the toolholder of "with offset" and "without offset" mentioned in the catalog ? |
|
|
|
|
| A6: |
If you use the toolholder of "with offset" on the machine such as the automatic lathe, whose tool post comes to the closest point to the chuck, the toolholder may interfere with the chuck. (Please see the drawing of "with offset" toolholder in the catalog.) In such case, if you use the toolholder of "without offset", it will not interfere with the chuck and good tooling will be obtained. |
|
|
| Q7: |
Chattering and vibration occurred during the face milling using a multiple-insert type milling cutter (Dia. 160mm, 12 teeth). Why ? |
|
|
|
|
| A7: |
The multiple-insert type milling cutter has an advantage of making the table feed-rate larger, but it may cause chattering or vibration, because a large number of inserts engages with the machining at the same time and cutting force becomes larger or the work is deformed. As the result, the finished surface may become worse.
In such case, please take several inserts out of the cutter and such problems will be solved due to less inserts engagement simultaneously. |
|
|
| Q8: |
Are there any good ways to improve the tool life at the difficult-to-machine materials' such as stainless steel's rough turning ? |
|
|
|
|
| A8: |
One recommendation is to use the method of "slant depth-of-cut (d.o.c.)".
For example, if it is machined by 2 passes at d.o.c. 2mm/pass, please change the d.o.c. as follows:
| 1st Pass: |
|
slant d.o.c. with 3mm at the beginning and 1 mm at the end. |
| 2nd Pass: |
|
slant d.o.c. with 1mm at the beginning and 3mm at the end |
(In this 2nd pass case, if the toolholder moves horizontally simply, the d.o.c. becomes slant naturally.)
If the d.o.c. changes during the machining, the point which the cutting edge receives the cutting load changes in order and the tool life becomes long due to less notch wear. |
|
|
| Q9: |
What is the point to machine resins or plastics ? |
|
|
|
|
| A9: |
A diamond tool is recommended to the machining of resins or plastics.
Cutting speed can be 200 - 800 m/min. But please be careful that at plastics' high speed machining, softened chips by the cutting heat may adhere to the finished surface. K-grade carbide is also available but use an insert with the rake angle as large as possible in order to realize the sharp cutting and prevent chips' adhesion. Cutting speed should be under 200 m/min. |
|
|
| Q10: |
What are the points to machine stainless steel at the milling operation ? |
|
|
|
|
| A10: |
Stainless steel is a so-called difficult-to-machine material and these are the points at the milling operation.
| 1) |
|
Restrain the cutting resistance low |
| 2) |
|
Lighten cutting load at the cutting edge |
| 3) |
|
Do not set up d.o.c. and feed-rate too small |
| 4) |
|
Milling at down-cut |
Therefore,
| 1) |
|
High rake cutter and high rake inserts are recommended so as to restrain the cutting resistance. |
| 2) |
|
Milling cutter with large corner angle is recommended so as to lighten cutting load to the cutting edge. |
| 3) |
|
Set up d.o.c. more than 2mm, and feed-rate 0.1 to 0.2mm/t so as not to cut the work hardened part. Cutting speed around 200m/min. is recommended. |
| 4) |
|
Check the position of the center of the milling cutter to the work so as to make down-cut milling. |
|
|
Japan
FAQ
