What's new
What's new

Swiss Lathe Question regarding Big depth of cut


May 16, 2022
Hi Everyone,

I am trying to turn a part in our KSI 38S swiss lathe, which is titanium Ti-6AI-4V grade Ø12mm bar. the finishing diameter is Ø4.45mm with step OD of Ø 11.5mm, and 160mm long. I used Walter DCMT11 R0.4 insert to cut the part in single pass by supporting with sub spindle. the cutting parameters were DOC- 7.5MM, SFM 200 and Feed is 0.05. I was able to finish the part, however, the part has runout/bend around 0.30 mm after machining.

is there any way to reduce the flex and decrease the cutting load?. The current load in Z axis varying around 50 to 60 percent.

The machine does not support Pinch turning, and also I cannot go multiple passes because the guide bush length is smaller than part length. so someone kindly advice regarding tooling or process.

someone told me to use 25*25 CCMT R0.2 tool/insert after milling it down to 16*16. But does C type inserts not flex the part more than D or V type inserts?.

Does anyone have experience with similar parts?

we have production requirements for 1000 pcs, any suggestions would be very helpful.

Thanks in advance.
I'm sure you're well past this issue, but I figured I'd offer up a suggestion.

I've got a repeating job that comes in 6-10 times per year. Its aluminum tho, not titanium.
The part has 8 different diameters (basically like a mini camshaft) ranging from .245 dia all the way down to .031 dia and its slightly over 4"
long. Most of the part consists of diameters under .077. With a couple larger diameters which are only between .150 - .250 long. Each diameter has its own tolerance ranging from +/- .002 down to +0/-.0005 (which applies to the .031 diameter) and it has a max r/o of .002.

After several trials & errors with using 2, 3 & 4 tools to make the part, I ended up cutting it in one shot (not including the cutoff)!

Its not the fastest cycle time ever considering how small the diameters are and how straight the part must be, but I end up with an immaculate looking part. It has a mirror finish and I'm dead serious when I say that I can take the parts, hold it on one of the bigger diameters at the end of the part in a 5C collet on an old toolmakers lathe. And I can turn the spindle on and there isvirtually ZERO run out/whipping. There is no noticable wabble, Its hard to believe even while I'm watching it spin. Its straight as an arrow. When I check it in a run out gage and its generally .0001 - .0003 from end to end.

Anyhow, the point of this novel that I've just written is that I bought a new tool to try cutting in 1 shot and never expected to see the results I've been getting.

I'm using a Kyocera KTKF toolholder with a
TKF___-AS insert which is a PCD insert good for alum & titanium. You'd just have to make sure theres enough DOC for your needs.

Sorry for such a long 1st comment.:reading::typing:
And if anyone is wondering....No, I dont work for Kyocera🙃

*Also to note, I'm using an extended nose guide bushing so that the tool is almost hitting the bushing. Theres probably a .015 gap between the guide bushing and the cutting edge of the insert which I assume is minimizing any bending of the part/stock while cutting.
Last edited:


Apr 1, 2012
Rk1989 I'm curious. Did you ever figure this out?
Hey Everyone,

sorry for the late response, like everyone suggested I used a ground insert(Seco-DCGT-R0.2), tight guide bush and proper coolant, well the part turned out to be OK.
the runout/warping is less than 0.002 to .004"( within tolerance). I was really surprised to see the result.

while I used DCMT-R0.4, the Z axis load was around 60%. and runout was more than 0.020" after machining. but DCGT worked like a charm, the Z axis load was 20% only, and the surface finish is impeccable.

I used 100 sfm, and 0.05mm feedrate while holding the front end with sub spindle, and used a sharp cutoff insert with low feedrate to avoid the radial force in the rear end.

thanking everyone again for their inputs and suggestions. 🙏