What are typical feedrate and CSS settings

[dmbgo]

I know this varies drastically with the properties of the material being machined, but for say a piece of bright steel bar (mild), 1" or 25mm in diameter, what are typical settings?

[Caleb]

Completely tool depend, if you use replaceable tips all the information will be on the box or supplier will be able to tell you the optimal speeds and feeds. Then you will need to tweak it to your machine and possibly job.

[tblough]

1018 mild steel, HSS, turning/profiling: 0.2" depth of cut, 632 rpm, 165 f/min, 4.78 in/min, 0.0076 in/rev, 1.68Hp

[dmbgo]

Thanks Caleb and Tom. Sorry I was slow to reply, I will experiment with these settings. FYI, my tool is a 60degree carbide insert. I sourced them from Ali, so there's no point asking the supplier.
Caleb, there is some info on the toolbit case - I'll look.
First I have to find out why my Z axis has suddenly stopped reversing (only when running gcode, it goes in both directions when I use the MPG). This is a new issue, Ill create a separate post if I can't fix it.
Thanks again
Dave

[Muzzer]

If you are using carbide inserts with a 1" dia bar, the answer to "what spindle speed" is probably "your maximum". Whether you can sensibly specify a constant surface speed as such may be academic. Carbide tooling requires a fair bit of heat in the chip to work properly, particularly for hardened materials. If you can get the chips to break up as they form, you may not be far off from where you need to be. This often requires increasing the feed per rev.

[tblough]

Uncoated carbide changes to: 2230 rpm, 583.6 f/min, 22 in/min, 0.0091 in/rev and takes 7.1 HP.

[Muzzer]

Korloy suggest 500-900 sfm, so 2000 - 3500 rpm at 1". Obviously if you attempt to maintain CSS, you would need to be able to exceed those speeds as the diameter reduces. My machine will only manage 2000rpm, so CSS isn't something I will need to worry about much. And as Tom points out, you'd need a seriously powerful machine to push these inserts. My main concern is getting the chips to break safely!

[tblough]

Getting chips to break is always a problem on smaller machines with their shallow depth of cuts. Most times the chip never makes it to the back of the chip breaker groove and instead flows down the chip breaker groove of the other edge of the insert.

I normally stay with the recommended SFM, but increase the feedrate (sometimes doubling the recommended) to get chips to beak.

[dmbgo]

Thanks Tom and Muzzer, although this is a subject I find really interesting, sadly my machine has developed an axis issue, that is preventing me from experimenting any further at the moment. When this issue is resolved, if you don't mind I will try what you advise and continue this thread.

[tblough]

HSMAdvisor and FSWizard are your friends.
https://hsmadvisor.com/