Need Help!- Feed and Speed trouble

[Tirena]

We are running a tm-1, vf2, vf4, vf6, and ec400pp using TiN coated carbide tooling with 100 sf/m and .001 chip load per tooth. I am new to machining and have only been doing it for a year. The material we are using is 1045 hot roll steal. Cutting at a dept of up to 1.25. The problem we are having is tool breakage and wear. I should also add most cuts are made threw the center area of the work piece with little room for chip clearance. We tried multiple passes at a depth of .2 but they are complaining about long run times which are up to 6 hrs in some cases. Any advise i could get would be great thanks.

[Ken_Shea]

Curious, What is the cutter diameter and number of flutes?

[DSIF]

You are running your endmill too slow. That is why it is breaking. 300-350 SFM in hot roll steel with a carbide 4 flute TIN coated E/M. Also,drill a pilot hole for the E/M to Z down.
Example: 1/2 E/M @ 300 SFM .001 per tooth:
Spindle speed: 2,292.
Feed: 9 IPM.
Hope this helps you-Dan
PS: The SFM you are running is for HSS. Many CAM programs default to HSS feeds and speeds.

[Ken_Shea]

Not sure how any advice could be given not knowing what cutter is being used, 1045 is medium carbon steel, 300-350sfm is too high and a chip load of .001 is likely too low depending on the diameter.

[dingo0722]

Buy and download Gwizard

GWizard: A CNC Machinist's Calculator

The only values I struggle with using this software is the feed rate in 300 series SS using a cobalt drill. All other values and optimization tools work excellent

[Pondo]

It depends on a lot of variables.
Ridigity of the machine
Ridigity of the workpiece
Ridigity of the tool + toolholder
Coolant or not
Air blast or not

A baseline to start from for carbide in 1045 HRS would be about 225 SFM and .002/tooth chipload. With air, no coolant. Up to 1X dia DOC.
Ask your tool distributor for the cutter Mfg's recommendations. They vary a lot.
For lower DOC, you can go a bit higher on the SFM and a lot higher with the chipload.
Coolant has it's pluses and minuses. I do not use it on steel for any milling because of the thermal shock giving poor tool life, but some people swear by it. Again, ask the tool manufacturer.

[HuFlungDung]

C1045 is fairly machinable stuff, I'd be pushing 300 to 400 SFM, and slow down for the tougher stuff like 4140 prehardened

If I understood the original post correctly, it sounds as though deep slotting operations are being performed with a tool as wide as the slot. It may prove worthwhile to investigate a high speed machining strategy, permitting deeper DOC, smaller tool, permitting some tool movement within the slot, and better chip removal, more use of the total flute length of the tool, etc. Plowing full width making deep slots is old school.

[Tirena]

We are using Tin coated carbide 4 flute sizes from .25-.75 tooling. I am thinking of trying to get them to let us try more passes at .02 DoC with the feeds and speeds in the Machinery's handbook.

[Perfect Circle]

Cutting Speed of Metals
Values for High Speed Cutters in Feet/Minute
Multiply x3 for Carbide

Aluminum All alloys 250 and up
Soft Brass Half hard 150-220
Hard Brass and bronze Full hard 60-160
Cast Iron All 60-100
Mild Steels 1018, Free machining stainless 80-120
Tough Steels 304 Stainless, Tool steels 40-80



Good Luck~!

Go here this might be useful to you.

Milling Speed and Feed Calculator

[gizmo_454]

I cannot say it enough. Talk to the manufacturer of the tool. Machinery's Handbook is giving starting points and, from my experience with it in today's day in age, is not very accurate for most CNC stuff today. It is all dependent on HP, rigidity, and the tool manufacturer's recommended feed and speed. Every type and size of end mill will be different to some degree. But even then, there still is some wiggle room for adjusting.

For roughing purposes, depending on the size of the slots you are milling, you might want to look into a high feed cutter. Several companies make them. I like Mitsubishi's AJX cutter. I only have a Mini Mill, but I can run their 3/4", 3FL at 0.03" DOC, 1/2" width of cut, 0.016" IPT, and 330 SF/M in medium carbon steel all day with no problems. That is very conservative for what the end mill is capable of in a more powerful machine.

Good luck!

Mike