Anyone milling steel...need some advice

Good day.
Today I had to make a few small parts out of mild steel.
I am using Spetool bits 1/4"

At the beginning I faced the metal and then cutout the shapes. everything was going great.
At the second part the machine seemed to dive into the work and I broke 2 bits.

It turned out the bit was slipping out of the collet.
I do think the collet got hot and started slipping it is also shiny inside.

Attached the settings used, also what cooling are you guys using?, where to buy good collet?


Thank you!

1 Like

Only twice. Wherever ever possible I cut steel on the milling machine.

In the two cases I had to I used continuous air blast to help clear chips (no mist). I also used single flute carbide cutters to help keep the router up in its rpm power band but lower the heat load. It also helps evacuate the chip, give the air blast more time to help evacuate the chip. In my case I was cutting precision slots that did not penetrate all the way through (rules out plasma) and the parts were physically to large to load in on the CNC mill. Even with the air blast and the single flute cutter I was targeting 0.0007 in chip load @9000rpm since parts of that cut are full width. For the parts that were not full width (after the initial pass down the slot) I was using a 0.070 step over and doubled the feedrate due to chip thinning. I was also using a 1/4 end mill and a similar (0.150) depth of cut… The ER-20 collets I was using are the ones I picked up from CNCRouterParts/AVIDcnc when I bought the machine. One time I ran a batch of 12-parts and the other time only 4, so since I normally use the milling machine when working with steel parts, I don’t have a very large data set to reference for that.

A few questions come to mind, beyond the typically cheap collets / run-out question and the one you are already asking about, heat build-up.

  1. Did you use acetone and a Q-tip to clean out any cosmoline from the inside of the collet? This is less likely the case as the taper on collet is very shallow and the mechanical advantage is pretty extreme for ER style collets to really grip. Typically, something else is going wrong, but it could be a contributing factor.
  2. Has the collet nut been correctly engaged with the collet before inserting into the spindle. Not trying to be insulting here. Some people do not know that most collet nuts need the collet (or the nut) to be rocked into position correctly. If one puts the collet straight into the spindle and then just pushes the nut straight on over it without correctly engaging them with a rocking motion bad things can happen to the collet or the nut or tool slippage as they can’t be tightened down as fully as they should be.
  3. Was the end-mill seated fully in the collet? I’ve seen many people buy the shortest carbide end mills they can trying to save money and then leaving them hanging way / way out to where the ER collet only has 1/2, 1/3 or scarily 1/4 engagement, because they needed more stick-out.
  4. Also maybe a silly question, but was the ER collet nut torqued appropriately?
  5. Assuming yes, but just checking, at those spindle speeds we are talking a carbide end-mill, not HSS?
  6. Run-out? Is the chip load changing drastically between the two teeth?
  7. is there a notable vibration when running that particular combination of RPM and federate that is causing a vibration in the machine? Often this can be heard during cutting and is often changed by varying the spindle RPM. In traditional machining (not always, but often) one goes up in RPM to clear past resonances where the machine is having problems with a sub-harmonic of the primary frequency.

Most likely your first guess on the end mill loading due to heat related problems and failure to evacuate chips are right on-track and that is a resonable place to start. The above are just a few additional pieces to consider.

There is often much to be learned by careful examination of the chips with a good microscope or 10x loupe when a cut fails.
=> Did the chips change to the wrong color? (go from silver to black or burned grey)(you won’t need a microscope or a loupe for that one.)
=> Did the chips change in thickness from one end of the cut to the other? That can be indicative of fully loosing a cutting edge which effectivly doubled the chip-load.
=> Do the chips have one clean edge and one torn edge? Can be indicative that the end mill chipped before the cut failed…


Your tool sheet is setup in inches and your passes are set in millimeters. I don’t know if it makes a difference but I try to keep them aligned to the same units. Your plunge rate looks to be too aggressive for aluminum let alone steel. I have never cut steel but have aluminum and brass and used much less aggressive feed rates and step overs than you have.

One thing the tool setup was for a 2 flute and the bit I used is a 4 flute (attached)

The part turned out good but I certainly have a tool setup issue.

What about these settings?
Since the manufacturer recommends a chip load of 0.00088 for slotting in steel?
What do you guys use for pass depth in steel?

I would be wary using tool manufacturer guidelines as gospel, be it wood or metal. They’re generally focused on large machines with much higher rigidity and horsepower.

I’ve used this table as a VERY rough starting point. Note the cautions at the bottom, as well as the RPM calculations. 12k on a 4 flute 1/4" in metal is sorta extreme on a gantry router.