I am trying to cut 14 gauge 304 Steel. Its mostly an experiment for a client, I wasnt sure if its possible or not, but I think I am mostly running into technical issues, specifically feeds/speeds, and was hoping you could help.
I have used 2 different 4 flute carbide endmills, specifically SPEED TIGER ISE Carbide End Mill 1/8" ā 4 Flute, Square Nose, AlTiBN Coated and SPEED TIGER ISE Carbide End Mill 1/4" ā 4 Flute, Square Nose, AlTiBN Coated.
I have messed with the settings some (higher RPM, different feeds, ramps/no ramps), but nothing really seems to do what I want.
Results I am seeing:
1/4 was able to ācutā the steel, but I saw smoke, and eventually glowā¦clearly too much heat, so I stopped it.
1/8 was also able to cut, it did a little better with small holes, but when I tried to cut a straight 2"x0.25" line, I saw a pretty bright glow before it even got 2" down the line, so I stopped that too.
Everything is tight on the table using TTrack hold down clamps in all corners, and a positive stop on 2 sides, I havent seen anything move, and I dont hear chatter during the cut. The cut is relatively loud, but I expected that for this setup.
@cniemann88 Iām not a machinist but Iām pretty sure that the spindle speed for cutting steel should be on the low side, much lower than what you have tried.
I do not cut anything harder than hard wood. Primaraly because I have no way to cool the carve besides maybe aplying coolant by hand. That however will create a mess because my machine is bolted on a slab of mdf and I fear it wont combine well with coolant spills.
I do not see you mention a coolant setup. I feel carving steel without an active coolant flow will end up heating things up prety fast to the point that bits will start to shine and spark.
According to the charts I found here 304 steel has a poor heat rating and would require flood coolant. The middle of the RPM range would be 3820 for a 1/4" bit and 7640 for and 1/8" bit. Thatās according to the formula they provide to calculate RPMās from SFM without a coating modifier. Depending on the coating, I didnāt find the exact one you mentioned, you could go 30-50% faster. With a āMachinabilityā rating of 45% itās one of the harder harder metals to work with.
Iāve only milled a little brass and aluminum myself so I donāt have any personal experience to offer. Mainly just sharing my findings because I was curious myself.
Usual preface, Iām with PreciseBits. So while I try to only post general information take everything I say with the understanding that I have a bias.
You probably have a couple of issues here.
As stated by multiple people your surface speed is too high and that will kill you right out of the gate with steel. Generally with 304 you are going to be somewhere around 250 SFM ~3,800 RPM for a 1/4" and ~7,600 for a 1/8" (as Michael indicated). If you want more info on the why of this see here:
After that you have chipload. If this is a true metal cutter and you donāt have other issues (see below) you should be somewhere around 0.0003"-0.0005" for a 1/8" and 0.0005"-0.0010" for the 1/4". You need a big enough chip to sink the heat into. But you donāt want to either overwhelm the cutting flute or introduce deflection. You could be over double that for a steel cutter and double again for high end cutters. But Iām going to assume āgenericā for now (huge difference between āmetalā cutters and āsteelā cutters, plus geometry, carbide grade, etc.).
The other thing that can straight up kill you is runout. Runout is basically the amount you are spinning off the central axis of the spindle. In most cases spindles are pretty good. Collets are mixed though. For metal cutting you are massively fighting an uphill battle if your runout is over 0.0002". For steel you ideally want half of that. Thereās multiple reasons for this but the big one that will kill you here is that runout adds and subtracts from chipload for different flutes (itās wobbling toward and away from the cut direction while cutting).
To use these together in an example. Letās say we are using the 1/8" 4 flute cutter at the 7,600 RPM and the 0.0003" chipload. That works out to a feed of ~9 IPM. Now letās say we have 0.0002" of runout. What will happen there is that for at least part of the cut we will be cutting at a 0.0001" chipload on one flute and a 0.0005" cut on another. Or a simpler way to think about is that for a programed 9 IPM cut we will be functionally cutting at 3 IPM and 15 IPM. That can put us in a position where we are cutting both too fast and too slow.
So what I would do is measure the runout to make sure you are within margins for your cut (If not look for graded collets). Then use the higher numbers at a very low pass depth (0.005"-0.010"). This lets you extend the chipload range while limiting the force and compensating for a small chip. You can only compensate so much though. If you are successful you can tweak these for production.
As others have said you will have a much easier time cutting the with a cutting fluid. Preferably an oil based one with a surfactant. Also make sure that you are choking the tool up as much as possible without either bottoming out the tool in the spindle or inserting any ground portion of the tool in the collet.
One final thing. Those tools that were glowing are dead, even if they look okay. At the temps to make it visibly glow you are well above the temperature to leach the cobalt out of the carbide. That will greatly embrittle the carbide and that flute will not have the strength to cut steelā¦ or probably even wood.
Hope thatās useful. Let me know if thereās something I can help with.
Iām assuming ā0.0003ā-0.0005" for a 1/8" and 0.0005"-0.0010" for the 1/4" is referring to chip load?
Runout wiseā¦I got the collets from you a couple months ago, there is nothing visible or audible that indicates anything wrong with them or spindle or the bit, although I dont have the tools to precisely measure runout.
I didnt state originally, but I am using hand applied cutting fluid, specifically āAnchorlube All-Purpose Metalworking Compound 16oz - Water-Based Cutting Fluid for Drilling, Tapping, Sawing - Great on Stainless Steel | No Oilā The area I am cutting is pretty much flooded (I am not planning on cutting a lot of often).
I did use the lower RPM with the 1/4 bit a few times, but it actually stalled, which is why I increased it, however, I havent gone below 10 for IPM, and Iād like to start with those for the 1/8 bit.
Appreciate it. What grade did you get? For metal cutting in general the bare minimum you could get away with would be UP. Ideally EP.
Iāve been running into that cutting fluid a lot latelyā¦ They have a marketing campaign or something? It will help with heat and tarnishing/oxidizing. However, you donāt pickup the benefits of the oil based fluids where they functionally let you cut a smaller chipload.
??? You arenāt even close to the power limit of that spindle. Even with a 1/4" bit at the 0.001" chipload and 0.015" deep you are only looking at around 67w of power.
I think you were fusing the cutter to the metal and thatās what stalled it. Keeping the chipload up should prevent that. If you want extra insurance ramp the cut in so itās never dwelling. The only other thing Iāve seen that does that is if the spindle is spinning backwards (you would be amazed at how many times weāve seen this). If you want to check it just mount a bit in the spindle and start and stop the spindle. Watch what direction itās spinning as it slows. Should be in the direction the flutes cut.
