2 flute vs 4 flute Question

[Mackenzie Robens]

For the life of me I cannot figure out the correct speeds and feeds for my CNC. I have an Axiom Elite 2'x4' CNC and am testing on multiple materials. I have been using two flute end mills, carving bits, etc. My main issue is when running the 2 flute end mills I am getting a screeching noise. I believe this means my speeds and feeds are off. I am using the manufacturer recommended settings. For example, the 2-flute 1/4" end mill I'm running at 18,000 RPM's and a feed rate of 100 IPM. Does anyone have any suggestions?

I'm not getting any issues with this with v-bits, just the end mills. Will switching to a 4-flute bit help? Thank you, any help would be greatly appreciated!

[Jim Becker]

More flutes requires recalculation of the chip-load. 4 flutes are kewel for metal cutting, but could complicate things with wood. That said, there's no need to run a .25" endmill at 18K RPM. I generally use 12-14K RPM but I listen carefully and adjust the speed slightly if it "sounds off". (I have a spindle and can vary the speed in real time in my controller software) If you run your RPM too quickly, the chips will be too small to take away the cutting heat. You will absolutely get a scratchy noise from an endmill like this, however.

[George Yetka]

Amana's tool catalog has been working well for me. I understand the need to learn the skills to adjust these for your use but they have worked pretty flawlessly for the 30 or so bits I use. Im not sure about others but you can add their catalog to vectrics

[Michael Burnside]

Your RPM is way too high. Unless it's from HSM or other tooling manufacturer, you cant trust the numbers they give you. Amana, BitsBits, Whiteside, etc. are all off. I've downloaded and reviewed all the major Vcarve libraries. Remember chipload depends a lot on machine capabilities and material so these manufactures can't possibly give you a number that is always the same.

For example, 18000 at 100 IPM is a crazy low chip load assuming 2 flute, 1/4" endmill. Not only will it screech, you're bound to dull or break a bit. If you haven't broken a bit it's probably because you're not using a depth of cut your machine is capable of (the diameter of the bit). This is typical of YouTube misinformation using words like "conservative" when they really have no clue. Maybe you don't break bits, but burning, dulling, etc. can still happen (and your job takes longer than it should)....all because chipload is too low.

Go here and use these numbers for starters:

https://gdptooling.com/chipload-calc/

Use diameter of bit for depth of cut and pick a conservative load. Say if you're milling hardwood and the target is 0.009, maybe your machine can't handle that, so try 10000 RPM and 100 IPM (0.005" chipload). If the chips are around 0.005 and you're happy with the cut, you have a starting point. Maybe your machine is cool at 100IPM and 1/4" depth of cut, so increase to 120 IPM. Maybe you want to spin a little faster due to the fact it's softer "hardwood", so increase RPM to 12000 RPM and keep the 120 IPM for 0.005 chipload still. Or increase feedrate if the machine can handle it.

A lot of people try to make it complicated, it's not if you just trust the numbers. Every single endmill I own I have tested with different types of materials, measured chips and created my own database. The numbers I use are very similar to the link I sent or within a reasonable margin of error and quality of cut.

I've milled miles of material. I have never, even when cutting foam, used 18000 RPM and my machine can handle it. I usually stay within 10000-15000 RPM for 95% and the other cases are super specialized material gleaned from experience.

If you use 4 flutes and change nothing else, you're going to have worse problems, not less. The more cutting surfaces you have the faster you need to feed unless it's foam or other specialty materials and in those cases you may melt the material before anything else.

[Mackenzie Robens]

Thank you so much, I really appreciate the time and thought you put into helping me out. I will go off of your link and tweak from there - again, THANK YOU!

[Mackenzie Robens]

Can I ask, for plunge depth for v-bits what do you use? If I am using a 1/2" 60-degree v-bit, how much would you plunge on each pass? Thanks again.

[Michael Burnside]

Sorry Mackenzie I missed this reply. Whenever I use v-bits I always think edge quality and minimal sanding after. So typically I spin a little faster and don’t take too much at once. Maybe 1/16 to 1/8” max. I also will replace these bits much sooner than others for the same reasons.

There might be some hard core v-carvers out there that have better answers.

[Carl Beckett]

Can I ask, for plunge depth for v-bits what do you use? If I am using a 1/2" 60-degree v-bit, how much would you plunge on each pass? Thanks again.

I do 0.150" depth per pass with v-bits. Many designs the total depth is this or less which means a single pass in some cases.

Not sure how a chip load would calculate due to the varying bit speed due to diameter coming to a point.

Spindle speed 10-12k. Feed rate 40 ipm.

But I have not tried to optimize so others may have better guidance.

[Michael Burnside]

I do 0.150" depth per pass with v-bits. Many designs the total depth is this or less which means a single pass in some cases.

Not sure how a chip load would calculate due to the varying bit speed due to diameter coming to a point.

Spindle speed 10-12k. Feed rate 40 ipm.

But I have not tried to optimize so others may have better guidance.

Carl, you seem to be similar to me by the sounds of it. Yea, never really think about chipload for these types of bits.

[Wes Grass]

Chipload is the same, SFM is less.

[Wes Grass]

Forgot, slotting with a 4 flute puts a flute on centerline, which is trying to deflect ... 'things' ... while the trailing flute is generating one of the walls.

A climb cut might need a finish pass to get the dimension and finish you want, depending on material, thickness ... and the rigidity of the machine.

A 2 flute ramps its way in and out of the cut, with less deflection... usually.

Tools last longer as well, on finish passes ... the flute gets a good bite into the material, instead of 'rubbing itself to death' from the progressive entrance with a conventional cut.

Disclaimer: I'm mainly a 'metal dude'.

[Carl Beckett]

Forgot, slotting with a 4 flute puts a flute on centerline, which is trying to deflect ... 'things' ... while the trailing flute is generating one of the walls.

A climb cut might need a finish pass to get the dimension and finish you want, depending on material, thickness ... and the rigidity of the machine.

A 2 flute ramps its way in and out of the cut, with less deflection... usually.

Tools last longer as well, on finish passes ... the flute gets a good bite into the material, instead of 'rubbing itself to death' from the progressive entrance with a conventional cut.

Disclaimer: I'm mainly a 'metal dude'.

And some of my 4 flute 'end mills' do not plunge. So a heads up.

[Wes Grass]

Another good point.

Even with 2 flute I prefer to ramp in if possible. Old habit ... hard to break ... but seems like there's less crud burned onto the tip. But 90% of the 'wood' I was routing was MDF. And I got lazy after awhile and just ran with what CAM spit out by default.

Cute term I heard 40 something years ago, regarding aluminum welding on an EM with a too aggressive plunge. Leaves a couple 'strings' flowing up and out of the flutes. 'Pronghorn'ing'.

[Jim Becker]

I use ramping, too, Wes.

[David Falkner]

I haven't changed the speed on my spindle in years, it runs at 18,000 rpm. My most used bit is a 1/4" compression and I cut mainly hardwoods - Walnut, Maple, Cherry - but often cut 1/2" Baltic Birch ply when I make fixtures or cut Longworth chucks. When I cut the 1/2" BB it's a single pass at full depth and 175 ipm. I'm creating chips, not dust, and the bit is cool enough to the touch that I can cut with it and remove it with my bare hands moments after stopping for a bit change. My second most used bit is a 1/8" downcut spiral and it also runs at 18k with a feed rate of 75 ipm. I could raise the feed rate but typically don't. It also produces chips, not dust.

I realize this contradicts what many of you have said but this is what's working for me and I get good results with these settings.