Biggest possible cutters vs smaller cutters for milling?

Hi All:
Hers's a subject Keith (my business partner) and I often disagree on: I will program a part to use the biggest cutters I can fit into the geometry whereas he believes in using smaller cutters and running them faster and at higher feedrates to maintain the same chipload.
I will also often prefer to stuff down a big cutter to hog out; then pick out the corners where he will "high speed-constant chipload" mill everything with the same cutter to save the cost of setup, the cost of the first rougher , and the toolchange time.

Keith claims the MRR is the same therefore the productivity is the same or better once he factors in those extra costs.

So he believes using smaller cheaper cutters confers some benefit beside the cost of the cutters, which follow:
He claims better finishes.
He prefers to interpolate generously around internal radii; I will program a 0.135" internal rad with a 1/4" cutter whereas he will use a 3/16 or 5/32 or even 1/8" cutter.
He claims less cutter pressure therefore better geometric fidelity.

His arguments are not unreasonable, but I believe them to be incorrect in a couple of ways:
First I can use a deeper DOC so my MRR should be faster.
Second I can use a bigger radial stepover so my MRR should be faster.
Third I'm using a stiffer cutter and my finishing passes are very small with correspondingly small tool pressures, so my geometric fidelity should be equivalent except with very flimsy features.
Fourth my cutter uses each flute fewer times to cut the same amount of material so my cutter should last longer, thereby making up for its higher price..

So who is correct?
I realize of course much depends on the situation, but assuming a rigid mill and a well clamped block with reasonably robust features...
As a general principle, do you typically pick my way or Keith's way when you start cutting on a job?
Why do you make the choices you do?

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
www.vancouverwireedm.com

What's to stop you from using a high speed roughing path with a big cutter? Surely using an eighth instead of a quarter takes more time than one tool change. It's hard to imaging a scenario where you're pegged for horsepower with an eighth inch cutter, almost regardless of the material and machine.

Rough with the smallest endmill that will eat up 100% of the mill's horsepower. Barring that, rough with the biggest endmill you can is my general rule of thumb. I'll only do the one-tiny-tool path when I need one part and am feeling exceptionally lazy.

Are you setting new tools for every job? I tend to keep a standard rack set up in positions 1-8 or so, so it doesn't take any more time to set up a job with three roughing tools versus one. I typically have 1/2", 3/8", 1/4", 3/16", 1/8", 1/16", 1/4" mill drill and 2" face mill as my permanent tools.

I'm with your partner. I use the smallest end mill that will reach the total depth I need. I really hate to use $100 end mills when $10 tools will work.

The much higher rpm more than makes up for the depth of cut advantage of the larger cutter, and the feed per tooth is often nearly the same . . . yields much higher inches per min feed.

Seems subjective to material/machine parameters.

If you're working aluminum, your spindle should be at top speed, in which case his smaller cutter certainly loses for the reasons you cited (his cutter will have a lower feedrate for the same number of flutes, as well as a smaller stepover).

If both cutters can be run at the same surface speed, the larger cutter should still be faster, as the increased chip load and stepover should compensate for the increased feedrate of the smaller cutter (assuming stepover size and IPT feedrate are both reasonably linear with endmill diam).

However for sidewall finishing passes where chiploads and stepover are purposely low, the smaller cutter should smoke the larger cutter, so long as it's not too flimsy and the flute counts are the same. For floor finishing, the two should be roughly equal, assuming they use identical % overlap.

Trying to make a basic endmill model: we could treat it like a driveshaft. To maximize MRR, you need to maximize power transmitted thru the endmill. Power is torque*speed. The torque a given endmill can handle roughly scales as the cube of the cutter OD. So all other parameters being equal, an endmill 2x larger should be able to handle roughly 4x more MRR (because it can handle 8x more torque but only half the rpm). Obviously this model is simplistic, but fits with intuition if you assume endmill DOC, WOC, and IPT feedrate are all roughly linear with endmill OD while rpm is reciprocal with OD.

implmex said:

Hi All:
Hers's a subject Keith (my business partner) and I often disagree on: I will program a part to use the biggest cutters I can fit into the geometry whereas he believes in using smaller cutters and running them faster and at higher feedrates to maintain the same chipload.
I will also often prefer to stuff down a big cutter to hog out; then pick out the corners where he will "high speed-constant chipload" mill everything with the same cutter to save the cost of setup, the cost of the first rougher , and the toolchange time.

Keith claims the MRR is the same therefore the productivity is the same or better once he factors in those extra costs.

So he believes using smaller cheaper cutters confers some benefit beside the cost of the cutters, which follow:
He claims better finishes.
He prefers to interpolate generously around internal radii; I will program a 0.135" internal rad with a 1/4" cutter whereas he will use a 3/16 or 5/32 or even 1/8" cutter.
He claims less cutter pressure therefore better geometric fidelity.

His arguments are not unreasonable, but I believe them to be incorrect in a couple of ways:
First I can use a deeper DOC so my MRR should be faster.
Second I can use a bigger radial stepover so my MRR should be faster.
Third I'm using a stiffer cutter and my finishing passes are very small with correspondingly small tool pressures, so my geometric fidelity should be equivalent except with very flimsy features.
Fourth my cutter uses each flute fewer times to cut the same amount of material so my cutter should last longer, thereby making up for its higher price..

So who is correct?
I realize of course much depends on the situation, but assuming a rigid mill and a well clamped block with reasonably robust features...
As a general principle, do you typically pick my way or Keith's way when you start cutting on a job?
Why do you make the choices you do?

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
www.vancouverwireedm.com

Click to expand...

.
.
obviously longer length cutter at same cubic inches per minute removal rate with small diameter will bend more under load. you must be toy makers making mini parts
.
many parts i have to machine at 12 to 20" depths. I use excel to calculate feeds and speeds and depth and width of cuts and sudden tool failures. obviously bigger dia cutters can take more inch per tooth feed and well as depth and width of cut. big facemill can easily take .012" per tooth feed where a little endmill might easily max out at .001" per tooth feed.
.
Excel can easily calculate things like
4" facemill
0.200 depth of cut
3.5 width of cut
600 sfpm
.012 ipt
feed 55. inch per min
38.504 cubic inches per minute removed
2117.7 lbs of force at cutter
38.5 hp required
.
good luck with removing at that rate with 1/2 dia cutter sticking out 9"

It seems like I have been gravitating towards smaller cutters with the new HSM paths available. Using a 1/2" deep pocket with .135" internal radius as an example, I used to rough with a 1/2" EM and then finish with a 1/4" EM. Now I am more likely to just use a 3/16" EM and with a HSM path and a finish path. Part of that is because I hate loading tools and wasting time with tool changes, and part of it is that I can keep that tool at max cutting capacity for more time and with a constant chip load. I really haven't done any time/ dollar studies, but my gut tells me that I am making more money using that $10 cutter at it's maximum possible depth of cut than the more expensive cutter at 25% of it's possible depth of cut and bouncing up and down on chip load.

I'm with Keith within reason. I can stick a 1/2" end mill down to 1.25" axial and 10% radial (steel example here) and run at 200 IPM utilizing the whole cutter length in an HSM toolpath. Sure I could try it with a 1" cutter, but it won't be pretty or fast and not a lot of machines out there are going to do a zig-zag or pocketing cut and sound or perform nicely with that kind of tooling. And the cost per tool is astronomically different to boot.

So here's one catch: in your 1/4" cutter example what's your axial depth? I'd bet a 3/16" can outperform the 1/4" in the same pocket using HSM vs traditional stepover cutting, and that's a better argument than just comparing cutter size. At those tool sizes though I think the cost difference becomes negligible. Other geometry matters too of course. If your feature is shallow the bigger cutter with a pocket routine may be much faster, but as depth increases HSM makes a lot more sense IMO.

I suspect two things are driving a change. First is direct drive spindles with no gears so higher speeds and lower cost and maintenance. Second is Cam, because programming was a big part of the total cost, and not so much now. Solid tools also have a cost factor. A 1" tool can have most twice the cutting edge but has 4 times the material as a 1/2" tool. So less wasted tool material.

I've beat machines to crap using the ol' bury the cutter technique.
I'm currently nursing an original 2002 Haas CaT40 machine using HSM/smaller tools whenever possible. My money; and haven't replaced the spindle in the 5 years i've been using it. That day is coming.
For your generic ferrous/steel cutting, I side with your partner and smaller faster cuts. It's been my experience that big tools impart large cutting forces without transmitting much in the way of spindle power to the cut. So i'm with Halcohead. Not to mention the old school method usually under utilized the flute length, which is expensive on time and cutter cost.
For aluminums and Titaniums, the scale starts to shift back to bigger cutters.
2 cents

Hi All:
This is shaping up to be a super interesting discussion; thanks all who've put in their two cents' worth so far.
To clarify a bit more, let me now set a hypothetical example and ask for your preferred strategy:

Suppose you were making a pocket in 4140 HTSR steel 4" x 4" and 3/4" deep with corner rads of 0.150".
You get to have TSC or air blast to clear the chips efficiently and you're not limited by the machine, so you've got the ponies, the rigidity and the spindle speed to do pretty much whatever you want.
Your setup time for each cutter is 5 minutes and your chip to chip time at toolchange is 10 seconds.
Your programming time is 10 minutes per toolpath.

Would you rough and finish with a 1/4" cutter to get the 0.150" rads with the same tool or would you rough with a 1/2" cutter, then HSM pick out the corners and lastly finish with a contouring toolpath on the sidewalls using a 1/4" cutter?
You're using HSM for all roughing toolpaths and you're planning your DOC and radial stepover to be at max comfortable capacity for the machine, the workholding and the cutters.

Remember, in this scenario, you still get to use HSM toolpaths for any cutters you choose and you can pick DOC and stepover as you prefer but you must respect the surface speed limits imposed by the material.
You can also pick standard length or stub flute cutters, 2, 3, or 4 flute as you prefer.
Your goal is to get an accurate pocket as quickly as possible for the lowest overall cost.
Budget only one cutter of each size you choose and estimate what percentage of the cutter life you'll use up in the roughing.
When you calculate consumable costs use those numbers, so if your 1/2" cutter costs $100.00, and you use up 1% of it you've used up $1.00 worth of the cutter.

What say ye now???
Does your strategy change if the pocket is bigger (say 6" x 6") or smaller (say 2" x 2")?
Does it change again if you have to make 10 pockets?

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
www.vancouverwireedm.com

These HSM toolpaths more-or-less came about after I got out of the biz professionally. That said, I learned from others' examples, but I also learned from my own experience. What I learned is that for critical finishes or tolerances, you need a rough and finish tool.

If you are running 6061, burying a small diameter tool, with an Ally specific coating an geometry, will probably give you decent tolerances and finish up to the life of the tool. With any harder or more abrasive Ally, you'll lose finish and tolerance before the economical life of the tool is shot, so you'll end up going for broke with a rougher tool and nursing a finisher tool to get through a decent number of parts.

4140 is a different beast, I turned a bit of that stuff and similar material, but the 1..2 step method I layout above is doubly important on that material. I'm told that 4140 cuts like crap unless the tool is really sharp. And with the turning experience, I'm gonna say that your rough/finish with a single tool is gonna result in really crappy finish quality long before the tool is well and truly paid for. With big endmills, you don't throw them out, you resharpen them because it's very economical. $5 or so for a new edge and tip, so what if you gotta pre-set the dia and length, that's what comp is for. Small tools get tossed because they are not economical to resharpen; the tool is 3x the cost of the edge.

That said, the quantity of parts has a lot to do with the strategy, so does the cosmetic quality. If I have a 4x4 pocket 3/4 deep, I can hog that crap out with an HSM toolpath and a 3/4 EM that costs $75-100. It'll make mountains of chips before it'll need changing, then switch to a .250 to get the corners and do a finish pass around the inside. You'll probably change the .250 EM 2 or 3 times to the 3/4 EM.

The problem I can see with the strategy above is that the bottom of the pocket might look like a snaggle-tooth tiger machined it because the gash-end/corner of the 3/4 might be used up. You'd need to take a finish pass on the bottom anyway, that makes 3 tools.

I know that in today's world, if you have a Brother, you'd see most guys burying a 1/4 EM and go to HSM town on that pocket. But HSM paths looks like beaver tracks on pocket floors, they are not pretty. For stuff that matters, you'll probably end up doing a finish pass with either a circular or horizontal path, just to make the floor look consistent.

I notice that old-school still has an application in machining, on big heavy rigid machines, 70% stepover with horizontal or circular toolpath still rules because they can bury the cutter and get the most CIM from it. In weaker spindle applications, if you have the RPMs and acceleration, HSM seems to be the flavor.

On an older machine that has decent spindle speed and okay feed rates, a combination of older and new principles I think is the ticket. HSM says 20% stepover, the algo will ensure the path has no more than 64% (magic number IIRC) radial engagement. If you increase the stepover to take advantage of bigger cutters and rigidity, you might find a happy medium.

I will say, there is one problem I faced that I think HSM is the magic bullet for and I'm itching to try the low toolpressure, many passes, approach to solve that. The way that I machined that pocket before, it took 4 tools and the result still wasn't something I was super happy about.

I'm almost entirely in Keith's camp on this as well. Diameter is only a small factor in the grand scheme of things, and largely only serves to provide your effective final gear ratio. Smaller tools have a tendency to offer greater flexibility, but you must consider the overall rigidity of the tool itself, the machine's rigidity and power band, setup condition etc.

Use the smallest tool that offers adequate rigidity and can transmit the available horsepower into the cut.

Yes the HSM floor looks like poop but you can HSM at 5% stepover and some insane IPM, then clear the floor at 80% stepover using a corner radius EM and a contour path.

Regards.

Mike

implmex said:

you're not limited by the machine, so you've got the ponies, the rigidity and the spindle speed to do pretty much whatever you want.

Click to expand...

I just ask the magical unicorn running the machine what to do, in this clearly non-farcical scenario!

implmex said:

Suppose you were making a pocket in 4140 HTSR steel 4" x 4" and 3/4" deep with corner rads of 0.150".
You get to have TSC or air blast to clear the chips efficiently and you're not limited by the machine, so you've got the ponies, the rigidity and the spindle speed to do pretty much whatever you want.
Your setup time for each cutter is 5 minutes and your chip to chip time at toolchange is 10 seconds.
Your programming time is 10 minutes per toolpath.

Click to expand...

Absolutely I would rough with a 1/2" or larger end mill and then finish the corners and clean things up with 1/4".

I argue programming time isn't necessarily relevant here because it's amortized over the life of the job. So if it's a one-off, sure use only one endmill. If it's 100+ parts, use two endmills because programming time is nothing compared to cycle time. Assuming a large number of parts being run, the setup time will favor the longer-lasting endmill because it will require fewer re-setups per part.

Regarding endmill cost, assuming all endmills of any size last for the same amount of in-cut time, then per my previous post, an endmill 2x larger in diameter should remove 4x as much material over its life. Note the larger endmill is running slower, so if it lasts for the same number of minutes, this implies its flutes are wearing twice as fast per chip produced, possibly due to increased chipload. I would be surprised if flute wear accelerated this rapidly with increased chipload, but i'm sure it increases somewhat.

If we assume each endmill flute can handle a fixed number of entries and exits of the material (ie each flute produces X chips before it's worn out), the larger endmill should cut for 2x as many minutes as the smaller one (because it's running at 1/2 spindle speed, so each flute hits the work 1/2 as many times per minute). In that case the larger endmill would remove 8x as much material over its life. This model seems optimistic.

Checking some random off-brand vari-helix coated endmills (T&O brand, via Travers Tools), a 1/4" OD x 1/2" flute is $23. A 1/2" OD x 1" flute endmill is $62. The 1/2" endmill has to remove 2.6x as much material to equal the cubic inch/dollar value of the smaller endmill. If we trust either of the models above, in terms of cubic inches of metal removed per dollar spent on cutter, the 1/2" endmill is a 1.5x-3x better value than the 1/4" endmill.

Obviously all of the above breaks down when chatter/chip packing/recutting/coolant starvation get involved (also when the machine crashes, everyone prefers the smaller cutter). So this doesn't mean larger is always better. But if there's adequate HP, rpm, and setup/spindle rigidity, I see larger endmills as substantially better values.

I know this was just more naiive theory, but the these theories match with my experience and what I've read from others on here.

DMF_TomB said:

...
4" facemill
0.200 depth of cut
3.5 width of cut
600 sfpm
.012 ipt
feed 55. inch per min
38.504 cubic inches per minute removed
2117.7 lbs of force at cutter
38.5 hp required
.
good luck with removing at that rate with 1/2 dia cutter sticking out 9"

Click to expand...

TomB, you da MAN. I couldn't have picked up a tool like that even when I was young and strong.

Clearly, smarter people than I have beaten this 7 ways to Sunday and have come away with more answers than I am able to retain.

That said, I do it _basically_ like you do, with the caveat of letting the work dictate the tool choices. I tend to use the largest tool I can reasonably fit in the cavities and step down to the largest tool that will fit in the smallest radius. Rarely does the depth exceed 2.5"/63.5mm. I have taken to really enjoying corner radiused mills for a lot of work, too.

Better? Worse? I honestly don't know. The parts we do are generally able to fit in one's hand, and often within the scope of one's index finger's nail. Milled parts are almost always 3D and can be classified generally as core and cavity type work. Nothing at all like Tom's work.

implmex said:

Suppose you were making a pocket in 4140 HTSR steel 4" x 4" and 3/4" deep with corner rads of 0.150".
You get to have TSC or air blast to clear the chips efficiently and you're not limited by the machine, so you've got the ponies, the rigidity and the spindle speed to do pretty much whatever you want.
Your setup time for each cutter is 5 minutes and your chip to chip time at toolchange is 10 seconds.
Your programming time is 10 minutes per toolpath.

Would you rough and finish with a 1/4" cutter to get the 0.150" rads with the same tool or would you rough with a 1/2" cutter, then HSM pick out the corners and lastly finish with a contouring toolpath on the sidewalls using a 1/4" cutter?
You're using HSM for all roughing toolpaths and you're planning your DOC and radial stepover to be at max comfortable capacity for the machine, the workholding and the cutters.

Click to expand...

In this instance, the 1/4" EM would be at 3xD projection and the 1/2" EM would be at 1.5xD projection (stub endmill).

If it were me, I'd be running the 1/4" EM at 5% stepover or less, and the 1/2" EM at 10% stepover.

Even though the 1/4" endmill spins 2X as fast to maintain the same SFM, the 1/2" EM steps over 4X as much, so the MRR of the 1/2" endmill is effectively 2X.

I only work with plastic and aluminum. Almost all my parts are housings with a high material removal rate.
Using HSM tool paths, I rough and finish with the biggest tool possible. In the corners, I sketch a radius a few bigger than the tool diameter, so you don't burry the tool in the corner.
Downsizing the tool diameter, I rest and finish each corner using the same process until reaching the final target. If the last tool diamter is very small, (like 2mm) and very depth (10X), I use a zig-zag tool path with high speed, and very low depth of cut.
Using smaller tools from the beginning, I think you put more wear on the spindle, ball screws, linear ways, etc...

In the specific case you stated, I would probably gravitate to the 1/2" EM followed by the 1/4" EM. 3/4" depth is just getting a little too deep for a 1/4"EM in my world due to deflection and guaranteed damage to the bottom floor.