Cut depth, Speed, and RPM

[BodaciousBrian]

I fired up Gwizard to calculate my cut depth, and its result is INCREDIBLY different from what I've been doing. Before I break something trying this, I though I would post the results here.
Taig CNC mill, no coolant, just air.
I'm cutting 6061 aluminium with a 0.25 4 flute carbide endmill. I want to use max rpm - 10,000. I set cut depth and width to 0.1" and it came up with 80 IPM. Seriously?

[strohkirchw]

You need to adjust your limits in the program as the defaults are blank. I'm not sure what the chip load is suppose to be on a 4 flute but assuming .002 you'd want to run 2nd pulley and 13IPM. There's no way you're going to get a decent chip load running at 10k rpm.

You could try 3rd pulley 22IPM but you're getting pretty close to .05HP according to Gwizard. So far I've found that right around .05HP seems to be the limit on my machine in terms of rigidity.

[Jeff-Birt]

I fired up Gwizard to calculate my cut depth, and its result is INCREDIBLY different from what I've been doing.

No matter how snazzy a feed rate calculator is the answers it gives you are only as good as the data you put in and even then it is only a SWAG (Scientific Wild Assed Guess.) There are far to may differences in tool geometries, materials, and machines for them to be accurate.

I'm cutting 6061 aluminium with a 0.25 4 flute carbide endmill. I want to use max rpm - 10,000. I set cut depth and width to 0.1" and it came up with 80 IPM. Seriously?

You will want to use a two flute end mill for aluminum. At 10,000 RPM you will have very little torque and you will be generating more heat than chips. I was doing some cutting yesterday with a 3/16" 2-flute carbide end mill, the belt was at the third from the top (4,500 RPM) and I was feeding at about 8 IPM with a 0.080" DOC. If I took a smaller DOC I could have bumped the feed rate up some more.

You really need to use coolant. Just a oil squirt can with some WD-40 in it will do wonders, just squirt a little on every once in a while. I like to mix about a tablespoon of ATF in which gives it some color and increases the viscosity just a bit.

[j_pniewski]

I like to use lighter cuts on aluminum w/ the Taig. Normal roughing with a 1/4" 3 flute (carbide) in 6061-T6 I use 10600 rpm, .04" doc, 30 imp with mist coolant. A 1/8" 3 flute I drop down to .03 doc. Machine sounds very smooth and without strain but I get good metal removal rates. I've actually cut as fast as 40 imp, but I'm not doing production work, so no need to push the envelope with stepper motors and risk losing steps. The mist coolant really helps. Finish passes done at 15 imp.

Joe

[strohkirchw]

Normal roughing with a 1/4" 3 flute (carbide) in 6061-T6 I use 10600 rpm, .04" doc, 30 imp with mist coolant.
Joe

Slotting?

Edit:

Looking that up in gwizard shows .063hp. Trying to do that would easily stall my spindle. I wonder if I don't have something setup correctly. I'm running flood coolant on mine.

[j_pniewski]

Yes, slotting.

Joe

[strohkirchw]

Well that sucks for me
Looks like I'm going to be problem solving tonight

[strohkirchw]

I stand corrected

2 fl 1/4" high helix carbide endmill with .04" DOC and 35IPM with no problems.


2fl 5/16" standard carbide endmill went up to a comfy 28IPM.

[SweetJustice]

I have the same question, but more general -- how do I find MRR charts for milling by horsepower?

At this moment, I want to know: what's an appropriate MRR for my 1/4 HP taig in unknown scrap aluminum? I've spent a lot of time googling for this, I've even gone to the library a couple of times looking for charts, and the only useful thing I've found was a suggestion of .3 in^3/min, somewhere in this forum.

It didn't work. Even at half that (2mm x 2.5mm x 800mm/min), I've still managed to stall my 10mm roughing endmill. Not immediately, but after maybe a meter of cutting.

[strohkirchw]

Gwizard is saying MRR .37 is what I'm doing with a 5/16" endmill for roughing. If I try to go much past this at 10600rpm, I can hear the motor start to strain some.

[BobWarfield]

I fired up Gwizard to calculate my cut depth, and its result is INCREDIBLY different from what I've been doing. Before I break something trying this, I though I would post the results here.
Taig CNC mill, no coolant, just air.
I'm cutting 6061 aluminium with a 0.25 4 flute carbide endmill. I want to use max rpm - 10,000. I set cut depth and width to 0.1" and it came up with 80 IPM. Seriously?

Yep, seriously. Take a look at what some of the other postings are getting. If I had 10K rpm I'd be running that on my IH mill easily.

But, and this is a big BUT, there are limiting factors.

For hobbyists, they will boil down to your machine rigidity, your coolant and chip clearing practices, and your CAM program. Let's consider each.

For machine rigidity, horsepower is your proxy. Horsepower is what will be pushing against the machine to overcome its rigidity. We'd like to think our machine manufacturers would not put a motor that's too big on the machine, so we can start with that. G-Wizard will scale back your cut to stay within the horsepower limit you set for your machine.

But, if you have a very lightweight machine, perhaps the motor is still a bit much. You will get a feel for that. Just scale back the horsepower limit. You can use MRR too, it's almost the same as HP.

BTW, that 10K rpm by 80 IPM cut is 0.4 HP. That seems like a lot for a Sherline. If we stick a 1/4 HP limit on, GW scales back to 7300 rpm and circa 50 IPM. Why scale back rpm? Because it adds tool life, so start there first. Also, scaling back feedrate too much reduces the chipload to the point that the cutter rubs, which reduces tool life.

What about coolant and chip clearing?

This has got to be the #1 reason I hear from hobby machinists for breaking cutters. Especially when slotting or going around corners, they fail to clear chips. If you don't have flood, or a continous mist with enough airflow to move the chips out, you have to stand over it with an air gun in your hand. Be very paranoid about recutting chips. On some materials (stainless!), the chips are work hardened. Imagine tossing handfuls of hardened sharp objects into the path of your cutter.

Some materials are sticky (aluminum and stainless). With nothing to lubricate, the chips want to stick to the cutter to the point they weld on and you have mess with eventually a broken cutter. Fix it by first (you knew I was going to say this) clearing the chips and second, making sure an appropriate liquid is available to lubricate, at least as a mist. If you don't have a mister, spray on some WD-40 every now and then. There are high end endmill coatings that lubricate for dry cutting, but they are material dependent and as a hobbyist, you don't want to pay the premium for them. So lubricate with mist or your can of WD-40.

Lastly, there is the CAM program, and some of it is how you use the program, and some is what the program is capable of.

If you've ever seen those crazy loopy HSM toolpaths, and looked at the feeds and speeds available for them in G-Wizard, you will know they appear to defy the laws of physics. If I take your same cut parameters, but specify I will cut the slot with a trochoidal path and no more than 30% engagement, suddenly I can go 10K rpm and 113 IPM, and that's with the 1/4 HP limit still on!

You've also no doubt experienced chatter in corners, or maybe even broken a cutter in a corner. HSM basically cuts corners without ever going around a corner.

What does this have to do with Hobby CAM? Well, let's say you have to profile the outside edge of a part. You have a choice. You can spiral out or spiral in. Always take the spiral in! If you spiral out, you're down in a slot with the cutter. That's much harder on it.

How you enter the cut matters, and there's lots about that on my mill surface finish page.

Lastly, there is the issue of jerking the tool around. If you look at the g-code, some CAM does a better job generating code that moves the tool very smoothly along the desired path. Others will jerk it around. Even a little micro-jerking matters.

Probably more than you wanted to know!

BW

PS Soigeneris, you need to learn more about feeds and speeds. The differences you talk about are all at the high end, not the bottom. It's very possible for a calculator to completely accurate in those conditions. In fact, its possible for it to be completely accurate exceeding manufacturer's recommended data if you have the right Knowledge Based-machining capabilities to compensate.

[Jeff-Birt]

PS Soigeneris, you need to learn more about feeds and speeds. The differences you talk about are all at the high end, not the bottom. It's very possible for a calculator to completely accurate in those conditions. In fact, its possible for it to be completely accurate exceeding manufacturer's recommended data if you have the right Knowledge Based-machining capabilities to compensate.

Well, I know enough to that the original numbers the OP got were garbage. It has a lot to do with the old adage about GIGO though. There are also so many different tool geometries (and vast differences in the quality of the tool themselves) that even with everything else configured correctly in a feed/speed calculator you will only every be close to an optimal number.

Then you have to consider the effect of how the tool paths themselves are generated as you were eluding to. If you use a CAM program like SurfCAM that can generate toolpaths based on tool engagement angle then the optimal feed/speed rates are drastically different than using toolpaths generated in a conventional manner. The other very large consideration is the effect of cutting feeds/speeds on tool life. You can 'push' a tool to cut much faster than what the manufacturer recommended but what does that do to its longevity. There is some range of settings where you strike a balance between optimal material removal and optimal tool life that is the most economical for operating a given machine. You would be amazed at the amount of chips generated by large companies like Boeing to test tooling and find the best feeds/speeds for their requirements. This data can then be fed back into their system for feed/speed rate calculations.

Most hobbyist folks also do not have flood cooling, or super rigid machines, or really high quality tooling so what works on other machines may not work on theirs.

I wasn't picking on your program in particular Bob, rather I was pointing out the fallacy in taking what ever numbers 'any' feed rate calculator pops out as gospel. When someone is just starting to learn about this stuff it compounds the problem as they just try to plug in what ever numbers the calculator says (not knowing any better). I can't tell you the number of support calls and emails I get about feed/speeds where folks are breaking bits because they are just plugging in numbers that a calculator gave them. (again a general statement not direct at your product in particular)

I'm also not saying that feed/speed rate calculators are not a valuable tool, rather they are a complex tool that you have to know how to configure properly, know how to use properly and even then you have to perform a sanity check on the figures they provide. If you understand that the numbers you get out of it are only as good as the numbers you put into it and treat it as an iterative process where one can keep refining the model (i.e. settings) used to perform the calculations based on experience then the utility of the tool will be improved.