[zerodegreec]

So I am nervous with the numbers G-Wizard spits out. I have recently converted my BF20 and my max RPM is 4400, and my max rapid is 1000 mm/min.

Last night I suffed (and broke) a 1/4" Roughing 3f HSS endmill running the feeds and speeds not even close to what Mach pumped out (cutting 6061). I am only using air to manage the chips until my enclosure is finished. G-Wizard told me to run at 4400RPM, 788 mm/min at a 2mm depth of cut (ramping) with 100% radial engagement. I run 150mm/min and thats all I feel "comfortable" with and I broke the cutter last night running at 130 mm/min. The cutter looked like it got plugged up and I was not getting the chips out fast enough. BUT I cant imagine running at 788mm/min!!!! Am I alone? How can you get up to the speed G-Wizard spits out? Tooling is not cheap and I am not willing to break a couple hundred bucks in endmills.

[SCzEngrgGroup]

It may be counter-intuitive, but you probably would NOT have broken the tool if you'd gone faster. When you go slow, heat builds up in the tool, and leads to the chip welding you got, which is what broke the tool. When you go faster, the heat is carried away by the chips, and the tool runs cooler. Also, for the kinds of speeds G-Wizard will give you, you must have coolant, not just air, unless you run a very shallow depth of cut. I run feeds in the range G-Wizard calculates all the time, and the only tools I break are when I do something stupid.

Regards,
Ray L.

[zerodegreec]

Sounds like I am going to have to man up (once my flood is running) and run with the big boys.... Nervous.

[SCzEngrgGroup]

Sounds like I am going to have to man up (once my flood is running) and run with the big boys.... Nervous.

Start at full RPM and feedrate, but shallow DOC, and see how it goes. If ok, then go deeper. Keep going until surface finish starts to degrade, or the spindle starts bogging down, or you run into unpleasant vibrations.

Regards,
Ray L.

[Winnfield]

Sage advice. That is exactly what I do when dry machining 6/4 Ti. Run at full speed with .005 DOC and adjust as necessary. It's the only way to do it without chipping/breaking tools.

[ChrisAttebery]

I've been using air blast and found that the feeds that FSWizard a suggests are pretty aggressive. Without flood you just won't be able to get the speeds he recommends. Off the top of my head I'd start at 350mm/Min and 1mm doc to start. Work your way up to 500mm/Min. Once you get to 500mm/Min start adding DOC. Others will tell you that's not right, but it is what has been working for me. make sure your air blast is getting the chips out of the way. I have been using 5psi through a .060" ID tube with the tip within 30mm of the end mill.

I've found that the sweet spot for slotting with my machine is about 30IPM/.060"doc/6000rpm with a 3/8" 3F carbide AL end mill. Smaller end mills are a PITA to slot with.

[jid2]

Try a 2 flute endmill, I can't get 3 flutes to stay clean past 15 IPM - but they do want to cut at the suggested 30 IPM.

[TiagoSantos]

Just to reiterate what everyone else is saying - yes, the G-Wizard feeds/speeds can be aggressive, but they're probably much closer to ideal that what you're doing now I was having the same problem a while ago, couldn't possibly imagine how I'd run any faster if I was having so much trouble at slow speeds. After reading a bunch of similar posts here on the zone, I decided to just go for it. The worst that can happen is you'll break another endmill - sounds like you're doing that already! In my case, the G-Wizard recommended speeds worked great, MUCH better than what I had been doing before, less noise, better finish, no heat, no chips stuck to the flutes, etc.

Pay attention to the HP rating of your cut, I believe there is a setting to limit that in G-Wizard. As was posted above, use the correct speeds and feeds, play with the DOC to end up a cut that your spindle can handle

[ChrisAttebery]

BTW: I just looked up my current problem child, a 3/16" slot in aluminum, 6000rpm, 3f carbide. FSWizard recommends 20.69IPM at 100% DOC. Even with mist cooling I'd have trouble making that cut. I've had much better luck at 12IPM and .060" -.090" DOC.

A good rule of thumb I found on another site is to start with a feed per tooth of 1/200 of your end mill diameter. That seems to work pretty well for me. Then adjust your DOC. I'll send you a PM with a link to that thread.

[ChrisAttebery]

Tiago,

Are you using flood or air blast?


Chris

[TiagoSantos]

I am using mist - fog buster using Kool Mist 77 and about 10psi or so..

I should add that I have almost zero experience using cutters smaller than 1/4"! And the smallest 3 fluter is 5/16" I have a couple of smaller 3 flute end mills on the way just to give them a try, but the common consensus seems to be that 3 flutes on cutters this small don't work well for slotting aluminum..

Anyway - my main point is, like Ray was saying, even if G-Wizards feeds can seem too aggressive, I'd try to at least get a lot closer. It seems there's a little hump that you have to go through - waaay too slow feedrate and it sort of cuts fine, but takes forever. Going a bit faster starts burning your tools, chip welding, snapping tools. Speed it up from there and it'll start to cut much better. Once you get over the hump, there's probably a fairly wide margin of feedrates that will "work", with the usual trade offs of tool life, spindle load, surface finish, MRR, bla bla bla..

[SCzEngrgGroup]

BTW: I just looked up my current problem child, a 3/16" slot in aluminum, 6000rpm, 3f carbide. FSWizard recommends 20.69IPM at 100% DOC. Even with mist cooling I'd have trouble making that cut. I've had much better luck at 12IPM and .060" -.090" DOC.

A good rule of thumb I found on another site is to start with a feed per tooth of 1/200 of your end mill diameter. That seems to work pretty well for me. Then adjust your DOC. I'll send you a PM with a link to that thread.

Chris,

Slotting with a 3-flute tool is less than ideal. 2-flute endmills are commonly referred to as "slot drills", for a good reason - they are FAR better than any other tool at slotting, because they have FAR more area between the flutes to eject chips. A 3-flute doesn't come close. Use a 2-flute for slotting, and you'll have far fewer problems, and be able to go faster. And the higher feeds a 2-flute will enable will also do a better job of keeping the tool cool. Using just air as a coolant is also less than ideal. In fact, air is a truly lousy coolant - what you're really doing is just clearing chips, and next to nothing in the way of cooling. A FogBuster would provide FAR better cooling, the same chip clearance as your air blast, and it would also allow you to go faster.

With small tools, machine rigidity, and runout, are MAJOR factors. If you can't reach the speeds GWizard suggests, lack of rigidity and/or excessive runout are probably a big part of the reason why.

Also, what is the length of that tool, and the stick-out? Those are MAJOR factors in determining correct feeds and speeds -a small increase in tool length or stickout will dramatically reduce the feedrate that is possible without over-stressing the tool. Even a 1/8" difference in length or stickout can reduce feedrate by as much as 10-20%, especially for small tools.

Regards,
Ray L.

[rlockwood]

Chris,

Slotting with a 3-flute tool is less than ideal. 2-flute endmills are commonly referred to as "slot drills", for a good reason - they are FAR better than any other tool at slotting, because they have FAR more area between the flutes to eject chips. A 3-flute doesn't come close. Use a 2-flute for slotting, and you'll have far fewer problems, and be able to go faster. And the higher feeds a 2-flute will enable will also do a better job of keeping the tool cool. Using just air as a coolant is also less than ideal. In fact, air is a truly lousy coolant - what you're really doing is just clearing chips, and next to nothing in the way of cooling. A FogBuster would provide FAR better cooling, the same chip clearance as your air blast, and it would also allow you to go faster.

With small tools, machine rigidity, and runout, are MAJOR factors. If you can't reach the speeds GWizard suggests, lack of rigidity and/or excessive runout are probably a big part of the reason why.

Also, what is the length of that tool, and the stick-out? Those are MAJOR factors in determining correct feeds and speeds -a small increase in tool length or stickout will dramatically reduce the feedrate that is possible without over-stressing the tool. Even a 1/8" difference in length or stickout can reduce feedrate by as much as 10-20%, especially for small tools.

Regards,
Ray L.

When limited to air, it becomes that much more important to take a nice fat chip, in order to remove the heat from the area. In order to take a nice fat chip, your tool needs to have enough clearance. All else equal, going from a 3-flute to a 2-flute will immediately improve both of these factors.

It will also increase tool rigidity. Which decreases deflection.

I've probably said it a million times, but i'll say it again. With a few caveats, 2-flute tools are better suited for aluminum than 3-fluted tools are. If you don't know what those caveats are, buy 2-flute. And probably buy un-coated carbide. Or maybe even HSS. I have no idea why every manufacturer seems to be shilling small-diameter 3-flute endmills designed for aluminum, except perhaps that each broken one likely needs replaced..

edit: realized my quoting of Ray might make it appear as though i'm disagreeing with him. However, my intention is the complete opposite. Everything he said is so important, it bears repeating.

[zerodegreec]

Thank you everyone for your contribution. I have plans well in place to build an enclosure and go to full flood coolant. I have another post on the go with suggestions to coolant options. My machine is not overly powerful so the limiting factor I see is that I can only run 4400rpm and my motor is slightly over 1hp. Add to that a cheap knockoff KBIC spindle drive and I get some good rpm drops with working the motor. For example the motor is rated at a max amperage of 7A. If I work it hard enough to get ~5A of load, the spindle RPM drops at least 300 to 500 rpm. This behavior is the project for tonight to see if I can tune the driver properly. I have not changed it from the factory settings and am starting to think that its just not setup properly.

[zero_divide]

I've been using air blast and found that the feeds that FSWizard a suggests are pretty aggressive. Without flood you just won't be able to get the speeds he recommends. Off the top of my head I'd start at 350mm/Min and 1mm doc to start. Work your way up to 500mm/Min. Once you get to 500mm/Min start adding DOC. Others will tell you that's not right, but it is what has been working for me. make sure your air blast is getting the chips out of the way. I have been using 5psi through a .060" ID tube with the tip within 30mm of the end mill.

I've found that the sweet spot for slotting with my machine is about 30IPM/.060"doc/6000rpm with a 3/8" 3F carbide AL end mill. Smaller end mills are a PITA to slot with.

Yes you are absolutely correct.
FSWizard like any other calculator assumes proper if not ideal cutting conditions.
There is absolutely no way to cut aluminum dry at those feedrates!

And yes, i have found myself that normally in order to get in the ballpark for dry cutting aluminum you need to get SFM and Chipload to at least 50% each
Also your depth of cut will have to be reduced to half of recommended.

People have requested to add consideration for coolant into the calculator, but i am reluctant to do that as conditions will change for different materials.(IE: milling steel above 450SFM is dry only)

But with flood coolant i normally exceed recommended feeds, sometimes by as much as 150%

[rlockwood]

Yes you are absolutely correct.
FSWizard like any other calculator assumes proper if not ideal cutting conditions.
There is absolutely no way to cut aluminum dry at those feedrates!

And yes, i have found myself that normally in order to get in the ballpark for dry cutting aluminum you need to get SFM and Chipload to at least 50% each
Also your depth of cut will have to be reduced to half of recommended.

People have requested to add consideration for coolant into the calculator, but i am reluctant to do that as conditions will change for different materials.(IE: milling steel above 450SFM is dry only)

But with flood coolant i normally exceed recommended feeds, sometimes by as much as 150%

I've always figured coolant is figured much like all of the other unspecified factors, which is to say "adequate for the application." I mean.. all of those other factors being inadequate have the same end result; reduced speed. Would you add a check box for inadequate workholding?

Keep up the good work btw, I use your calculator on a multi-daily basis and find the calcs to be generally right on point.

[ChrisAttebery]

On my way home I picked up a couple 2F 3/16 Best Carbide AL end mills. I just added a Fog Buster type system to the machine last week. But even with mist cooling the 3F end mills were just loading up. With the 2F AND MIST I was able to hit 30IPM and .054" DOC at 6000rpm.

I think the 3F end mills are great for profiling and even finishing, but to put it nicely they aren't that great for slotting.

[ChrisAttebery]

That lines up pretty well with what I found as well. How about adding this info to the FS Wizard page somewhere?

What I have found using mist is that if I'm slotting I can use the FSW recommendation for 100% DOC and it will give me a pretty reasonable feed for my machine. Then I play with the DOC to keep the machine happy.

Yes you are absolutely correct.
FSWizard like any other calculator assumes proper if not ideal cutting conditions.
There is absolutely no way to cut aluminum dry at those feedrates!

And yes, i have found myself that normally in order to get in the ballpark for dry cutting aluminum you need to get SFM and Chipload to at least 50% each
Also your depth of cut will have to be reduced to half of recommended.

People have requested to add consideration for coolant into the calculator, but i am reluctant to do that as conditions will change for different materials.(IE: milling steel above 450SFM is dry only)

But with flood coolant i normally exceed recommended feeds, sometimes by as much as 150%

[zero_divide]

I have big plans for FSWizard.
But i got a problem: i am no google and if i put too much stuff in there performance will suffer greatly.
As i cant afford premium web hosting.
Also with HSMAdvisor being in development i dont have enough time for it.
But one day it will come.