X4 Owners.... What are your *REAL* WORKING Speeds and Feeds?

[Mac Tech]

Hello everyone,

I would like to get some feedback from other X4/X4+ owners. (and other benchtop owner too)

What are your everyday WORKING feeds and speeds?

Let me be clear here guys.... I'm NOT asking what's the max the machine can do or how fast you can move to axis. Just because you can run a .5" end mill full width with a DOC of .75" at 20ipm, that doesn't you do it all the time. Same goes for rapids. Those type of max numbers are fine for bragging rights, but they're meaningless in the real world. OK, I'm done with my ranting...



So far, for myself, I believe I have been very conservative on my cuts. A typical cut in 6061 Alum for me is - .1875" HSS TiN 4 Flute end mill, 3000RPM, 6ipm, DOC of .03" with mist coolant. Sometimes I fell like these numbers work, sometime I adjust on the fly.

So what are you guy running? We all know that these are specific to the machine you are running, I'm looking for numbers for the X4/X4+ (mine is the 2009 model). If you've got some other benchtop mill, fill free to chime in, but please list your machine type. If you've made any mods to your machine that you think effects these numbers, list the mods.



Let's try for posts something like this.... (you guys running metric, change as needed)

Machine - X4+(2009)
Material - 6061 aluminum
Cutter - .1875" HSS TiN 4 Flute end mill
RPM - 3000
IPM - 6ipm
DOC - .03"
Coolant - Mist


Thanks for the info guys

[Mac Tech]

Wow, I guess this is top secret info that no one will share....

[fatal-exception]

GWizard says 21.6ipm with your parameters.

You might be better off not using a coated end mill for aluminum.

I think your numbers are very conservative, but it's whatever you feel comfortable with. If you really want to see where it will run, keep ramping up the feed till you break the endmill. You might be surprised.

[syil canada]

Hello,

according to my math,

for this cutter i would be @ about
3300 rpm
5ipm
and increase the depth of cut to .06"

I have cut at this depth with this same tooling, though 99% of every thing we use is carbide.
i have found the best to be Solid Carbide End Mill 3/16 3 Flute Uncoated For Aluminum

http://www.shars.com/products/gallery/6199/

or

4 Flute Rougher-Finishing Solid Carbide End Mills

A rougher / finsher we use the Guhring brand and you can hog more material and still finish with the same cutter.

[Mac Tech]

Thanks for taking the time to post guys.

fatal-exception - I've read that the uncoated end mills are better for Alum. Sounds like the uncoated end mills have less problems with the Alum gumming-up. Take no offense to this, but.... There are dozens of little apps out there that spit out numbers for speeds&feeds. Because of limited RPM, HP and rigidity, none of them will give numbers, at least not at the default settings, that are reasonable for the X4+ (or any benchtop class mill).

Syil Canada (Keith maybe?) - I've cut at that F&S with that end mill, but not at that DOC. When doing that cut, did you use coolant? Thanks for the links.



The end mills I've been use so far are from a set I got from Grizzly when I first bought the X4+. It's a set of 20 end mills, half 2 flute, half 4 flute all TiN coated. I've been working mostly with the .187" and the .25" 4 flutes for my pieces. I use the .75" 4 flute to surface and size material. They have served me well. As I start to replace them I want to get end mills better suited for working with 6061 Alum. I'm leaning toward carbide end mills, I'm hoping they will get enough extra life to justify the cost.

Please keep posting F&S info guys. I am hoping to get more info from people using the X4 mills. If I can get enough REAL data, I can use it to ADJUST the typical F&S formulas. That would be a great starting point when trying to fine tune the capabilities of my own X4+.


Thanks for posting, I hope the info gathered here will help others as well.

[syil canada]

hi mach tech,

through much trial and error, i personally been taught a hard lesson. The more expensive the endmill the longer it lasts, i can increase my depth of cut, and i get a better finish. We now use alot of nachi and Guhring carbide tooling, we just recently purchased bunch of the 1/4 Guhring rougher / finshers @ about $40 per endmill (with out checking the invoice).

expensive yes, but they cut in titanium for 8hrs and one lasted 2 days, with our old endmills we could go through up to 2 - 3 per day.

i have also found the carbide 3 flute, that are designed for alum work great. you can go alittle quicker and a larger depth of cut.

we also use alot of the serrated carbide roughers, in alum we were removing .8" depth of cut @ 30% step over @ 4imp on our x4. It sounded like crap and there was a shower of chips, but it got the job done quick!

i hope this helps, if not let me know and ill try to help.

keith

[dpaish]

Give me a month and I will post data and maybe a video of a X4 profiling SS knives.

DP

[Mud]

I just did a Video card upgrade (Radeon 9550 I think), now with 6061 I am cutting at 12ipm feed/8ipm Plunge/ .06doc for Roughing and 18ipm feed/8ipm plunge for Finish. End Mill is .375 4fl Rougher (Non Coated) with flood and
.375 2fl Ball nose (Non Coated) for finish work.

X4+ 2800rpm

[BobWarfield]

I will generally use whatever parameters G-Wizard spits out.

It's important to note we need both a width and a depth of cut to fully describe the cut. I'll assume since no one has quoted a width, that's full slotting.

On my IH mill with the 0.1875" endmill, I'd use a 3 flute HSS. Full slot, 0.03" DOC, and limited by my spindle to 1600 rpm in 6061 I would be feeding at 8.64 IPM.

Now if I didn't have to cut a full slot and wanted to have a little more fun profiling or pocketing, I'd go for a much thinner width of cut that allows some radial chip thinning.

For example, if I cut 0.030" width of cut, I can feed at 21.6 IPM. I try not to step down too little either, so I would cut full cutter diameter depth of cut (0.1875") deep in the hole, at a feed of 15.1 IPM.

If I can get a bigger cutter in the hole, my preferred endmill is a 1/2" 3 flute. At 1/2" depth, 0.030" width, 1600 rpm, I get 67 IPM.

FWIW, this is an an IH RF-45 mill. I mostly use pure air with no mist for coolant with aluminum. Keep the chips out of the hole and the endmill is happy.

Despite my 2HP spindle, I set a limit in G-Wizard of 1 HP. I know from experience that if I push past that limit I better have a really rigid setup, and everything better be just right.

Cheers,

BW