Reply with QuoteA better description of what you're trying to do might help. I run 3/16 end mills as fast as 5,000 RPM and 30 IPM depending on what I happen to be doing.
Feeds and Speeds
Hello,
I am currently working on milling an Aluminum (6061) part, and am having trouble deciding what feeds and speeds to use. I have been using the GWizard Calculator program and even done some of the math by hand, but am not comfortable with running the machine at such high feeds and speeds. I can't imagine running this machine at 3,700 rpm and 32 ipm. The milling I have done for the 6 weeks I've been working here has been accomplished using spindle speeds around 1500 rpm and feedrates of only 1 or 2 ipm, but I have also already broken a lot of end mill tools. For this project, I am using 4 flute end mills with diameters of 7/16" (or 0.4375") and 1/4". I have heard that 2 flute tools are better for roughing aluminum, but my tool library is very limited at the moment. Does anyone have any advice for this sort of project? I appreciate any help I can get.
Similar Threads:
Re: Feeds and Speeds
A better description of what you're trying to do might help. I run 3/16 end mills as fast as 5,000 RPM and 30 IPM depending on what I happen to be doing.
You can buy GOOD PARTS or you can buy CHEAP PARTS, but you can't buy GOOD CHEAP PARTS.
Re: Feeds and Speeds
I'm essentially hollowing out a 1" by 1" by 1.5" aluminum cube. I have the machine plunging down .0025 inches at a time, then going around in a circle, repeatedly. A picture of the part is attached. Im not quite sure what other information would be helpful.
Re: Feeds and Speeds
The rpm for me is 5140 for most cutters under .5, and various feedrates from 20 to 45 ipm. I do use flood coolant for all of my parts.
Typical is .250 4 flute carbide or hss at .125 depth of cut, 35 ipm slotting on a profile cut 6061 aluminum.
.5 cutter, feedrate 20 30 ipm and approximately .080 doc 5140 rpm, any deeper and I get chatter on a full length cutter.
I would call my machining conservative.
My rule of thumb is if the cutter chatters, slow down on the feedrate or depth of cut, dont let the cutter rub (low feedrate) as that will shorten cutter life.
I like the shortest possible cutter for the job as well.
On a new program, I find the feedrate slider a big plus!
mike sr
Re: Feeds and Speeds
Hole pocketing like this I would drill a center hole first. Then I would use 5140 rpm, 20 ipm feedrate, plunge .1, .250 endmill, flood coolant. be sure to set your doc in cam so it doesnt exceed the cutter flute length.Originally Posted by brokellermann
I'm essentially hollowing out a 1" by 1" by 1.5" aluminum cube. I have the machine plunging down .0025 inches at a time, then going around in a circle, repeatedly. A picture of the part is attached. Im not quite sure what other information would be helpful.
You didnt mention your machine, this is how I would do it on a Tormach 1100 machine.
I use a waterline op on some of my parts, the hole is .625 dia. at the top and is .625 deep, irregular shape, I use a .25 ball mill at 30 ipm and .020 depth of cut roughing, and finish at 20 ipm .010 doc flood coolant.
The feeds and speeds can be tweaked on subsequent parts.
mike sr
Re: Feeds and Speeds
Yes Im working with a Tormach 1100. How many flutes would you use on your .250 endmill? Mine has 4 flutes, and I think that has been one of my main issues. Thanks for your help so far.
Re: Feeds and Speeds
currently on the .25 profile I am using a 3 flute, because I had one, a 2 3 or 4 flute would be okay.
For roughing, a 2 flute is good for getting the chips out and is somewhat better for plunging. 3 and 4 flute are better for rigidity and surface finish.
I would reccomend just machining some scrap aluminum to get a feel for the diffeent speeds and feeds using the mdi window.
I cut a lot of wood when I started, just to get a feel for what the machine would do.
I used a Bridgeport for a number of years making parts as needed for my buisness, it took quite awhile to get used to CNC machining as everything a lot faster than what I was used to.
CNC is really nice for multiple parts, not so much for one offs, as the cad cam and tweaking the cam takes me more than one part to get it right!
I have programs that I run over and over, some I am still tweaking!
mike sr
Re: Feeds and Speeds
Don't get too hung up on the 4 flute vs 2. You can drive a 4-flute 1/4" end mill through aluminum a lot faster than you'd expect, especially with coolant.
Re: Feeds and Speeds
I also would suggest watching some of the videos by Tormach and nyc cnc, grimsmo, or any of the videos about cnc machining.
mike sr
Re: Feeds and Speeds
Ok thanks a lot! I think I'll be taking some time to test different feeds and speeds on the scrap aluminum I have. I didn't think about doing that before.
Re: Feeds and Speeds
Also, don't be afraid to run the mills a lot faster than your first post describes as "comfortable". It took me a a little while after going from a manual mill to CNC because I always wanted to baby everything. Once you get past that and drive your end mill, it sounds so much smoother, cuts better, and removes way more material.
My last job on my PCNC 1100 series 3 was in unknown steel (seemed similar to 4140). Roughing at 4528RPM/60 IPM with a 1/2" rougher, .3125" DOC, .02" WOC. Light buzzing sound the entire time, great chips flying and cut my machining time in half compared to the slow and steady approach. These numbers were straight out of HSM Advisor.
My advice: Try the numbers your calcs provide... double check your cam and let 'er rip with the "cycle start". You'll probably be pleasantly surprised and you'll probably break fewer tools. Just be careful with the slider in GWizard, keep it further down to the left until you get the feel for your machine and tooling.
Re: Feeds and Speeds
At the feeds and speeds you have been using, you are rubbing the material off not cutting it. At 1500 rpm and 2 ipm on a 4 flute end mill, you get a .0003" chipload. A good rule of thumb for roughing chipload in aluminum is 1% to 2% of cutter diameter for endmills over 1/8" and about half that for smaller. So for your 1/4" end mill at 1500 rpm, you would need to be running in the 15-20 ipm range. However at 1500 rpm that is no guarantee that your surface finish will be as good as it could be. You are only cutting at about 100 surface feet per minute and aluminum likes to be cut much faster than that. 500 sfm and up isn't unusual.
Tormach is selling some endmills with a coating that is optimized for aluminum: Get to Know Your Cutting Tool: 3-Flute CrN Coated Performance End Mills | Milling Around
As others have mentionned, don't be afraid to push the machine. It is really cool to see the chips come off when you get it dialed in right. You get this constant stream of tight little chips flying everywhere, getting into your hair and onto everything within a 5-10 ft radius. It really makes you want to get an enclosure if you don't have one.
bob
Re: Feeds and Speeds
Okay. Thanks everyone, this has really helped a lot! One more thing. Im not sure if I totally understand what exactly "plunge" means. Correct me if Im wrong, but isn't it just the depth of cut you should run the operation at? If so, does it matter how shallow you go? I know that the deeper you go, the more work your tool has to do, but can it be bad for your tool to run it shallow. If Im going to start testing higher speeds, I would feel more comfortable starting with minimal cuts before moving to deeper ones, unless this is another "playing it too safe" situation.
Re: Feeds and Speeds
It is better to take deeper DOC and a shallower WOC if anything. Otherwise, you will wear out the tip of your endmill and have to throw a way a 95% brand new mill with a trashed end.
Obviously, machine HP comes in to play some point (the amount of power a cut takes is directly proportional to the DOC, so it's a good variable to play with when tuning your cuts). Generally you want to shoot for at least 1x diameter in DOC. When slotting with larger end mills, you may run out of HP before anything else though.
What I normally try to do: keep your SFM near mfg recommendations. Keep your chipload near mfg recommendations. Adjust your DOC until your machine is happy. I am still relatively new to CNC, so take this suggestion with a grain of salt =)
Re: Feeds and Speeds
Plunge rate is the feed rate that the tool descends into the cut. So if your DOC is .05 and your feed rate is 10 IPM then generally plunge rate will be half your feed rate or 5 IPM.
Dave
Re: Feeds and Speeds
While I agree with the other responses that your feeds and speeds are leading to rubbing, once you've broken the first end mill and replaced it with a new, sharp one it should still last fair time, but you don't say how many parts you're trying to make. If you're breaking a "lot of end mills" then I suspect you may also have other issues. How are you evacuating the chips? I've seen videos on YouTube where chips aren't cleared out of holes and the end mill just wades through them. It's very important to get the chips out of there, even more so if you're using a 4 flute cutter, which I presume is not optimized for aluminium, and will most likely have a limited flute depth. Are you evacuating chips with flood or air blast? If not, then flutes are likely to clog and prevent the cutter doing its job altogether - leading to breakage.
You should definitely increase your speeds and feeds but if you're starting off you can get away with quite a lot, you do however need to ensure that you're getting rid of the chips.
Step
