Speeds and Feeds Aluminium broken end mill

[al010964]

Hi All,

I have my first 3D part that I am trying to mill out of Alu 6061 T6 on the 770, using the following below end mill and speeds and feed from Gwizard.

1/4 3FL Carbide End Mill SE 38 Deg Helix 1.125 loc ZrN Coated
Feed 16
Speed 2500
Cut Depth 0.016
dry cutting

The program takes about 2 hours to run, and is a mold for an rc plane part.

Got about 5 minutes in and managed to snap the end mill, have I gone too conservative on the speeds and feeds ? looking for a quality finish to reduce sanding an polishing time.

It hadn't cut cleanly ..... which I thought may be due to the small depth of cut but it looks like it has started to melt along the edge.

I was getting some chatter but not lot.

Any thoughts.

Thanks in Advance.
Adrian

Similar Threads:

• Tuning my feeds and speeds and my mill
• Aluminium milling speeds, feeds & cutting oil
• Newbie- speeds and feeds insert mill
• Micro End Mill Speeds and Feeds

[dblox]

With such a low depth of cut I'm surprised you are having trouble, but 2500 rpm is unusually slow for a carbide cutter that size in aluminium so you might try upping the RPM to whatever maximum your machine has and adjust the feed per tooth to about 0.03mm.

If coolant is unavailable you need to try using a blast of compressed air to help keep the chips from melting inside the cutter flutes and breaking the end mill. This may be what happened to you given that the chip load was fairly high for dry machining.

[philbur]

Don't know how you managed to come up with 2,500 rpm for a 1/4" carbide cutter.

Try 8,000 to 10,000 rpm and up the feed rate by 50 to 100%.

16 ipm is too fast for 2,500 rpm and 2,500 rpm is way to slow for carbide on aluminium.

The basis for any calculation is the surface speed per minute for the cutter material/part material combination. Everything else is based on this parameter.

You should make yourself a table for each combination you use and use it as an approximate check when you run a calculator.

Phil

[mike sr1]

I use .22 doc
4000 rpm
20 ipm
With coolant
.250 carbide ballmill 4 flute
series 3 1100
I am machining a 3d hole in a part with this cutter.

The coolant will help clear the chips and get rid of the heat.

[al010964]

Thanks guys,

Will ramp it up to 8000 and run at F26 which will give me the 0.0011 chip loading.

Phil - ignorance lets u come up with all kind of random ideas

Cheers,
.adrian

[jrm850]

When I run your setup in gwizard it comes up with 10000rpm and 60IPM for a .002IPT. Do you have any of your fields locked in Gwizard?

[riabma]

Hello,

With a 6 mm 3F carbide end mill I am using this parameters:

4800 rpm
880 mmpm
180 mmpm (for vertical plunging)
DOC: 1 mm (depending the geometry)

I am making a final pass at 3000 rpm for finishing with the same feeds (almost cutting air).

Of course, with coolant. The finish is good (at least for me).

I hope it helps.

Ricardo

[txcncman]

If you do not want to run coolant (flood or mist) at least consider air blast for chip removal. Recutting chips just causes extra heat which then causes the aluminum to weld itself to the tool. Which then in turn causes breakage.

[al010964]

Hi All,

Thanks for all the feed back, made a few changes after going and buying an air compressor.

(a) Now running fogbuster with coolant
(b) Clearing chips with constant hi pressure air
(c) changed code to 8000 rpm and f48 ipm and chip load sitting at 0.002.

Managed to break the other (second last) 1/4 cutter, it broke along the centre section as it enters the left square (i.e. not on a plunge .... the machine sounds like it was kind of laboring during all the cuts (however not sure as to the noise it should make as I have only cut plastic to this point). It wasn't what I would call really uncomfortable sound .... if that makes any sense.

I have included a photo....

Starting to think maybe the cutters are the wrong ones ... or another random thought ? could it be a motor / belt problem I had the spindle stop mid cut when i tried to make a 0.1 cut with the tormach face mill the other day, same material. I don't think the belt is slipping, but I think the motor did stop in this instance.

I only have one more 1/4 cutter which is a ruffer .... happy to take on some more input before I break this one as I will need to order some more in once this one is gone as you can't buy them locally.

Happy to post code if that helps.

Cheers,
Adrian

[txcncman]

Looks like it was not cutting at all. Those ragged edges are the main clue. Almost as is the corners of the endmill were gone from the start. What was your plunge feed? I rarely plunge more than 1 IPM. Sometimes you can get away with 4 IPM when ramping in. Was the endmill pulling out of the holder and cutting deeper as it went along?

[Steve Seebold]

Hi All,

Thanks for all the feed back, made a few changes after going and buying an air compressor.

(a) Now running fogbuster with coolant
(b) Clearing chips with constant hi pressure air
(c) changed code to 8000 rpm and f48 ipm and chip load sitting at 0.002.

Managed to break the other (second last) 1/4 cutter, it broke along the centre section as it enters the left square (i.e. not on a plunge .... the machine sounds like it was kind of laboring during all the cuts (however not sure as to the noise it should make as I have only cut plastic to this point). It wasn't what I would call really uncomfortable sound .... if that makes any sense.

I have included a photo....

Starting to think maybe the cutters are the wrong ones ???

I only have one more 1/4 cutter which is a ruffer .... happy to take on some more input before I break this one as I will need to order some more in once this one is gone as you can't buy them locally.

Happy to post code if that helps.

Cheers,
Adrian

What are you using for coolant in your FogBuster? Are you conventional cutting or are you climb cutting? If you conventional cut, you don't really cut the material, you just push it out of the way.

What is your entry method? If you plunge, you're most likely going to gum up the end mill in the way down. Then when you start to move sideways with an end mill that's already gummed up on the bottom, you're probably going to break it. I would suggest you either helix in to your part, or ramp down.

Something you need to remember, THE ABSOLUTE BEST WAY TO INSURE THAT YOU WILL BREAK A SMALL CUTTER WHEN YOUR SHOP IS 100 MILES FROM YOUR TOOLING SUPPLIER, IS TO ONLY BUY ONE.

[mike sr1]

That looks like a big burr being pushed up along the outside cut of the part, if thats the case youre still generating too much heat. If the spindle sounds as if its laboring with a .250 cutter then its pushing the metal out not cutting it.
At those speeds and feeds the cutter can get hot with that type cooling, I use about 3500 to 4000 rpm, 15 to 20 ipm .020 depth of cut on 6061 aluminum with flood coolant on one particular 3 d part and there is no discernible burr on it.

Make sure your spindle is turning clockwise if its a right hand cutter.
If the cutter is sharp and the rotation is correct and you have cooling, there should be no large burr on the material being cut at the speeds mentioned above.

I have seen aluminum cut like that before but it wasnt 6061 t6, some grades arent "free machining"..........

[philbur]

Judging by the photo there is something seriously wrong happening with the cutting action. It seems to be mostly melting its way through the path.

Have you checked the actual rpm of the spindle. Is it in the high ratio. Is it rotating in the correct direction.

Have you looked closely at the cutters, what make are they, do they have positive relief angles on the flutes. Are they center cutting. Is the cutter loaded with melted aluminium when you finish the cut. Photo of the cutter please (all angles) before and after cutting.

Several years ago I achieved something similar to what you have but worse. The Gcode called for a plunge start and I had, without thinking, loaded a 4 flute none center cutting 0.5" end mill. It partially melted its way into the plunge, loaded the cutter with aluminium, and then started to melt it's way round the tool path. I got quite some distance before I realise something was wrong, I wasn't paying attention. The result looked very similar to yours but worse, my depth of cut was something like 0.2".

Phil

[al010964]

Hi All,

Appreciate you guys sticking with me on this.

I will answer the questions in a list, and not via contributor (to make it easier), apoligies in advance.

(a) Photo attached ... sorry don't have a before photo

(b) Cutters are maritool, spec's of the last tool are:

Centercutting: Yes
Coating: ZrN
Cutting diameter: .250
End style: Square
Flute length: 1.125
Material: Solid Micrograin Carbide
Number of flutes: 3
Shank Size: .250
Total Length: 3.00
38 deg helix end mill

(c) Yes mill is spinning in the correct direction

(d) It is on the correct pully's, for the speed, mach3 indicates 8K but I haven't checked it beyond that.

(e) positive relief .... not 100% positive on this one hower the cutter sweeps forward in direction of motion if this is what you mean, by the looks would say 38 degrees ?

(f) I was using axial plunging - now considering using spiral @ 15 degree to try something different.

(g) I did have the milling type as both conventional, will change this to climb only.

(h) Using Premier 600 lubricant + de mineralized water ration 10 to 90.

(i) am pretty confident that the alu, is 6061-T651 as i have a mill certificate, and reputable shop.

(j) This last cutter was brand new - never been used.

(k) It does have a little bit of gumming up, not a lot see photo

(l) Plunge I had set to 16?

Included a photo of the last 1/4 inch mill that i have it is a ruffer.

Note the worst of the burr is from the first cut at slow speed..... ie the first cutter and pass, that broke

Cheers,
Adrian

[philbur]

That makes a big difference. I think you need to stop trying to make your part and use the current part for practice.

From what I see you clearly have a temperature problem which either comes for lack of cooling or from pushing things to hard, or of course both.

So without flood coolant I would reduce the speed to 5,000 rpm and reduce the feed to 12 ipm just to see what happens. Just cut a staight path on the side of the part with say 25% step-over. If you are still pushing up a burr then stop and have a rethink.

Phil

Not the worst of the burr is from the first cut at slow speed..... ie the first cutter and pass, that broke

[al010964]

Ok .....

Sorted out my woes ... simple answer... stupidity ! however I can't explain something.

The short answer is cutter was going ccw.

I thought I noticed this when I dry ran the part e.g. cutting air. So i stopped the spindle in Mach 3 as I was in single blk mode (going through a zillion lines of code) and started it again, and it started up CW. I did this is about 3 times to confirm and simply thought my mind was playing tricks when it started for the first time.

Anyway after responding below, that it was going in the right direction it was playing on my mind so went through the code ... still learning G and M codes.

And noticed that it was set to CCW in the code ... (my screw up.) !

However I was able to repeat the above again i.e. ccw stop spindle, start spindle with the mach 3 button. and it re-starts it cw.

Is it supposed to do this ?

Thanks again for every ones help .... as it was doing my head in.

Cheers,
adrian

p.s. my first complete 3d part

[SCzEngrgGroup]

I have, more than once, seen GWizard generate completely wacky numbers. This looks like just such a case. Something seems to get "stuck" internally, and it stops updating come parameters. 2500RPM is obviously WAY too low for such a small cutter. Re-start GWizard,re-enter the parameters, and I bet you see completely different numbers.

Regards,
Ray L.

[MichaelHenry]

Is there any chance that you are running the spindle with reverse rotation or that you are using left-hand cutters?

[BobWarfield]

Yep, as he said, he ran CCW. That'll get you every time, LOL. Did that one time my self. The bad news is even if you catch it and reverse direction, you've seriously dulled the cutter if the material was at all hard. OTOH, I have seen machinists recommend doing a pass this way with like a thou of cut depth to get a burnished finish using an old dull endmill. Never tried it, but it is an interesting idea.

BTW, nothing wrong running 2500 rpm at 16 IPM. That's about right if you want to override the rpm's recommended by G-Wizard. The main thing would've been to avoid too little chipload, and in this case, he's right on target with that value. It wouldn't have been rubbing.

OTOH, no particularly good reason to run that slowly either.

Also, other than Ray just now, I haven't had a report of odd values popping up. Ray hasn't been a legal user since 2010, so hopefully whatever had befallen him is no longer a possibility. You should only get such values if you override, in which case a little padlock pops up to indicate what's happening. If you can duplicate a case that behaves otherwise, I'd love to see it. The code is simple enough though that I will be surprised to find it happening.

Cheers,

BW

[al010964]

Hi Bob,

I did over ride the default spindle speed, I don't believe I was getting any odd results. And put the whole thing down to wrong rotation of the spindle.

I have now (re) read up on the mach 3 documentation and now under stand how the spindle button works, in Mach3. As I thought i was doing a check, of the rotation direction; when I was actually changing the direction it was spinning.

Thanks again for everyone's help!

Cheers,
.adrian