PDA

View Full Version : First cut in aluminium. Disaster.



Edward
27-01-2017, 12:37 PM
With my Sieg2.7 mill all cnc converted, I have been testing it with a few scrap pieces of Delrin, cutting pockets holes, etc, to fit various ballbearings.

This helped me get acquainted with Fusion360, using Adaptive clearing first, then finishing off with 2 passes of Contour, etc.

So far so good, perfect and smooth results and I was feeling quite smug:)

So this morning I tried aluminium for the first time, just a typical hole of 30.05mm on a 15mm thick scrap, like you would do to fit a ballbearing, so I could check accuracy and so on.

My feeds were 200mm/min and the adaptive cut was set to 2mm both for radial and plunge. 8mm endmill, at top 2000revs.


It all started very well......but then, as the endmill got close to the periphery of the 30mm circle, disaster struck. The whole thing jammed. Luckily I was there to press the e-stop and no major damage happened. I lifted the Z. The endmill had some aluminium welded to it, I tried to snap it off, but it is too welded, so goodbye endmill, it was nice while you lasted:) F&^%*

So next time I will be more conservative, maybe I will reduce the feed to around 150mm/min and the depth (both radial and axial) to around 0.4mm. I know this will be fine because I regularly use this when milling manually on another smaller mill. If successful, I will increase this depth as I gain experience, just to find the limits of the machine, which I reckon may be at around 1mm deep at 150mm/min or thereabouts. Trial and error.

Any advice?

Edward

Dangle_kt
27-01-2017, 12:43 PM
I had the same problem, chip weld isnt really about speeds and feeds from what I can tell (well it might be if they are way out I suppose).

Anyway - chip clearance is critical, as is the right endmill - to begin with try 3 flute HSS endmill of a decent size, and use compressed air directed at the endmill at all times.

I used a 3 flute endmill, but it was TiLAN coated, and thats no good for alu! OOPS! Lesson learned, either plane carbide or HSS for Alu.

Edward
27-01-2017, 12:55 PM
Thank you. It was a nice 8mm carbide endmill that I normally use with manual milling and it cuts nicely, though I normally go a lot more conservatively. I have the helicoidal ones made for aluminium too, but in any case, I think the depth I set was quite brutal for this machine, even though the manufacturer recommends 3.2mm cuts, but of course this is for big professional machines.

Edward

Dangle_kt
27-01-2017, 01:32 PM
Am I right in thinking it was cutting ok at first? If so its not the aggressive cut that was the problem.

The more extreme cut will make many more chips, which need evacuated - When I get chip weld its from a build up, once it starts it then snow balls. What were you using to evacuate the chips?

Edward
27-01-2017, 01:57 PM
I think it soon started to clog up, as you say, progressively, I was vacuuming the swarf as it happened. I am now going to try the same, but reducing the feed and depth, so how it goes.

bikepete
27-01-2017, 02:07 PM
Also try squirting on some WD40 as a cutting lube - may help prevent sticking...

njhussey
27-01-2017, 03:36 PM
Blowing air is much better for clearing chips than vacuuming.

Ideal scenario is an 8 mist system from ebay coupled to a pot of WD40 and a compressed air supply.

Sent from my HUAWEI VNS-L31 using Tapatalk

komatias
27-01-2017, 03:57 PM
Reducing the feed will not do much. You need to evacuate the chips and keep the cutter cool.

With a carbide tool on, I have in the past, when out of soluble oil, just used compressed air with fine results.

That said, how many flutes endmill did you use? Not good to use 4 unless you know what you are doing. Preference is 2 with a rapid helix to assist evacuation.

Edward
27-01-2017, 04:04 PM
It was a four flute normal carbide end mill, and not the ones designed for aluminium.

I have now tried the same but with a reduced depth of cut and reduced feed and it has done it well, albeit taking quite long.

Guys, I have a lot to learn regarding the optimum feeds and depth of cut, and lots of tests to do, I don't want to run before I can walk. But I thought I would post my first experience as I am sure many of you have been there too:)

Thank you for all the suggestions.

njhussey
27-01-2017, 04:12 PM
Best way is to do what you've done, try...ask...listen then try again, ultimately only you'll know what works for your machine best which you'll find by trial and error. You'll snap bits, ruin work pieces and all that before you find what works!

Sent from my HUAWEI VNS-L31 using Tapatalk

Edward
27-01-2017, 04:16 PM
Absolutely, making mistakes is part of the process of learning. I'd better stock on some more endmills then")

Edward

njhussey
27-01-2017, 04:28 PM
Get some 2 flute ones or single flute....I get mine from APT, not the cheapest but good service.

Sent from my HUAWEI VNS-L31 using Tapatalk

Zeeflyboy
14-02-2017, 11:19 AM
Just FYI for future reference, if you can't get the chip weld off then just buy some caustic soda (better to go with pure than drain cleaner) and it'll dissolve the Alu but leave the carbide.

I've also had some great success with single flute aluminium end mills from aliexpress - there are some very high quality ones and they don't cost a fortune... but friendlier to high rpm and feed.

Some Alu is more gummy than others too - do you know what type you were milling?

Zeeflyboy
17-02-2017, 03:56 PM
This thread actually reminded me that I had two gummed up roughing bits that I needed to sort out. totally welded solid and couldn't pick it off.

Bits before:

http://i.imgur.com/CohLwa3.jpg


Magic stuff:

http://i.imgur.com/ESUXXvB.jpg


bubbling away (and no I wasn't using the hob on bare glass, it was just the best place to put it with the extractor right above):

http://i.imgur.com/hHcLJze.jpg


Magic!

http://i.imgur.com/hfv0uiu.jpg

Robin Hewitt
17-02-2017, 04:27 PM
Make sure it is not pure aluminium, almost impossible to cut. Is it rucking up in front of the cutter? Always a risk when you grab a piece of "scrap" :culpability:

A_Camera
17-02-2017, 08:14 PM
This thread actually reminded me that I had two gummed up roughing bits that I needed to sort out. totally welded solid and couldn't pick it off.

Bits before:

http://i.imgur.com/CohLwa3.jpg

I had pictures like this in my mind before I decided to try and make my first cut in alu, so I was very surprised that it went so well for me.


https://youtu.be/LFFyb2XtpkE

I was so glad to see the aluminum chip spraying, and the end results were really nice.



Magic stuff:

http://i.imgur.com/ESUXXvB.jpg

Good to know in case I need it next time. Did some more aluminum since the first time and the results have been good so far.

I am using 4-flute, dry milling at pretty high RPM and feed rate and it seems to work well on the material I used so far.

Zeeflyboy
17-02-2017, 08:27 PM
Yeah it generally only happens to me when I'm trying out a new bit and figuring out limits or pushing too hard without lube (oi oi sailor!)

I usually use single flute with aluminium and it works a treat - check out the size of these big beautiful chips!


https://www.youtube.com/watch?v=kUc4bTgPjoI&feature=em-upload_owner

A_Camera
17-02-2017, 10:23 PM
Yes, single flute means bigger chips but also slower feed rate and higher rpm. Anyway, I just started with aluminum so I will experiment. What I can't do is using cutting fluid, so I will experiment without. I understand that tool wear is heavier without but that's OK.

Zeeflyboy
17-02-2017, 11:00 PM
Depends what spindle you are using - when you have the 2.2kw 24krpm spindles Like I'm using there they really don't perform well at low rpm, so for good alu cutting on them you need to either have unrealistically high feed rates for a hobby machine where you start running into rigidity issues, or you need to move to something like a 2 flute or single flute cutter.

I wish there were some 12,000rpm options in the water cooled spindle variety at around 2.2kw but it seems you either drop down to 8krpm max (and those are massive!) or stick with the 24k rpm and try to make do with single flutes etc for the best results.

JAZZCNC
18-02-2017, 03:24 PM
It's all about how you approach the job with high speed spindles. If you use 3 flute roughing cutter you can hog away big lumps at good feeds then finish with full depth pass. Works out quicker and cheaper because less wear on tooling.

Now to the OP your always going to struggle with 4 flute cutters with such low feed rate. Know this is going to sound crazy but needed to be more aggressive not less.! . . You really should have been double the feed.

Ukmiller
12-05-2017, 12:31 AM
I would cut alloy at 6000rpm and take smaller cuts and go faster on the feedrate with coolant on.
If the chips get big then it will jam up.
My machines have flood coolant.
The ideal would be air jets to blast out the chips.

Boyan Silyavski
13-05-2017, 08:34 AM
On a small mini mill i dont see how a good result will be obtained when deeper cuts than 1mm??? Normal 2 flute carbide cutter 30 degree upcut will give best results all over. 5 euro from China. There are better made for aluminum bits but they are not made for small machines anyway. They are made for serious machines and can give much higher material removal rate, which in this case is not viable.

What aluminum you are cutting? No name piece of aluminum could be absolute shit to cut. Buy only aluminum alloys made for certain purpose.

From my experience i can cut using any bit up to 3 flutes. Even straight ones or carbide tipped made for wood only. And result is always perfect. The key i say again is the machine rigidity. Any vibration heats the process excessively and things happen. Use the HSMAdviser calculator and you will see that perfect cut is never so deep as many people think.

As a general rule of a thumb that perfect cut happens at 12k rpm 1500mm/min 1 mm depth with any bit 6-12mm.


the tool stick-out is the another detail you should pay attention to. As even if machine is sturdy, the unnecessary stick-out changes the game quite much.


21618

Ukmiller
13-05-2017, 09:45 AM
I have some end mills that are the following spec.
12 diameter 4 flute.
30mm flute length.
42 degree helix.
Solid carbide with a high hardness rating.
They are what i use for every material.
I can use them on plastic and alloy and stainless no wories.
If i am cutting an external profile in alloy i can go full depth cut and cut with the side of the cutter and cut 1mm off the profile at 3000mm/ min with coolant on.
Internal holes and pockets i just run 0.5mm cuts at high feedrate so it doesnt take long anyway.
But we dont do high volume work so thats ok to us.
Maybe if we had a high volume we would have to use specific alloy cutters to speed up internal machining

Edward
13-05-2017, 10:57 AM
Well, since I originally posted, I've been learning a bit about my mill and no more endmills have been broken.

I now use the Alu-power carbide 2 flute and 3 flutes from Cutwel. They are a little more expensive but they work well. I know it's overkill but I like good quality sharp and shiny tools :)

My mill can only do 2000revs. which I always use.

Using Fusion360 with Adaptive to cut a pocket or remove material I use an 8mm 3 flute cutter, Helix plunge down fairly slowly (20degree angle) to about 6mm depth with a plunge feed of 300 and WOC of 0.5mm. Once it reaches the 6mm depth, I go faster at 350 feed and 0.5mm to enlarge the pocket. Then repeat the same with the next 6mm depth and so on.

I use no coolant or air, just a vacuum to suck the swarf. No problems at all at these settings.

It's fairly conservative, I am sure I could go deeper at these settings.

I have tried more WOC, up to 1mm, but that's when the problems start. The TTS type tools can start pulling out of the collet with the consequent accident to follow.

I am sure that if I just used a normal R8 collet only, I would be fine with 1mm width cuts, but with an 8mm cutter it seems to be too much force for the collet to grip the TTS tooling properly. It's fine with smaller diameter endmills though.

Edward

Ukmiller
13-05-2017, 11:03 AM
2000 is quite slow for alloy but if you have no coolant or air then i would say you couldnt go any faster anyway.
Aluminium melts so easily and can break cutters

Edward
13-05-2017, 11:20 AM
This video shows it all, fairly slow plunging, then faster feed (350mm/m) when it reaches its depth. 6mm tool at 2000revs. Using adaptive, leaving 0.2mm to the sides, then finally Contour to finish off to size. Then a tool change to a chamfer tool. This was a test for small ball bearings holes. They fitted to perfection.


https://www.youtube.com/watch?v=c8XeTECem5M


Edward

Ukmiller
13-05-2017, 05:00 PM
That shows how you machining very clearly.
I would get sacked if i machined that slow though!
But we have 6000rpm and coolant blasting.
Can i ask why you cut clockwise?
I always cut holes anticlockwise to reduce chatter.
Try running the same program the other way to see if it improves the finish you get.

magicniner
13-05-2017, 08:32 PM
I would get sacked if i machined that slow though!

Surely if you had good reason no one could argue


But we have 6000rpm and coolant blasting.

And having 3 times the spindle speed would seem to be a contributory factor in allowing you to cut faster?

Edward
17-05-2017, 01:58 PM
That shows how you machining very clearly.
I would get sacked if i machined that slow though!
But we have 6000rpm and coolant blasting.
Can i ask why you cut clockwise?
I always cut holes anticlockwise to reduce chatter.
Try running the same program the other way to see if it improves the finish you get.

I think I machine at the speed that my machine allows me to, give or take. I could use coolant or air, but I am happy to compromise and go slower without it.

Regarding climb or conventional milling, as you can see in the video if you have the patience, or fast forward, as I know these videos can be boring, I do the Adaptive clearing in Fusion360 using conventional milling and then as a finish pass I do a last pass (Contour in Fusion360) using climb milling removing the last 0.2mm. This gives me a perfectly shiny and smooth finish, in fact, as good as what I get from any professional workshop.

Regarding the alloy, I normally use 6082T6 which seems to machine fine to me.

So I am happy with a general feed speed of around 350mm/min. WOC around 0.5mm at 2000revs. If and when I have the need for faster speeds, I will build myself a nice router and I will study the good advice that this forum contains. Or I will convert a larger mill. I think for the moment I have a nice little mill that is sturdier than many a cheap router, and does what is supposed to do quite nicely, albeit relatively slowly.

Yes, I broke about 4 endmills at the start, but now things seem to have settled down and if something breaks, it's usually my fault.

Edward