Aluminium – yuck.

[Dave SParticipant @daves59043]

First part.

just a pocket and a boss.

As I have a fair amount of Scrapbinium thought I would try that.

Yuck.  I’ve not got coolant sorted yet,  and that might make some difference, but chip sticking nightmare.

3mm carbide, coated with probably the wrong thing but all my small mills are. 20k rpm, 1200mm/min feed – fusion seems conservative there, although it did try to do 100% step over a lot.

Managed to catch it as it clogged with the pause button and clear the chips then resume, so got a part out without snapping anything (unusual for me 😉 )

Surface finish is smooth, need to check dimensions and I think the tram/nod (it’s literally bolted together and I’ve not verified square yet)

Lots of learning in the tool path generation to do, but the basic machine seems sound 🙂

 

Dave

 

 

 

 

[FulmenParticipant @fulmen]

Anything is better than nothing. WD40, 556 or kerosine should all work. Even plain water would work, but corrosion might be an issue. Isopropyl alcohol is said to work wonders on aluminum, but the flammability probably isn’t worth it.

[John HaineParticipant @johnhaine32865]

Hardly worth trying to mill ductile/pure ali.  IIRC I have a lot of T6061 which mills beautifully, even without coolant/lubricant.

[Dave SParticipant @daves59043]

Don’t actually know what grade it is – came from a previous place of work, where it formed part of the product.

It was previously machined, suspect it’s a 6000 series based on what it was used for.

I think the main issue was chip recutting/not clearing, and the coated endmill…

I applied wd40, but it’s a spray bottle and so not that good at clearing.

 

[Nigel Graham 2Participant @nigelgraham2]

If you are going to try WD-40, try white spirit. It might be cheaper for much the same. WD-140 is thin oil dissolved in white spirit.

[Julie AnnParticipant @julieann]

We’ve all been there and clogged cutters and drills!

Most aluminium alloys machine reasonably well. I have mostly used 6082 and that machines fairly cleanly with a few caveats such as using lubrication/coolant. A few comments:

• Don’t use stuff from the scrap bin, it is unknown and might well be unsuitable for machining.
• Use the largest cutter possible given the tool path; it could be bigger than 3mm looking at the part?
• Use a cutter intended for aluminium, they have larger flutes, are polished and are not coated. Some coatings, such as TiAlN, encourage aluminium to stick to it.
• Ignore feeds and speeds from Fusion, it’s a CAD software package. Go with cutter manufacturer charts as a starting point. For the 3mm cutter you are running too high an rpm with too slow a feed. Speeds and feeds vary according to the type of cut so adjust them as needed. Manufacturers data usually specify cutting data for a range of cut types, eg, deep but shallow width or full width slotting.
• Climb milling helps and, without coolant, gives a much better finish.
• For manual milling of aluminium I use the odd squirt of WD40, for CNC milling I use flood coolant, as well a preventing sticking it washes the swarf away.

Hope that helps.

Julie

[VicParticipant @vic]

I’ve had this happen a couple of times. I put some of it down to the wrong type of cutter (coating), but maybe I was feeding too fast as well. At least you can reclaim the cutter by putting it in caustic soda.

[JasonBModerator @jasonb]

I think Julie has covered most things.

Aluminium is the only thing I cut with some fluid, small jobs just brushed on paraffin, and for larger I add the liquid to the air as I don’t want to stand there for a couple of hours brushing it on.

All use air to keep the chips out the way.

Uncoated ali specific cutters and climb cutting for me.

You don’t give cut details but generally if using the full width then the feeds need to be quite a bit less than if using just the edge particularly as the cutters get small.

Not sure what you looked at on F360 but a 3mm in aluminium comes up at 12,000rpm and a feed of 1200mm/min so your 20K was fast and the feed slow for that given spindle speed. They also assume flood cooling for those rates so you need to adjust them for dry or minimal lubrication and chip clearance.

I’d only be using a 3mm if the job specifically needs it such as where a larger cutter won’t fit or I want to leave a small internal fillet. Even then I may rough with a 6mm and then go back and do rest machining with a smaller cutter.

If in doubt start with a conservative feed and if all is going well you can overide the feed as the job progresses but do watch out as certain path types will do a full width cut first as they start a new area before stepping over and it is those that can often catch you out and start th ebuild up.

[Dave SParticipant @daves59043]

I foresee some polished uncoated carbide in my near future.

All my current stash of end mills have a coating of one sort of another.

The speeds and feeds seemed about right to me (I set them), so maybe I’ve misunderstood how to figure them out:

3mm cutter @ 20Krpm has a surface speed of 188 m/min according to the fusion calculator.

That seems to fit with the general speeds I’ve seen in tool data sheets – possibly on the lower side.

Then a 3 tooth cutter at 20K rpm and 0.02mm per tooth is 1200mm/min (again the fusion calculator).

I thought a good general place to start was 1 thou per tooth (I know I’m 0.005 short), and then rpms to give the SFM?

I didn’t think a huge shipload on a 3mm cutter was a good place to start, and the chips (you can see some in the pic) are swarf like, even if they are tiny swarf…

 

Dave

 

 

 

 

 

[JasonBModerator @jasonb]

Couple of numbers

YG-1 Alu-Power, 3mm 3-flute. 7000rpm 0.035mm chipload slotting, 0.045mm sidecutting(adaptive)

Put a corner radius on that and they up the revs to 10000

YG-1 A+ can run faster at 25K for a 3mm 3-flute but chip load is much lower at around 0.01mm.

APT55degree 3mm 3-flute 25K and 1800mm/min feed for edge cutting but drop that by upto 70% for slotting.

All this are based on flood coolant

Those big engagements where your little man has his spanner are going to be what is loading up the tool, not quite sure what you had set to leave those. Also you could reduce the tool stickout, hold at least upto the coating or right to the top of the flutes

[Dave SParticipant @daves59043]

The big engagements are where the model stock isn’t. I trimmed a big slot first, but I guess the tool path ran further out than I thought.

Ive not got a vice sorted yet, so I left the stock long so I had something to clamp on without crashing into the clamps.

So aluminium chip load as a starter point should be quite a bit bigger per tooth?

This is the stuff I have not experience with – my manual mill chipload is how much ‘feels’ about right, and how fast can I crank the handles in some cases…

why does the chip load drop when running faster rpm?

I designed this to have flood, hence the enclosed sides and the tray under it, so that’s on my list, but Ketan seems to be out of neat little flood coolant boxes at the moment.

Dave

[JasonBModerator @jasonb]

Around about a thou or 0.025mm chip load is not a bad starting point. When using the side of the cutter and small stepovers the actual load is a lot less than when slotting due to chip thinning.

My typical setting is 0.033mm or about 1.3 thou. For most materials combined with a vertical cut of 1 x dia of the tool x a stepover of 0.1 x dia.

So for adaptive cuts with a 6mm dia 3-flute I would be running my max 5000rpm, feeding at 500mm/min cutting 6mm high and stepping over 0.6mm. A 4mm cutter would also be same speed & feed but 4mm vertical x 0.4mm stepover.

I’ll adjust these to suit the job in hand so if the part is 8mm tall I won’t do a 6mm and a 2mm cut but one of 8mm and maybe reduce the stepover down a bit to 0.5 rather than 0.6 for a 6mm cutter.

It’s worth just setting up a block and taking the same cut off it at increasing feed rates to get to see what the machine can do, mine is OK upto 1000mm/min with it’s 5000rpm max on Aluminium but I’m more likely to run 5-600mm as I can keep up with swarf control and it will happily do that for a few hours non stop without getting the spindle too warm.

 

 

With my adaptives I’ll usually leave 0.3mm radial and axial material snd then use either a 2D contour or 3D Horizontal to finish those and may well push vertical to the full flute length of the cutter but stepover 0.2, then 0.1 and slow the feed 10-20%

 

[Dave SParticipant @daves59043]

Thanks for the tips. I’ll give the block tests a go. Presumably just a set of move, step and move using feedrate / spindle override to vary the cut?

first a clean up of yesterdays swarf and some measuring for spindle tram, nod and general squareness.

Dave

[JasonBModerator @jasonb]

Yes, I was just over riding the feed rate and resetting Y zero after each cut. But remember they will be for side cuts so slotting may need less though if it is a pocket I generally cut down into it with a helix and then use adaptives to remove the waste just like the outside cuts.

I did find a video where I am using a 3mm cutter. Details in the description below the video but you can see I used a slower 200mm/min feed for the helical ramp and once to depth took it back up to 500mm. You can also see the final two contour passes to remove the slightly facetted surface that the adaptive leaves.

With a higher spindle speed you can run these cutters faster and the feeds will go up proportionally but build up to it.

[Julie AnnParticipant @julieann]

I looked up some of my old 6082 aluminium alloy CNC machining parameters.

First one: 6mm 3 flute carbide cutter cutting 16mm deep and 6mm wide slot, so full width engagement. Depth per pass was 2mm, speed 4000rpm and feedrate 720mm/min for a chip load of 0.06mm.

Second one: 2mm 2 flute carbide slot drill cutting 4mm deep, 2mm wide slots, full width engagement as above. Depth per pass 1mm, speed 4000rpm and feedrate 150mm/min for a chip load of ~0.02mm.

Julie

[Author]

Posts