Speeds and feeds for 6082 T6 alloy

[Dean jeffery]

Need a little help on a more reliable cutting process, the only issues I'm having is profiling and was going just fine for about 6 off of the pictured parts.

I'm using a HSS uncoated 3 flute 6mm ripper from cutwel speed was 13500 feed 2500 DOC 1mm 10mm deep, using mist on my cnc router.

Then did some new parts and that's when it went tits up, I used a new ripper for a custom high profile part and gummed up within 2 mins of running same speeds and feeds.

Put the old tool back in and went fine I sent the new tool back to cutwels and they sent a replacement, they said the other was faulty but no tech report.

Now I've made a couple more this weekend and on the second part it started to load up, they said the new tool as been checked and pasted off.


Now I need a more reliable cutter or speeds and feeds, I've got a decent batch of these parts to make and reluctant to make them.

https://uploads.tapatalk-cdn.com/20180212/bf49bcd9c795ededb41a80787f15f8bf.jpg

https://uploads.tapatalk-cdn.com/20180212/d14f467659d598d231616102bc2ebe03.jpg

Not issues with the finish at all

https://uploads.tapatalk-cdn.com/20180212/f1d76a290579f95e078b0e536240fbe6.jpg

[johngoodrich]

well going by cutwels data they recommend 6300rpm and 280mm/min so I think you are going much too fast for it.
https://www.cutwel.co.uk/FileDepository//ProductId%20-%2074/Cutting%20Data%20E2752.pdf
is there any reason you are using a ripper for it? I would personally use a 3 flute carbide end mill with the same doc and speed but about 1500mm/min. I use a lot of these:
https://www.shop-apt.co.uk/3-flute-carbide-end-mills-for-aluminium-45-helix-uncoated/3-flute-carbide-end-mill-for-aluminium-6mm-diameter-45-helix.html

[Dean jeffery]

Got this app and it came back with those results, but checked again and change quite a bit.

https://uploads.tapatalk-cdn.com/20180212/b00582d608a517ec5f67ca423c3e1d90.jpg

Used a ripper because there are roughing specific so thought that would be the way to go, I use a 4mm solid carbide for finishing 3 flute.

[Dean jeffery]

Ripper info from that same site mate

https://uploads.tapatalk-cdn.com/20180212/e574adc2202a0c95441ca74394449b96.jpg

[Chaz]

Those are guidance and machine specific.

Try uncoated 2 flute endmills for alu (both for roughing and finishing). Roughing 3 flute endmills (corn cobs) work well and like to be driven hard (much harder than you expect) but you must keep chips (or swarf) away from the flutes.

[Dean jeffery]

I use those corn cobs for roughing out carbon fibre, prices are peanuts cheap and swap out after half hr use.

Not tried with alloy though

[Washout]

Hi Dean

A lot will depend on your machine type, rigidity etc. but:

I use 6082 for almost all my projects and use a 6mm 3 flute serrated carbide rougher when clearing lots of material and when cutting out. Both use a trochoidal or adaptive clearing strategy using 15,259rpm, 2.4mm stepover, 5mm DoC and 1,779mm/min.

I've gone a lot deeper with adaptive strategies, but my machine does have its limits.

For clean up (especially the scallops adaptive leaves) and the horizontal lines from the serrations I use a single flute carbide cutter (6mm again) with 19,900rpm, 0.5mm stepover, 5mm DoC and 1,458mm/min.

I use quite a few other tools but you can check my feeds and speeds on my videos - latest one here:


https://www.youtube.com/watch?v=B2T5Uw0FLEU

[Dean jeffery]

Cheers mate

Machine was made by Dean on here and it's a capable machine but I'm limited in cut methods with using Vcarve and that's all the more reason to dial in speeds and feeds.

I've ordered some of those cutters John linked above, slower feeds that I was using with the ripper but will only add a few mins per part but could save time in the long run.

[Washout]

Ah if its one of Dean's then it should easily be able to to handle my feeds and speeds. In fact I'm surprised you aren't taking flak for going too gently :tongue:

I would also agree about the limitations of vCarve/Vectric products. I have Cut2D/3D and vCarve and they were fine to get started on, until I got into Fusion 360 and adaptive clearing, which frankly have been a game changer (iMachining and Solidworks are even better, but you need deep pockets).

[Dean jeffery]

Yeah it's been a great machine around 19 months old now.

F360 and the likes is a bit to much of a learning curve, I don't have the time to learn it work loads increasing and limiting even custom work.

But adaptive would band those alloy parts out way quicker, still only takes 28mins minus cutter changers.

See the vid just starts to change tone last pass.

https://youtu.be/PYtKZlAzJA8

[JAZZCNC]

Yeah it's been a great machine around 19 months old now.

Bloody hell Dean can't believe been 19mths.!!.... Seems like 6mths. The machine does well to say was never really designed to cut aluminum.!

Listening to that video you need much more air you can hear it re-cutting chips this will cause extra heat with high potential to weld chips to tool also give a poorer finish.
Does your cam software have a function to use spiral tool path? This helps keep constant tool engagement and also quicker and easier on tools because not retracting and plunging at end of each pass.

Also because of high spindle speed/low torque you really need carbide tooling. HSS requires much lower RPM and these spindles don't have enough torque at low speeds. These spindles provide most torque at full RPM so the higher you can run the RPM the better and with HSS tools your always going to struggle.

Carbide lasts much longer and can be pushed much harder. Often people don't push them hard enough so when the get chatter etc they back off when often all they need to do is increase feed rates which changes the tool pressure. Obviously there's limit and machine strength does then start coming into play.

[Dean jeffery]

Bloody hell Dean can't believe been 19mths.!!.... Seems like 6mths. The machine does well to say was never really designed to cut aluminum.!

Listening to that video you need much more air you can hear it re-cutting chips this will cause extra heat with high potential to weld chips to tool also give a poorer finish.
Does your cam software have a function to use spiral tool path? This helps keep constant tool engagement and also quicker and easier on tools because not retracting and plunging at end of each pass.

Also because of high spindle speed/low torque you really need carbide tooling. HSS requires much lower RPM and these spindles don't have enough torque at low speeds. These spindles provide most torque at full RPM so the higher you can run the RPM the better and with HSS tools your always going to struggle.

Carbide lasts much longer and can be pushed much harder. Often people don't push them hard enough so when the get chatter etc they back off when often all they need to do is increase feed rates which changes the tool pressure. Obviously there's limit and machine strength does then start coming into play.

Yeah I had to check my phones pics and 29/06/16 [emoji12]

Never planed on cutting alloy just the odd part but done more than a few now, may need an upgrade [emoji23] or modification.

That's the second tower I machined and I had a 15psi regulator and an iffy mist system, both not reliable.

Now I've got a new reg 30 psi and mist system that actually works [emoji23]

Yes I have spiral but only used to interpolate holes, never used on profiles so maybe try that instead [emoji106]

But I don't plunge anyway I used ramp

Tbh Dean it's the only time I used HSS was been a tight ass and if it broke or a massive fail it was only £24 gone, but worked well so stuck with it and it's a ripper in the vid leaving .25 for a finish pass with a 4mm carbide 3 flute.

If I tap carbide in my app is calls for almost 24k but 7000 mm/min

Running carbon parts and plastic parts I'm at 24k all the time.

But I'm pretty new to cutting alloy done the odd part here and there but not really enough to gain any real learning from it.

[JAZZCNC]

Yes I have spiral but only used to interpolate holes, never used on profiles so maybe try that instead [emoji106]

But I don't plunge anyway I used ramp

Don't mean spiral tool entry into the material, suppose could be called ramped profile.?. The toolpath I'm talking about will ramp/spiral down the whole way around the profile to the depth you set.
Ie set 3mm doc and it starts at Z0 and does one lap until reaches until reaches 3mm then does another until reaches 6mm etc. It never lifts or retracts tool until at the finished depth.
It's much faster and less stressful on tooling.

[Dean jeffery]

The reason why the tool leaves the material is because I set a lead in, I've also set a smooth ramp 3mm

I remove lead in and just left ramp now this keeps the tool into the material as you say.

I've just tested and takes the profile time down from 3:45 to 3:28 but I increased ramp to 5mm.

Then slowed the feed from originally 2500 down to 1500, slowed it down based off johns link and cutters above slows the profile time down to 4:35 with that small amount of increase it ain't really an issue.

[Dean jeffery]

This is a tweaked program today using the tooling speeds and feed John said on page 1

https://youtu.be/qXMss-2S90M

[Dean jeffery]

Seemed to go a lot smoother with that carbide VS ripper, could be a number of things.

Carbide over HSS but for the price of those carbide cutters I got 3 cheaper than the price of one HSS ripper.

[Dean jeffery]

Got 2 of these made today so the speeds and feeds of those 3 flute carbide cutters so far so good.

https://uploads.tapatalk-cdn.com/20180216/0313f6b0cc4874172c83b9e335449c66.jpg

[johngoodrich]

Glad they are working for you Dean. I use them myself at work so I know they are good, plus a lot cheaper

[Dean jeffery]

Been cheap is an added bonus reliability is key though [emoji106] they will be my go to tools for alloy now though, will use cutwels for plastic.

[johngoodrich]

Cutwels alupowers are good for ally as well but a bit more costly

[Dean jeffery]

Yeah I've got those for finishing mate triple the cost a bit more expensive [emoji23]

[Dean jeffery]

Shinny bling before anodising the guys I use don't do HD ano, anybody recommend anybody they use.

https://uploads.tapatalk-cdn.com/20180219/10ebc400d4dcafeedc9219f619cb5d23.jpghttps://uploads.tapatalk-cdn.com/20180219/d8309d1e2c15ab75dd17b72910d73ada.jpg

[Boyan Silyavski]

Push it to 24kRPm and 2000mm/min, Do NOt BE SHY. Use carbide only, whats that with the HSS??? I use HSS for foam only. Or rarely for deep reach somewhere when i dont want to spend on expensive tool. When profiling the profile needs to consist of 2 passes at say 10mm wide/ if tool is 6mm, as there must be a place for the chips to evacuate

This is how it should look when is cutting well, just adjust accordingly depth to your machine rigidity.


https://www.youtube.com/watch?v=XXR3396MAvg

[Dean jeffery]

I ain't shy mate I ran the ripper at 13500 speed 2500 feed but was HSS

Vids on page one description on the tube vids says what I'm using mate, the latest tool and vid is 13500 1500 feed with a 3 flute carbide.

When testing alloy a good few months back I did 4mm depth 5mm carbide 4 flute 2500 feed .7 WOT 20k

I'm not so bothered about the time to some extent I just need constant results (reliable)

Facing off like your vid don't really give much griff chips are always going to move out the way, profiling brings its own issues [emoji106]

[Boyan Silyavski]

have you tried 1 flute for aluminum? I was always shy, avoiding the extra cost, but the finish they give is incredibly perfect. Now carbide bits are so cheap, its good to try all. I also have problem with profiling when 2 or 3 flutes used. I use 1/8 one flute with perfect rresult and am thinking of buying some 1/4 one flutes to try.

[Dean jeffery]

The 3 flutes are working fine mate and prob single flutes worked out better with been on the small side, I don't really have time for trial and error of cutters.

I've used single flute 2mm carbide for some details because they gave me the flute length needed.