Try 1000mm/min and 12000 rpm, and 0.3mm depth per pass.
What type of tool are you using?
Hi guys, can anyone tell me what I've done wrong here. First time cutting alloy and was a disaster as per the photos show. Machine is a stepcraft with a kress 800 spindle. 2mm 2 flute end mill. 1st cut was at 150mm/min at 12000rpm, 2nd at 70mm/min 10000rpm and 3rd at 50mm/min at various speeds from 10000 to about 14 or 15000rpm. As you can see the results are all very similar. Intial pass was set at 1mm step down then set it at .5mm. Had air blast on 2 attempts then just wd40 on the last. Using fusion 360 for software. Alloy is 6060. Hopefully I've included enough/correct information.
Similar Threads:
Try 1000mm/min and 12000 rpm, and 0.3mm depth per pass.
What type of tool are you using?
Gerry
UCCNC 2017 Screenset
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
You could try wiping the surface with some kerosene first too, some alloys of aluminium just gum up cutters really badly.
Shannon.
Thanks will try that before next cut. Is it possible that the alloy is not as was stated? maybe it is of a softer grade? Could you comment ger21 more on your suggested feed of 1000mm/min, to me that seems way too much for a small 2mm cutter but I am inexperienced so I could be far from the truth.
The softer grades are harder to cut and often do need some cutting fluid. The same grade of aluminium can also vary a little from sheet to sheet, one sheet might cut well and the next not so much.
Shannon.
The mess gets worse as your feed goes down. Yes?
You are not cutting the metal, you are rubbing it and melting it.
Lower spin and higher feed, and make with the kero.
And make quite shallow cuts if it's a 2 mm cutter!
The aluminium looks a bit crappy for machining as well.
Cheers
Roger
Well it didn't seem to change much as I went down in feed, I'm thinking the cut was too big but I am also starting to wonder about the alloy, just like you say. My thoughts too that it seems to be melting it and not cutting it. The kerosene, it is for lubrication/cutting?
I cut 5000-series sheet, which is a complete pain. Speed about 2,800 RPM and feed about 200 mm/min. It works. You are melting the stuff, and it is a marvel you have not smashed the cutter with Built Up Edge (BUE). (Google it.)
The kero wets the surface of the cutter and prevents the aluminium from sticking. The ideas behind the conventional and very out of date 'flood coolant' are all wrong for aluminium.
Cheers
Roger
unfortunately I can't go that low in speed. But I am using wd40 which seems to be good as I'm lead to believe. Actually the first cut I did break cutter, but the following to cuts were ok, at a lower feed. but I think now by the comments and my own thoughts that the cut was to big and/or bad alloy. Yes I see what you mean about BUE, looks like my problem.
The solution or next attempt should be ;
smaller cut with higher feed, does 150mm/min sound ok? as thats what the original speed was.
Sorry, I was sleeping...
No, you need to go much faster.
Try 1000mm/min, as I said, but with a shallower cut, like .2mm. I thought you were using a 3mm bit.
And use a lot of WD40.
Gerry
UCCNC 2017 Screenset
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
As Ger says - with those RPM you need more surface speed, but shallow cuts. Creep up on it from very shallow.
WD40 works but is $. I use a mix of 3 parts kero to 1 part olive oil - pretty harmless stuff.
Cheers
Roger
Thanks Roger, thats good info, I have a bit of wd40 there as I use it for other things. Going to try all the above suggestions this weekend and will report back with good results hopefully.
Ok looks like we may have some success and ger21 was spot on with his 1000mm/min feed suggestion.
these were cut at lowest spindle speed, 10000 rpm and fed at either 1000 or 1100mm/min with either a .1 or .2mm cut. Wasn't much difference between each of them though I think at .1mm cut you may be able to up the feed even more. Best thing is, no built up edge, success! Thanks again everybody for the help.
Now my next question is will these settings work with 6061 and 7075? Also as I'm probably only ever going to cut with these alloys (and maybe acrylic/delrin/other plastic) is it worth investing in a feeds and speeds calculator such as g-wizard or other suggestion?
Keep experimenting. A 0.1 mm DoC might be a shade too small if the surface is not absolutely smooth. Cut, don't rub. On the other hand, I have been machining 2011 aluminium with a DoC of 0.05 mm, but with a 1.2 mm carbide ball end cutter at 3,000 RPM. Have to keep the sideways loading down when the cutter is that thin.
6061 and 7075 are harder materials that 5000-series, so the load on the cutter may be a shade higher. But not by much if you use a sharp cutter rather than a cheap one with a square face, and they are both much nicer to machine. I have been using sharp cutters designed for HR55+ steel on aluminium - and liking it.
Plastics - DROP the spindle RPM! You can pour heat into the Al chips and they will flay away, taking the heat with them. Pour the same heat into plastic and it may melt. Trouble! You may find it well worth while to reserve some new and very sharp cutters purely for plastics. Don't let any metal blunt their edges at all. Acetal/Delrin is nice to machine, nylon is OK, PE is a pain as it feathers. But it does have some nice engineering prioperties, so I persist.
Cheers
Roger
Hey Roger, great tips mate thank you, I will certainly now get some cutters solely for plastics. As far as a feeds and speeds calculator is it worth getting or not really as I now know ballpark figures for feeds/speeds on the grades of alloy I will be using?
Some people swear by them. Me, I don't have one: I go on experience. I guess - cost me a few cutters over the years.
Actually, there are some 'free' versions on the web, suitable for a first pass with a new material. And some catalogs from up-market cutter mfrs have very useful tables in the back. Catalogs can come as PDFs.
Cheers
Roger