CNC Aluminum Melting problem

hi there, im new and this may be in the wrong place, so just move it admins if it is and sorry for the troubles. on to the problem

i am engraving some stuff into a piece of aluminum, its a street sign, i cut squares out of a stop sign and am engraving on the non painted side. i am using a 1/16 inch carbide end mill. when i start the engraving it just melts the aluminum instead of actually cutting the aluminum away. i have tried changing the feed speed and spindle speeds up and down and the problem hsant been fixed. two questions: what can i do to make it actualy cut away the aluminum and is it bad for the bit if i melt the engraving all the way through? thanks

One thing I found was that you have to clear the chips, either by flushing with coolant or compressed air.
Especially if you are using 4 flute cutter.
Al.

Not all aluminium alloys are suitable for machining. The alloy you're using may simply be too soft. It's a bit like trying to drill or machine lead. Machining soft materials like that will also shorten the life of your cutting tool due to the heat and friction. Maybe the use of kerosene as a lubricant may help. Try machining some alloy which is known to be ok for machining and see how that goes.

Welcome fredmoreno42...I suspect what you are witnessing is not the melting of aluminum but the abrading and rubbing of aluminum......

You've a problem with whatever you're using as your cutter......you're not cutting....but pics will help us analyze what is happening.

Does the aluminum have any film on it??

its hard to get pics now, i can get some in a couple days though this is a project at school and im still on break. but no there isnt any film i dont think at least. whether im melting it or not it looks like its coming off the sides in little ribbons. ill get some pics soon

As Splint says, not all grades of aluminum (`Al-You-mimi-um, down under) are machineable. I've seen some that machines worse than a Hersey Bar.

I'll throw out one more little item and I humbly beg your indulgence and forgiveness for saying this, but.... do you have the end mill turning the correct direction?

hmm i never realy thought about that, i just kinda popped it in and assumed it was. ill check that though, i hope that isnt the problem though cause then ill feel pretty dumb but we'll see. thanks for your fast replies

sounds to me to be a lube problem and the chips are probably not being extracted and are being pushed back into the part , if your concerned about dealing with a mess from the coolant or oil ,you can mix a little oil with some grease and make a light paste (something i use for tapping hard steels , or soft material), and you can brush it on the part ahead of the cut , the material may posssibly be soft but i have yet to see alumuminum that is not machinable ,just some material is softer than others , ive had the same issues with 6061 which is nearly the most common material out there if the speeds and feeds were not right or not enough coolant , or using a 4flt , dull cutter etc

Aluminum needs very high cutting speeds. With a 1/16 end mill ideally you would run the spindle at about 40,000 rpm. Most machines won't get anywhere near this speed so run the spindle as fast as you can ( how fast can you go without getting vibration ?). You need to push the feedrate up when you run high spindle speeds so the tool advances far enough to get a bite into the material and doesn't just rub. Some Tips: Use a 2 flute high helix endmill (preferably with polished flutes). Spray some WD-40 on the cutter while it is cutting ( this helps stop the material from welding on to the cutting edge.) Take the tool out as soon as it starts to load up. Buy some muriatic acid at your local hardware or swimming pool supply store. Put some acid in a small plastic cup and put your used tools in the acid. Do this OUTSIDE as the fumes are nasty! The acid will remove the built up aluminum but will not harm the carbide. Most endmills can be reused 10 to 20 times if you pull them before they begin to chip. (PS most toilet bowl cleaners work too )

What worked for me on a mill drill cutting Aluminium was:

1/16" 2 flute EM
2500 rpm (max of the machine)
5 IPM
.02" depth of cut
I went down .1" total
a mist oiler was used

I'm trying to engrave some black anodized (Type II) 6061-T6 parts with a .0156" 2-flute uncoated carbide endmill, 3/64" LOC. I'm engraving just thru the anodizing down about .0025" deep. My machine is capable of 14,000 RPM, flood coolant is on. I keep breaking the bits and I've slowed it down so much and its taking almost an hour to engrave one part.

I'm going to get some .020 endmills with a .030 LOC, but I was wondering if anyone had any recommendations on what I should be doing, any better options for cutters, etc. This is driving me nuts.

frenzy

Have you tried using a pointed cutter instead of a mill? I have used the small cone shaped dremel toolbits for similar engraving with good results. I was running .005 deep, 3k rpm and 60 ipm.

Depending on your machine you may also be able to attach a standard engraver. I have thought about doing this but haven't gotten around to it.

Good Luck

Matt

Maybe there is a runout issue?

E

Quote:

---

Originally Posted by megafrenzy

I'm trying to engrave some black anodized (Type II) 6061-T6 parts with a .0156" 2-flute uncoated carbide endmill, 3/64" LOC. I'm engraving just thru the anodizing down about .0025" deep. My machine is capable of 14,000 RPM, flood coolant is on. I keep breaking the bits and I've slowed it down so much and its taking almost an hour to engrave one part.

I'm going to get some .020 endmills with a .030 LOC, but I was wondering if anyone had any recommendations on what I should be doing, any better options for cutters, etc. This is driving me nuts.

---

Quote:

---

Originally Posted by fredmoreno42

hi there, im new and this may be in the wrong place, so just move it admins if it is and sorry for the troubles. on to the problem

i am engraving some stuff into a piece of aluminum, its a street sign, i cut squares out of a stop sign and am engraving on the non painted side. i am using a 1/16 inch carbide end mill. when i start the engraving it just melts the aluminum instead of actually cutting the aluminum away. i have tried changing the feed speed and spindle speeds up and down and the problem hsant been fixed. two questions: what can i do to make it actualy cut away the aluminum and is it bad for the bit if i melt the engraving all the way through? thanks

---

Make sure spindle is on M3 mode / aloy with failure tool most be cut easily /with good tools is like cheese and knife .

Step down 1Mm
Feed 2000
Spindle 3000rpm
Test this
D16EN /D40EN
-----------------------
Step down 0.5 mm
Feed 600~1800
Spindle 3500 ~6000 rpm
D10EN/D8EN/D6EN

Hi,
by far and away the single biggest thing I did to cure the Built-Up-Edge problem was flood cooling. Its not really about cooloing as much as its about flushing the chips out of
the cutzone, recutting chips will result in BUE in short order.

I run my four flute 1.5mm endmills at 24000 rpm, the max my spindle can do, for a surface speed of 113m/min. I would ideally get up to 250m/min, but thats the spindle I've got.
The feed rates are determined by the strength of the tool. Its a mistake to be 'too gentle', all you do is rub the material rather than cut and evacuate chips. Chips carry away
the majority of the heat, you must create chips and get them out of there.

With small tools I allow 1% of diameter per tooth per revolution. With bigger and stronger tools say 6mm then you can get up to 3% per tooth per rev without overloading the tool.
1% of 1.5mm =1.5um per tooth per rev
1.5um x 4 (no. of teeth) x (24000)=144000um/min or 144mm/min.
If the tool can handle that load try upping it a bit until you find the limit where it breaks.

Soft and sticky aluminums like 3000 series and some 5000 series can be a challenge. Good coolant flow or air blast is a minimum. With harder 6000 series and any of the 7000 series
moderate coolant/air blast is enough.

If you get into real trouble try di-boride coated tools, not cheap but so much better than any other coating in aluminum.

Craig