Printable View
Dear all,
When I do circular milling operations with small end mills, chips tend to weld to the endmill until it breaks. It happens even if a drill a pre-hole before using the end mill to make it bigger.
I solved this issue using coolant fluid, but I would prefer to avoid the coolant.
Do you have any advice?
For your information I use uncoated 2 fluts 4 mm end mill at 24000 rpm with 2mm WOC and 0.4 mm DOC
What kind of material do U cut?
Smell's like some kind of aluminium alloy. Can u change it for other (like PA6)?
If not be sure U have good mill with polished edges and try as low rpm as possible.
Sorry, I forgot to mention that I mill aluminium 6082
Generally you do not want to run an end mill right down the center of a previous cut. Better to have it past center.
Ty to at least use and air blast to clear chips.
"For your information I use uncoated 2 fluts 4 mm end mill at 24000 rpm with 2mm WOC and 0.4 mm DOC"
You left out very important information. What is the feedrate being used, and how big of arcs? Inside arcs or outside? How heavy or what type of a machine? Router spindle?
That is a tiny depth of cut. Hope your end mill has a sharp tip. Unless that is the full depth of your part, it's better to go with a deeper DOC and narrower WOC.
I hear a lot of folks use WD-40 on aluminum if not wanting coolant.
Hi,
4mm diameter at 24000rpm works out to a surface speed of 301.5m/min.....and that should be in the sweet spot for aluminum.
I personally have had same problem and as a consequence use flood coolant on all materials and have done for years. Plastics are bits of b****ds for the chips welding themselves back into
a lump, so even, perhaps especially, on plastics I use coolant.
There are two parts to using coolant, firstly as the name suggests is to keep the tool and workpiece cool, but in this instance the more important effect is to flush the chips
away from the cut zone. If you re-cut the chips you will end up with 'Built Up Edge', BUE. If you had a good and well directed air blast that would also clear chips and BUE is
reduced , even eliminated, but even just a few moments where the air blast is misdirected and BUE results.
I use small tools in steel as well, and then re-cutting chips is important but keeping the tool cool is essential, and for that purpose it's hard to beat flood coolant no matter the inconvenience.
I used a 1/8 'th four flute coated Destiny Tools Raptor in med-tensile steel yesterday for six and a quarter hours before it crapped out. I run it at 18000rpm and that works out to 148m/min, which is at the top end for
steel. Without coolant the tip turns red hot and destroys itself in under a minute.
I follow the rule: 'If using coolant....use lots of it' The second rule is 'If its not squirting direct at the cut zone its not flushing chips'.
Craig
The federated is 400 mm/min and I use a small homemade milling machine.
I can't use more DOC because the pre hole has the same diameter as the end mill, so I am using a helix with 2mm radius for entry motion and it's in this phase that the chips weld.
Hi,
at one time I had some Harvey 1/8 th inch Diboride coated tools. They are made for aluminum. The Diboride coating is a 'greasy as a butchers prick' in aluminum.
I loved those things, I wore them out eventually.....and as they are costly I didn't get any more. If you are struggling then they are recommended.
Craig
Maybe just try a dab of WD40 or similar in the start zone. Might be enough to get you going.
There are so many unknowns on a home built and I'm not used to working with such a light machine. The start diameter is very small, so the feedrate will have to be reduced a ton. A straight line slotting feedrate at .4DOC on a rigid machine could be 1500 or more, but that means nothing on a small radius. You may need to go down to under 50.
Anyway... coolant is always going to make a big difference, especially at a high rpm. Sorry I can't be of more help.
Hi M80 - if you are cutting at 400mm/min and 24000rpm with a 2F bit then your chip thickness per tooth is 0.008mm. This is way too small and you are rubbing the material away vs cutting it. Hence the material is fretting to the tool. A good starting point for chip thickness is 0.05mm (this also depends on your machine stiffness). Your surface speed at 300m/min is Ok but could come down a bit to decrease the friction and heat. Now CL=feed/teeth number/rpm so to acheive 0.05mm and maintain the 24k rpm you need to speed up the feed to 2400mm/min. If your machine can do that go there, if it can't recalculate to get 0.05mm and as slow a surface speed as possible. Peter
have a play with fs wizard it calculates all this sort of stuff. https://fswizard.com/
WD-40 is mainly kerosene try metho or ethanol it evaporates faster. Using the nominal settings in the wiz for 6061-T6 which is machining wise same as 6082-T6 gives feed= 1658mm/min Fx(tooth thickness) =0.07mm and rpm=11648 and surface speed 146m/min. Use a good lub and see how you go. Once you find the sweet spot chip thickness for your machine on that material stick to it! Adjust your feeds and speeds but keep the same chip thickness. This is the thing that is doing the work. Machine compliance means the tool is being pushed away from the material and poor tool runout may mean only one tooth is cutting the job even though you have 2 teeth (so the trailing tooth is rubbing hence fretting). Try 1F tools they can run faster and runout does not affect them as much. Keep us informed of the results....
Hi,
I use small tools down to 0.5mm two flute endmills and down to 0.2mm drills.
With small tools I allow a chip thickness of 1% of diameter per tooth per revolution.
As an example with a two flute 0.5mm endmill:
1% of 0.5mm is 5um, two flutes =10um pre revolution. At 24000rpm means the feed rate is 240mm. This is conservative, I might go even slower with steel and half that in stainless
but twice or three times in aluminum.
0.5mm two flute 24000rpm (1% rule = 240mm/min)
Stainless 120mm/min
Steel 180mm/min
Aluminum/Copper/Brass 400mm/min
Plastics 800mm/min
1.5mm four flute 24000rpm (1% rule with four flutes=1440mm/min)
Stainless 300mm/min
Steel 500mm/min
Aluminum/Copper/Brass 1500mm/min
Plastics 3000mm/min
It is true that you can 'rub' the surface if you attempt to take too smaller a cut, but with small tools you can very easily break them by trying to cut too much. I use 0.5mm endmills
to cut copper circuit boards and I get eight and ten hours per tool. Try to cut too much and you get fractions of a second.
With tools over 2mm, you can increase the chip thickness to 2% without snapping the tool.
Craig
Hi Craig - Using fs wiz for a 0.5mm 2F tool keeping with aluminium for the discussion, its nominal settings would be 24k rpm, 140m/min feed, 0.003mm feed per tooth and surface speed of 38m/min. Is that within your guidelines? Peter
Hi,
no not really The problem is that ideally you'd spin a micro tool like this at 40,000 rpm plus, but few spindles can do that.
24000 rpm with a 0.5mm tool results in a surface speed of 38m/min. Best you can get with commonly available spindles.
I run 0.5mm endmills at the 1% per diameter per tooth per revolution. Using these micro tools in steel and stainless is an expensive business, they break so easily.
In aluminum and copper though I run them at 400mm/min. I have some really thick copper layer circuit boards for high current designs, it has a 420um layer or 0.42mm.
I run the wee 0.5mm tools at 50% stepover at full depth, ie 0.42mm at 600m/min. They last all day. Usually it some small mistake you've made that shocks and breaks them rather than
them wearing out.
My suggestion is based on what I find works for me, and its easy to remember.......1% diameter per flute per rev. Easy. Slow by a half or more for stainless, 60%-80% for steel, 200%
for soft metals and 400% for plastics.
For OP the same rule works out to 1% of diameter = 40um, two flutes=80um per rev, 24000rpm =1920mm/min and if you wish and the machine can go that fast take it up to 200% ie 3840mm/min.
Craig
I agree with everyone else: coolant is the best option to keep the chips from welding onto the end mill and Air Blast or a Misting System would also help and be a great option for a home built machine. You can get a magnet mounted Mister or Cold Air Gun you can setup with the nozzle directly pointed at the tool for cheap and it should help solve your issue.
The other option is to look at the tool you are using: are you using a General Purpose 2 Flute End Mill or a High Performance 2 Flute End Mill for Aluminum? A High Performance 2 or 3 Flute End Mill for Aluminum with anywhere from a 35-45 degree helix will have a sharper & smoother cutting edge so chips do not get stuck as well as more room in the flutes for the chips to evacuate, which could also help solve your issue. Like Joe Average mentioned, the Coating can also help when cutting dry: a Diboride, ZRN or DLC Coating on the End Mill improves lubricity to help the chips evacuate and not get stuck on the cutting edge.
Hopefully this helps!
Mike
Hi,
most carbide endmills for aluminum are uncoated. The coatings which are applied and common on carbide tools for steel tend to be trivalent, things like Ti Nitride,
Al Nitride or some combination thereof. The problem is that these trivalent coatings show an affinity with aluminum, which is also trivalent. Diboride is a quadvalent coating
and has high lubricity i aluminum.
I bought them because I was having a real battle with a 5000 series aluminum for marine use. It seemed to be very 'sticky' and even flood coolant was marginal.
Diboride fixed that right up.
Craig
I machine a lot of hard and soft Aluminium and various plastics.
I use a strong air blast with a pulsed misting. The air blast prevent second cuts, and the mist keeps the cutter 'wet' so chips don't stick.
I use a mix of 3-4 parts kero and 1 part olive oil. The olive oil is biocompatible so it does no damage to my skin. Commercial coolant can be toxic.
Look up Minimum Quantity Lubrication, or MQL.
Your 2 mm WOC seems too big to me for a 4 mm cutter. Try half that with an increased feed.
So far so good, for the last 10+ years.
Cheers
Roger