[izzydog312]

hey guys! wondering if someone could please assist me so im not going through so many bits.

we have a sheet of 6061 aluminum that we a trying to get a nice texture ( about 1/8 '' deep for detail ) out of but we are running into problems.


We have used a 3/8 '' end mill for the rough in, which took a fair amount of bulk away, no problems with that, cuts perfectly fine, not breaking bits.

Once we took the most of the bulk with the 3/8'' end mill we switched to 1/8'' BALL nose bit and ran into some serious trouble.

The 1/8'' ball nose is getting aluminum welded around the bit quickly and causes us to shutdown because there is no profile left on the bit because of all the aluminum welded on

(note we are using the machine relief tool-path on artcam for the 1/8'' ball nose bit)

Here is the feeds and speeds that we are running our bit at : Step over : .18
Step Down .005
Feed rate : 60
Spindle : 20 000 If someone could point me in the right direction, would be much appreciated ! thanks !

[izzydog312]

Bump

[GerryG]

You've included no information about the toolbit beyond the diameter and tip profile - what's it made from/coated with, how many flutes does it have? Is it made of some kind of Chinesium of questionable provenance?
I'm guessing that you're using a router, given the spindle speed and the fact you're using artcam. Are you using any kind of lubricant while cutting?

[izzydog312]

1/8 TAPERED ball nose carbine coated, short staffed made for aluminum..... From amunra.com ( the bit company )

Yes we are using a router, and are useing artcam.... We have a cold air gun and use a little wd40

[izzydog312]

looking forward to your reply.... iv also been thinking, maybe were not clearing out enough bulk before we come in with the 1/8 '' tappered ball nose ?

we've only used a 3/8 end mill to do the bulk on a fairly high detailed mold and still lots of bulk left for the 1/8 ball nose

first time cutting aluminum obviously so im not very educated

[GerryG]

I'm no expert at routing Aluminium myself, so don't get too worked up about any pearls of wisdom that I'm likely to generate.

Personally, I'd clear as much out on the roughing pass as possible, and possibly have a light roughing pass followed by a finishing pass with the ball nose.

I found with doing complex 3d routing on acrylic (obviously not the same, but it loves galling on to the router bit just as much) that it was best to get it as close as I could to 'finish' territory on the roughing pass, then have a couple of sequential passes with the actual finishing bit to get a good finish.

To minimise the galling, I'd also take a good look at how much cooling you're applying to the work - it sounds to me like you might need more.

[skrubol]

Here is the feeds and speeds that we are running our bit at : Step over : .18
Step Down .005
Feed rate : 60
Spindle : 20 000 If someone could point me in the right direction, would be much appreciated ! thanks !

I assume you meant .018" stepover? That's a bit high to get good surface finish, but shouldn't cause welding.
Your step-down is way too small I think, you'll mostly be cutting with the point of the ball, which is the the worst part to be relying on. I would do a single stepdown, or 1 semi-finishing pass, leaving .005" stock and then a finishing pass. You're probably rubbing more than cutting.
Feed rate seems too high for such a small end mill at a relatively slow spindle speed. How many flutes? Assuming it's 3, that's .001" per tooth, which would be fine for most square end mills, but for a ball I think it should be derated.

1/8 TAPERED ball nose carbine coated, short staffed made for aluminum..... From amunra.com ( the bit company )

Yes we are using a router, and are useing artcam.... We have a cold air gun and use a little wd40

Link doesn't work and I couldn't find anything about amunra end mills.

[QuinnSjoblom]

You said coated, but with what? Some coatings are much worse than no coating at all if it's not the right kind for aluminum. Zrn is great for aluminum. As for cooolant, 6061 was a nightmare for me when running dry. Instant chip weld. You said you're using a bit of wd40 which is fine, but are you applying it every couple minutes as it cuts? I use a cheap 20 dollar mist setup from Amazon with kool mist coolant. Works great, never chip welded since. I'm also using what some would consider a "router" but a very rigid one with a 2.2kw Chinese spindle. Check your tool runout with an indicator on the flutes close to the end of the tool, turn the tool backwards by hand to see where each flute peaks at. Runout is very important with these smaller tools. If you have a thou of runout, only one flute is gonna be cutting which means your chip load is gonna be much higher than what you calculate. If you find runout, try turning the tool and the collet in different positions until getting it as good as you can. As others have mentioned, you will benefit from multiple passes. I would rough, then do a semi finish leaving maybe 5 thou, doesn't need to be as fine of stepover for semi finish. For the final pass, you want the endmill taking a consistent amount of material for the whole cut. If it's passing through a variance of material thickness, tool deflection changes and gives inconsistent surface

[izzydog312]

Thank you everyone for your suggestions, will be firing up the cnc in a couple days to try some new things.... Things i plan on trying are :

Changing stepover from .18 to .05

Useing a 3/8 , 1/4 and 1/8th bit for the rough in, instead of jst the 3/8th bit

Spraying every so often with wd40

change stepdown from .005 to . 03

Anybody have an idea for Feed rate and spindle speed ? a lot of controversy about it online and tough to find the right speeds we are currently running feed rate : 60 and 20,000 spindle speed

Amanatool.com is the site we get out bits and they are Solid Carbide ZrN Coated

If anyones got any other suggestions to try, please let me know asap! thanks

[izzydog312]

Bump

[QuinnSjoblom]

Thank you everyone for your suggestions, will be firing up the cnc in a couple days to try some new things.... Things i plan on trying are :

Changing stepover from .18 to .05

Useing a 3/8 , 1/4 and 1/8th bit for the rough in, instead of jst the 3/8th bit

Spraying every so often with wd40

change stepdown from .005 to . 03

Anybody have an idea for Feed rate and spindle speed ? a lot of controversy about it online and tough to find the right speeds we are currently running feed rate : 60 and 20,000 spindle speed

Amanatool.com is the site we get out bits and they are Solid Carbide ZrN Coated

If anyones got any other suggestions to try, please let me know asap! thanks

Your coating is good, for spindle speed and feed rate, you need to calculate sfm and chip load. This us going to give a different rpm and feed rate for each cutter. I usually go 800 to 1000 sfm on aluminum, but that's with a constant spray of kool mist. For chip load I usually go a bit under a thou with a 1/8, and 2 thou for a 1/4.

If you aren't familiar with speeds and feeds, watch this video. https://youtu.be/uw8uL2jjEBs

[izzydog312]

Your coating is good, for spindle speed and feed rate, you need to calculate sfm and chip load. This us going to give a different rpm and feed rate for each cutter. I usually go 800 to 1000 sfm on aluminum, but that's with a constant spray of kool mist. For chip load I usually go a bit under a thou with a 1/8, and 2 thou for a 1/4.

If you aren't familiar with speeds and feeds, watch this video. https://youtu.be/uw8uL2jjEBs

Appreciate your reply, curious to what SFM is ? and does anyone know of any easy to use calculators ?

[Rza25]

Appreciate your reply, curious to what SFM is ? and does anyone know of any easy to use calculators ?

Hi, 'I use this
https://play.google.com/store/apps/d...lter_tools.wmc