Cutting Aluminum with 1/8" bit

[FSICM]

I run a PRS Standard with a 4 hp spindle and I'm trying to cut 5052 aluminum at 15000 RPMs and feedrate at .7 plunge rate at .4 with a pass depth of .040 and using an air cooler . I'm using an 1/8" single flute upcut bit. A bigger bit wont fit inside the pieces that need cut and so far everything I've read says to use a 1/4" bit. Any suggestions?

Thanks

Frank

[jerry_stanek]

I cut some at 10000 and .70 IPS with a .125 bit the stuff I was cutting was old that had been a sign that was being reused most of it cut good but some areas cut real hard. I would break the cuts into small sections in case of a broken bit. I did break 4 or 5 bits cutting it.

[FSICM]

Jerry
What pass depth?

thanks

[blackhawk]

Frank,

I would start out at 0.3IPS for Z and X,Y feed rates. 10,000 rpm and .030 depth of cuts. I would also try a two flute upcut endmill. You also do not want to plunge straight down into the cuts.

[Brady Watson]

You can use ANY size bit you want, but you'll want to adjust speeds accordingly. I often cut AL with a 1/16" single flute spiral O from Onsrud @ .015-.02" deep per pass. You can bump that depth up a little the larger you go on the tool - to a point. You want nice smooth tool movement void of sudden or shocking moves. You want to keep the tool loaded and cutting until it gets all the way through.

Although this has been covered ad nauseam, it bears repeating that you should never drill or plunge straight down into AL. ALWAYS ramp into the cut using the ramp options in PartWorks for a profile or pocket toolpath. Also, machining AL sounds COMPLETELY DIFFERENT and even ALL WRONG compared to anything else that you have cut if for nothing other than material and tool harmonics. Make sure you are getting little chips off of the tool to help keep things cool. 13,000-15,000 should do it, but your results may vary.

Speaking of ramping...you may need to temporarily adjust the first 2 parameters of your VR settings if you want the tool to go slower than 0.4 IPS. You can tell it to go .05 IPS, but it will still go the speed set in the VR. When done with the slow speed work, put the setting back to 0.4 on the first 2 settings in VR or your tool won't run properly at higher speeds.

-B

[jerry_stanek]

I cut it .02 deep here is a picture of how it came out the letters are 4 inches tall. The aluminum was painted black when I got it but they repainted it. Like I said there were some spots that were real hard you could hear the change in sound when it cut into those spots

[FSICM]

ok got a New Bit in today Belin 33317 Whoo Hoo! made for aluminum.
I did the calculations, does this sound right 1/8" bit
15000RPM
.3175 ips feed XY
probably plunge at 0.2 z

.04 depth and I am cutting .080

does this sound like I am on the right track
would hate to break another bit seeing I got the right bit this time. HAHA

Thanks for everyones input!

[MogulTx]

I can't comment on the bit, because I don't use this one. I use a 1/4".. but the fact that aluminum will vary from one section to another is true, true, true. I just was experiencing that the other night on my machine. I get a little bit of slurring and balling of the material from time to time- in different areas on a 5 x 10' sheet. ( not all over the panel, and not during or after a direction change. along a straight line at a fixed speed and feed).

So watch out for aluminum. If you need a lube, I understand that alcohol would work well. I sometimes use WD40 if going into heavy stock.

Mostly, I have learned to slow the feed rate and slow the plunge rate and can pull more air across my bit with a shop vac. I want to find an air cooling nozzle, but haven't the CFM available to me (yet).

[Brady Watson]

Just to add...

The aluminum alloy is important. Try to find out what alloy you are going to be machining in order to anticipate some of the issues you may run into for a given alloy. For instance, 2000-series alloy machines well, as does most of the 6000-series, whereas the 5000-series tends to be tough to machine, mostly because it has a tendency to get gummy.

When you use an upcut O-flute and dust collection (which aides in cooling), you really don't need lubrication or coolant. It is only when you start machining thicker AL parts that the material can get heat-soaked and coolant becomes more important. This is usually handled with compressed air (like a football inflator tip shooting on the bit), a cold gun, or an occasional shot of alky to provide some evaporative cooling. Lube is usually not required, and not advised on an MDF spoilboard. Alcohol OR WD40 are NEVER advised when using a vacuum hold down solution - BOOM!!!

Don't be skeered...just be prudent, careful and start cutting already! How do you think I learned? (Seriously...how do you think I learned?) :D

-B