[themagicman]

I have a 48 X 48 cnc router table. I have bought a aluminum cutting bit and now am trying to figure out how to use it without blowing it up. The bit is a 1/4 inch carbide single flute. My router is capable of speeds from 8000 to 23000. When i have looked in programs to help me with feeds and speeds the feed rate is much faster than my machine can go (540 ipm).

I had originaly planned on using WD40 and an air hose and lubricate the bit. (I know a mister would be better). Hearing now that rubbing alcohol is better?

Any help would be appreciated.

Thanks

[ger21]

What exact bit do you have, and what type of aluminum is it?

It depends on a lot of things, but somewhere between 30-60ipm, at 10,000-12,000 rpm is what I've used on mic6 and 6061. Depth of cut depends on how rigid your machine is, and how powerful you're spindle is. I would try somewhere between 1/16 and 1/8" depth per pass, or even less if you have rigidity issues.

[themagicman]

I bought the bit from toolstoday and it is an amana bit. I have no idea what aluminum i am cutting. Just a scrap i picked up somewhere. Also i forge so much of the aluminum i may be cutting may have been forged into something totally different.

[themagicman]

The machine is quite rigid. Not milling machine rigid but pretty good.

[zero_divide]

I have a 48 X 48 cnc router table. I have bought a aluminum cutting bit and now am trying to figure out how to use it without blowing it up. The bit is a 1/4 inch carbide single flute. My router is capable of speeds from 8000 to 23000. When i have looked in programs to help me with feeds and speeds the feed rate is much faster than my machine can go (540 ipm).

I had originaly planned on using WD40 and an air hose and lubricate the bit. (I know a mister would be better). Hearing now that rubbing alcohol is better?

Any help would be appreciated.

Thanks

540 ipm at 23000 RPM ????
Which program exactly recommend you those values?????
That is goo much of feedrate.
Will probably work for wax only.

Anyway have you tried this one ->FSWizard

I ma getting:
SFM=1200, IPT=0.00261, RPM=18344, FEED=47.92 IPM
DOC=0.125, WOC=0.25

[themagicman]

What is meant by surface speed. Yes this is the program that gave me the screwy feed rates. I was probably not using it correctly.

[zero_divide]

What is meant by surface speed. Yes this is the program that gave me the screwy feed rates. I was probably not using it correctly.

Surface speed is a material dependant cutting speed. Expressed in surface feet per minute. Basically its how fast the cutting edge of the tool is trafeling relativeto workpiece. SFM is directly dependant on workpiece-tool material.

I guess you need at least a little knowledge to use any calculator.
Wikipedia is your man here.

[jwatte]

What is meant by surface speed. Yes this is the program that gave me the screwy feed rates. I was probably not using it correctly.

"Surface speed" is measured in the US in "surface feet per minute" and is a measure of how fast you can spin your bit. From this, and knowledge of the bit geometry, all the other parameters can be calculated.

The SFM specified for hard steel with carbide cutters is typically in the 80 SFM range. Aluminum is typically in the 250 range.

The math works as so:

Your-RPM = SFM * 12 / (3.1416 * bit-diameter-in-inches)

Increasing SFM for a material will lead to worse finish and higher load on the machine, and at the extreme, may start melting the material or cause other terrible breakage. Possibly the first thing to go is your tool bit, though, so you'll have some warning that you're doing something wrong :-)

Other math I've found online and that seems to work for me:

Your-feed = (your-RPM * bit-number-of-flutes * chip-load-per-tooth)

The "number of flutes" and "chip load per tooth" are sometimes multiplied together (and are the same thing for single-flute tools.) I've seen values between 1/100 of the tool diameter and 1/10 the tool diameter, with 1/10 being very aggressive and for softer materials, and too thin a cut also causing problems with chip welding etc.

Finally, for a rigid, strong mill, you can set your depth of cut to 30% of bit diameter; for less rigid mills, decrease as appropriate (say, to 10%.) Similarly, if you run faster than indicated, you may want to decrease D.O.C.

Note that 8000 rpm is pretty high -- if you use a 1/4" bit you'll be running at something like 500 SFM, which is higher than "finish rates" for aluminum, but it can probably still work OK. A 1/8" bit would be within spitting distance of spec. Also, for a given SFM rate and chip load percentage, the feed stays constant across different bit diameters, but the depth of cut goes down.