machine feed rates for aluminum

[DerHammer]

Can some of you more experienced machinists out there suggest a good feed rate to cut aluminum. I bought myself a cnc mill fairly recently and I'm now getting pretty close to actually doing some metal cutting.

I plan to use flood coolant and I'm probably going to be using a combination of end mill sizes for my parts between 1/4 to 1/2 inch. Mostly my questions are on how much depth I should cut per pass and how much step over can I get away with? also what kind of IPM should I be running? Any advice is greatly appreciated. thanks

[SORCHEROR]

with aluminum you want a good flood of coolant or the cutters get alum stuck to them real fast,how fast and how much depends on the endmill you use,two flute high speed endmills work great for roughing fast,they are cheaper too,but mostly i use 3 flutes high helix data flute carbide,i rip a 1/4 off at a pass full cutter width at 50-60 imp no sweat when roughing on a 5/8 cutter,best thing to do is experiment,some machines dont have the horse power to take heavy cuts,so just take a scrap chuck and have at it,good luck

[big_mak]

I've got some 1/2" diameter 3 flute solid carbide endmills Slotting 1/2" deep 10,000rpm and 100ipm and they sound nice. These are from Gorilla Mill. When I'm taking smaller deps of cut, I'm routinly in the 200+"/min range with roughing cutters.

Wind your machine up, and see what it can handle!!!! Flood all the way!

[DerHammer]

Thanks for the info.

I have an NC knee mill made by WEBB " its a Bridgeport copy". Its equipped with a 5hp spindle and weighs about 4000lbs. Its pretty stout I think because the manual claims the table can take an 800lb workload. I think the spindle will crank up to about 3600 RPMs also according to the indicator, so the next question is....

How fast should I have the spindle turning? Is there an ideal RPM for aluminum. Any general formulas for calculating what a guy can get away with as far as federates, rpm, IPM, and step over goes or is it pretty much just trial and error?

[big_mak]

Feeds will depend mostly on what your machine can handle at a particular Depth of cut as for Cutting speed try (Surface Feet per Min*4)/Cutter Dia.= RPM With HSS cutters in aluminum, I'd start @ 300SFM. For Solid Carbide Tools for your machine, just max out your RPM and you should be safe!!!!

[crazythunder]

Well I say always balls to the wall. I will try 1x dia and .012 to .02 per tooth and max RPM's. Then push it from there till it break back off 10% and call it a day.

[ctate2000]

You should have no trouble running a carbide emill at 1000-1500 surface feet per minute (SFM). Feed will be dependant on diameter of the tool and depth of cut(DOC). RPM=(SFM/Diameter)*3.82. Refer to emill manufacturers catalog for proper chip loads. Feed Rate=RPM*chip load*number of flutes. You will find it difficult to obtain proper SFM from your 3500 RPM spindle using small tools. You will also find controling your machine at high feed rates when interpolating will be difficult. I would advise you to be conservative with the feed rates or your accuracy will be compromised.

As said earlier you can use very high removal rates when machining aluminum but you must be careful not to ask to much from your machine.

[fpworks]

Yep...just start out conservative, and if it sounds good, go faster until the tool breaks or your machine either shakes or runs out of power...exactly like crazythunder says ;-)

Cutting aluminum is "easy" but achieving maximum removal rates can push any machine to it's limit. I would say that your spindle's rigidity is going to be your limit with larger tools and rpms will be your limit with smaller tools.

With a 5 hp spindle in aluminum, you should be able to achieve about 15 cubic inches per minute removal rate IF you can find a tool and cutting parameters that will allow you to get there. For instance, a 0.75" endmill may rattle your machine to death before you can reach that limit, and on the other hand, you can't spin a 3/8" endmill fast enough before breaking the tool. (to reach that removal rate) Finding out what works for your machine will take some experimentation on your part.

I suggest using two flute tools...they are more forgiving than three flute tools for pocketing and plunging. I also suggest using stub length endmills if possible...they really help if your spindle is weak. You can really push those...we were cutting at 500 ipm at only 10,000 rpm with a two flute 0.75" endmill the other day, and not a light cut...we were removing 110 cubic inches/minute (that is about 12 lbs/min). No coolant either. I would have gone faster, but out of horsepower.

[DerHammer]

Thanks for all the great info. I'm just an hobbiest doing this out of his garage, so I'm not under the pressures of maximizing every minute like a production shop is, so if going slower will extend my machines life, then I'm all about it.

Also, When you mention having a "weak spindle", you are talking about when the motor bogs down right? It is an older machine and I believe its only capable about 150 IPM, so I don't know how much SFM that is. Guess I could Google it

[fpworks]

In regards to being a hobbiest...you can still take advantage of high performance tooling and machining strategies. Often these will give your projects better results in less time, and it is generally part of the learning experience ;-)

I don't think you have to worry about speed vs longevity at those speeds. That becomes more of a factor with faster machines. But even faster machines are made to accommodate the higher speeds to a certain degree. Crashing and operating the machine so that it vibrates (lower frequencies) will tear it up.

In regards to a weak spindle...I'm talking about the spindle's rigidity. Your machine's base/table is quite rigid, but those type of machines have relatively lightweight spindles.

You stated 150 ipm...that is your axis feed rate in inches per minute (IPM).
SFM is in regards to cutter size and spindle speed. SFM (Surface Feet per Minute) It is simply the velocity of the outermost cutting edge.

[DerHammer]

Thanks, learning something new everyday here. I love this site! Ok, so then SFM and IPM are measurements for completely separate areas of the machine.

Without ever even turning it on, is there a best way to take my HSS end mills of difference sizes and say myself something like "since this is 1/2 end mill.. I need to be feeding at (blank) IPM and turning at (blank) RPM." I've found some formula charts off the net, but ill admit that there a tad confusing because it seems like each formula is dependent on some other chunk information I don't have. Is there a rule of thumb where I should start in figuring that out, or should I just throw some metal in and see what happens?