[thenewguy3]

Hi, i'm relatively new to machining and have a few questions about aluminum milling. I am trying to create a very small and detailed aluminum model with very small end mills. Unfortunately, my machine has a max RPM of 8000, and cannot possibly meet the requested SFM for these end mills. Is there any way I can compensate for this? Thanks...

[mcphill]

2 or 3-flute endmills.

[peteeng]

Hi TNG - The surface speed is more about wear then cutting. The max SFM is a number that gives you good tool life. This is the rubbing speed of the tool. Friction generates heat that creates wear. Friction is generally a function of surface pressure and surface rubbing velocity.

Look up chip load or chip thickness and relate that number back to your 8000rpm. This will give you good cutting characteristics. The end mill supplier usually has a chart for chip loads...Contrary to mcphill when you look at chip load you will find using a 1F tool maybe better....Peter

[joeavaerage]

Hi,
I use small diameter endmills, down to 0.4mm with 0.5mm being my preferred size....cost verses tool strength.
Even with a 24000rpm spindle I would spin them faster if I could. The problem with these small tools is that they are fragile.

When cutting soft metals like aluminum, copper and brass I use this rule-of-thumb to calculate the feed rate.

For a 100% DOC, that is for a 0.5mm tool a 0.5mm depth of cut I allow 1% of diameter per flute per revolution.

Using my own spindle I run small tools at max, ie 24000rpm:

1% of 0.5mm =0.005mm or 5um. I have two flute endmills so 2 x 5um =10um per revolution or 24000 x 10um = 240mm/min.
This is pretty conservative, you can increase the feed rate but eventually you'll load up the tool and snap it.

Lets do the calculation with your spindle, ie 8000rpm:
1% of 0.5mm = 5um. Two flute 2 x 5um =10um per rev or 8000 x 10um = 80mm/min

I have four flute 1.5mm tools, a few rather expensive four flute 0.8mm tools and everything below 0.8mm is two flute.

Doing the same calculation, ie 24000 rpm but with a 4 flute 1.5mm tool:
1% of 1.5mm =15um Four flute 4 x 15um = 60um per rev or 24000 x 60um = 1440mm/min

The strength of the tool is related to its diameter and the stronger the tool the greater thickness chips you can take. Start at 1% per flute per revolution and work your way up.

Note I always use flood coolant on metals...no matter what. If any of the chips begin to adhere to the tool, called 'Built up Edge' then the tool load goes sky high
almost instantly and snaps the tool. Whether you use air blast or mist or flood you must avoid BUE at all costs....it will break your tools faster than you can put them in the machine.

Craig

[peteeng]

Hi TNG and Craig - I was communicating with Suttons Tools the other day about this issue. The guy said 2% was "normal and 4% was heavy, so 1% per tooth per rev is a light cut and I'd expect a light cut with bits under 1mm. Peter

chip load x rpm x N = Feed rate where N is number of teeth, rpm is spindle speed and feed is in compatible units with feed rate eg mm/min or inches /min

[joeavaerage]

Hi,
by in large 1% is pretty light, but then tools under 1mm are pretty tender.

Even then a blanket 1% is an oversimplification, it has a number of variables.

For a given diameter three and four flute tools have greater core area and are stronger......so that 1% may go up, whereas two and single flute tools tend to have less core area
and 1% is ample. Single and two flute tools have larger flutes which aid in chip evacuation and reduce the propensity to BUE. It is perhaps this reason that I really like flood coolant, is does a great
job of washing the chips out of the cut zone and therefore three and four flute tools are not disadvantaged in regard to chip evacuation allowing three and four flute tools with increased core strength
which in turn allows a more aggressive cut or simply a greater safety margin.

The other important consideration is whether this is a slotting cut or a stepover cut. Slotting cuts are always more difficult and are usually done at around half the feed rate. With such light cuts its probable you
are in the territory of giving the material 'a good rub' which is counterproductive. In this circumstance I would reduce the DOC to 50% but keep the feed rate the same.

For example, I have some copper clad circuit board with very heavy copper layers, 12once/yd² or 420um thick or 0.42mm. When I make PCBs with this material the first cut is always
by definition a slotting cut. I therefore make two passes, the first at 0.21mm DOC and then repeat at 0.42mm, but in both cases keep the feed rate up at 400mm/min. The third and subsequent passes
are all stepover passes. I use 50% stepover and 100% DOC still at 400mm/min. I use flood coolant on this PCB material as cutting copper can easily result in BUE.

I might say that it took some experimentation before I arrived at a satisfactory combination that results in a good job and good tool life. My earliest experiments proved that any deviation from this plan
breaks tools fater than I can fit them. Now I can get eight hours cutting with a two flute 0.5mm tool which I consider to be excellent tool life.

The last thing that deserves mention is run-out. Any run-out very dramatically increases the forces on a small tool. Use the best collets you have, make sure they are spotlessly clean and perfectly
fitted and torqued to the spindle. I might get eight hours per 0.5mm tool....if I'm careful.....and fractions of a second if not!

Craig

[peteeng]

Agreed - runout means the chip load theory falls over as one of the teeth will have more load than the others so will lead to early wear or failure. The less the runout the better the cut etc. Peter