Aluminium milling on the shopbot

There is a lot of misunderstanding out there regarding milling aluminium on CNC routers. i am sharing todays work with some data on feedrates and cutters that you can use as a baseline for doing similar work in your labs. The parts shown is for a ongoing work, my hexapod robot.

The first cut! as you see, these are quite deep pockets. when roughing out areas like these, the key is to always have a good chipload. meaning, that instead of going to slow and just rubbing the metal, go deep and remove it!

Here i took a cut of 7mm, removing 4mm the first pass, then 3,5, before the finishing pass where the last 0,5mm millimeter was removed. all this using a feedrate of 8mm/sek, with a singleflute 6mm carbide bit.

I maxed out the spindle at 18K rpm.

when you buy your bit, buy a upcut! A compression bit will leave good finish on wood, giving a smooth finish with out fraying. on aluminium however, the key is to evacuate the chips as fast as possible. an ucput bit will do just that, dragging the chips out of the cut.

A downcut will do the opposite, it will compress it it down in the cut you are leaving. Wile this works for the first pass, the cutter will break in the next, when you mill over all that compressed swarf.

Do you think you need to buy those expensive german made tools? No. they will last longer, they will give a better finish, but you will do just fine with cheap ebay tools when practicing.

On the long run however, the german and american made carbide tools are the more economic choice, as they can be ran at much higher feedrates, doing the job quicker.

A good tool will also leave a better finish, so that less work is left to do manualy. all the feeds and speeds i post are done with carbide mills. if you buy HSS tooling, i advise you to slow down a little.

This is a huge area that needed to be faced. when doing facing, you should be a bit agressive, so the chips are thrown away, so you dont mill over the chips you just cut loose. in my case, the vacuum system on the CNC mill was wery helpfull.

Here the deapth of cut where kept low at 2mm/sek, but at a higer feedrate of 15, which is realy pushing it when milling hard alloys like this.

Also, see the tiny holes? when drillling deliate features like this, activate peck drilling in vcarve.

This commands the shopbot to only go engage a certain depth of cut at once, then retreat to safeZ.

the depth it will use is set usingPassdepth at the cutter settings. this will break the chips, and avoid clogging the drillbit at the bottom of deep holes.

peck driling also reduces the chance of breaking delicate bit. in my case, the bit measured 2.1mm.

when dealing with tougher materials as aluminium, it is important to secure parts that will fall off, be cut loose or otherwise risk to be dragged into the cutting bit. not only would such an incident break an expensive bit, but can also cause serious injury as the cutter will often exceed speeds of 10K RPM.

when adding such screws, it is advised to make these holes in the vcarve file itself, so that you have specific controll over their position relative to other ares that will be cut.

If you drill these holdown holes by hand, the CNC will not be aware of their position, and may very well crash into them.

can you notice the stepped edge on the part being cut out?

when making deep cuts, you may clog the cutting bit, or risk welding the chips back onto the part itself. to avoid this, make an offset Pocket when making the first pass.

On the next pass, the cutter will not rub the previous edge, reducing workload, chatter and leaving room for clearing the chips. then, in the finnishing pass, make the cut at zero offset, so that you get a nice, shiny edge.

i have found that using climb cutting on both roughing and finishing, leaving 0,5-0,15mm is enough to achive a good finish, as leaving to little will result in rubbing, and a bad finish

For the finishing cut, a feedrate from 4-10 has given me sucsess, depending on the diameter of the cutter. as i mainly make small precise parts, i usualy use a 3mm upcut with one flute for finishing.

The freshly cut upper plate, with circuitboard and other parts mounted. When fitment of other components are determined, the plate will be removed, and the backside machined in a jig cut for the purpose.

I did not bother to do anything about the surface of the aluminium, but if you want to remove the pattern from the machining, a sanding pad with 800+ grid will do it in a few seconds.

This is the underside. for the servos to fit, i had to take a finnishing cut with the 3mm bit. The reason was that the 6mm bit left an excess radius, not alowing the servo to fully slide in. for this operation, i used the following data:

18000 RPM

1,5mm passdepth

5mm/s for feedrate

with a

single flute upcut 3mm carbide bit.

in comparison to the 3mm depth @10mm/sek with the 6mm bit, this went quite slow.

for other tools, you could use as a rule of thumb with pass depth: that you have 50% of the cutter diameter as max, meaning a 5mm bit would yield good results with 2,5mm as pass deapth.

The chips sould be quite rough and sharp. if they are tiny and flaky, or just like powder, you are not cutting agressively enough. That will wear your cutting tool down faster than using the right settings.

remember that milling will always create heat. you don't want that heat to stay in neither the cuttingbit or the material, you want to throw it away With the chips.

To be able to crete such large chips, it is importatant that you use a single or doube flute tool. As having more flutes increase the amount of material removed, you must also increase the feedrate, or lower the RPM to keep the amount of removed material constant.

The aftermath. These will be used to cast the other components of the hexapod.