I'm going to cut some sponsor logos in a ignition-cover for a race car.
I suppose it's made in some kind of alu alloy.
The cover is powder coated in black.
My spindle speed is 8000-30.000rpm
My max feed is 800mm/min (~30")
Anyone have some running settings to share?
The cutting will be detailed, so I need to use small bits. (~1/8 or smaller)
I never cut in metal before, and if possible I want to run without cooling liquids...
(or maybe a beer or 2.. )
mr Bond, I've done this several times on steel and alum. I use a .062 ball end mill with 15 inch per min. You want the spindle speed as slow as possible for aluminum since it may get gummy. I use parafin wax on the tooling to keep it clean. You may want to warm the bit first then coat it with the wax. I never used any coolent.
Hope this helps,
Bryson
Mr Bond,
You will get better quailty cuts using endmills intended for aluminum not router bits. And I have had mixed results with the different alloys , 6061 T6 cuts good and the softer alloys tend to smear and coat the bit. Coolant can be a real mess and can be replaced by a proper amount of well directed air. I used a mister that I have for my milling machine but just left the fluid tank empty and turned up the air pressure and mounted it to my router. Be prepared for more noise than you would expect. Keep the RPM down . The feed rate you will just have to play with as you go. Having you machine set up tight and free from vibration will show in your cut quality much more that in wood. I am sure you have thought all of this out in advance and will not have any problems. I have also made some engraved brass plates that turned out good also, just take light cuts and watch chip load. I start off at 8000. RPM (slow as I can go) a feed rate of 0.2 IPS you settings will be different. One last thought , be ready for a big mess to clean up chips end up everywhere.
Tom B
Visalia Ca
This is the result of the cutting.
I'm not 100% sastisfied with it, and 3 bits are now garbage.
The surface was arched in all directions, and I hade to cut deep in some areas to get through in others.
But it is interesting learning new techniques!
I'm not happy with the "tracks" from the bit.
Anyone tried to mask and sandblast it afterwards?
I bet that powder coat was a bugger to cut through
Looks good......bead blasting will get rid of the machine marks....make sure the rest is masked off very tight.
I will use three layers of masking tape over the area to protect and then use light passes with the wand.
Another way to help reduce the machining marks, Is to turn up the RMS and take another .005", you can also increase the feed, but don't increase the feed much.
For anyone having difficulty with machining aluminum, and having the material build up on the cutter, here are a couple of pointers.
1) A lot of commercial products out there are manufactured using 'commercial aluminum' which most times is 1100 grade - utility aluminum. There are
other grades used, but you need to find out what material you are working with if you hope to maximize your machining. 1100 grade is really crappy stuff
to have to machine, so stay away from it if you can. The better grade to use is 6061-T6. This machines much nicer, but it will also build up on your cutter
if you are not careful. Know also that there are various hardnesses of material out there as well. For example the 6061-T6 is different than 6061-O, which is
soft, as it has been annealed to 'O' condition, and creates the same trouble as the 1100 series.
Really nice aluminum to machine is 2024-T3 and 7075-T6 which are standard, common aircraft grades, but quite expensive and they can be hard to find in billet.
2) For cutting fluids, you can use most any standard machining coolant or cutting oil, but there is a cutting oil called 'A9' which is designed for aluminum but it is expensive and
messy to clean up. There are other commercial products out there, but the easiest to use and find is WD-40. Buy it in the gallon containers and use it in a hand
sprayer. It works perfect, it is easy to clean up with soap and water if need be. If you get it too hot, it will create some light smoke and fumes, so you might need
to think about an air exhaust fan in your shop. WD-40 does not provide you with very much, if any cooling ability, it just helps to prevent material build up on the cutter
and it helps to prolong the life of the tool as well. If you dont like the liquid approach, then bee's wax also works well for aluminum, but this is more dangerous as you
need to constantly apply it to the spinning cutter, and fingers are expensive to replace. Just use the WD-40, you dont need a lot, just a periodic light spray as the cutter
moves along. If you need to, you can protect your router table surface with a sheet of plastic, or use a waterproof type of material for the spoil board.
3) For speeds and feeds when machining metal, use the standard speed calculator, which is 'cutting speed x 4 - divided by the diameter of the cutter'. This is a general
rule of thumb for all metals, and is designed for single point / single flute cutters. So if you are using a 2 flute slot drill, then divide the resulting speed by 2, or by 4 if
you are using a 4 flute end mill. If your cutter is made of carbide, then the rule of thumb is to multiply the resulting speed by 3.
So for example, the cutting speed for aluminum is 300, mild steel is 100. So to use a 1/16" diameter 2 flute end mill in aluminum, we take the cutting speed of 300, multiply by 4 to get 1200, and divide by the diameter of .0625 to get a resulting single flute rpm of 18,641. You can now divide this by 2 because we are using a 2 flute cutter and you end up with
a cutting speed of approx 9,000 rpm for your cutter. If this is a solid carbide cutter, you can then assume an approx speed of about 27,000 rpm for the cutter.
I do not like these sort of speeds, so I never use these high speeds anyway. As a machinist, my mill wont go that fast anyway, so for me, I would run the cutter about 2500 rpm
and set the feed at about 15 or 20 ipm. These are just values that I have learned and gotten used to over the years, but you see that the theoretical speeds can be quite high. Note also that if you choose to use these high speeds, you will have heating issues in the metal, and you will likely need to use a flood coolant, which is another argument for slower speeds, and a little squirt of WD-40. The WD-40 will do nothing for you in steel, you need to use cutting oil or coolant. You can cut brass with a dry cutter, but a bit slower than aluminum.
If you are trying to machine aluminum using a router that will not go below 8000 rpm, you may have some problem with heating. Lighter cuts will help, and you will need to keep the feed rates somewhat higher.
