I read where someone posted (not an exact quote) “The X Carve is not designed or intended to cut aluminum, but it can, you just have to do it slower.” I don’t disagree with that comment if by “do it slower” means it takes longer to cut to the target depth.
Any bit cutting aluminum on any machine is going to generate heat. The amount of heat generated is dependant on the amount of force being applied to the bit as it is cutting and how long the bit stays in the same area. A deeper cut means more of the bit is engaging the aluminum which in turn brings up the temperature of the bit and surrounding aluminum. To cut deeper you have to slow down which means the bit is rubbing more than cutting which also increases the amount of heat generated.
When you reach a critical temperature with aluminum, the aluminum chips become soft and sticky. They begin to stick to your bit and t he aluminum behind your bit that you just cut. This problem compounds itself causing more and more aluminum to stick to your bit until it reaches the point where your bit is no longer cutting the aluminum but plowing through it instead which will result in either a broken bit or your machine stalls. At that point your bit, if it isn’t broken, is full of welded aluminum and no longer usable… trash. Not to mention the part is pretty much ruined as well.
All of the above is assuming that you aren’t already getting an insane amount of chatter that forces you to abort first.
So the key is figuring out how to remove the max amount of material without generating too much heat and or chatter. Chatter can only be eliminated by properly tramming your machine and not putting too much force on the bit by limiting Feed Rate, Depth of Cut, and Step Over.
Here is how each of those affect cutting aluminum.
Feed Rate. Your Feed Rate needs to be fast. High feed rates keep the bit from generating heat by keeping it away from away from the just cut aluminum that has a rising temperature. Think of the temperature increase as a wave moving across the aluminum. You must move fast enough to stay ahead of the wave.
Depth of Cut. A deeper cut depth means more of your bit is engaged with the aluminum which translates to a faster temperature increase. Trying to outrun the temperature “Wave” will likely cause chatter which will ruin your cut. Slowinmg down the feed rate to prevent chatter will allow the heat wave to overtake your bit and everything goes south quickly. So Shallow depth of cust tend to generate less heat and allows your to up your feed rates to outrun the heat wave.
Step Over. I personally never recommend using a stepover between 41% and 80% when cutting anything, especially aluminum. The problem with that range of stepover is that it can cause chatter and doesn’t allow for good chip evacuation. Chip evacuation is critical for aluminum because you never want to re cut chips. That just increases the load on your bit, causes more heat, and reduces the quality of your surface finish. So your stepover needs to be as high as your machine can take up to 40% without developing chatter. Anything greater than 40% I would consider slot cutting which is 100% of the bit diameter. Still doable with the right Feed rate and depth of cut.
So how do you get the correct feeds and speeds? The answer is to start out with the most important one of the three parameters - the Feed Rate. Set this fast enough to outrun the Heat Wave. I suggest 90 to 120 inches per minute. Be sure to always use a Climb cutting for your tool paths - never conventional. Then add a Step Over of 10% to 15% of your bit diameter. Finally add a Depth of Cut starting at 0.003 to 0.005 inches. If you are cutting a pocket then be sure to add ramping to your plunge moves which eases the bit into the aluminum instead of just drilling straight down to depth.
Then try a test cut and see how things go. If all is good, start increasing the depth of cut or step over but not both at the same time. Do another test cut and continue to increase the depth or step over. You will know when you have gone to far because you will either develop chatter or too much heat and the aluminum chips start sticking to the freshly cut walls and or your bit.
Those Pesky chips. Aluminum chips are almost as much an enemy of a successful cut as heat. The best thing you can do is get them out of the way. This can be done with either a vacuum system or forced air. However you decide to do it, just do it.Your bit will thank you. Forced air can blow them out of the path of your bit and offer a bonus of helping to cool the aluminum in the process. Another great way to help control both heat and sticking aluminum is the addition of lubrication.
Lubrication. Lubrication is one of the best possible things you can do to increase your success rate with aluminum. It is also creates the biggest mess. Lubrication can help with chip evacuation when combined with forces air but it’s biggest impact is that it reduces the heat buildup effect of bit rubbing. Watch any youtube video of someone cutting aluminum on a lathe or milling machine and you will see them either using flood coolant or mist coolant systems. At the very lease on a lathe they will use cutting oil. Both flood and mist systems provide a way to either rinse or blow away the aluminum chips and provide lubrication for the bit. The liquid used in these systems is specifically formulated for this purpose and can be a little costly if you aren’t doing a lot of aluminum cutting. A suitable alternative is a spray can of WD-40 with a plastic straw on the spray nozzle to direct the spray and an occasional blast of compressed air. Both will have a significant positive impact on your results especially when used by alternating between them.
With all that said, what you can do on an X-Carve with relative ease is engraving
aluminum with a V-Bit. In fact, I still use my (heavily modified) X-Carve to do the engraving on the Triquetra Touch Plates to this date.
In conclusion, yes you can carve aluminum on an X-Carve if you use the correct settings and control the heat and chips. However the X-Carve is not something that I would want to use for mass producing aluminum parts. That is better suited for a proper cnc milling machine costing at least 10 times that of an X-Carve.
I hope this gives you some insight. If you have any questions please feel free to ask away.
someone tell me I can go to 6-900FR and .5DOC 
