Easel Aluminum Speeds & Feeds

Yes, I did search the forum. But my Australian mm to your American weird inches confuses me. Not to mention some of your dont use easel.

I have 18mm 6061 Aluminium. I’m wanting to cut it using a 1/8 bit (3.175mm).

I used the “Recommended” settings in easel which came to 22 hours. Someone please tell me this isn’t true.

I pretty much always have my Dewalt router setting 3-4 who knows what they mean, not me. But it’s in the middle so seems like that’s what I should have it on.

Easel recommends:
FR: 124mm/min
PR: 76.2mm/min
DOC: 0.1mm

Total Machining time 22h 38min. I don’t have that long :stuck_out_tongue: someone tell me I can go to 6-900FR and .5DOC :smiley:

I have a 2 flute endmill (the one inventables sells).

I always deal in hardwood, never metal, so this is new to me. I’d rather not test on a 22 hour cut.

Choose speed setting #1 (16k RPM)
Try 1200mm/min, keep plunge/DOC as-is and see how that works out.
If that works okay try 0.2mm DOC. With Easel you can change FR on the fly to dial in further as you go.

For 0.5mm or deeper DOC you need a rigid/tight machine.

When you go deeper per cut you need to change the feed rate a little since the cutting edges now do more work, vs tip only when doing 0.1/0.2mm DoC.

Then try RPM setting 1, 640mm/min and 0.5mm DoC (320mm/min per tooth)
This allow for a chip thickness = 0.02mm per revolution/tooth.

Test on a smaller piece before going full scale.
Lubrication will also aid a fair bit, WD40 in a pinch, even air only is better than nothing so chips are cleared from the cut path.

1 Like

The Dewalt manual does. This is for the 611 but it’s probably the same for the 220 version if you have it.

I’ve cut at 48 ipm (about 1200 mm/min) into aluminum with no real issues. Keep the depth relatively low (0.2mm should be fine, I think I did 0.005” which is like 0.15mm.

But overall, yes the Xcarve takes longer to cut aluminum than wood because it’s harder to cut aluminum and honestly, it’s not really what the Xcarve is designed for. Not saying it can’t, it just can’t do it very fast.

BTW - if you are doing pockets and using the 1200mm/min/0.1-0.2mmDoC set step over = 75-80% vs the default 40%
This will further reduce the carve time for pocket/facing operations.

For single line, deep slotting a nicely trammed Z is vital otherwise the shank will rub the slot walls. Chip clearing is also very important for deep slot cutting aswell.

Obstacles of cutting aluminum.

  1. Flexing you will encounter if you try to go too deep with each pass. To see the flex I am talking about simply push down on the top of your router and you will see it move due to the twisting of the gantry and movement in the V Wheels of the Z axis and the Z axis carriage. Shallow cuts help to avoid this flexing.

  2. Feed Rate is critical. Too slow and your bit heats up too much and causes the aluminum to stick to the bit. Too fast and you put too much stress on the gantry and causes flexing or twisting. This will cause the bit to wobble during the cut and can break your bit or at the very least yield a terrible cut finish. I have had success with a feed rate of 75-120 inches per minute with a depth of cut of .007". FR 1905-3048 mm/min DOC 1.778 mm) Keep in mind that I have a beefed up X Carve that has had stiffening mods applied and very good tramming. The higher feed rates keep heat buildup from melting the thin chips that come off the cut.

  3. Tramming. Your Z axis must be trammed as close to perfect as you can get it. If you are out of tram you will get wobble in your straight and ball nose end mills. V bits don’t suffer as much from a slightly out of tramm machine but they don’t like it either. If your way out of tram then a Vbit will drag in one direction and dig in the opposite direction.

  4. Bit selection. No more than 2 flutes on end mills. More flutes will collect the aluminum chips and they will stick to your bit generating too much heat. They will also start sticking to the cut you just made. If you are going to do much aluminum cutting you should get bits designed for cutting aluminum. Drillman1 has an ebay store that sells bits for aluminum. They will last longer and give you a better finish.

  5. Chip Evacuation. One of your worst enemies. The last thing you want to do is let the chips you just cut get in the way of the bit. It’s like chewing sand. Very bad. Keep some air flow going during the cut to blow them away. Air flow also helps keep the bit cool.

  6. Lubrication. Lub is for more than the more fun things in life. It will help to cool your aluminum and bit pluss keep the chips from sticking to your bit and make your bit cut cleaner. WD-40 in a spray can works well because it does more than just lubricate. It can help coll the bit because it comes out cold and also blows the chips away.

Best of luck to you. Cutting Aluminum with the X Carve is possible. I do it daily.

Charley Thomas
Triquetra-CNC

8 Likes

I was reading your comment and I was like this guy sounds like a teacher/professional! Then I seen your sign off and realized you are lkl

lkl ???

It’s the same as “lol” :sweat_smile:

I know I’m a little late here, but what kind of speeds would you recommend?
Do you still suggest the FR 1905-3048 mm/min DOC 1.778 mm?
Thank you!!

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.

2 Likes

If using vcarve (recommend) use ramping in.

I’ve seen an X-Carve with mods doing more depth of pass, slower ipm, with an O flute bit and the cut was beautiful. Like 18ipm feed rate, 18ipm plunge rate (ramped) and 0.01" to 0.015" per pass. Dry. No lube. With dust collector running. If you use lube without flood, you are just asking for the chips to stick to the bit instead of clear.